Model Engine Maker

Supporting => Tooling & Machines => Topic started by: Jasonb on February 20, 2019, 02:20:51 PM

Title: Going over to the dark (CNC) side!
Post by: Jasonb on February 20, 2019, 02:20:51 PM
This turned up earlier today

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/825074.jpg)

And one of these KX-3 machines was inside

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/825076.jpg)

So it looks like I'm going to have to work out what it does. Where are the handwheels :headscratch:

Not been a bad week for packages as these turned up earlier, now that's what I call a generous chucking spigot :)

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/20190220_141123_zpsiqq8z3vv.jpg)

Title: Re: Going over to the dark side!
Post by: steamer on February 20, 2019, 02:45:57 PM
Do let us know about the KS3
Title: Re: Going over to the dark side!
Post by: b.lindsey on February 20, 2019, 03:00:37 PM
Where's that Darth Vader emoji when you need it  :lolb:

Bill
Title: Re: Going over to the dark side!
Post by: kuhncw on February 20, 2019, 06:04:56 PM
Nothing dark about it.

Enjoy the CNC!

Chuck
Title: Re: Going over to the dark side!
Post by: Jo on February 20, 2019, 06:34:19 PM
Just need a bigger workshop so you can fit it in  ::)

Jo
Title: Re: Going over to the dark side!
Post by: Admiral_dk on February 20, 2019, 09:12:28 PM
Google  "KS-3 machine" did not give any clues and adding CNC to the search was no help either  :headscratch:

Will you elaborate with more info later Jason ?
Title: Re: Going over to the dark side!
Post by: crueby on February 20, 2019, 09:25:02 PM
Google  "KS-3 machine" did not give any clues and adding CNC to the search was no help either  :headscratch:

Will you elaborate with more info later Jason ?
Typo - its a Sieg KX-3
Title: Re: Going over to the dark side!
Post by: kvom on February 20, 2019, 10:09:25 PM
Rather than going to the dark side you have seen the light.   :cheers:
Title: Re: Going over to the dark side!
Post by: Jasonb on February 28, 2019, 09:05:06 AM
I got my Mack3 licence yesterday which meant I could run more than 500 lines of code so had a bit more of a play. The Sieg logo comes as a demo code so I ran that first.

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/825586.jpg)

This machine was a customer return and was known to have issues with the Z axis having been crashed into the top of the column and I was having problems getting the heights right so pulled all the electronics off the back (8 screws) so I could have a better look at the mechanicals, found something loose and tightened that up.  I ran this code about 8 times last night and could not get depths right - (tool finished up higher than when it started) before tightening the loose part. Have run it 3 times this morning and so far all seems OK, will run it a few more times later..

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/825631.jpg)
Title: Re: Going over to the dark side!
Post by: Jasonb on February 28, 2019, 11:21:52 AM
https://www.youtube.com/watch?v=KdVKuZ7b9XI
Title: Re: Going over to the dark side!
Post by: jadge on February 28, 2019, 12:37:42 PM
Never thought I'd see the day..................  :o

Andrew
Title: Re: Going over to the dark side!
Post by: Jasonb on March 01, 2019, 05:55:38 PM
Looks like my days of buying cast iron flywheels could be coming to an end if I can produce ones like this in metal, notice that it even has the spoke halves out of line just like the real thing :shrug:

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/825715.jpg)

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/825716.jpg)
Title: Re: Going over to the dark side!
Post by: b.lindsey on March 01, 2019, 06:30:33 PM
What is the material Jason? Some type of plastic I assume, but looks fuzzy in places so wasn't sure.

Bill
Title: Re: Going over to the dark side!
Post by: ddmckee54 on March 01, 2019, 07:37:19 PM
With fuzzies like that, it's most likely some flavor of that brown stuff that Jo hates.

Don
Title: Re: Going over to the dark side!
Post by: Jasonb on March 01, 2019, 07:50:55 PM
It's just some offcuts of UPVC facia board which has a dense foam type core, not the best for getting a good surface on but ideal for getting the hang of using the machine as it's a bit more forgiving if I get feed rates wrong. Having said that it's happy with me cutting it at 5000rpm and 1500mm/min (60"/min) feed with a 3mm 3-flute cutter.

It does have a black woodgrain finish on one side ;)
Title: Re: Going over to the dark side!
Post by: Admiral_dk on March 01, 2019, 07:58:36 PM
I can relate to your trials as I either cut air first time I try a new G-code file or a piece of soft scrap if possible - my very first was soft wood. Now I just need a mill / router that will do aluminium and steel without problems ... the one at work is for PCB (Printed Circuit Board).

Congratulations with yours and enjoy  :cheers:
Title: Re: Going over to the dark side!
Post by: kvom on March 01, 2019, 10:02:33 PM
I use GWizard for feeds and speeds.  I break very few mills as a result.
Title: Re: Going over to the dark side!
Post by: TobyTetzy on March 02, 2019, 08:21:32 AM
Hello Jason,

you have a great machine, I like it.
I also use Mach3, which CAD and CAM software do you use?

Greeting Toby
Title: Re: Going over to the dark side!
Post by: mikemill on March 02, 2019, 10:23:26 AM
Jason

Welcome to the wonderful world of CNC, you are about to discover a whole new world of model engineering.
Models you made in the past such as enlarged Antony Mount's engines without castings become a lot easier.

I took the plunge eight years ago and have made many models on the mill since. also had bags of fun

A few tips, watch out for is rapid movements crashing into work hold clamps, easy tool change method is to use 6mm throw away cutters in one collet you get a range from 1mm through to 6mm

The only restriction is your imagination

Enjoy

Mike
Title: Re: Going over to the dark side!
Post by: jadge on March 02, 2019, 11:15:48 AM
A few random notes:

Personally I don't like Mach3 - I used a customised version for the Tormach, but the screens are messy and inconsistent, and a lot of the 4th axis stuff plain didn't work. And tool tables weren't stored at the time of filling. I now use PathPilot, which I believe is based on Linux.

Early on (10 years ago) I had a number of issues using a basic PC for control - I've still got the clamp bolt with half the diameter missing after the cutter went doolally. Turned out there was an internal issue with the PC that caused the program to change to incremental mode at a tool change, but only about 1 in 20 times.

After a lot of faffing about touching off tools to fill tool tables I took the plunge and bought an electronic tool height setter - really makes life easy.

I used to air cut before cutting metal for real. Experience shows that my CAM program doesn't always generate G-code that reflects the toolpath it is displaying. I now check the actual code with a backplotter (NcPlot) which gives enough confidence that I don't need to air cut first. If nothing else I get bored air cutting a program that may take several hours to run.

I've tried feed 'n' speed programs, but they seem to produce silly answers. I prefer to use experience to set spindle speeds and the calculate feeds from the cutter manufacturer's recommended chip loads, which can vary within a program according to width of cut to account for chip thinning.

I don't recall anyone mentioning post-processors? I've written my own to include a setup line to ensure I always operate in the planes and units I want and to cancel unwanted modal commands. The post-processor also tells the machine how to interpret some commands, like G02 and G03, that have multiple possible parameters. Since I don't have an autochange tool system I also use the post-processor to move the tool somewhere sensible (home) when a tool change is needed.

One of the real challenges of CNC, which rarely gets a mention, is fixtures. It can require some imagination to design fixtures for the work so that the total area to be machined is clear, the toolholder clears clamps (note toolholder, not just the tool) and the work and/or scrap material doesn't jam things as the cut finishes.

A significant proportion of what I CNC mill are parts I've designed. It pays to think about the machining while doing the design, and there are important differences from manual milling, which requires a different mindset.

There's probably other things I've forgotten, but I now need to get my rear in gear and drive over to Oxford Airport to collect the oxygen cylinder for my glider, which has undergone it's five yearly inspection and pressure test. It runs at 2000psi and sits alongside me in the glider, so it would be messy if it failed.  :embarassed:

Andrew
Title: Re: Going over to the dark side!
Post by: RonGinger on March 02, 2019, 01:23:40 PM
CNC is by far the best way to break tools. A couple days ago I was using a 1/4" end mill to cut out a pocket in a loco frame. A combination of a dumb programming error, I missed a plunge depth setting and went to fast. That overloaded the X motor and a mounting screw slipped so the tool stalled and did a great attempt to friction weld itself to the work. I actually turned the tool cherry red for about a 1/4 inch long. The end is now a melted glob.

All CNC machines seem to have the big red Estop buttons. I believe these are quite useless, as the damage is always done well before you even have the reaction that says its time to hit the button. I saw a custom control panel once that had that button labeled "Oh Shit", I believe a much more appropriate label.

But I will never give it up, when its right it is very good.
Title: Re: Going over to the dark side!
Post by: Woodguy on March 02, 2019, 03:11:29 PM
Just a suggestion - buy or make some machinist's wax, or as an alternate, use blocks of insulating foam for testing.
Title: Re: Going over to the dark side!
Post by: Jasonb on March 02, 2019, 04:30:47 PM
Toby for CAD I have Alibre Professional but not their CAM so may have a go with Fusion360, the code for the things I have cut so far has been done with Vectric Cut2D

Mike, that is what I'm hoping for, I won't be getting rid of the manual mill and can't see me putting a casting onto this one but it should open up some possibilities for creating my own engines where manual would take a long time of just not be possible. I do tend to use FC-3 cutters for most things below 6mm so have a good stock of them.

Andrew, I'm going to try Mack3 to start with especially as it is all  ready set up for this machine and then as I get more used to it decide what way to go. As you know I'm not one for working out speeds and feeds prefering to suck it and see but you don't get the feel through a keyboard like you do on the manual machines but will base my settings on what I am use dto on teh X3 and that is one of the reasons I have recently fitted a tacho to it so I can see what speeds I was actually running at. The funny thing is that bot this and the SX2.7 have the direct belt drive brushless motors and they hardly seem to be running compared to the X3 with its brushed DC motor and gearbox which is so much louder when running.

Ron the UPVC board I have been cutting does have a ridgid foam core so it's a bit forgiving if settings are wrong and I have found the feed override buttom in Mach3 :)

Having said that there is only so much foam you can cut before the lure of metal becomes to much so I mounted up one the 80mm vice on loan from ARC rather than risk my own and put an offcut of 1/4" unknown aluminium in place. The part depth pockets were done with a 3mm FC3 cutter at 2500rpm, 150mm/min feed and 1mm DOC per pass. Different shapes are 1, 3 or 3mm deep. The Cut2D does seem to lift and ramp the cutter down more times that I think it really needs to and there is a slight over cut each time it does this which shows the most around the star. Apart from that you can't feel the pattern left by the cutter with a finger nail.

The two through holes were done with a 6mm FC3 cutter, 2500rpm, 150mm/min and I set it to work out its own depths in 5 passes. Finish seems nice and crisp with no indication of the hole being formed in 5 passes and a quick measure of the the square hole gives 19.99 x 19.98mm for the 20mm on the drawing which I'm reasonably happy with considering the mill is still just sat on the pallet and I have not looked at the gibs or tram.

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/825823.jpg)

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/825824.jpg)

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/825822.jpg)
Title: Re: Going over to the dark side!
Post by: Dave Otto on March 02, 2019, 07:34:15 PM

All CNC machines seem to have the big red Estop buttons. I believe these are quite useless, as the damage is always done well before you even have the reaction that says its time to hit the button. I saw a custom control panel once that had that button labeled "Oh Shit", I believe a much more appropriate label.


Very well could have been my control panel.  :lolb:

Dave
Title: Re: Going over to the dark side!
Post by: kvom on March 02, 2019, 07:39:21 PM
The CAM system I and a number of other here use is CamBam.  You can try it out for quite a while for free.  I think it's quite intuitive.  You'd export DXFs from Alibre and load into CB; then apply a series of machine operations (MOPs) to the drawing.  You can also load STLs for 3D machining.  One benefit from CB is that the user forum is very active, so getting help or answers is quite quick.

The first advantage of CNC is that you never need to use a horizontal rotary table ever again.  Any cut involving and arc or curve is straightforward.

Nothing wrong with Mach3;  I used it for 6 years, although the parallel port interface and kernel interrupt pulsing meant my rapids were limited to 75 ipm (1900 mm/min).  I now run PathPilot;  here a card from Mesa generates the pulsing, and it's much smoother.  I've set rapids to 150, although I could have gone faster.  The screen layout is a lot better too.  The main disadvantage of PathPilot is that one can't jog the axes during a tool change, which is possible with Mach3.  So I need to stop the program, jog to where I can change the tool, and then select the line at which to restart.  The gcode is pretty much identical between the two controls.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on March 03, 2019, 10:43:04 AM
In this thread Jo commented that parts can take a long time to machine by CNC

http://www.modelenginemaker.com/index.php/topic,8873.0.html

I mentioned in that thread that the Forest engine I have been working on had several parts that I thought would be ideal for making with my new machine. I already have the parts modeled in Alibre so quickly exported a DXF of the leg into the vectric Cut2D software and 10mins later as there was a bit of a learning curve as it is the first time I have imported a DXF and have only been using for a couple of days it has produced the code.

The picture attached shows the simulated part after the metal had been "cut" on screen and you can see the top left that it will take 8.23 to cut, add another 1.28 for cutting teh web from the other side and th epart will take approx 10mins to cut, 20mins for the pair.

Doing it manually took me about 5 hours!

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Woody/20190121_1517041_zpszlsrpegf.jpg)

Think I may just cut one for the practice :)

As I said earlier I'm not going to throw my manual machines away but it does seem to make sense to use CNC on some parts.
Title: Re: Going over to the dark (CNC) side!
Post by: Jo on March 03, 2019, 11:38:11 AM
In this thread Jo commented that parts can take a long time to machine by CNC

I asked how long it took:

I can see lots of uses for one but its like 3D printers if it takes hours and hours to do the printing/machining  :Doh:

A CNC mill is a desirable item for the workshop. Being given one for free even more so  ;)

Jo

P.S Mike will confirm that I had been looking to buy a CNC mill  :-X
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on March 03, 2019, 11:49:32 AM
How are going to hold the stock for that part?

For the pocket, another option is to cut the inner through pocket first.,  then machine the flange with a profile.

Does your program support nesting?  That's the kind of part where you could do both at the same time.  If nesting isn't an option, then duplicate the polylines.

Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on March 03, 2019, 12:01:16 PM

The picture attached shows the simulated part after the metal had been "cut" on screen and you can see the top left that it will take 8.23 to cut, add another 1.28 for cutting teh web from the other side and th epart will take approx 10mins to cut, 20mins for the pair.

Jason,

 I will believe you when you have actually done it in that time.

Mike
Title: Re: Going over to the dark (CNC) side!
Post by: Muzzer on March 03, 2019, 12:20:27 PM
Jason

Check out the standalone controllers like this one https://madmodder.net/index.php/topic,11598.0.html (https://madmodder.net/index.php/topic,11598.0.html) which doesn't require a PC, software, breakout board etc. John Stevenson and Steve Blackmore looked into this and were very pleased with what they found. I'd have thought something like that would be ideal for this machine.

If you want something a bit more serious, there are things like this https://newker-cnc.en.alibaba.com/product/60612188303-804601673/CNC_kit_NEW990MDCa_4_axis_for_cnc_machine_all_replace_for_gsk_cnc_controller.html?spm=a2700.icbuShop.41413.10.441e5e63dmyi40 (https://newker-cnc.en.alibaba.com/product/60612188303-804601673/CNC_kit_NEW990MDCa_4_axis_for_cnc_machine_all_replace_for_gsk_cnc_controller.html?spm=a2700.icbuShop.41413.10.441e5e63dmyi40) I got one for around £400 but that may be a bit OTT for what you need.

Murray
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on March 03, 2019, 01:40:46 PM
Jo,

 I based my comment on this one of yours, my bold

Quote
I can see lots of uses for one but its like 3D printers if it takes hours and hours to do the printing/machining  :Doh:

Kvom,

 I actually cut from a larger piece of material and if you look at the simulation there are some tabs around the outside. I'm happy to leave tabs as the parts had all the corners knocked off after machining to make them look more like castings and less like cut from barstock.


I've not looked for nesting but will do so and can see it would be good if you had several parts, for now just moving the flat bar along in the vice is OK.

Mike (Vixen)

I ran a test in the UPVC and it cut in that time though could have been a lot faster. After doing that I thought I would play safe as it's early days and reduced DOC to 1mm but did up the speed to 3000rpm and added an extra tab. This added about 3mins to the job according to Cut2D.

I'd be interested to know what sort of time you would expect it to take from your machine or anybody else for that matter, let me know if you want the part file. I'm just using a 6mm FC-3 cutter for now and could go faster if I changed to an aluminium specific cutter, also don't have any chip clearance or lubrication sorted yet so need time to keep up with that manually.

Murray,

Good to see you chipping in here, would definately be interested in how long this would take you as having seen your machine in action it can shift metal at a fair old lick :o

Yes I remember the posts about the alternative driver over on ME but will stick with this setup for a while until I find out what I want out of the machine.



So this is the test piece done in the 8mins for the main side, you can see the tabs around the edge but it has not cut through as its thicker than the metal part.

(http://img.photobucket.com/albums/v156/jasonballamy/Engineering/DSC03554_zpsooinstol.jpg)

Now when I loaded up the revised code for the metal version I noticed that there was an extra path showing on the screen. Should really have stopped there and sorted it out but decided to just keep the mouse over the stop button.

(http://img.photobucket.com/albums/v156/jasonballamy/Engineering/DSC03553_zpsgoru6qf6.jpg)

At least I have learn one thing today as with about 30secs left to run I got one of the unique features that Jo mentioned but stopped it soon enough so I need to trust whats on the screen

(http://img.photobucket.com/albums/v156/jasonballamy/Engineering/20190303_122727_zpszatyultn.jpg)

I did not video all the cutting but have stitched 3 clips together which show approx the first cut of each of the three paths, think I could also speed up the ramping which would reduce overall time a bit.

https://www.youtube.com/watch?v=zyzXaDW7chs




Title: Re: Going over to the dark (CNC) side!
Post by: steamer on March 03, 2019, 02:05:32 PM
Yup    cnc tends to be pricey..    Yup it takes a while to climb the learning curve hill.   What isnt being mentioned is the set up time saved.   The tooling saved.

Think about those curves.   On the manual, theyre a RT job and a break down and set up cycle.   Everytime you break it down and set back up is time and loss  of accuracy.   You need to spend money ona rotary table and the furniture it takes to use it.    You need to schelp it on and off the mill, and you need to store it.  With CNC...you need an endmill Nd one set up.    Used right, cnc rocks!
Dave
Title: Re: Going over to the dark (CNC) side!
Post by: b.lindsey on March 03, 2019, 03:49:53 PM
Dave, remind me which tormach you have at work?

Bill
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on March 03, 2019, 04:26:49 PM
Apart from the fact that I used a scrap bit of 6mm aluminium that had a hole just in the wrong place this is it with all the machining done from the front. Just under 12mins from pressing run to completion.

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/DSC03555_zpsdp0kqawh.jpg)

I'm sure it could be run faster, at least that is what Ketan is telling me but then again I don't think he knows machines can be run slower than 5000rpm  :ThumbsUp: Also he and the late JS used these these machines to make parts to sell so they don't want to be wasting time.

I'm sure JS has a chuckle in his grave when people say they prefer British Made tools, what would they say if they knew he was banging them out on a similar machine to mine along with all those extras for Myfords :LittleDevil:

(http://www.stevenson-engineers.co.uk/files/lathetools1.jpg)
Title: Re: Going over to the dark (CNC) side!
Post by: crueby on March 03, 2019, 04:28:45 PM
Much satisfaction to be had from cranking the mill with your own paws,  but there is!      Hmmmm!!
(https://i.postimg.cc/9F1NqK7D/IMG-2336a.jpg)
Title: Re: Going over to the dark (CNC) side!
Post by: steamer on March 03, 2019, 04:29:42 PM
Dave, remind me which tormach you have at work?

Bill
Tormach  PCNC 440
Title: Re: Going over to the dark (CNC) side!
Post by: b.lindsey on March 03, 2019, 05:02:20 PM
Ok thanks.

Bill
Title: Re: Going over to the dark (CNC) side!
Post by: Woodguy on March 03, 2019, 05:10:58 PM
I converted my SX-3 to CNC and have used it quite a lot. The problem with it though is that is has a maximum spindle speed of 1800 rpm. Since many of the parts I wanted to make were small, and needed small cutters, the machine required extremely slow feed rates. A good feeds and speeds calculator like GWizard is very helpful in keeping cutters in one piece.  Using the biggest cutter that would do the job was essential.


Fusion 360's cam really works well and the adaptive clearance toolpath is particularly useful.


I solved my spindle speed problem by shifting those parts to my CNC router with a 24K rpm spindle.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on March 03, 2019, 05:19:37 PM
Yup    cnc tends to be pricey..    Yup it takes a while to climb the learning curve hill.   What isnt being mentioned is the set up time saved.   The tooling saved.

............................................

Quite so Dave, I needed two plates machining to mount the parts onto with a different ctr point on each and each part needed to be mounted and removed six times. Not to mention the constant worry of winding a handle too far!
Title: Re: Going over to the dark side!
Post by: jadge on March 03, 2019, 08:17:16 PM
I now run PathPilot;  here a card from Mesa generates the pulsing, and it's much smoother.  I've set rapids to 150, although I could have gone faster.  The screen layout is a lot better too.  The main disadvantage of PathPilot is that one can't jog the axes during a tool change, which is possible with Mach3.

Yes, that's a bit of a pain. I used to manually add a G00 Z move to the program just before each toolchange. But I kept forgetting, so I've now set a reference point on the machine and I've tweaked the post-processor to include a G30 command as part of the toolchange sequence.

Another issue with PathPilot is that being a US program the metric side is a bit cavalier. A maximum jog increment of 10mm is likely to require an underwear change if you're not expecting it! Although I design in both metric and imperial I run the CNC mill solely in metric, mostly with metric cutters.

Andrew
Title: Re: Going over to the dark (CNC) side!
Post by: jadge on March 03, 2019, 08:51:35 PM
A few more random thoughts:

A CNC mill and 3D printer are not the same. One is a subtractive process and other is an additive process. The way parts are designed for each machine is different. Something that is easy on a CNC mill may be difficult on a 3D printer and vice versa. The 3D printer is certainly the slowest, as one is limited by the fixed nozzle diameter and limit range of height steps. Whereas for a CNC mill you can just use a bigger cutter, within the power limits of the machine. A useful feature of the more complex CAM programs is re-machining. As an example take the nameplate made by JasonB. To decrease cutting time you could rough out the shape using a large cutter. And then remachine with a smaller cutter to finish off the small internal radii. The CAM program knows where the larger cutter has been, so the smaller cutter only mills out the features it needs to.

My CNC machining times have ranged from less than a minute to over 6 hours. But of course you can go and do something else, like make tea or cut the lawn while it's running. Same for a 3D printer, I sometimes leave mine running overnight.

I'd have tackled the engine pillars in a slightly different way. I'd have done a helix all the way through in the centre and then incremented out, leaving about 0.5mm of stock. Then I'd have done a profile pass full depth to finish using a circular approach and retract. That way you avoid possible tool marks from multiple passes, and minimise tool deflection. I'd then take out the recess in one pass. For the outer profile I'd probably do it in two depth passes, again leaving about 0.5mm stock. Followed by a full depth profiling pass. I'd probably leave the tabs, but experience shows they're a PITA to remove without impairing the visual appearance of the part. At least I'd try and put them in places that mate with other parts so they're not seen.

Using a CNC mill has changed the way I design parts and assemblies, and has also changed the way I machine, some of which has fed it's way back to the way I use the Bridgeport mill.

There are several uses for the CNC mill in my workshop:

To make repetitive parts, like traction engine wheel spokes that would be a pain to do manually

To make parts that could be done manually but would be time consuming to set up - like radii and fancy profiles

To make parts that are impossible on my manual machines like special cutters and true bevel gears

To save time and avoid foul ups when making parts commercially

Andrew
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on March 03, 2019, 11:55:16 PM
My PathPilot screen has 1mm as the maximum jog.  I also set jog feed rate to 40% of rapid.
Title: Re: Going over to the dark (CNC) side!
Post by: steamer on March 04, 2019, 12:54:29 AM
My PathPilot screen has 1mm as the maximum jog.  I also set jog feed rate to 40% of rapid.

Ditto
Title: Re: Going over to the dark (CNC) side!
Post by: Jo on March 04, 2019, 07:31:36 AM
Using a CNC mill has changed the way I design parts and assemblies, and has also changed the way I machine, some of which has fed it's way back to the way I use the Bridgeport mill. There are several uses for the CNC mill in my workshop:

To make repetitive parts, like traction engine wheel spokes that would be a pain to do manually

To make parts that could be done manually but would be time consuming to set up - like radii and fancy profiles

To make parts that are impossible on my manual machines like special cutters and true bevel gears

To save time and avoid foul ups when making parts commercially

Thanks Andrew, all of those confirm my thoughts of having CNC at home.

Short term I am delaying acquiring CNC as it is too much like what I used to do at work and I am trying to forget that horrible time of my life  :ShakeHead: Longer term with the likes of Honda pulling out of the UK I suspect there are going to be a number of machine tool acquisition opportunities to be had over the next two years and I can see CNC being in the mix of tools that become available so it could be something to spend some spare cash on invest in  :-X The far easterner tool manufacturers, once you get above their built down to a price DIY machines, do a reasonable compact CNC - the one Jason was given was one I was looking at but I couldn't justify the cost  :hellno: .

As for uses of a CNC ... I do have a number of engines with multiple items - there are a few traction engine spokes to make :) but the items that are really going to be multiples are my big rotary/radial builds - the Anzanis, the Bentley and the Gnomes. I am not sure if the straight 4 engines would benefit from CNC as much  :noidea:


One of the advantages of being retired is you have plenty of time  :headscratch:

Jo

 
 
Title: Re: Going over to the dark (CNC) side!
Post by: jadge on March 04, 2019, 09:22:31 AM
My PathPilot screen has 1mm as the maximum jog.  I also set jog feed rate to 40% of rapid.

That's useful to know. I contacted Tormach about the issue and they promised to change the values. I'm still using an early version of PathPilot, so it may be that Tormach did indeed update the values in a later release.

Andrew
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on March 04, 2019, 01:03:31 PM

I'd have tackled the engine pillars in a slightly different way. I'd have done a helix all the way through in the centre and then incremented out, leaving about 0.5mm of stock. Then I'd have done a profile pass full depth to finish using a circular approach and retract. That way you avoid possible tool marks from multiple passes, and minimise tool deflection. I'd then take out the recess in one pass. For the outer profile I'd probably do it in two depth passes, again leaving about 0.5mm stock. Followed by a full depth profiling pass. I'd probably leave the tabs, but experience shows they're a PITA to remove without impairing the visual appearance of the part. At least I'd try and put them in places that mate with other parts so they're not seen.

Andrew

Thanks Andrew, that make sense as you get to use all of the cutter and as you say no risk of the various passes showing down the edges. I've done that with Cut2D and it does not make much difference to the suggested time though I did do the outer profile in 4 rather than two. May give it a run if I can find another bit of scrap Ali.
Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on March 04, 2019, 01:37:56 PM
My PathPilot screen has 1mm as the maximum jog.  I also set jog feed rate to 40% of rapid.

That's useful to know. I contacted Tormach about the issue and they promised to change the values. I'm still using an early version of PathPilot, so it may be that Tormach did indeed update the values in a later release.

Andrew

PathPilot is derived from LinuxCNC.

With LinuxCNC, the jog increments are defined in the . INI file.

Go to the machines . INI file, in the [DISLAY] section you will find the INCREMENTS parameters listed. You can change and save the INCREMENTS parameters

I do not know if this works for Pathpilot as well as LinuxCNC. It is worth a try, you can always return to the original setup. :zap:

Mike

Title: Re: Going over to the dark (CNC) side!
Post by: jadge on March 04, 2019, 03:57:38 PM
I do not know if this works for Pathpilot as well as LinuxCNC. It is worth a try, you can always return to the original setup. :zap:

Me + fiddling with computer software internals =  disaster

Company IT managers have been known to turn white when I appear at their desk.  ::)

It's pretty windy here today, so I haven't gone out to the gliding club to rig my glider and measure the control deflections. Instead this afternoon I have updated my PathPilot to Tormach version 1.9.13 and lo and behold the metric jog steps have changed to slightly more sensible numbers. PathPilot is now on version 2.x, but to upgrade to V2 I need to buy a USB stick. Which will probably cost more to ship to the UK than the cost of the stick.  :(

Andrew
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on March 04, 2019, 04:18:14 PM
A good practice is to place tabs on straight surfaces rather than curves.  Easier to clean up.  They don't need to be as large as yours.

For your engine parts, a no-tab solution would be to use stock thicker than needed.  The outer profile would then be milled so that it doesn't cut through.  Then fill the slot with an epoxy gel, wait for it to harden, and then face mill the back side to reveal the part.  The place in boiling water to release the epoxy.

Instead of epoxy, cut a pocket in some soft jaws that matches the output profile.  Then you can hold it securely when removing the bottom layer.  This is a good solution when making a lot of copies.
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on March 04, 2019, 04:25:03 PM
@jadge

I'm running the 1.9 version myself on non-Tormach equipment and see no reason to update.  The CD version costs $100, and I doubt the USB stick would be more.

Notice that typing G20 in MDI will change the jog steps and DRO values to imperial; G21 back again.  Even when machining a metric part, I will often switch to imperial since I'm using an edge finder with a .200" diameter.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on March 04, 2019, 05:02:41 PM
This is the Cut2D version with the paths suggested by Andrew.

I have used smaller tabs but put them on surfaces that are not going to mate with others - the flat bottom and concave top therefor have clean machined mating faces. As I said the rest will get the corners knocked off with a dremel and files to get a better "cast" look and then be painted so my thinking is better to have the tabs there in this instance.

https://www.youtube.com/watch?v=Gmv35vSUwtY
Title: Re: Going over to the dark (CNC) side!
Post by: jadge on March 05, 2019, 08:42:55 AM
I'm running the 1.9 version myself on non-Tormach equipment and see no reason to update.  The CD version costs $100, and I doubt the USB stick would be more.

The USB stick for V2.x is $24.95; I've ordered one. Unexpectly the order went through with 'free' postage. Not sure I believe that! I had some trouble updating my profile (clunky website software) but it should be clear I'm outside the US. We'll have to wait and see what happens.

Andrew
Title: Re: Going over to the dark (CNC) side!
Post by: gary.a.ayres on March 06, 2019, 12:27:05 PM
Jason -

the potential of this is huge.

Enjoy!
Title: Re: Going over to the dark (CNC) side!
Post by: DICKEYBIRD on March 06, 2019, 08:33:10 PM
@jadge00

 Even when machining a metric part, I will often switch to imperial since I'm using an edge finder with a .200" diameter.
After screwing up a part or 2 doing the edge finder switch-eroo, I recently started touching off my .200" E/F @ 2.54 mm.  Works great & no more miscues!
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on March 06, 2019, 09:17:04 PM
@jadge00

 Even when machining a metric part, I will often switch to imperial since I'm using an edge finder with a .200" diameter.
After screwing up a part or 2 doing the edge finder switch-eroo, I recently started touching off my .200" E/F @ 2.54 mm.  Works great & no more miscues!

One reason I do it the other way is when my stock isn't metric and I'm center finding using opposing sides, seeing the DRO at expected dimension + .2" gives a degree of confidence that I didn't screw it up.  Note that until the current engine build I'd never machined any metric parts, so habits are hard to break.
Title: Re: Going over to the dark (CNC) side!
Post by: jadge on March 06, 2019, 09:54:12 PM
I use a Haimer Zero Master to pick up edges. Using one means you don't need to worry about imperial or metric units, simply jog until the needle is on zero.

Andrew
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on March 06, 2019, 11:58:00 PM
I use a Haimer Zero Master to pick up edges. Using one means you don't need to worry about imperial or metric units, simply jog until the needle is on zero.

Andrew

I recently bought a Haimer Taster.  The problem I've had with it is that I don't have a pendant and use the keyboard to job.  Accidentally hitting an arrow key instead of PgUp has resulted in destroying 2 of the probes at a cost of $50 each time.  So now it's confined to the Bridgeport.   >:(
Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on March 07, 2019, 12:32:58 PM
For edge finding, centre finding and other work, I use a 3 axis touch probe and the LinuxCNC Probe Screen utility

(http://lister-engine.com/coppermine/albums/userpics/10013/P1070333.JPG)

The probe is permanently mounted on a quick change toolholder and has a replaceable Haimer stylus.

The LinuxCNC Probe Screen utility will automatically find an inside or outside edge, corner, hole centre or bar centre at the touch of a button. The probe makes some beautifully choreographed moves to find the required edge or corner or centre, then moves to the clearance height resetting the appropriate X or Y coordinates to zero.

I crashed one of those expensive Haimer stylus tips while initially setting the search parameters. After that, I set the search speed fairly low ( 10 and 2 inches per minute) to be within human reaction times rather than having it whizzing about at the speed of light. The lower search speeds only add about 10 to 15 seconds to each operation, but is much safer.

I am very pleased with the touch probe and the  LinuxCNC Probe Screen utility. It works for me.

Mike
Title: Re: Going over to the dark (CNC) side!
Post by: jadge on March 07, 2019, 12:35:43 PM

Accidentally hitting an arrow key instead of PgUp has resulted in destroying 2 of the probes at a cost of $50 each time.  So now it's confined to the Bridgeport.   >:(

I feel your pain. At the end of last year I broke the probe on my Zero Master. I managed to break mine on the Bridgeport by turning the handle the wrong way while in a rush to finish a job for work. :'(

Andrew
Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on March 07, 2019, 01:18:21 PM
Here is the tutorial, installation and user guide for the LinuxCNC Probe Screen utility.

https://vers.by/en/blog/useful-articles/probe-screen

If you are a LinuxCNC user, you will find this a very useful tool. It may also work with Pathpilot, but I have not tried that yet.

Mike
Title: Re: Going over to the dark (CNC) side!
Post by: Muzzer on March 09, 2019, 01:02:02 PM

Murray,

Good to see you chipping in here, would definitely be interested in how long this would take you as having seen your machine in action it can shift metal at a fair old lick :o

I couldn't answer that without the CAD file of course but generally my approach is to select a modern cutter, look up the manufacturer's data for its feeds and speeds and use these as my starting point in Fusion to program the CAM. These are often a lot more aggressive than I'd have guessed and with a bit of testing you can get a feel for what you can actually achieve on your machine. Some of the modern cutters and inserts are significantly better than those of a decade or so ago, so it's worth trying a few out. They are often less prone to chatter and give higher removal rates (MMRs), lower cutting forces and better surface finishes. Generally I do a roughing operation followed by a finishing operation, rather than one single pass.

Currently Fusion doesn't report the spindle power required to support the resulting feeds and speeds so sometimes I've checked it won't exceed the available power by using one of the tool apps from Iscar, Sandvik etc. I believe Fusion will soon include an estimate of spindle power, so that extra step won't be needed soon. However, although I have only(?) 3kW available, that's enough for some pretty decent MMRs.

I always try to use as much of the flute length as possible, which is made easier by these modern adaptive toolpaths. It evens out tool wear and makes best use of adaptive toolpaths. My "big" machine is from the 1980s and cost as much as a house back then but the toolpaths at the time were very basic, manually coded rectilinear and circular things, whereas modern toolpaths can essentially follow almost any locus. The result is that the machine is now much more versatile and able to much achieve greater MMRs with less risk of breakage than it could previously. The original owner would be pretty surprised to see what it can do now!

To answer your question, once the part is programmed into Fusion CAM, the simulation gives a pretty accurate machining time estimate. In practice I find any significant difference is due to my manual tool changes rather than the machining itself.

One thing I learned fairly early on is the need to clear the (aluminium) swarf from the cutting zone to avoid it being "recut" when achieving high MMRs. Recutting can result in an inconsistent surface finish but above all it leads to the risk of swarf becoming welded to the cutter (ping!). Air and/or high flow coolant is the best way to avoid it!

Murray
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on March 09, 2019, 03:43:58 PM
I myself tend to be conservative with feeds and speeds as very few parts I make as a hobbyist are critical as to machining time.  A production shop may well decide to test a cutter to destruction, or at least run with spindle power meter at 100%.

Recently CamBam has added an operation for trochoidal pocketing and profiling, which is quite similar to adaptive paths.  Large depth of cut (use more of the side slutes), small stepover, and higher feeds.  This definitely improves chip clearance when machining aluminum as well.
Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on March 09, 2019, 09:30:50 PM

Recently CamBam has added an operation for trochoidal pocketing and profiling, which is quite similar to adaptive paths. 

Hi Kvom,

I am considering changing over to CanBam. The latest documented issue, available over here in the UK, appears to be Issue 0.9.8 which does not appear to offer trochoidal pocketing. Can you tell me which version of CamBam I should be looking for which includes the trochoidal pocketing or whether it is an external add-on produced by an outsider.

Thanks

Mike
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on March 09, 2019, 10:31:41 PM
The latest is v1.0 "CamBam Plus".  While is says it's developmental, the reality is that most long term users have moved over from .9.8.  Trochoidal pocking and profiling were added by a user, and work quite well.

It is installed in the base product by copying the trochomops.dll to the Plugins directory.

The trochoidal profile and pocket DLL is available for both versions
Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on March 09, 2019, 11:13:45 PM
Thanks for the advise to use issue V1.0 of CamBam and how to add the trochomops.dll to the Plugins directory. I will certainly give that a try.

In the mean time, do you have a copy of a small trochoidal pocket G-code file that I could use to test my Emco F1 mill? That would give me confidence in my machine's ability to cope with this type of high speed machining.

Thanks again for your help

Mike
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on March 10, 2019, 12:43:49 AM
Attaching the .nc file.  The pocket is 50mm square centered on 0,0, 5mm deep.  Tool is 1/4" (6.35mm) endmill.  Roughing clearance 1mm.

Toolpath is plunge to 5mm, then spiral out with a .2 stepover until the sides are reached,  Then each corner is milled with arcs of decreasing diameter.  I didn't know what material or tool, so feeds are notional.  You can do a global replace with appropriate values.  Here I specified only climb milling, so each arc is followed by a G1 to the start point of the next arc.  The program does allow bi-directional arcs, but I usually do it this way to allow chip clearance in aluminum.

If you'd like a better test, provide a DXF/tool spec/meterial and I can easily generate it.

FWIW, all of the aluminum pieces of the hummingbird were machined this way.
Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on March 10, 2019, 01:00:50 PM
Due to our time zone differences, your trochoidal tool path file arrived overnight. I only got to play with it after all the mornings household chores were done.

My Mill runs under LinuxCNC control and is set up to machine in inches. Your toolpath are in metric units. I thought that could be a problem but fortunately LinuxCNC recognised the G21 (metric units) and made all the necessary conversions to inch measurements and displayed the trochoidal toolpaths accordingly. That's another first; something else learned.

I pressed the 'RUN' button with some trepidation and off went the machine. The spindle ramped up mto 4,000 rpm and machined air at a feed rate of 24"/ min (600mm/min). All appears to be working well, my mill can handle the feed rates and acceleration in both axes without apparent problem. However, the speed at which the tool moves arround is staggeringly fast, many times faster than I have ever machined anything before. That will take a bit of getting used to. The next thing is to try machining some metal.

Before I can do that, could you please generate a smaller test program, so that I can use the cutters and stock material I have available in the shop. I do not yet know how to attach a file to these posts, so I will have to use words instead. Please could you generate the tool path to make a rectangular pocket, again with 0,0 in the centre, measuring 20mm x 30mm and 6mm deep in aluminium, with a HSS, 5mm diameter three flute end cutting tool. My machine can go to 6000 RPM. I have air blast to clear the chips but no pumped coolant other than a can of WD40

Feeds and speeds must be critical to this high speed machining. What feed and speed calculator do you use? How close to maximum theoretical do you need to run the feeds? Is it OK to slow the feeds down or does that upset the way this high speed machining works?

Thanks again for your support

Mike

BTW.   my petite Colibri hummingbirds built a nest and laid some acrylic eggs.

(http://lister-engine.com/coppermine/albums/userpics/10013/P1050478BB~0.jpg)



Title: Re: Going over to the dark (CNC) side!
Post by: jadge on March 10, 2019, 01:49:02 PM
High speed machining is a bit of a misnomer. It would be better to call the toolpaths constant engagement. To machine a pocket with a conventional rectangular toolpath at each step the cutter has to move across to the next path potentially at full width. So the DOC, and feeds, need to take that into account, despite the linear cutting being done at less than full width. The idea of the high speed paths is that the tool moves so as to keep the cutter engagement constant. Thus DOC, WOC and feeds can be set for those parameters, which are used for the whole machining cycle.

The term high speed machining really relates to maximising the metal removal rate by keeping the cutting parameters constant. It doesn't inherently imply running the cutter at high spindle speeds and feeds. Although of course that would normally be done in a commercial environment to minimise time. Any high speed toolpath will run perfectly well with slow speeds and feeds.

Andrew
Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on March 10, 2019, 02:38:33 PM
Andrew,

Thanks for you excellent explanation. The concept of constant engagement toolpaths now make perfect sense. The knowledge that a high speed toolpath will run perfectly well with slower speeds and feeds is very reassuring. I guess the wear and tear on the machinery will also be considerably reduced at the lower rates.

It looks like the high speed, Trochoidal pocketing and profiling plug-ins to CaBam will be very useful addition.

Mike
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on March 10, 2019, 04:00:43 PM
Attached file as per your request.  I use G-Wizard for feed and speed.  I specified 20mm stickout and 50% roughing as additional inputs.  So feed rate is conservative.  Deflection of the tool is .01mm or 56% of breaking point.  Power is .038 kw, mrr 4.33 cc/min, estimated machining time 1:06.

The CB implementation doesn't allow for the non-cutting chords between slices to be generated as rapids, so I chose 1000mm/min arbitrarily.  You could do a global change of the g-code to reduce the speed or to replace G1 F1000.0 with G0.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on March 10, 2019, 04:38:26 PM
Thanks for the detail answer Murray and all the other posts which have been interesting to read. I have not had a chance to play with the KX3 this week (see Allman thread)  but hope to get some time soon.

J
Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on March 10, 2019, 04:53:03 PM
Kvom, thanks for all your help and support,

66 seconds to demolish all that material...........and you say you have used a conservative feed rate!!!!!!!!

Off out to the workshop to try it for real :noidea:

Thanks again

Mike
Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on March 10, 2019, 05:53:02 PM
Kvom,

I found I could only command the spindle to 5,400 RPM, so I slowed the feed rate to 80% to compensate.

I have never seen chips fly so fast and so far.

With is Trochoidal milling strategy, I can now achieve the same (once seemingly impossible feeds and speeds and MMR) as Andrew

Thanks

Mike
Title: Re: Going over to the dark (CNC) side!
Post by: fumopuc on March 11, 2019, 01:11:24 PM
Hi Jason, I am following your learning curve with the Sieg CNC milling machine with great interest.
I have seen that you are using Vetric software for your first steps. This was also my first choice in 2013, when I have entered the dark side.
In April 2017 I have started the Fusion 360 adventure.
My regular process during the Fusion CAD learning curve was:
Creating a 3D model in Fusion followed by creating a DXF export for the CNC operation.
Importing the dxf file into the Vetric software and getting the toolpathes there.
At the end a very complicated process, but due to laziness or " I have done it always like this" I have used this process until end of November last year.
In my Christmas holidays I took the opportunity and tried the CAM Modul in Fusion360 seriously.
After doing the first parts, I have quickly recognized, that there is a huge and comfortable tool hidden behind this  "CAM" button in Fusion360.
So every possible minute was used to follow some Fusion360 CAM tutorials for learning.
The current status at this issue is, that since beginning of December 2018 my Vetric software is hidden in a dusty corner of my hard disc and I am afraid it will stay there for longer.
Finally is there only the question for me, why does it took so much time to find this way ?
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on March 11, 2019, 02:29:58 PM
For someone who uses F360, the built-in CAM makes a lot of sense. 

I use Solidworks which I get for free as a veteran, but the CAM packages that integrate with it are from 3rd parties and not free.  For that reason I use CamBam, which is relatively cheap for a lifetime license and which I find intuitive to use.  I still do the DXF export/import, but it's not overly complex.

Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on March 11, 2019, 04:18:47 PM
Achim, I got the vectric thrown in for free so that was really my only reason for using it and it seems quite simple to use. Although I draw in Alibre I had already looked at teh F360 CAM and will give that a go now that the machine seems to be behaving itself. I have already imported some STL files from alibre and done some simulated cuts to get curved surfaces (in Z) which you can do with a DXG file in Vectric Cut2D.
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on March 11, 2019, 07:55:25 PM
FYI.  Cambam can do 3D surfaces and supports molds, where the positive surface is inverted in Z.  One of the most active members on the CB forum has a business making molds for fishing lures.

One thing that CB lacks at present, that other 3D CAM software may have, is "rest" machining.  The simplest type of 3D machining is a roughing pass for which one can use regular endmills, and the finish pass where a bullnose type cutter is needed.  What one would like ideally in some cases is two or more roughing passes where extra passes can use smaller tools to get close to the desired surface;  in other words, roughing the rest.  If that feature isn't present, then the machine spends much of the time cutting air on the second pass.

One needs to be careful with STL files found on the internet, as they may have problems that CAM programs can't handle.  There are several programs available for repairing the meshes on STLs.  Meshlab is one I've seen recommended.
Title: Re: Going over to the dark (CNC) side!
Post by: jadge on March 19, 2019, 10:45:21 AM
The USB stick for V2.x is $24.95; I've ordered one. Unexpectly the order went through with 'free' postage.

I received the USB stick today. It was indeed free postage. But I got stung for £20.57p by ParcelForce for import duty and "handling" charge. Not so much force as darn right extortion.  >:(

Andrew
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 07, 2019, 12:09:21 PM
It is all well and good cutting random shapes into bits of scrap to get the feel of things but nothing beats making more productive swarf. To this end I have been drawing up the next stationary steam engine for a while and was possibly going to get a couple of the parts laser cut but now that I have the CNC what better way to learn and be productive at the same time. The base "casting" of the engine will be a sandwich of 3 layers so I started with the bottom one, the upper is similar but has some different holes and bosses.


A Step file of the required part was exported out of Alibre and into a F360's CAM program where I generated the G-code for the holes and the actual shape as separate sets of code to make it easier for me rather than have to incorporate tool changes. I air ran the code first of all and then again into some PVC which showed up a slight error in heights which was corrected before cutting metal.

I started by clamping the stock onto some MDF and first ran code for eight 3mm holes, then after changing bits ran another code to enlarge four holes to 6mm. After that these holes were used to screw the 2.5mm thick plate to the MDF so that the clamps could be removed. After changing to a 6mm 3-flute HSS FC-3 cutter the button was pressed. I'm more than happy with what came out for my first proper part using CAM and the first time cutting steel and this plate is a bit gummy.

A couple of areas did not quite cut all the way through which was probably due to the scrap MDF that had been sitting around for a while but that just tore away. You can also see that I left some 1mm thick tabs to stop the larger pieces of waste moving about.

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/828461.jpg)

After a quick clean up

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/828462.jpg)
Title: Re: Going over to the dark (CNC) side!
Post by: Admiral_dk on April 07, 2019, 08:33:19 PM
Looking good Jason  :ThumbsUp:

I can't say that I'm surprised that you had a few places that didn't go all the way through ....

When I use the small CNC-Router at work, I use a template cut in high quality plywood that holds an Euro-Card PCB (160x100mm.) and even though the router itself has cut that pocket, I still get small variations.
This means that if I need to cut the PCB to a "strange" shape when all the rest of the milling is done, I let the cut go aprox. 0.5mm into the wood in the pocket (except the tabs) in order to ensure a clean cut-out.
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on April 08, 2019, 01:33:44 AM
Does the single STP file encompass all sides of the part?  If so, how do you select the view and edges that encompass the machining?

In SolidWorks, I select a view of the part and export a DXF of that view.  For 3D surfaces, I export STL.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 08, 2019, 07:18:18 AM
Yes, it comes out as a complete 3D part in F360 so I can pick any feature as the geometry to cut. You can also select what way the part will be orientated on the machine if you did not draw it with the axis in the best position for machining. You can also enter the size of the stock so it knows what you are starting with.

This is the imported part showing the path of the tool and the second picture shows the end of the cutting simulation with the stock shown

This series of videos are what I used to see how to do it with F360

https://www.youtube.com/watch?v=6FzbZNhey2w
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 09, 2019, 06:26:18 PM
I had a bit of time this afternoon so thought I would do the top plate, I did not air cut this time but did practice on some PVC before cutting metal.

First was to drill 15No 2.5mm holes with a split point stub drill which meant I could get away without spot drilling first

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/828628.jpg)

Then a change to a 6mm stub drill to open up six of the holes

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/828629.jpg)

Using these holes the plate was screwed down to the MDF below and clamps removed. Using a 6mm dia 3-flute cutter but carbide this time the profile was cut, not a bad finish on the bottom of the first pass.

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/828630.jpg)

All complete, the 6mm piloted holes that open out to the edge were enlarged to 8mm as part of the contour cut and I left tabs again to stop the waste flying about.

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/828631.jpg)

After a clean up with the bottom plate that I cut at the weekend.

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/828632.jpg)

I've stitched two videos together here, the beginning shows the first pass with the cutter at full width but 1mm away from the finished edge, second half shows the final full depth finishing cut, you can see the tool rise and fall where the tabs are located. The upload to Youtube seems to have added some high pitch noise which was not there at the time.

(https://www.youtube.com/watch?v=HWVk5nqtSXc)

I could quite get to like this CNC lark, next part has been through the CAM and will let me try some adaptive clearing cuts!
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on April 09, 2019, 08:33:50 PM
You could have added additional screw holes for the 3 extra pieces, and then avoided using and cleaning up the tabs.

Another hack that can save time is to use center cutting endmills for drilling.  In this case a 2.5mm tool could be used to spiral drill the 6mm holes.  That saves a tool change, but here you needed the 6mm tool for the next op.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 09, 2019, 08:44:34 PM
Funny enough I was thinking the same about the extra holes as even with a ctr cutting bit and a slow plunge the drop down after the tab was the one item where the cutter did not seem happy.

Not tried spiral cutting a hole yet but hope to give it a go soon.
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on April 10, 2019, 12:43:16 AM
Spiral cutting is especially useful when you don't have a drill of the size you need.  Plunge milling makes a lot of sense for  roughing deep pockets; the Z axis of mills is almost always stouter than the X or Y, and there are no lateral forces to bend the tool.  In place where you might do chain drilling, you can plunge mill at less than a 100% stepover.

I usually make my tab length 3x the height.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 13, 2019, 08:14:55 PM
The adventure continues with this part which will be the bottom mounting flange of the cylinder.

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/828892.jpg)

First operation was to run the code which put the four 3mm holes into an oversize piece of 1/4" flat steel bar. I then put an offcut of aluminium into the vice and ran the code again but this time with a 2.5mm drill, the holes were then hand tapped and the two screwed together without removing the aluminium tooling plate from the vice.

With a 6mm dia 3-flute carbide cutter I first ran an adaptive clearing cut around the outside followed but a final contouring cut to finished size. I started off quite tame at 3000rpm and 150mm/min feed but found that could be upped as the flat bar cut a lot better than the steel plate I was cutting the other day.

The next part of the code had the adaptive clearing to form the 4 raised bosses, this again had been programmed as above but found I could go faster and ended up at 3900rpm and 225mm/min feed.

Again Youtube has added some high frequency noise but you can see the first cut around the outside where the DOC varies as I only rough centered the work followed by 3 clips of the top clearing at various stages.

https://www.youtube.com/watch?v=dd4sHBimQ-g

Final job was to skim the bottom off, final size will be done after silver soldering the assembly together.

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/828889.jpg)

Intention is to have a 20mm block between the bosses so a quick test with an ARC 10-20-40 block to see what the fit is like

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/828890.jpg)

Can't get much better than this

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/828891.jpg)
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on April 14, 2019, 01:12:22 AM
Why is the return move on each clearing cut so slow?
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 14, 2019, 07:34:52 AM
Why is the return move on each clearing cut so slow?

Because I still have a lot to learn :-[

I have now found the box where the "non engagement feed rate" can be set, looks like it defaults to the cutting feed rate so I have now increased that and will know it needs to be done the next time I use the Adaptive.

Out of interest do you set the speed of these return movements the same as the rest of your rapids or less?

J
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 14, 2019, 10:43:02 AM
Over on ME Forum I have also been advised to set the adaptive to cut in both directions which makes it quicker still, I had just been using climb cutting.
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on April 14, 2019, 12:32:06 PM
The bi-directional feed rate is good, but for aluminum I use only climb.  That allows air blast to clear any chips and prevent welding during the non cutting move.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 16, 2019, 07:13:32 PM
To finish the sandwich construction of the engine base some form of filling was needed and as I have quite a few off cuts of Corian I decided to use that rather than metal.

The sequence was much the same as the top and bottom plates but I tried out peck drilling for the 3mm holes as they were quite a bit deeper than before, I could have gone faster with the retract speed and not lifted so far out of the work, drill was running at 5000rpm.

I used a chip breaker feed for the larger holes, you can't see it that well on the video but can hear when the drill pauses the feed which if I was drilling steel or Ali would shorten the swarf, dropped down to 1000rpm on the 6mm and 7.8mm holes.

Finally machining the contour where you can see the tool ramp down and then start cutting in 2mm deep passes before it starts to get lost in the swarf which is when I stopped filiming and got the vacuum running. The 3-flute Carbide cutter romped through this at 5000rpm and 350mm/min feed.

https://www.youtube.com/watch?v=QekBlcNrIqI


I did not use any tabs this time as the material was thicker than needed, bottom milled off afterwards.

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/829128.jpg)

Quite pleased with the cut edge, no sign of cutter marks when held upto the light, this was a full depth finishing pass

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/829129.jpg)

I used a 50mm face cutter to thin the work down to 10mm moving the clamps to complete the ends, only downside to working with Corian is the mess.

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/829126.jpg)

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/829127.jpg)

I'll bond it all together with JB Weld but that won't be until the bearing supports have been fabricated and silver soldered to the top plate but could not resist a quick trial assembly.

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/829132.jpg)

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/829130.jpg)

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/829131.jpg)
Title: Re: Going over to the dark (CNC) side!
Post by: Admiral_dk on April 16, 2019, 09:46:33 PM
Nice progress so far and I like the combination of the different materials  :ThumbsUp:
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 18, 2019, 06:49:00 PM
A post on another thread brought up the subject of the "Star Wheel" used on the Alyn Foundry "Sphinx" engine which is an alternative to timing gears and operated the exhaust valve on alternate strokes. A casting is supplied but I happened to mention that  it would be something worth trying to cut on the CNC. Well that was all it took to get me trying it out.

Video firstly shows the adaptive clearing, I speeded things up 20% after filming so that was a 6mm Carbide 3-flute cutter at 3600rpm, 150mm/min, full 8mm height cut with a conservative 0.25mm DOC. I went with Andrews suggestion of cutting both ways which reduced the time quite a bit. It was cutting very nicely and I did not bother with brushing on anymore suds which only seemed to make the swarf stick to the work.

There is then a clip of a 4mm dia cutter clearing further into the internal corners which went well but during the final contouring cuts it went pop which almost made me go poop. It was a cheapie and at a cut height of 2D I was probably asking for trouble. I had drawn in a corner radius of 2.1mm but that probably should have been more.

Video ends having reverted back to the 6mm cutter for the final contour cuts which I slowed down so that it would not chatter in the corners.

https://www.youtube.com/watch?v=ypy7-kxYlIQ
 
This pic shows the star wheel after the first clearance cuts, you can see the faceting of the curves.
 
(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/829227.jpg)
 
This is after all the milling where the curves flow better. Interesting to see the three height bands left by the tool, although it has not done much they show the wear from the 2.5mm plate, the 1/4" flat bar and the best finish at the top which can be seen better in the video is unused edge.
 
(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/829231.jpg)
 
All that remained was to file out the internal corners, casting shown alongside. Just need to put it away somewhere safe and resist all temptation to do more on this engine for a while.
 
(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/829232.jpg)

Simulation of the cutting

https://www.youtube.com/watch?v=DIVmWdXQ8d8
Title: Re: Going over to the dark (CNC) side!
Post by: Johnmcc69 on April 18, 2019, 07:03:03 PM
 :ThumbsUp:
 Pretty cool stuff Jason! Modeling the parts, creating the program, & watching it work, is pretty exciting.

  :popcorn:

 John
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on April 18, 2019, 10:07:17 PM
That is the type of part I prefer to make from stock vs. the casting as well.

Thoughts:  The big nut on top meant that your tool stick out was higher than it needed to be.  Generally you want the collet to be clamped as close to the flutes as possible and the profile cut to be as high on the flutes as possible.  4mm mill got deflected too much.

According to G-wizard, if the stickout were 12mm, a DOC of .25mm would allow a feedrate of 800mm/min in 6061 for a MRR of 1.68 cc/min.  But a DOC of 40% of tool diameter (2.4mm) with a feed of 213 mm/min has a MRR of 10.25.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 21, 2019, 05:26:56 PM
Just a small item today in the form of an elliptical gland flange, used an aluminium specific cutter as they also work well in other non ferrous metals and a split point Dormer stub drill for the 2mm holes.

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/829424.jpg)

I cut another star wheel but took the different route of drilling 2mm holes at the root of all the internal corners which made filing to final shape a lot easier than leaving the 2mm radius from the 4mm cutter.

(https://oimg.photobucket.com/albums/v156/jasonballamy/Hit%20n%20Miss/20190419_185827_zpsnjjbrvtz.jpg)

(https://oimg.photobucket.com/albums/v156/jasonballamy/Hit%20n%20Miss/20190419_192428_zpsrgthoqk1.jpg)
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on July 04, 2019, 07:03:50 PM
I've not had the need to do much on the KX3 over the last couple of months but thought I had better blow the dust off it and see if it (and me) could handle something a bit more complicated. I have been drawing up a 24mm bore single cylinder 4 stroke with side rods loosly based on a design published in Practical Mechanics in 1938 with the intention of CNC machining the two crankcase halves.

So with a piece of 1" 6082 T6 aluminium mounted onto a holding block I loaded up the code and let rip.

The first 3 clips in the video show the 3D adaptive clearing which was done using one of ARC's 6mm 2-flute aluminium specific HSS cutters, I was in two minds whether to use this as I had noticed a bit of chatter when using it in the manual mill in the past particularly as I wanted 27mm sticking out of the collet so that would not crash into the work but after a chat with Ketan a while back I decided to give it a go. 5000rpm, 8.5mm height of cut (1/3rd stock height) 1mm depth of cut, feed rate of 300mm per min giving achip load of 0.03mm which was just right and did not need altering. 0.5mm material left for finishing

4th clip is the same as above except height is reduced as the surface was between the two 8.5mm increments, this is where a tiny amount of chatter could be heard on the lighter loaded cutter.

Clips 5-7 are the 3D contour which was used as the sides of the crankcase all have draft angle rather than vertical sides. I used a 2-flute carbide 6mm cutter with 1.0mm corner radius. Again run at 5000rpm, with a 0.5mm stepdown and the DOC was the 0.5mm that was left, feed 400mm/min. In hindsight a 4 flute cutter would have been better as the amount of swarf was not great so the 2-flutes extra clearing capacity was not needed and then I could have fed faster.

Clip 8 Spotting the bolt holes with a 5mm HSS spotting drill at 5000rpm

Lastly drilling the 3mm holes with a Dormer A002 split point drill at 5000rpm and using a pecking cycle to clear the swarf.

https://www.youtube.com/watch?v=IDQwAdshtOQ

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/834211.jpg)

The bit of flash around the bottom is due to me doing the CAM for 25mm stock but using 1" , there are a couple of things I will alter slightly for the other half but overall I'm quite pleased with how it turned out. particularly the tapered surfaces as I was expecting them to need more fettling but they are quite smooth and will just need a quick rub with emery before blasting the surface to get it to look like a casting.
Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on July 04, 2019, 09:45:44 PM
Looks like you are getting the hang of this CNC stuff. Well done.
Remind me again who's software you are using. Is it Fusion 360 for the CAD/ CAM and Mach 3 for the machine control?
The draft angle slopes look good. Can you go curvy slopes or just straight angles?
Mike
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on July 05, 2019, 07:13:45 AM
I draw with Alibre Pro and then export a STEP file into F360 to generate the code and use Mach-3 on the machine, I wanted to get the part done before Saturday so you could look it over and point out any things I could try differently.

Yes the CAM will let me do all sorts of shapes and I should probably have done a finer stepdown on the curved section under the cylinder mounting flange so will see if I can add that to teh other half.

Is this curved enough for you?

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/829660.jpg)
Title: Re: Going over to the dark (CNC) side!
Post by: Muzzer on July 05, 2019, 12:40:42 PM
Looks pretty reasonable Jason! Takes a while to get used to creating the toolpaths, feeds and speeds, heights etc but in the end I find I can do things you simply couldn't make on a manual process and even with the extra time for programming the CAM, the overall time is a lot less for those that you could - there's considerably less faffing about with setup between ops.

One real benefit of Fusion is the fact that the CAD and CAM are closely integrated which means you can quickly and easily alternate between the CAM toolpath generation and the CAD model design and back again. The reality is that when you come to programming up the CAM, you often find you want to finesse the CAD model. Moving only one way (via STP format) is very limiting. Just saying....

One neat and powerful feature of Fusion CAM is the ability to save the part-machined output of one CAM setup as a mesh (STL) file and then reuse that as the stock for the next setup eg when you turn the part over to finish the other side. When you run the toolpath simulation, you can right click on the resulting machined stock and "save as" an STL. Then "insert" it into the CAD environment - this creates a body. When you do the next CAM setup, you can select that body as your stock and Fusion will know where what is really in front of it. Works really well and avoids "surprises".
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on July 05, 2019, 01:18:50 PM
Thanks Murray, good to have your input which I've missed from ME

I noticed early on when watching a couple of Lars' videos that he jumped back into the CAD to make an alteration, as you say easy when it is all in one place and would be useful as the final design is tweaked. What I need to look into now is using the same set of operations for the other half which is basically a mirror image rather than having to enter them again though the practice will be good for me anyway.


I don't have any air/lube set up yet so tend to stay by the machine so probably not as productive as leaving it to it's own devices but at this stage I'm happy to watch and see if it is doing what I hoped it would. I've not yet tried anything with a second setup but may be tempted to at least do the main cavity inside the crankcase as that has no critical surfaces but either way will bore the bearing holes in the lathe with the two halves fixed together to ensure things line up 100%. It would be easier than a second setup after turning to bore the area around the cam shaft.
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on July 05, 2019, 01:40:49 PM
(http://One neat and powerful feature of Fusion CAM is the ability to save the part-machined output of one CAM setup as a mesh (STL) file and then reuse that as the stock for the next setup eg when you turn the part over to finish the other side.)

This is called "rest" machining; you can program to the rest of the part after a roughing op.  That's something I don't have with CamBam.  One use of this feature that would be very welcome is multiple roughing passing.  Large tool to start and smaller tool afterwards, to save machine time.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on July 05, 2019, 01:45:23 PM
(http://One neat and powerful feature of Fusion CAM is the ability to save the part-machined output of one CAM setup as a mesh (STL) file and then reuse that as the stock for the next setup eg when you turn the part over to finish the other side.)

This is called "rest" machining; you can program to the rest of the part after a roughing op. 

Fusion seems to do that anyway, for example on that part i first did the adaptive clearing to leave 0.5mm and then without saving or altering the setup did the 3d contour and it just removed the remaining 0.5mm, then did a couple of parallel cuts to do the flat surfaces the contour missed. Drill started from that flat surface.

EDIt, just tried it with two sizes of cutter and there is a "rest" setting that comes up when doing the clearing cuts which has option such as"from stock" or "from previous machining" but that is with the part held in the same position.

Title: Re: Going over to the dark (CNC) side!
Post by: jadge on July 05, 2019, 05:46:51 PM
In my CAM system, for 2.5D, it's called re-machining. The key point is that one can pocket or profile using a large cutter and then re-machine only the corners using a smaller cutter. So overall machining time is considerably less. In 3D things get rather more complicated, in name anyway. There are several operations, such as re-roughing or valley machining, that all add up to the same thing. Using a smaller cutter to remove just the material left in awkward corners or fillets.

Andrew
Title: Re: Going over to the dark (CNC) side!
Post by: Muzzer on July 05, 2019, 07:37:38 PM
Yes, "rest machining" relates to a series of operations within one "setup". If you turn the part over, you create another setup. My comment about saving the part machined stock as a model for the next setup is relevant when you come to machining the rest of your engine block eg from a different direction.

Dunno how you are supposed to insert an image into this thread but I've attached a view of a part machined component from one setup which has been used as the stock for the next setup. This worked very nicely.

One of the best improvements I've made to my machine setup has been the addition of a proper electronic touch probe. I got an old Renishaw probe from ebay which connects into my Acorn controller and allows me to pick up features within 5um or so, which is better than my machine can machine to. It means I can return the part to the vise and finesse dimensions etc by tiny amounts (10um increments). It's also invaluable for picking up the part origin on the next setup. With thought, you can choose a feature that was machined in the previous setup and use that to transfer your coordinate system without introducing an unintentional offset.
Title: Re: Going over to the dark (CNC) side!
Post by: RonGinger on July 06, 2019, 02:38:25 AM
Wow! what a finish on that part. Can you tell us about the tool used, speeds and feed, and the type of machine it was done on. It must be a very rigid machine.
Title: Re: Going over to the dark (CNC) side!
Post by: Muzzer on July 06, 2019, 12:56:34 PM
It's a 1983 Shizuoka AN-S fitted with Centroid Acorn controller and CNCdrives DC servo drives. When fitted with these modern controls and running modern tools and toolpaths, even old machines are capable of some amazing output. It's bigger than a Bridgeport but is a turret mill too.

I find that good quality modern tooling is easier to drive (variable helix, sharper edges, lower forces, less chatter) and produces a better surface finish than classical cutters of a decade ago, in the same way that lathe tooling continues to progress. I have some cutters with lapped edges that produce a mirror-like finish in aluminium but they are razor sharp and lethal to handle. The variable helix cutters are particularly good for machining steel and I really like the YG-1 V7 range (stocked by Cutwel in the UK). They are on "3 for 2" offer at the moment...

The cutter that did most of the work is a 10mm three flute uncoated long series end mill from APT Tools, although Ketan's are probably just as good. I tend to use big step downs (to use as much of the flute length as possible) and use the adaptive toolpaths where possible. The term "optimal load" refers to how wide the cutting zone is relative to the cutter diameter, so a typical 20% would equate to 2mm here. I always use climb milling to avoid rubbing and get a better chip. It also tends to chatter less. And I try to avoid using the end of the end mill to do a finish pass, if at all possible using the side of the cutter instead.

It's worth exploring what your machine is capable of, either by being prepared to sacrifice a couple of cutters in the interests of science or by being human and accidentally overdoing it from time to time without bottling out. Often I have found that spindle speed is the limitation that prevents me following the manufacturer's advice on feeds and speeds for a given cutter. Chatter tends to happen when I have excessive overhang or am taking a heavy cut in thin stock.

For aluminium I use flood coolant or WD40 but above all, clearing the swarf is critical, to avoid recutting and tool welding / breakage. Like Jason, I attend closely to avoid mishaps. If I had a fully enclosed machine with high flow coolant, perhaps I could leave it unattended. In my dreams.

If you have a few idle moments, I posted some videos of various operations, including a couple of "moments":
https://www.youtube.com/channel/UCo5vJdD8q3xQ0xCrZfi9dIA (https://www.youtube.com/channel/UCo5vJdD8q3xQ0xCrZfi9dIA)
Title: Re: Going over to the dark (CNC) side!
Post by: RonGinger on July 06, 2019, 02:23:26 PM
Thanks, that is pretty impressive. My modified JET knee mill has never come close to that kind of finish.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on July 21, 2019, 05:34:14 PM
Nothing too adventurous this weekend I just used the mill to contour and drill the square cylinder flange for the Little Midget engine.

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Midget/20190721_085620_zpsk79bxzxb.jpg)

Must be doing something right a sit fitted onto the two crankcase halves OK.

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Midget/20190721_090733_zpsi6gs32ep.jpg)

Unfortunately word has got out that I have the CNC and I got a call from my brother asking if my new toy tool could make a replacement part for a lamp my Niece had bought for when she goes off to Uni in the autumn, couldn't really say no.

https://www.youtube.com/watch?v=URk_F6GPeUI
Title: Re: Going over to the dark (CNC) side!
Post by: vcutajar on July 21, 2019, 08:41:48 PM
Always love to see small CNC machines in action.

Vince
Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on July 23, 2019, 10:39:17 PM
Today was a hot day and I spent all afternoon working the Emco Compact 5 CNC Lathe. I had a batch of 30 small diameter (0.125", 3.175mm) brass rods to make, which needed to be a tight clearance fit in a ceramic bead. When I started the workshop air temperature was a pleasant 21*C, the air temperature rose to 30*C during the afternoon. The CNC stepper motors were noticeably hotter than normal and must have contributed to the workshop temperature.

I machined the brass rod to the required diameter in small diameter increments followed by three spring cuts to produce a consistent final diameter. I noticed that every hour or so, as the temperature increased; I needed to correct the final diameter by a thou (0.001") to continue to achieve the required tight clearance fit. I put his down to thermal expansion of the whole lathe structure, due to the higher than normal ambient temperature and the hotter running stepper motors.

Technical tip: The normal axes convention for a CNC Lathe is Z axis for length and X axis for diameter. I find this can lead to confusion and possible errors if you frequently switch between the CNC mill and the CNC lathe. To avoid this pitfall, I have a second set-up for the lathe, based on mill practice. I use the X axis for left/ right (length) movement and the Y axis for fore/ aft (diameter) movement. I find this mill like set-up on the lathe to be far more natural and less prone to error. An added advantage is being able to use the same CAM software to produce tool paths for both the mill and the lathe.

Mike
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on July 28, 2019, 01:15:04 PM
Another epic adventure to the very dark side with some Cast Iron needing reducing to swarf, one additional advantage of using the CNC is you don't get dirtly which seems to put some people off using this material

After a slight glitch with the latest Alibre update which was very promptly dealt with by their forum and support on a Saturday morning I was able to do the CAM for the cylinder head. The stock was roughed out on the lathe from some 50mm CI bar and two holes drilled and tapped where the valve holes will eventually be bored and I used these to hold it to a block that could be held in the vice.

Video starts off with the adaptive clearing with a 6mm 3-flute carbide cutter, 4500rpm, 300mm/min feed. 5mm high cut x 1mm DOC. I set the  CAM to cut in 5mm deep increments to use the edge of the tool and it then works back up in 1mm steps to cut to the specified 0.5mm that is left for finishing. Bit of chatter from the tool when cutting conventionally but it's happier climb milling. Same tooling for the finish contour at the top of the valve guides as I wanted a sharp internal corner.

Then onto the 3D contour using 6mm 4-flute R1 corner radius carbide bull nose cutter, 4750rpm, 400mm/min feed and 0.33mm stepdown, could have done finer on the more horizontal surfaces but happy to do a bit of file work to get that "cast look"


Finally Drilling with 3mm split point stub drill 2500rpm.


It's about time Jo diverted some of her casting fund to a CNC machine, ideal for knocking out multiple Anzani Heads :LittleDevil:

https://www.youtube.com/watch?v=A3ymCvgD5-s

Title: Re: Going over to the dark (CNC) side!
Post by: Johnmcc69 on July 28, 2019, 02:40:01 PM
 :ThumbsUp:
Very nice Jason!

 John
Title: Re: Going over to the dark (CNC) side!
Post by: fumopuc on July 28, 2019, 03:05:32 PM
Hi Jason, seeing your last video, it looks like that Fusion does not mil a circle, it looks like several small faces added.
Did you try already the tick in the box at "Glättungsfilter" ?
I know it is German, but I am sure you will find it in your Fuison immediately.


Title: Re: Going over to the dark (CNC) side!
Post by: Muzzer on July 28, 2019, 03:53:28 PM
That's "smoothing" in the English language version. It's present as an option in most of the Fusion CAM operations but for some reason it's not set by default. I always try to remember to enable it.

The adaptive toolpaths are roughing operations, so to get the best finish, you need to select a Contour operation to follow the Adaptive - and remember to set smoothing! Sounds as if Jason did use a Contour toolpath at the end but it's not clear if that was applied to the surface(s) you were talking about.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on July 28, 2019, 04:41:32 PM
The first 5mins are adaptive clearing (roughing) cuts leaving 0.5mm material as Murray says and these do tend to leave a "faceted" edge which can be seen on the top small diameter of the valve guides, around the sloping spark plug surface and also the lower flange particularly on external curves where the tool leads in and leads out. Not really visible in the concave "counterbores" where the holes go

At about 5mins into the video it starts on a contour where the cutter spirals down around the tops of the valve guides and you then cannot see the facets, you don't get to see any remaining contour cuts on the above mentioned surfaces, just some around the elliptical shaped section

I did not have smoothing on for the contour cuts as it did not seem to make a difference on the simulation both in appearance and time taken to cut. Looking at the finished part under a magnifying glass I cannot see any signs of facets (flats) just the slight ripple from the tool which is the same on the flat flanges either side, can't feel anything either.

If I get a chance I will do a test piece with smoothing on and off and report back
Title: Re: Going over to the dark (CNC) side!
Post by: Muzzer on July 29, 2019, 06:03:32 PM
There's some pretty useful background on smoothing in Fusion 360 CAM here https://forums.autodesk.com/t5/fusion-360-manufacture/understanding-smoothing/td-p/6636189 (https://forums.autodesk.com/t5/fusion-360-manufacture/understanding-smoothing/td-p/6636189) if you are interested / have a few spare minutes.

If you prefer sound and light, John Saunders did a short video on the subject:
[youtube1]https://www.youtube.com/watch?v=kSI8FaNpO8k&t=147s[/youtube1]
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on July 29, 2019, 07:04:02 PM
Thank's for that Murray, I opted for the video.

If I do as he shows and click to show the points along the tool path I can see that I just have a point at the start of the circular flange and one at the end so it is moving in an arc not a series of facets, then cuts a short straight cut out to the oval flange, arc around the corner and then straight along the face of the oval flange. This is confirmed by looking at the code with is all G2, G1, G2, etc

So no need to use smoothing on these finish contour cuts.

J
Title: Re: Going over to the dark (CNC) side!
Post by: Muzzer on July 29, 2019, 07:38:58 PM
Indeed - nothing to be gained there. It comes down to the fact that machine moves are a series of either straight lines or circular arcs (or both together, aka helices). Once you understand that, you have an idea where smoothing could benefit you and where you would be wasting your time.

The main source of noncircularity on my work is the residual backlash. Even with reasonably minimal backlash on my machine (perhaps 10-20um on a decent cut), I see a witness mark where the X or Y axis changes direction. Although some controllers claim to have backlash compensation, the reality is you can't get rid of such a nonlinearity in the plant model with smart control software and you have to live with it.
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on July 29, 2019, 11:55:28 PM
In CamBam, the Cam I use, splines need to be first converted to polylines, and then the equivalent to Fusion smoothing is to do an arc fit with a specified tolerance.

I suppose Fusion can import DXF files, and some CAD programs may generate polylines or arcs with many small segments.  The same smoothing techniques are applicable here as well to reduce the number of segments.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on August 17, 2019, 08:35:27 PM
next part for the Midget engine that could be done on the CNC were the rocker arms which were cut on the opposite ends of a bit of 1.5" x 0.25" flat steel bar.

First a clearing cut all round with 6mm 3-flute cutter at full depth plus 1.1mm to give the later 1mm R corner mill clearance, this then rises up and roughs out the top contour in 0.5mm steps.

Followed by a 4mm dia 4-flute 1mm R corner cutter working it's way down in 0.2mm steps on the flatter surfaces then 1mm as it gets to the vertical.

Side shot of the work so far.

Then a shot after it was sawn off the bar and held in machined jaws to bring down to 5mm thickness in the X3

Then back with the 4mm bit to contour the other side again held in the machined jaws

Finished parts after a lick with a needle file.

https://www.youtube.com/watch?v=kO9qIaB77vA
Title: Re: Going over to the dark (CNC) side!
Post by: vcutajar on August 17, 2019, 11:39:58 PM
Nice  :ThumbsUp:

Vince
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on August 21, 2019, 04:14:34 PM
Thank's Vince

I found a bit of time to run the CAM for some cams. In the past I would either have used CamCalc with multiple offsets of the mill at angular increments around the cam or used the inside out boring head method particularly on cams like this with a flank radius. Both of which take a while to setup and in the CamCalc case a long while to cut.

This time with 0.4mm deep x 5.5mm high roughing passes and a slightly slower fed 0.2mm DOC finish pass on the silver steel the cam was done in 2.30secs mins with no need to do any blending with files after. I can't see me wanting to go back the the old ways of doing things.

https://www.youtube.com/watch?v=LymJwG9oBi8
Title: Re: Going over to the dark (CNC) side!
Post by: tangler on August 21, 2019, 06:41:34 PM
 That's the way to do it.
 :ThumbsUp:

Rod
Title: Re: Going over to the dark (CNC) side!
Post by: Muzzer on August 21, 2019, 07:57:46 PM
I was impressed by the idea of completing the operation in 2.3 seconds. However, 2.5 minutes is still pretty respectable!

Nice result.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on August 21, 2019, 08:10:56 PM
Did I not say the video was in slow motion :-[
Title: Re: Going over to the dark (CNC) side!
Post by: Admiral_dk on August 21, 2019, 09:13:42 PM
Very nice Jason  :cheers:

I can't remember if you have a fourth axis for your CNC, but if you do, I'm curious about doing the same at 90 degree to what you just did - why - well if you need several cams on the same shaft, it could soon be necessary ....

Best wishes

Per
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on August 22, 2019, 07:15:37 AM
I only have 3-axis but the machine comes with all the boards and drivers for a 4th axis, I also have a Sieg rotary table here so would just need to fit a stepper motor and then plug it into the socket provided at the back of the machine.
Title: Re: Going over to the dark (CNC) side!
Post by: jadge on August 22, 2019, 08:53:39 AM
I can't see me wanting to go back the the [sic] old ways of doing things.
Blimey, that's a handbrake turn from what you wrote recently on another forum about willy-waving rights when doing it manually.  :o

Andrew
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on August 22, 2019, 09:11:10 AM
I'm happy to not wave it about as much.  ;)

Having done it both ways I still think those who make their cams manually deserve a right to wave and I would probably still do it for a one piece camshaft with multiple lobes but seeing as I now have the machine it would be rude not to make use of it for certain jobs.

Though I wonder if a short cam could be cut vertically using something like a tee slot cutter to do several lobes :thinking: Might have to put the Hoglet cam into F360 and see if I can do it. Would certainly make it a lot quicker to play with different cam profiles and timing if you were after performance from an engine.
Title: Re: Going over to the dark (CNC) side!
Post by: jadge on August 22, 2019, 09:23:52 AM
I'm happy to not wave it about as much.  ;)
Better nip over to the other forum and correct the blooper in your reply to ChrisJ this morning then. I can't imagine many people wanting to hit it with a lump hammer.  ::)

Andrew
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on August 22, 2019, 09:52:55 AM
I can't imagine many people wanting to hit it with a lump hammer.  ::)

Certainly won't do any good to the hardening :o
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on August 22, 2019, 02:07:32 PM
I have mentally designed a system to machine cam lobes with a 4th axis, but it requires programming.  The idea is to draw the lobe profile in CAD, and then break the polyline into some number of straight lines.  Each line is defined by the points on its ends, and the pointlist is somehow exported from CAD.

The program code then calculates for each line the A-axis angle needed to bring it horizontal plus the Y and Z axis values  of the line's center once rotated.  Then one can generate G1 moves consecutively for each segment.  If roughing pass(es)  needed, just run the same code with Z values larger than final.
Title: Re: Going over to the dark (CNC) side!
Post by: tangler on August 22, 2019, 03:00:27 PM
Nobody is much impressed by willy waving (not in my case anyway).  Although I have a proprietorial fondness for CamCalc,  drawing the profile in CAD and then getting the machine to cut it is much less tedious than Manual Numerical Control.  All our skills get superseded - I was really proud of the analysis and plotting routines I used to write for Thermal Analysis and then Excel came along  >:(
Rod
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on August 28, 2019, 06:55:09 PM
Nothing too exciting on the machine this week so I did not take a video. Firstly did the eliptical flange on the end of the stock that will form the carb body.

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Midget/20190825_143056_zpslbfc1usl.jpg)

Then used that to hold a bit of 1.5mm stainless steel that will be the exhaust flange

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Midget/20190825_143018_zpsruta8pzj.jpg)

Rest of the carb was done with conventional tools and has a throttle barrel rather than the straight through venturi type.

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Midget/20190828_141503_zpsdfbut0bg.jpg)
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on September 05, 2019, 05:20:25 PM
Today we have a Conrod which may be of interest to Rod (Tangler)

2014 (HE15) aluminium, I made up the two parts on the manual mill, screwed them together with sacrificial brass screws and then popped in the two holes and while I was at it made a plate to hold it on for machining.

3D profile done with a 4 flute 6mm dia cutter with 1mm corner radius so no stress risers at 5000rpm, modest feed of 300mm/min. Then change to a 4mm cutter again with the 1mm radius to do the recess in the middle. Runtime was 12mins for the two ops plus 2 x 1mins for the other side.

Quite pleased with how it came out.

https://www.youtube.com/watch?v=XGB7FHfdGsE

Title: Re: Going over to the dark (CNC) side!
Post by: tangler on September 06, 2019, 01:52:27 PM
That's what I was trying to.  Sadly my mill won't  communicate with a PC at the moment and I've  already wasted too much time on it.  I need to get on with the Farm Boy.
Cheers,
Rod
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on September 25, 2019, 08:20:12 PM
Time to make a bit more swarf or more precisely 86.5% swarf and 13.5% left in the part which is the ignition bracket for the Midget engine.

6082 Aluminium, 3-flute carbide 6mm dia, 55deg helix, uncoated

Facing 5000rpm, 330mm/min feed, 0.5mm DOC, 5.0mm WOC to remove the saw marks and level the top

Adaptive 5000rpm, 330mm/min feed, 5.0mm height of cut, 1.0mm stepover. The cutter was not so happy with conventional cutting causing a bit of vibration in the chip tray but OK climb cutting.

Contour 5000rpm, 330mm/min feed, 3mm height of cut, 0.5mm depth

Helical bore 5000rpm 330mm/min, 0.5mm pitch. First time I had done this and very happy how it turned out. The hole was rough bored with a 0.5mm pitch followed by a 0.25mm full depth finishing cut and then a spring pass at the same diameter.

Finished off with conventional machine and hand tools.

https://www.youtube.com/watch?v=cZrL3pbNxis
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on October 13, 2019, 12:31:34 PM
When I first entered the dark side I was hoping that there would be some light on the other side. Well today the light shone brightly.

With all the Midget parts finished, 57 individual items plus a further 30 custom made nuts, screws etc.

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Midget/20191005_182555_zps1sw3xgzj.jpg)

It was time to see if I remembered how it all went back together. Valve timing was set by eye while turning the engine over slowly watching when the valves opened and closed. A little more oil than the normal running level put into the crankcase, some Colemans with a drip of 2-stroke oil into the fuel jar and give it a go. I got some pops straight away and with a bit more retardation of the timing it fired into life with a couple more pulls of the cord.

Throttle is by rotating the jam jar fuel tank but quite slow to react due to sizeable flywheel, advance & retard are a better way to set the speed which I had always intended was going to be for looks and noise rather than outright speed and performance.

Had to turn it off as I need to get that curtain cord back before anyone notices it is missing. Just needs a bit of colour to finish it  :pinkelephant:

https://www.youtube.com/watch?v=CNndvvWaN-g
Title: Re: Going over to the dark (CNC) side!
Post by: vcutajar on October 13, 2019, 01:17:09 PM
Great runner Jason.

Looking forward to your next project and more CNC machining videos.

Vince
Title: Re: Going over to the dark (CNC) side!
Post by: Dave Otto on October 13, 2019, 05:01:11 PM
Nicely done Jason, she runs great!

Dave
Title: Re: Going over to the dark (CNC) side!
Post by: Admiral_dk on October 13, 2019, 07:30:29 PM
Nice Jason and a good runner and starter too  :ThumbsUp:

There is one part that stick out in the family picture for me - the upper leftmost next to the O-ring ....
To me it looks like it has something to do with oil .... a breather perhaps ?
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on October 13, 2019, 07:46:33 PM
Thanks for all the comments

Yes it is a breather, the one in Popular mechanics had a big ugly thing off to one side but I went for something smaller and centrally placed. Also doubles as the oil filler and I added the brass screw lower down as level/drain

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Midget/20190929_113444_zpsekloib6o.jpg)
Title: Re: Going over to the dark (CNC) side!
Post by: Kim on October 13, 2019, 10:24:32 PM
Very nice little engine, Jason!
Kim
Title: Re: Going over to the dark (CNC) side!
Post by: Art K on October 15, 2019, 05:04:58 PM
Jason,
Great build on that Popular Mechanics engine. They are right, I missed the build article. Is it a Midget because its smaller scale than original? :lolb: Great job on the cnc it was nice to see it in action.
Art
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on December 24, 2019, 07:33:21 PM
I wanted a "tee" shaped part similar to a plumbing tee where the 3 branches flow into each other rather than an abrupt junction for the top of the column of the engine I'm making at the moment.

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/847235.jpg)

I could have done a simple cope joint and added the fillets with JBWeld or actually welded it and ground back the welds but thought as I have got teh CNC that I may as well use it.

The bit of 40x20 flat steel bar was machined to overall size and the holes put in on the manual mill then over to the KX-3 to do the shaping. Just two paths, firstly a clearing one with a 3-flute carbide cutter then the final contour with a 4-flute 1mm corner radius cutter. quite pleased with how it turned out, just a tickle with files and or Dremel to blend in the cuts as I on;y went with 0.5mm stepdown.

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/847236.jpg)

https://www.youtube.com/watch?v=_Due-1nIHfE

Title: Re: Going over to the dark (CNC) side!
Post by: propforward on December 24, 2019, 07:36:24 PM
Holy Moly - some lovely and impressive parts there.  :ThumbsUp:  :praise2:
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on December 27, 2019, 07:59:20 PM
Another part for the same engine, this time the valve block at the base of the column cut from a block of bronze.

https://www.youtube.com/watch?v=2N_M1hH0NTA
Title: Re: Going over to the dark (CNC) side!
Post by: mikemill on December 28, 2019, 10:06:15 AM
Jason

What CAM program do you use, I am intrigued by the way the tool cuts both ways, conventional and climb.
I have used ArtCam Pro for many years now, maybe time for a change?

Mike
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on December 28, 2019, 01:13:23 PM
I draw in Alibre but do the CAM with Fusion 360, it defaults to climb milling but you also have the "both ways" or conventional option, you can also set a different feed and DOC for the conventional as the cutters seem happier with climb cuts so can take a bit more off in that direction. Andrew Johnston pointed me that way early on and I use it all the time for the main adaptive and a lot of the time for everything else as it saves a lot of time.
Title: Re: Going over to the dark (CNC) side!
Post by: steamer on December 28, 2019, 04:23:02 PM
I draw in Alibre but do the CAM with Fusion 360, it defaults to climb milling but you also have the "both ways" or conventional option, you can also set a different feed and DOC for the conventional as the cutters seem happier with climb cuts so can take a bit more off in that direction. Andrew Johnston pointed me that way early on and I use it all the time for the main adaptive and a lot of the time for everything else as it saves a lot of time.

You'll get better finishes as well with a climb cut

Dave
Title: Re: Going over to the dark (CNC) side!
Post by: gerritv on December 28, 2019, 06:49:05 PM
Jasonb, are you using the Fusion360 Hobby/non-commercial license with 2.5 axis only or the next level up (which now costs money?)

I am heading to CNC land again myself, getting some stuff ready.

Gerrit
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on December 28, 2019, 07:18:07 PM
I just have the free one but can use the 3D CAM functions.
Title: Re: Going over to the dark (CNC) side!
Post by: Muzzer on December 29, 2019, 12:20:37 PM
Look again, gerritv - the hobby users get the FULL simultaneous multi axis version (aka Ultimate) with NO limitations. Costs you nothing unless you are running a commercially viable company. The conspiracy theorists like to infer that Autodesk will start to charge once everyone's hooked but instead they seem to be intending to continue on this model, with paid-for "extensions" for some of the newer, more professional features (part scanning, generative design etc), and stuff like technical support limited to the subscription versions (that seems fair enough), as explained in this link:
https://www.autodesk.com/campaigns/fusion-360-for-hobbyists (https://www.autodesk.com/campaigns/fusion-360-for-hobbyists)

For amateur use, the excellent support forums and myriad Youtube tutors are more than enough for most learning styles.

What's really handy is the ability to switch quickly back and forth between CAD and CAM within the same environment so you can modify the model when you come to creating the toolpaths - in practice this is what you need to do in any CAM application to get the best result and (ahem) beats creating the model in one program and the toolpaths in another ;-)
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on December 29, 2019, 01:15:00 PM
Thanks for the confirmation Murray.

As you say being able to pop back to CAM to make alterations is handy, I have still done it with my imported parts but not as easy and also if you alter the part in a different CAD program you have to import again and start the CAM from scratch. There is still far more than I'm ever likely to need in the free version.
Title: Re: Going over to the dark (CNC) side!
Post by: gerritv on December 29, 2019, 03:47:15 PM
Thank you Muzzer. I now went back and looked again, you are correct. At some point early in the switch over to 3 types of licensing I was reading too many posts elsewhere :-) Software development is not trivial or inexpensive so they at some point need to monetize the product to stay in business.

Gerrit
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on January 12, 2020, 04:25:07 PM
Having spent quite a while on Frday evening and even more on Saturday flicking the RMC type A flywheel round I came to the conclusion that it is not going to work on propane instead of the now unobtainable MAPP gas I drew out a new head for it last night so it can be built as a 4-stroke, did the CAM this morning and then after lunch got the Sieg KX3 to spit out the new head in just over an hour. Still needs some holes here and there but will do those on the lathe and manual mill and then give it a lick with the needle files to get rid of the contour lines..

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/RMC/20200112_151455_zpshw3yhjwb.jpg)

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/RMC/20200112_151526_zpsgqrugdlg.jpg)
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on January 26, 2020, 04:28:35 PM
I have machined a few more bits for the 4-stroke conversion of the RMC engine. Rocker arm to operate the exhaust valve and a post to mount it on that is fixed to the head. I will bond this on with JBWeld and also fill the CSK screw holes and add some fillets to the internal corners so that the post looks like it was cast as one with the head. Both done on the KX3 and needing two setups each so that both sides could be machined.

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/RMC/20200126_104311_zpscvgayrxe.jpg)

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/RMC/20200126_104247_zpshohhs1qu.jpg)


And made a start on the epicyclic gearbox by cutting the eccentric on the CNC which did the profile with ease and also made light work of the doglegged end that lofts from a rectangle at the eccentric to a circle where the rod enters with just a light touch of a needle file required to blend the remaining too step overs. That is a 10-20-40 block not a 1-2-3 one!

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/RMC/20200125_185505_zps7x0n9t8r.jpg)

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/RMC/20200126_105208_zps2zfb3iz6.jpg)
Title: Re: Going over to the dark (CNC) side!
Post by: scc on January 26, 2020, 09:48:11 PM
I'm enjoying progress with this one :popcorn: :popcorn:    but cnc, etc is not for me :old:    Regards       Terry
Title: Re: Going over to the dark (CNC) side!
Post by: zeeprogrammer on January 26, 2020, 10:37:14 PM
Love the finishes.

... of the now unobtainable MAPP gas ...

Perhaps I missed the posts regarding this. Why do you say it is unobtainable? Is it a UK thing? Or are you referring to the original MAPP gas? I understand it's production was stopped (or reduced) some years ago and products called MAPP are substitutes with a different composition.

Title: Re: Going over to the dark (CNC) side!
Post by: crueby on January 26, 2020, 10:42:26 PM
Love the finishes.

... of the now unobtainable MAPP gas ...

Perhaps I missed the posts regarding this. Why do you say it is unobtainable? Is it a UK thing? Or are you referring to the original MAPP gas? I understand it's production was stopped (or reduced) some years ago and products called MAPP are substitutes with a different composition.
The original stopped production in the US at the only plant that made it in 2008, the current stuff labelled as MAPP is not the same chemically, I've noticed that in my torch made for the original stuff it does not burn anywhere near as hot, harder to start it burning correctly, and goes out once in a while. Still works fairly well for small jobs.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on January 27, 2020, 07:02:52 AM
Zee, as Chris says the original is no longer made, it had quite a lot of hydrogen in it which was what these engines like in fact the ones at places like Coolsprings run on about 85% Hydrogen with the remainder made up of propane and a few other gasses as it is the nearest to the old illuminating (town) gas.


Terry, I felt the same and even turned down an earlier offer of a machine for free but now that I have this one it certainly has it's uses though I'm not going to be going over to a full CNC only workshop anytime soon. If I had also had to learn CAD to draw the parts and also learn to write the G-code then that would have been a big put off but I could do the CAD anyway and Fusion360 does all the CAM so I don't need to write actual G-code.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on February 15, 2020, 10:24:44 AM
Who Needs MAPP gas when you can design your own cylinder head and other bits to make the engine run as a 4-stroke, looks like all the parts work :pinkelephant:

In fact they almost work too well as I am making so much compression it is hard to flick the engine over to get it started there is so much bounce :)

https://www.youtube.com/watch?v=cbcQfBEcZmc
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 08, 2020, 05:08:06 PM
The current lockdown has allowed me to spend a bit more time on the darkside :)

I was not going to bother videoing this but there was a query last night on ME forum about profiling cuts so I used this to illustrate a point. I did two tool paths in F360, one a roughing contour leaving 2.5mm stock all round and then the final contour taken at the full 16mm depth of the material in 0.5mm depths with a 0.25mm finish past & a spring pass which was not really needed. However I actually did the roughing on the vertical bandsaw to a Sharpie line drawn around a paper template so only needed to run the second path.

This shows the smaller of the two parts which is tapped and screwed to some scrap being held in the vice so the tool can extend just below the bottom of the work.

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Filer%20and%20Stowell/20200408_084103_zpsxgb5fpbu.jpg)

This is the larger part being milled with one of ARC's 10mm dia aluminium specific cutters running at 4000rpm and feed at 300mm/min. Quite pleased with the finish from what is a quiet well used cutter as you can see from my finger reflection if you skip to the end.

https://www.youtube.com/watch?v=geKWDVsKAeg

It was then mounted the right way up to mill the "S" shape on what will be the side.

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Filer%20and%20Stowell/20200408_110604_zpsm0bwebg6.jpg)

Can you tell what it is yet?

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Filer%20and%20Stowell/20200408_114102_zps1oclpnmu.jpg)

The crank disc in the photo above had the recesses either side done on the CNC as did the cylinder end cover and its boss which were both shaped at the same time.

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Filer%20and%20Stowell/20200406_083907_zpst2im64f4.jpg)

J
Title: Re: Going over to the dark (CNC) side!
Post by: nj111 on April 08, 2020, 05:54:59 PM
That's really great, that little mill does give you some pretty good results. I'm quite impressed for it's tiny footprint. Now that you are used to "the dark side" I'll bet you find you use it more and more and would miss it if was no longer an option?  I've been programming for over 30 years and over the last 20 years have acquired some obsolete industrial CNC machinery at home.  The down side I find with my old (low cost) CNC machines, other than being quite heavy to move and sensitive to run off 3 phase convertors,  is there is sometimes some frustration fixing faults  (these being late 80's - mid 90's  machines). Usually just when I don't want them to go wrong they will! But I don't find old CNC controls (Fanuc & Heidenhain)  limiting - so long as offline programming software is good and efficient those work fine and drip feed seamlessly with any long 3d programmes which exceed their tiny memory capacities.  Heidenhain has a language of it's own which I never bothered to learn as I discovered that control also runs G code if one machine parameter is changed. Keep up the good work!
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 15, 2020, 05:30:34 PM
Hi Nick. yes I'm getting to like it, still won't be getting rid of the manual machines but the CNC does open up the options available and enable some projects that may not have seen the light of day be brought forwards.


For the current engine that I'm working on I wanted a flywheel with quite a wide but thin rim and  oval spokes tapering in width and thickness .

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Filer%20and%20Stowell/flywheel%20pic_zpsleokacjs.jpg)

 I have often used cast flywheels from other models but could not find anything to suit. Fabrication was an option but by the time I had sourced some thick wall tube, a disc to cut the spokes from and added something to beef up the hub area it worked out cheaper to go for the solid option so I ordered a 30mm length of 130mm diameter EN3 steel.

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Filer%20and%20Stowell/20200411_095953_zpsh36emf7i.jpg)

I decided to rough it out on the lathe and manual mill leaving material on all surfaces.

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Filer%20and%20Stowell/20200412_144012_zpstowe9x1e.jpg)

i did a dummy clearing program to mimic what I had done on the manual machines so that the CNC would not try and remove the metal again and then a clearing program was run starting at the height of the "disc" with a 1mm stepdown that left a finish like this

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Filer%20and%20Stowell/20200413_102738_zpsrqpwc3qe.jpg)

Then a finishing ramp with 0.2mm stepdown to give the draft angle to the inside of the rim and hub and then carry on down further to shape the spokes with a 6mm dia R1  tool

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Filer%20and%20Stowell/20200414_091535_zpsxy4xinq0.jpg)

It then just needed a bit of fettling with the Dremel to blend the 0.2mm steps and I also added the bits to make it look like a 2 part flywheel.

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Filer%20and%20Stowell/20200415_091401_zpszktytgro.jpg)

A couple of coats of filler/primer and it's ready for colour.

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Filer%20and%20Stowell/20200415_142104_zpst6hlvrtt.jpg)

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Filer%20and%20Stowell/20200415_142116_zps8t70bh0j.jpg)

Looks like I won't be needing many castings in the future. ;)

https://www.youtube.com/watch?v=OFS41VbX6DA







Title: Re: Going over to the dark (CNC) side!
Post by: crueby on April 15, 2020, 05:59:26 PM
Wow, that came out great!
Title: Re: Going over to the dark (CNC) side!
Post by: nj111 on April 15, 2020, 06:01:32 PM
Very very nice, you've certainly mastered the art of making a part machined from solid look just like a casting!
Title: Re: Going over to the dark (CNC) side!
Post by: Chipmaster on April 15, 2020, 06:34:34 PM
Splendid.

Andy
Title: Re: Going over to the dark (CNC) side!
Post by: Muzzer on April 15, 2020, 06:53:20 PM
Great result Jason!

You can also create a 3D model of the stock and then point Fusion to it when you come to create the setup. I've done this when I start with a part machined piece of stock like yours.

Another handy "stock option" method to be aware of is to simulate all the CAM operations you've just used, then save the finished (simulated) part as a solid body. You can then import and save that as a body within the file - and use that as the stock when you come to create the next setup. This is very handy when you come to turn a part over to machine the other side. That way it knows what is there and what isn't. Fusion can't use "rest machining" between setups but this method gets around that. Can save a lot of time (and cutters!).
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 16, 2020, 07:55:24 AM
Thank's Murray, I'll try doing a drawing of the roughed out part to use as the stock next time, would have been handy as I could have set the six holes as entry points as it was I just used a steep ramp and large diameter to speed things up as the tool was ramping down into air rather than the metal it thought was there.

From posts over on ME I have realised that the Ramp path was not the best for the spokes as there is no option to deal with shallow areas like there is in Contour so would have been best splitting the job into layers doing the inside of the rim with the Ramp that worked well and then the spokes with contour and setting max stepover of shallow areas so that I got a finer finish on the upper parts of the spokes.

There is so much in F360 that only using it for CAm maybe a couple of times a month (when not locked down) I probably don't get to use it enough to learn all the options but I'm slowly getting there and am sure that the next one will come out even better, at least it's all good fun.  ;D
Title: Re: Going over to the dark (CNC) side!
Post by: Jo on April 16, 2020, 08:51:11 AM
Who helped you broach that keyway JB ? I am sure it was not your normal helper, she would have made sure the keyway lined up with a spoke or the centre between the spokes   ::)

Very very nice, you've certainly mastered the art of making a part machined from solid look just like a casting!

Castings are rather cheaper than a CNC milling machine.  :noidea:

Jo
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 16, 2020, 11:11:42 AM
But you are limited to what's available unless you make patterns and invest in foundry equipment or sub that out and then you could get back castings of poor quality.

There is also the time factor as pattern making is likely to be as long as making the solid flywheel or longer if you can't CNC or print it. Then there is travel to and from foundry which can't really do under lockdown or maybe too far for you at any time. I was able to leave the mill to it on the finishing path so could get on with other things while it was cutting.

Well spotted on the keyway, it was lined up with a spoke and then I added a bit of packing under it so not to push against the unsupported hub and it moved while I was not looking.

J

PS Not at the price my CNC did not cost me ;)
Title: Re: Going over to the dark (CNC) side!
Post by: nj111 on April 16, 2020, 12:06:31 PM

[/quote]

Castings are rather cheaper than a CNC milling machine.  :noidea:

Jo
[/quote]

Jo, I agree there is a higher initial investment to make than with our other workshop machines, but it's more a case of cash tied up in something that still has a value. I bought my first CNC mill for home 19 years ago , it was 5 yrs old at the time, Czech made and about Bridgeport size. If I threw it away today it would have cost me just £5 per week to own and run, but actually being a small industrial machine it's probably still worth half what it initially cost! £5 per week now becomes £2.50.  During that time it's run many thousands of hours. I hope it will continue to run for many more years! Don't get me wrong I love manual machines as well, the older the better!
Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on April 16, 2020, 01:09:46 PM
Same storey here,

My first CNC Emco F1 mill was bought over twenty five years ago. It has been in daily use, machining untold numbers of 'castings' from the solid. The cost of ownership workes out at less than £1.50 per week.  Last year, I sold it on for almost what I originally paid for it. When you chose a design for which there are no castings, machining from solid is your only option. CNC makes that possible.

If you can find an engine for which castings are available, you have to move pretty quick, before Jo and Sorass add them to their collection.

The storm cannot last forever. Stay strong

Mike
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 16, 2020, 01:16:34 PM
The cost of ownership workes out at less than £1.50 per week.

I bet it costs more than that to keep Sorass supplied with peanuts each week.

Luckily as I have only purchase ONE manual Mill and One manual lathe so even if I had paid full price for the CNC I'd still have money in my piggy bank compared with those that need mutiple machines and even then could not do some of the things a CNC can with them :LittleDevil:

Are you still holding out for those overlength Seal casting's Mike?


Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on April 16, 2020, 01:46:52 PM
Are you still holding out for those overlength Seal casting's Mike?

Kirk at Hemingway's  has hopes that the foundry will be producing castings again, someday soon. As an insurance policy, I have ordered a large block of HE 30. So my first engine ever to be made from a  foundry casting may well have the 'casting' machined from solid.

Not actually been out in the workshop much over the last month. More important things to make than engines.

The storm cannot last forever. Stay strong

Mike
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on April 16, 2020, 02:34:08 PM
Quote
keyway lined up with a spoke

Learned something today.

My CNC mill is 10 y/o since new, cost just under $10K, so about $2.75/day
Title: Re: Going over to the dark (CNC) side!
Post by: Alex on April 20, 2020, 11:36:54 AM
Castings - and CNC.

Yeah, I built Kozo's first shay, no castings. (some of the details of the build are covered in my CNC articles in Model Engineer, a while ago now). I'm really looking at the Kozo Heisler, but do have a few unfinished projects to finish before I start on another.

Sending castings overseas from the UK is very expensive, and fabricating from solid is easier and can look a lot better, especially with CNC as Jason is showing to great effect.

Now, I have to get off my butt and do more in my workshop - in this current COVID lockdown, I'm still working full-time, should stop it sometime sooner than later, and get back to it.

I appreciate Jason, KVOM, and others that are active with CNC, AND put pictures up. :-). JohnS.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 23, 2020, 05:34:28 PM
Some of simple drilling and profiling cuts produced a couple of parts destined to become part of a "casting"

I think it's S275 steel at 3mm thick, 3mm dia holes were drilled with the first code and then screws added to help hold the part down before before changing to a 3-flute 4mm dia cutter to do the shape in 4 depth increments and then a final 0.25mm full height finish pass. Couple of tabs used just to hold the bits in place.

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Filer%20and%20Stowell/20200420_143935_zpssr5jzjdq.jpg)

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Filer%20and%20Stowell/20200420_151715_zpswbnjgkns.jpg)

Small one in place and the other to show how it mimics the shape of the other parts but is 1mm larger all round.

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Filer%20and%20Stowell/20200421_084052_zpsqxadnki0.jpg)

No video of this one as it's not particularly exciting.
Title: Re: Going over to the dark (CNC) side!
Post by: Johnmcc69 on April 24, 2020, 03:07:16 AM
 :ThumbsUp:
 Looks good!
 :popcorn:
 I may have missed it, but what engine will this be?

John
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 24, 2020, 07:19:55 AM
I don't think I have said what it is. It's my version of a Rocking valve engine, there was a one started on here (http://www.modelenginemaker.com/index.php/topic,6798.0.html) based on the Jesse Livingston design that got me interested as it's something different to the usual slide valve arrangement but I have tried to make mine look more like a Filer & Stowell

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Filer%20and%20Stowell/20200418_110058_zpsqdrov9ao.jpg)

Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 30, 2020, 04:35:32 PM
Lockdown has allowed me to get on with this engine to the stage where I could give it a tickle of air. Only got a few screws tacking it together, no gland packing or piston rings and the valve links only have screws as pivots not fitted pins but it run straight away as soon as the air was turned on. :cartwheel:

Learned a lot doing this one not just with the CNC but working out the rocking valve construction as the source of drawing that were on the web has been removed so I just had to make up the details myself, fairly happy with how it's turned out just needs some finishing touches now.

https://www.youtube.com/watch?v=tC_klQJhhhQ
Title: Re: Going over to the dark (CNC) side!
Post by: vcutajar on April 30, 2020, 05:08:51 PM
Jason, video is private.
Vince
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 30, 2020, 05:47:48 PM
Should be OK now
Title: Re: Going over to the dark (CNC) side!
Post by: crueby on April 30, 2020, 06:10:23 PM
Great! Nice smooth runner, very well done!
Title: Re: Going over to the dark (CNC) side!
Post by: kuhncw on April 30, 2020, 06:46:35 PM
Very nicely done.

Chuck
Title: Re: Going over to the dark (CNC) side!
Post by: Johnmcc69 on April 30, 2020, 07:19:19 PM
 :ThumbsUp:
 Nice work Jason!

 John
Title: Re: Going over to the dark (CNC) side!
Post by: Admiral_dk on April 30, 2020, 11:12:10 PM
Fantastic result especially when one consider that you used a few bits that aren't the right ones, as a quick fix.

One question - the threaded hole pointing us under the valve - is that the exhaust ?

Per
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on May 01, 2020, 07:49:20 AM
Thanks all for the comments

I think the light is making the boss on the side of the cylinder look threaded but the hole is plain, the boss needs to have four holes drilled like the inlet to take the flange of the exhaust which will then bend 90deg and go down into the base.

I meant to point out to Jo how true the flywheel runs, not just the machined bright surfaces but the painted "cast" ones as well, don't get that with a casting that has the two halves out of line and distortion :LittleDevil:
Title: Re: Going over to the dark (CNC) side!
Post by: Jo on May 01, 2020, 07:54:30 AM
I meant to point out to Jo how true the flywheel runs, not just the machined bright surfaces but the painted "cast" ones as well, don't get that with a casting that has the two halves out of line and distortion :LittleDevil:

You are still missing the point Jason: I am explaining to the reader the challenges of working with castings and how to get round them. Not everyone is as experienced as you are.

Jo
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on May 01, 2020, 08:12:40 AM
Yes Jo just like I describe machining all the cast flywheels that I have used in previous threads. However I am willing to accept that there are other methods available such as fabrication and cutting from solid and that castings are not the only way. I show these other methods to the less experienced who may want to go down that route.

Having machined 35 cast iron flywheels maybe I now just find something else a bit of or a challenge :-\
Title: Re: Going over to the dark (CNC) side!
Post by: kuhncw on May 04, 2020, 01:55:49 AM

Hi Jason,

In your reply #166, you mention using a dummy clearing program. 

Quote: "i did a dummy clearing program to mimic what I had done on the manual machines so that the CNC would not try and remove the metal again and then a clearing program was run starting at the height of the "disc" with a 1mm stepdown that left a finish like this"

I understand why you did this, but I don't understand how you accomplished the dummy clearing.  Would you please explain this a bit or point me to a reference.

Thanks.

Chuck
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on May 04, 2020, 06:58:44 PM
The dummy clearing was simply a 2D clearing pocket that mimicked what had been removed by the lathe so the bottom depth was set as the depth of the recess in this case 9.5mm down from the edge of the rim that I had turned and the radial material to leave was set as the same as I had done on the lathe at 1mm. Pic 1

On the simulation the green is the finished item and the blue material still to be removed Pic 2

This allowed my to then do the other operations without the CAM thinking that the tool was plunging down into metal that was not really there and throwing up a load or crash warnings. or trying to machine metal that was not there. When it came to post processing I simply suppressed that first dummy pocket and created code for what was left.

J
Title: Re: Going over to the dark (CNC) side!
Post by: kuhncw on May 04, 2020, 08:51:05 PM
Jason,

Thank you for the explanation.  I've not tried suppressing an operation prior to posting the code.  I'm using MecSoft's Visual Mill Standard for CAM.  I'll see if I can do this in my version of Visual Mill. 

Chuck
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on June 01, 2020, 07:17:45 PM
just a small part this time which is the exhaust pipe elbow for the Filer & Stowell, having learnt that I was not using the best cutting paths when I did the flywheel this was a good simple part to try out F360's  "steep & shallow" which gave a nice even step over all around the bend which was cut with a 3mm dia 4-flute ball nose cutter at 5000rpm and 300m/min feed. I pinched the idea of milling inside a square from Dave Otto's valve.

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Filer%20and%20Stowell/DSC03949_zpsycbcflv9.jpg)

It was then just a case of plunging in from each end with a 6mm ball nosed cutter and then a 7mm flat to form a recess so that I could locate matching spigots on the ends of the 8mm OD pipe which was all JBwelded together.

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Filer%20and%20Stowell/20200530_132721_zps9htkk2dm.jpg)

(https://img.photobucket.com/albums/v156/jasonballamy/Engineering/Filer%20and%20Stowell/20200531_082036_zpsututnqzc.jpg)

A lick of paint was all that was required to complete this part and the whole engine.

https://www.youtube.com/watch?v=xMA_-hx1dSo
Title: Re: Going over to the dark (CNC) side!
Post by: steamer on June 01, 2020, 07:43:42 PM
That just got dropped into the pile of good ideas!   

 :DrinkPint:

Dave
Title: Re: Going over to the dark (CNC) side!
Post by: Johnmcc69 on June 01, 2020, 10:47:54 PM
 :ThumbsUp:
 Fantastic engine Jason! I like the slow running. Looks like you'll need to tame that govenor a bit.

 Will you be creating drawings? I would think this would be a popular design.

 Great work!

 John

 Also...nice touch running the wood grain parallel with the engine...  Cool little effect. :ThumbsUp:
Title: Re: Going over to the dark (CNC) side!
Post by: kuhncw on June 01, 2020, 11:01:08 PM
Very nice work, Jason.

Chuck
Title: Re: Going over to the dark (CNC) side!
Post by: Dave Otto on June 02, 2020, 12:58:35 AM
Beautiful engine! I like how you have it angled on the base, it gives it a much different look.

Dave
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on June 02, 2020, 07:17:23 AM
Thank's chaps.

Not sure about drawings but have started the build thread over in "own designs" It would be possible to do it all on manual machines as all the curved bits were drawn at a time when I would have had to do it on the rotary table so would not limit it to those with CNC

The governor drive belt is really too short, I need to get another so they can be joined together and take some of the load off the long overhanging pulley that is only on a 1/16" shaft which I think will help.

Dave, the angled engine does make a bit of a change to the usually mounting parallel to the sides and gets rid of that blank space on the inlet side of the cylinder with the added bonus that I could make the base a bit narrower as the exhaust did not stick out the side
Title: Re: Going over to the dark (CNC) side!
Post by: nj111 on June 02, 2020, 02:13:19 PM
Really nice result Jason.  That actually reminds me of similar work by Clen Tomlinson. (I am going back 15 or more years here). Some may remember the incredibly complex Napier Deltic engine he was making?
Here is a picture I took of how he made such items. They were in brass, machined both sides, bolted together then silver soldered, then cut off to length and finally nickel plated.  I have in mind Barry Hares used similar techniques (obviously without going to the dark side!)  to produce this sort of part on his remarkable Merlin and Eagle engines.  It seems a good option for items where it's not possible to machine the bore like you were able to.  Nick
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on June 23, 2020, 05:56:54 PM
I thought it was about time to dust off the KX3 and make a bit more swarf. The chosen candidate was the base for my current engine project which I had made a bit more shapely than the engine it is based on but making the four sides concave rather than just rectangular and the curve from top out to the edges is a 1/4 ellipse so not easy to do with an off the shelf cutter particularly to get it to flow around the corners of the upper rectangular mounting surface.

(https://hosting.photobucket.com/images/v156/jasonballamy/base.JPG)


Roughing

The usual 3D clearing using a 6mm dia cutter was showing quite a long run time in the simulator as it was basically just doing an ever decreasing rectangle so lots of movement and little cutting to start with as it just nipped off the far corners so I thought I would try one of ARC's 25mm insert cutters. I changed to a pocket clearing cut which spiralled down 1mm and then worked around the waste before spiralling down again, I generally prefer to use more of the cutters edge but with the inserts the cost of a couple of corners is not too great even if the sides don't see an equal amount of wear.

I will need to look at the helix that the tool follows as it spirals down if I use the method again and also support more of the work as it was getting a bit chattery as I got down to the 4.5mm (4mm plus 0.5 finish) thickness. I have already played around with this and got the tool to ramp down as it moves along which together with a few more tweaks cut about 40% of the run time.

Contour

I had already sawn to rough shape on the vertical bandsaw so only needed a couple of 0.5mm clean up contour passes and a final 0.25mm finish one and it was while doing these that I realised something was wrong as there was a lot more coming off the left hand side than the right Turns out that I had located the work based on the ctr position I had used when drawing it which was the middle of the rectangular top section (black sharpie marks on video) but F360 defaults to the ctr of the stock which being an asymmetric part was off to one side, luckily there was enough to play with except for a couple of the rounded corners so out with the JBWeld. Just a 6mm 3-flute from NC for this

3D "Steep and Shallow"

From the earlier Filer & Stowell flywheel I had found that I was using the wrong type of path with some input from Andrew and Barrie so opted for what F360 calls "steep and Shallow" that I tried on teh pipe bend posted previously which allows you to set the stepover or scallop for both steep and shallow surfaces which results in a more even finish, I went with 0.25mm in both cases and used a 4 flute Arno ball ended cutter. Quite happy with how that turned out as it needed almost no cleanup work prior to paint.

I also drilled the holes on the CNC, the larger than normal spotting holes are due to me not having modified the file after altering the hole spacing on the mating part so had to run the spotting path again with a slow downfeed so the 6mm spotting drill did not get pulled over by the previous overlapping holes.

Final job was to add some bosses around the corners which still need a bit more filleting but the Upol Rapid filler was living upto it's name this afternoon and almost setting before I could apply it so just gave it a blow over with etch for now.

Feeds 'n' speeds etc in video description

https://www.youtube.com/watch?v=JCuUzREEjy4
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on July 16, 2020, 05:22:19 PM
I carved a cylinder head for my current Thompson engine out of a bit of 50mm cast iron bar at the weekend, this is the finishing "Steep & Shallow" cut from Fusion after the adaptive clearing leaving 0.6mm and external contour finish cuts had been done.

6mm 4-flute R1 cutter at 5000rpm and 400mm/min feed with a 0.25mm stepover.

https://www.youtube.com/watch?v=CruYbOx9OR8

From the other side

(https://hosting.photobucket.com/images/v156/jasonballamy/20200711_102500.jpg)

I also did a cooling fan from 0.5mm steel. 2mm HSS cutter made quick work of it.

https://www.youtube.com/watch?v=BdN2PFKBvoU

(https://hosting.photobucket.com/images/v156/jasonballamy/20200626_115517.jpg)

With the rest of the holes machined into the head on lathe and mill it's starting to look like an engine

(https://hosting.photobucket.com/images/v156/jasonballamy/20200712_122201.jpg)

Title: Re: Going over to the dark (CNC) side!
Post by: crueby on July 16, 2020, 05:30:10 PM
Great parts, very interesting to see the CNC in action.   :cheers:
Title: Re: Going over to the dark (CNC) side!
Post by: kuhncw on July 17, 2020, 01:51:45 AM
Very nice work.  Thanks for posting the CNC videos.

Chuck
Title: Re: Going over to the dark (CNC) side!
Post by: Muzzer on July 21, 2020, 12:51:08 PM
Hi Jason - I guess your trial period of the steep and shallow "extension" has now ended? That and the multiaxis support are outside of the normal licence, so become unfeasible for hobby users who aren't made of money.

IIRC, they extended the trial period to get us hooked but I don't see it any more.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on July 21, 2020, 01:08:24 PM
It took a couple of clicks but I was still able to get it, don't know how long for though.  :) Managed this at the weekend from a bit of EN3 but may have been EN8 going by the colour code although that can vary. I think the Z-axis damage that was done to the machine before I got it may still be affecting things slightly in the way of backlash as there are a few over depth areas - ring on inside of rim and outside of the hub and also where the cutter goes up over the spoke so need to look into that a bit more.

(https://hosting.photobucket.com/images/v156/jasonballamy/20200717_183044.jpg)

(https://hosting.photobucket.com/images/v156/jasonballamy/DSC03985.JPG)

(https://hosting.photobucket.com/images/v156/jasonballamy/20200719_104556.jpg)

Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on July 24, 2020, 07:24:46 PM
Those with an aversion to the brown stuff should look away now.

I thought I would see what a bit of Beech machined up like and as I happened to need to make a pattern for a bearing cap what better excuse to make some sawdust.

https://www.youtube.com/watch?v=F8n4mKccHaM
Title: Re: Going over to the dark (CNC) side!
Post by: crueby on July 24, 2020, 09:12:43 PM
No problem watching woodworking here (my avatar should prove that! ), though I may have to get you to make me up some wooden plane bodies!   :ThumbsUp:
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on August 12, 2020, 05:25:43 PM
Before cleaning up the machine from cutting the brown stuff there was one other little item that I have had drawn out for a while. Originally intended to cut from some wood grain UPVC facia so that the lettering showed up white on the darker material but did not have any off cuts wide enough so I decided to make it from some 6mm melamine coated MDF.

Pleased with how it turned out particularly the engraving as it was the first time I had tried that and pleased with the "square" ends to the numbers rather than rounded that you often see, F360 works out the magic and lifts the 90deg vee tool at the ends though it did have a strange way of doing the rounded parts of the numbers such as 6 & 9 first?

I actually mucked up the first one having also entered the 5000rpm spindle speed as the feed rate giving 5000mm/min so the order of cutting is not really right. It should have been hole with the 6mm cutter then engrave and chamfer with the 90deg chamfer mill. Now I can get rid of the wooden rack the original 1-10 set cam in and the boxes from the ARC half mm and imperial ones.

https://www.youtube.com/watch?v=WJAPIldGSB0
Title: Re: Going over to the dark (CNC) side!
Post by: Alyn Foundry on August 12, 2020, 06:28:51 PM
Oh dear, Jason. Perhaps you shouldn't have mentioned engraving??

How difficult would it be to knock something like this out at 1/4 the size?

Cheers Graham.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on August 12, 2020, 06:45:19 PM
Way too difficult ;)

What is the approx full size, one obvious thing is that the open/shut looks to be set well back from the horizontal part above. To cut around the letters would need a very small dia tool which usually does not have much reach so could be a problem getting in close enough without hitting the shank. Also would you be wanting a one off in brass or a pattern?

J

PS full set kinky ones done and a main cap
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on August 12, 2020, 08:16:31 PM
The lettering could be done on a separate material and the top and bottom attached.

But 3D printing would be better all around.
Title: Re: Going over to the dark (CNC) side!
Post by: Alyn Foundry on August 12, 2020, 08:17:26 PM
Hi Jason.

Not to worry, it would have been nice to fit it to this engine....   ;)

https://www.youtube.com/watch?v=eNfzFZMWXQg

Cheers Graham.
Title: Re: Going over to the dark (CNC) side!
Post by: jadge on August 13, 2020, 03:53:05 PM
Should be possible, albeit with some fiddling and depending upon the size needed. It would be tedious to reproduce the poorly defined fonts from the original casting though. In due course I'll let people know how the cover for my regulator goes:

(https://listerengine.com/coppermine/albums/userpics/10022/normal_Regulator_5.jpg)

The lettering is much tidier than the original casting. In model size the font is 2mm high and each letter is individually scaled to allow machining with a 0.5mm endmill. Currently my CAM is saying just over an hour in steel with the endmill running at 24000rpm and 100mm/min.

Andrew
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on August 13, 2020, 06:50:47 PM
In due course I'll let people know how the cover for my regulator goes:

Should be an open and shut case ;)

Look forward to hearing how it goes. I think I may try an engraving bit as the tapered end will hopefully be a bit more durable than a straight shank cutter though with it's single cutting edge and my 5000rpm max it may take some time.

The way that F360 generated the path to square up the letters was being discussed on ME forum so I took a short video of the tool moving around to cut the number "1" which may also be of interest here. You can see how it ramps in and then lifts to ramp up the other side of each end. I will have to see if it does similar for raised letters which would give nice crisp internal corners.

Best watched full screen on Youtube

https://www.youtube.com/watch?v=tvnde64xjcU
Title: Re: Going over to the dark (CNC) side!
Post by: Muzzer on August 13, 2020, 06:51:05 PM
I made a couple of toolholder racks from MDF. I still use them but be aware they puff up at the slightest presence of coolant or WD40. In my case that was the excuse needed to buy some 16mm acetal and have another go.

Fusion 360 now has some pretty smart engraving / embossing functions that work on non planar surfaces. Your video is a great illustration of how they have implemented the engraving. That valve plate thing should be fairly quick and easy to do.
Title: Re: Going over to the dark (CNC) side!
Post by: steamer on August 14, 2020, 01:06:49 AM
My fusiong 360 version on my 440

its to mounted to a 15 degree sloped enclosure....I have the tool paths....and can share the files

Made from a strip of cut off from a polypropylene cutting board....


Dave
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on August 14, 2020, 07:32:54 AM
Oh to have quick change tooling :'( Murray, I thought you would have an auto changer to stack the tooling in by now ;)

If anyone wants to make one like my ER16 rack then this will take you to theF360 file https://a360.co/2PXHrwF

I used the same melamine coated MDF to make a rack for my ER32 collets and that's still fine after a couple of years use.

Murray is that Emboss feature at the design stage? I still tend to draw in Alibre and just use F360 for CAM.

Have any of you used the tapered engraving cutters? Toby looks to have used them to good effect and I have been watching a few videos by a guy who also uses the Sorotec cutters on a rather nice home built epoxy framed machine.

Toby's results
http://www.modelenginemaker.com/index.php/topic,7050.msg156640.html#msg156640

Cutters
https://www.sorotec.de/shop/Zerspanungswerkzeuge/sorotec-werkzeuge/Gravurwerkzeuge/Gravierstichel
https://www.sorotec.de/shop/Zerspanungswerkzeuge/sorotec-werkzeuge/Gravurwerkzeuge/Gravierstichel--Standard-/

Sebastian End
https://www.youtube.com/watch?v=rep3HAdxfKU
Title: Re: Going over to the dark (CNC) side!
Post by: Muzzer on August 14, 2020, 09:16:12 AM
Jason - yes I actually have an ATC for my machine but it's so big and cumbersome I can't bring myself to go to the bother of fitting it. I'd also need to come up with some form of controller to drive it from my system IO. I think I may ebay it or possibly strip out most of the dead weight to create a minimalist version.

Yes, the emboss functions are within the design space. Fitting text and features etc to non-planar faces used to involve all manner of workarounds but now it uses an "unwrap" process to project perpendicular to the surface and extrude cut a consistent distance. At some point you need to try out the design space. For one thing, it's really useful to be able to rapidly move between design and manufacture to finesse the part as you make it.

The emboss function also works well with chamfer to create the sharp vertices noted earlier in this thread.
https://www.youtube.com/watch?v=aAjhTFxi2_w
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on August 14, 2020, 01:04:00 PM
I have a set of engraving cutters from Bits&Bits, all 1/8" shank and different tip widths.

So far I've used the one with .020" tip in brass to good effect.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on August 14, 2020, 03:55:18 PM
Looks like I would need a 4th axis to make use of that emboss feature.

Think I may get a 0.5mm engraving cutter (0.020") and maybe a 0.3 to have a play with.

Still waiting for Graham to confirm sizes but I can't imagine that valve being any more than 2" dia on full size so that's only going to be 1/2" dia on the 1/4 scale model which makes for some very small writing
Title: Re: Going over to the dark (CNC) side!
Post by: Alyn Foundry on August 14, 2020, 04:39:30 PM
Looks like I would need a 4th axis to make use of that emboss feature.

Think I may get a 0.5mm engraving cutter (0.020") and maybe a 0.3 to have a play with.

Still waiting for Graham to confirm sizes but I can't imagine that valve being any more than 2" dia on full size so that's only going to be 1/2" dia on the 1/4 scale model which makes for some very small writing

Oh, sorry Jason.

I was being a little facetious, for the few that looked at the video the nameplate was a casting and the pattern was done by a deep photo etching process. The Brass foundry had no problems in casting, as you can see.

Further patterns were going to be made until I decided to finally close the project due to the engines poor running performance.

Thanks for your indulgence.

Cheers Graham.
Title: Re: Going over to the dark (CNC) side!
Post by: Muzzer on August 14, 2020, 05:15:56 PM
You would only need a 4th axis if you wanted to wrap text or patterns around a cylinder. For planar, slanted, concave / convex surfaces etc, you could use a std 3 axis machine. Not something I've felt the need for recently but when I tried the previous method on a curved surface, it didn't really project features radially or perpendicular. That's fixed now.
Title: Re: Going over to the dark (CNC) side!
Post by: jadge on August 15, 2020, 08:54:06 AM
Have any of you used the tapered engraving cutters?

Yes, many years ago. I used to have a Taylor Hobson engraving machine and their tapered cutters worked fine. Later I tried engraving on my CNC mill; which was a failure. I tried chamfering cutters and short and long taper single edge cutters. The chamfering cutter left burrs and the tapered cutters broke within the cut. I came to the conclusion that a 5000rpm top speed simply wasn't high enough for the tapered cutters, at least in the aluminium and steel I wanted to engrave. I now have a high speed spindle, but haven't had the need to engrave. Nameplates have been the other way round with proud lettering for which I've used small (~1mm) endmills.

Andrew
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on August 15, 2020, 10:19:44 AM
Quick Questing to those that may know where do you take the cutter diameter when working out the speed of the tapered cutters?

Completely pointed one would be hard to calculate at the end but the flat ended coul dbe calculated at that dia, dia at top of cut or maybe half way up. I suppose it's a bit like a facing cut on the lathe.

J

PS I've ordered a few of the Sorotec ones.
Title: Re: Going over to the dark (CNC) side!
Post by: nj111 on August 15, 2020, 10:39:17 AM
Given that the taper is most likely not a huge angle it probably doesn't matter, unless the cutter goes to a point in which case you need a high speed spindle.  Assume you have manual override of spindle speed so that you can tweak it so it sounds right during cutting? This is far more of a problem in woodworking, I have CNC routers which can swing very large profile cutters,  the diameter of the tool might be a small as 20mm at one part and 125mm at another part of the same cutter. In this instance spindle speeds become a compromise between an acceptable level of burning (peripheral speed too high) and a poor surface finish requiring handwork to clean up where the peripheral speed is too low. There is no easy way to overcome this.
Title: Re: Going over to the dark (CNC) side!
Post by: jadge on August 15, 2020, 10:43:42 AM
The engraving cutters I used had a small cutting edge at an angle on the end, like a D-bit. Given the shallow DOC one should take that edge as the cutter diameter. From a practical point of view most hobby equipment will not be able to run anywhere near fast enough. So simply run flat out and concentrate on picking a sensible chip load.

Andrew
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on August 15, 2020, 01:27:20 PM
Yes I was expecting to run at my max of 5000rpm and will go with the lowest value of the suggested Fz range. I don't see me doing much engraving but if th need was their could make a bracket to take my laminate trimmer which should be good for 30,000rpm.
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on August 15, 2020, 02:52:56 PM
I used G-Wizard to calculate and even in brass at 4000 rpm the suggested speed was around 1 IPM.  This was for engraving letters at .003" DOC. 
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on August 15, 2020, 03:02:40 PM
But what diameter do you enter into the Wizard?
Title: Re: Going over to the dark (CNC) side!
Post by: Jo on August 15, 2020, 04:35:54 PM
But what diameter do you enter into the Wizard?

I am pleased Dave is not reading this  ::)

Jo
Title: Re: Going over to the dark (CNC) side!
Post by: Bluechip on August 15, 2020, 05:07:46 PM
But what diameter do you enter into the Wizard?

I am pleased Dave is not reading this  ::)

Jo

Oh but he is  :ThumbsUp: 

It's a long time ago but if my memory serves the advice from the School Nurse was ' As much as you can muster without passing out '.   :whoohoo:

HTH

Dave
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on August 15, 2020, 05:18:44 PM
I think you two have been in lockdown for too long and need to get out a bit more, just make sure you keep at least two wand lengths apart :Jester:
Title: Re: Going over to the dark (CNC) side!
Post by: Bluechip on August 15, 2020, 06:36:50 PM

 :headscratch:

Any arrangement we may or may not have vis a vis 'wands' is no concern of yours.   :lolb:

Might I draw your attention to the last verse of the following:

https://www.youtube.com/watch?v=xvH1oPVULyI

Off now .. it's  :DrinkPint: time. ( And not just one either).   :lolb:

Have fun folks. I'm off ...

Dave

Title: Re: Going over to the dark (CNC) side!
Post by: crueby on August 15, 2020, 08:58:48 PM
.... I'm off ...

Dave
Yup!   Six or seven bubbles off plumb....   :lolb:
Title: Re: Going over to the dark (CNC) side!
Post by: Bluechip on August 15, 2020, 09:49:48 PM

Yup!   Six or seven bubbles off plumb....   :lolb:



 :lolb:  :lolb:  At the very least.

IMHO Sobriety negates nearly all the reasons for getting out of bed in the mornings.   :ThumbsUp:

Incidentally, my dear old Granny, who in WW2 was bombed and nearly killed in Birmingham, ( ours, not yours ), used to lecture me at length on the consequences of my youthful slurping. 

The easiest way to counter this was to remind her that Herr Hitler was teetotal.  ;D

Anyway, off for a read and a kip. Top secret mission deep into the hinterland tomorrow to secure more rust for person  whose identity cannot be disclosed.

Dave



Title: Re: Going over to the dark (CNC) side!
Post by: john mills on August 15, 2020, 11:07:35 PM
for tapered cutter calculate for the bigger dia  that has to last
for engraving  i found the best was to use D  bits   just practice grinding them .
when i started with CNC one of the jobs i did was embossing dies    they were in tool steel  MST  the dies were used in a 20 ton crank  press.and larger ones in upto 150 ton hydraulic presses which the pressure turn up to
who knows.
i asked an engraver what they used and he showed me a D cutter i around up the shape tappered with radius on the end.i only had a tool and cutter grinder to use.some lasted and some did not .i made lots of those dies on cnc machines and operators used my programs over 20 years in that work shop.some times that job had been sent to a specialist engraver .seeing someone who work there that had to do them they hated doing them they must of found them difficult.i just did them.the machines they were done on only had 3500rpm top speed so that was the speed .     just a feed rate too suit  i think it was about 20 or 30mm a minute   
                                          John
Title: Re: Going over to the dark (CNC) side!
Post by: Muzzer on August 16, 2020, 10:37:19 AM
I used G-Wizard to calculate and even in brass at 4000 rpm the suggested speed was around 1 IPM.  This was for engraving letters at .003" DOC.
No need to waste valuable beer tokens on G Wizard. The sums are very simple - feed per tooth x number of teeth x rpm = feed rate.

I assume 3 thou is the depth of the engraving INTO the surface, since 3 thou feed per tooth would give 12 IPM feedrate at 4krpm.

If you are using Fusion 360, it does the feedrate calculation for you when you set up the tool.
Title: Re: Going over to the dark (CNC) side!
Post by: jadge on August 20, 2020, 12:30:21 PM
After some experimentation, and broken cutters, I've managed to finish a regulator cover plate:

(https://listerengine.com/coppermine/albums/userpics/10022/normal_Regulator_6.JPG)

The key was to change from a 2-flute economy cutter (from a professional supplier) to a 3-flute mid-range cutter from another supplier. The new cutter is from the YG K2 general purpose range, which I use for most of my general machining. Supplier, in the UK, was Cutwel. I ended up with a stepdown of 0.05mm, stepover of 60% of cutter diameter and a feedrate of 120mm/min. Total machining time was a bit under 2 hours. I suspect that the stepdown and/or stepover could be increased, as could the feedrate, but I'm only making two of these so it's not worth breaking more cutters in an attempt to speed things up. At least I now have some hard numbers to play with for future machining with small cutters.

The original program included code for opening out the O and P. These are very small openings so I deleted the original code and ran them as a separate programs. Rather to my surprise the code for the O ran perfectly given that my CNC mill is at the larger end of the hobby market and is old and has been worked fairly hard. I decided that the code for the letter P would be a step too far. The letters on the fullsize cast plate are poorly defined, including no opening on the letter P, so I claim I'm following the prototype in that respect.

Andrew
Title: Re: Going over to the dark (CNC) side!
Post by: nj111 on August 20, 2020, 03:18:04 PM
Good work.  Another approach might be to build a little spark eroder for detail jobs like that.  (I did so about 15 yrs ago from Ben Flemings first EDM How To book). Then all you have to do is machine the negative image into graphite, with which there is no danger of a broken cutter. Then spark away a few of those!
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on August 20, 2020, 09:55:43 PM
The way to speed up the process is to divide the area so as to separate the letters from the rest of the pocket.  The flat areas can be done with a much larger cutter and faster before switching to a tiny cutter to finish the area containing the letters.

But as always as a hobby project, if one is not rushed then the machine won't get tired either.
Title: Re: Going over to the dark (CNC) side!
Post by: jadge on August 21, 2020, 10:39:04 AM
I'm well aware of the concept of re-machining with different cutters. Grannies and eggs come to mind.  ;D  In my CAM program you don't need to separate the areas. Simply machine most of the material away with a larger cutter. Then, on the same area, select re-machining using a smaller cutter. Knowing what size larger cutter was used the system uses the smaller cutter to machine away the remaining material. However, on my high speed spindle I can't repeatably set tool lengths and so can't use tool tables. That means manually reseting the tool each time. For a 2 off I judged it was easier to let the mill get on with it while I did something else rather than muck about with tool changes.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on August 21, 2020, 06:45:24 PM
Good service from Sorotec in Germany with plenty of e-mails to let me know what was happening with order together with a DHL tracking number.

Cutters arrived today.

The one with the spiral flute is 60deg pointed and the two more traditional half round ones are again 60deg but with 0.3 and 0.5mm flat at the end. Just need something to try them out on now.

Second photo shows that it will not be such a problem if I break one and have to reorder as there was a little extra in the jiffy bag :P
Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on August 21, 2020, 07:23:51 PM

it's nice when your supplier adds some unexpected goodies.

But they have a long way to go to get to the standard of these customized candies from 'Just Castings Ltd' (by Royal Appointment)

(https://listerengine.com/coppermine/albums/userpics/10013/P1070033.JPG)


Mike
Title: Re: Going over to the dark (CNC) side!
Post by: crueby on August 21, 2020, 07:26:29 PM
Now if I could just get my candy supplier to throw in some castings....
Title: Re: Going over to the dark (CNC) side!
Post by: Admiral_dk on August 21, 2020, 08:44:33 PM
Correct Mike .... but if the price of you're castings are compared to the candy you got and you do the same with the mill bits Jason brought to the little bag of Haribo he got as a treat - you were skinned ...!   ;)   ;D

All that said - I think you both did great in the end  :cheers:
Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on August 21, 2020, 09:25:12 PM
Correct Mike .... but if the price of you're castings are compared to the candy you got and you do the same with the mill bits Jason brought to the little bag of Haribo he got as a treat - you were skinned ...!   ;)   ;D

Per
The cost of the goodies is of no real importance. The 'value' of a little surprise gift is enormous. You will always remember where to go back to.

BTW if you check the cost of those Sorotec engraver bits and the DHL delivery costs, you will understand why they handed out the 'sweeteners' :ROFL:

Mike
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on August 22, 2020, 07:30:12 AM
Funny enough they cost no more than going to a UK supplier such as APT or Cutwell who don't send sweeties
Title: Re: Going over to the dark (CNC) side!
Post by: Admiral_dk on August 22, 2020, 04:37:54 PM
Agreed Mike - it was kind of a joke - and I also agree that the price has nothing to do with the pleasant surprise when you open the package and discover the treat  :cheers:

Jason - this was not meant as a derailment of your excellent thread ...:

If you (as a company) buy those treats by the cubic meter -> ridiculously cheap and you compare that to the positive customer experience (they come back) -> they more or less payed for themselves ~ same price as the competitors ...!
Title: Re: Going over to the dark (CNC) side!
Post by: awake on August 22, 2020, 05:06:20 PM
Now if I could just get my candy supplier to throw in some castings....

 :ThumbsUp: :ThumbsUp: :ThumbsUp:
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on August 30, 2020, 07:09:51 PM
So after that brief engraving interlude it's back to the pattern making.

having done the bearing caps that retain the beam pivot it was time to make the "Yoke" pattern this is the U shaped top to the column that the beam fits between and would requite a core print so that the iron would not flow into the middle of the U shape. I decided to make each pattern half from tow pieces which saved materials and also meant that teh 6mm cutter did not have excessive stickout. First make the outer edges.

(https://hosting.photobucket.com/images/v156/jasonballamy/20200725_123000.jpg)

Then the inner part complete with the longer core print.

(https://hosting.photobucket.com/images/v156/jasonballamy/20200725_190847.jpg)

This is how each half will look once glued together, the bearing cap described earlier is also shown sat on top

(https://hosting.photobucket.com/images/v156/jasonballamy/20200725_184854.jpg)

https://www.youtube.com/watch?v=xBFrADdGgxA

I had also drawn up the almost 16" diameter flywheel for Graham with the hope that the finished item would look something like this

(https://hosting.photobucket.com/images/v156/jasonballamy/Flywheel_Render.JPG)

Enquiries to have teh patterns 3D printed or CNC cut from foam prooved too expensive and the size was well beyond what the KX3 could handle. However I said to Graham that it may be possible to CNC cut individual spokes and then biuld them into a rim.

A single spoke half was extracted from the pattern drawing and a trial spoke cut, starting with roughing out using a 10mm 2-flute flat ended aluminium specific cutter

(https://hosting.photobucket.com/images/v156/jasonballamy/20200727_114518.jpg)

Followed up with the 3D contour cuts using a long shank 6mm 4-flut ball ended cutter that can be seen in the photo above.

(https://hosting.photobucket.com/images/v156/jasonballamy/20200727_122601.jpg)

I was very pleased with the finish straight off the mill with a very little sanding left to do.

(https://hosting.photobucket.com/images/v156/jasonballamy/20200727_122852.jpg)

With the success of the first spoke it was time to set up to batch cut the remaining 11. I opted to use a stop so that each blank could be roughed and then the tool changed and all the finish cuts done.

(https://hosting.photobucket.com/images/v156/jasonballamy/20200806_152350.jpg)

(https://hosting.photobucket.com/images/v156/jasonballamy/20200808_114219.jpg)

The beech spoke material had been glued to the MDF holding blocks with a sheet of paper between which makes it very easy to separate the parts as the paper just delaminates and can be sanded off

(https://hosting.photobucket.com/images/v156/jasonballamy/20200810_160026.jpg)

Now with an 11" swing lathe the 16" rims could not be turned so two MDF rings were rough sawn and then profiled using co-ordinates while being "turned" on the rotary table.

(https://hosting.photobucket.com/images/v156/jasonballamy/20200816_094746.jpg)

All that then remained was to cut the six notches into the rim to locate the spoke ends and glue it all together followed by a wipe of filler and some sanding.

(https://hosting.photobucket.com/images/v156/jasonballamy/20200823_135045.jpg)

All the patterns ready to post.

(https://hosting.photobucket.com/images/v156/jasonballamy/20200823_135242.jpg)

https://www.youtube.com/watch?v=CSzUr8B03S0

Title: Re: Going over to the dark (CNC) side!
Post by: awake on August 30, 2020, 07:32:27 PM
WOW! Those spokes came out gorgeous, as did the assembled pattern. Superb work!
Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on September 03, 2020, 08:11:20 PM
I have a small EMCO Compact 5 CNC lathe, which I use for all sorts of small work and also for thread cutting. The machine uses a spindle encoder to synchronize the carriage movement with the spindle rotation for screw cutting. It also provides a spindle RPM readout. Actually there are now two RPM readouts, one on the old EMCO electronics box and one on the LinuxCNC display screen. You will all know by now that the Number 11 (below the RPM display) was the machine number from this machine's days in the rehabilitation center at Parkhurst Prison on the Isle of Wight, home of some rather 'tough nuts'.

(https://listerengine.com/coppermine/albums/userpics/10013/P1080454small.JPG)




Over the last few weeks both RPM displays had become intermittent and when I wanted to do some thread cutting, I found the spindle/ carriage synchronization had also stopped. So no more thead cutting. Faults with forty year old electronics are always a problem, due to the unavailability of spare parts etc. To add to the confusion, the synchronization function was now split between the old EMCO electronics and the newer LinuxCNC control system. I was not looking forward to the investigation an eventual repair. In the event it was a quick and easy fix. The optical sensor which detects the spindle rotation was covered in fluff and rubber dust from the drive belt, which had accumulated over the part forty years. A quick cleanup with a clean rag wetted with IPA and I was back in business again.

You may be interested in the LinuxCNC display screen for thread cutting

(https://listerengine.com/coppermine/albums/userpics/10013/P1080453small.JPG)


The tool position graphic and DRO are in the centre top window, The RPM bargraph and numerical display are to the right. Dead centre if the G-code file text. The icons at he bottom are a selection of the pre-prepared.thread pitches available. There is a selection of TPI threads, BA threads and ISO threads. It's not to difficult to write a new macro for an new or unusual thread.

All the thread cutting information is contained in one line of G-code. You can see it in the middle of the G-code text window. The single line of the G76 thread cutting cycle contains all the parameters necessary to cut a perfect thread. The P parameter specified the thread pitch. The Z parameter specifies the length of the thread. The I parameter specified how far the tool retracts between passes. The J parameter specifies the depth of the first pass and the number of passes to reach full depth of cut. The K parameter specifies the depth of the full thread. The H parameter specifies the number of spring passes at full depth to clean up the thread. There are also other parameters which control the thread lead-in and lead-out taper and also the compound slide angle.

Sorry if that's all a bit 'techy' but I am sure some of our members will be interested in the finer details.

Anyway, I am so pleased I have thread cutting function working again

Mike


Title: Re: Going over to the dark (CNC) side!
Post by: Admiral_dk on September 03, 2020, 08:57:24 PM
I'm so happy for you Mike - it's always great when it's a simple (and cheap) solution  :cheers:

I can also say that I'm not particular surprised as it's often the sensors (or wiring to them) that fails and dirt and grime on the sensor is a very common occurrence ....
Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on September 03, 2020, 09:04:32 PM
Per,

It's the aging and oxidising, tin plated connectors which are now the weak link ( :Jester:) in old Emco machines. I have more trouble with them than anything else.

Mike
Title: Re: Going over to the dark (CNC) side!
Post by: Hugh Currin on September 04, 2020, 05:45:30 AM
Mike:

Are the "files" at the bottom of the LinuxCNC screen shot just G-code files? Load the file you need when you need it? How do you set the parameters in the G76 command? Some of those, like starting point, can't be hard coded.

I found a lathe front end for LinuxCNC  here  (https://forum.linuxcnc.org/41-guis/26550-lathe-macros?start=0#34357). I have not tried to implement it yet but it looks interesting. I did download the *.zip file and study the codes, particularly trying to understand threading. I learned quite a bit about using "variables" and "routines" in LinuxCNC.

I remember writing a lathe threading code, from all this, but can't locate it. I hope it hasn't disapeared.

Glad to hear your EMCO is up and running. Is that another lathe next to it?

Thanks.
Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on September 04, 2020, 10:51:38 AM
Hello Hugh,

Dont forget, it was you who got me off the ground with LinuxCNC by recommending a certain Intel Atom processor. Since then, I have committed all my machines to LinuxCNC. In it's 'free to download' form it has proved 110% reliable and virtually bullet proof. The screen display are a little basic, but perfectly usable. Over the years,  alternative screen displays, such as Pathpilot and the different front ends from the likes of Andy Pugh and other LinuxCNC forum members, have become available.  My only comment is that the fancy display screens do not actually machine the metal any differently or better. The sexy new display screen with their rendered 3D graphics etc, simply put a greater burden on the PC and often still contain programming bugs. You need the latest and fastest PC to keep up with the fancy graphics while the basic LinuxCNC machining processes can live on a much simpler and older PC.

The files at the bottom are short G-code files, one for each of the commonly used thread types and sizes. You click on the one you wish to use. Having a selection of pre-programmed files is so much more convenient (from a machinists point of view) than trying to produce the thread cutting code on the day.

The P and the K parameters of the G76 command define the pitch and thread depth. You get these from engineering tables and enter them into the G76 command line with a text editor. The only thing you may need to change is the Z parameter which defines the length of the thread to be cut.

I set both axes to zero, after manually positioning the cutting tool at the end of the bar stock and 0.1 inches out from the surface.

I used the Stepconf wizard to configure the lathe for the standard ZX lathe configuration for the threading work. I have an alternative XY configuration (same as a mill) for most turning work. I find XY working less confusing than ZX.

The machine beside the Compact 5 lathe is an EMCO F1 mill. It has a much modified compact 5 lathe bed bolted to the table, I use it as my 4th (rotate) axis for indexing etc. Over the years the 1970's paint colour has faded from a lurid bright orange to a mellow yellow.

Keep trucking

Mike
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on September 04, 2020, 12:52:38 PM
I replaced Mach3 on my mill with PathPilot; definitely an improvement.  My little CNC lathe has sat unused for a good while; it uses Mach4, which I like less.
Title: Re: Going over to the dark (CNC) side!
Post by: Hugh Currin on September 04, 2020, 05:50:27 PM
Mike:

I tend to agree with everything you said. I've found LinuxCNC very solid and useful. I'm glad you're not cursing at me for dragging you down that rabbit hole. I used the first display (TKEMC) for years but have now drifted to the "new" AXIS display. Both are bare bones by today's standards, but as you say they cut just as well as any and are solid. Pathpilot is reported to be nice (kvom) but I've not been tempted, and don't know how well it works on a lathe.

I downloaded Andy Pugh's lathe interface (as I linked) but haven't tried to incorporate into my system. After looking at his code my plan is to modify this to a general purpose G-code routine for threading. Probably a subroutine to do the work and a header program to just call it. That way I'll be able to hand code the subroutine into larger programs if needed. I found my notes on this to realize I've not complete it. I studied Andy's code enough to understand it, but still need to modify it for my needs. (He's done the heavy lifting already). Soon. I'll let you know when I get it, it might be useful to you.

After years of thinking about and designing timing belt fourth axis configurations, I bought a harmonic drive off E-bay. It's smaller than I thought but will work for light work. Just need to build the framework and add a fourth driver to the control box. One more effort demanding my time. :-)

I've used the Sherline lathe off and on the last year or two. But I should have a 10" lathe arriving any day now specifically for CNC conversion. The Sherline is boxed up so the threading routine is academic till I get the lathe converted.

Way too many projects, and I still need to get back to my Stirling engine effort.

Thanks.
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on September 04, 2020, 09:34:48 PM
(http://Pathpilot is reported to be nice (kvom) but I've not been tempted, and don't know how well it works on a lathe.)

If you look at some of Tormach's videos on their slant lathe, it appears that almost every standard lathe op can be invoked via the graphic wizards and no knowledge of g-code.  Turning a curved surface would require either CAM or canned procedure.  Since there's LinuxCNC under the covers, conversion to a non-Tormach lathe would be primarily concerned with the hardware interface.
Title: Re: Going over to the dark (CNC) side!
Post by: gerritv on September 04, 2020, 10:29:06 PM
Tormach's conversational is why I am using PathPilot for my gantry mill build. For US$28.95 plus shipping it is a bargain IMHO. A Mesa 7i92 and off to the races. I'm using it with an old PMDX-132 and a custom cable to keep the pinouts the same as Tormach 440. Regular updates and fixes are free.

An added bonus is not having to mess about with Linux too much, not my fav way to waste time :-( Just install and go.

gerrit
Title: Re: Going over to the dark (CNC) side!
Post by: Hugh Currin on September 04, 2020, 11:01:53 PM
I've not used a conversational cnc controller. I'm so used to not having one that I'm convinced they are not useful. What a closed minded person I am.

I see contradictory information about obtaining PathPilot. I can find no listing on the Tormach site. But a few threads I just looked at say it isn't available without a Tormach machine serial number. Others say yes it still is, for around $100. It could be worth a call to Tormach to see. For $100, or even more so for $30, it would be worth trying. The interface looks nice and clean. I'll put this on the to do list and wait for it to percolate to the top. It's getting to be that energy, instead of time, is the limiting factor.

Gerrit: The install and configuration of LincuCNC keeps getting easier

Thanks.
Title: Re: Going over to the dark (CNC) side!
Post by: gerritv on September 04, 2020, 11:21:47 PM
The specific item to look for is the 2.0 upgrade USB stick. Can be had with or without a printed manual: https://tormach.com/catalogsearch/result/?q=pathpilot+upgrade

Sadly like so many things with the www and Linux in general, there is much conflicting information. In reality Tormach do not care if you buy the SW with or without a machine. Their distributors OTOH do seem to care. I tried buying the USB stick locally in Canada, they "couldn't sell it to me without a machine serial number" so ended up ordering it directly from Tormach.

While I agree that there have been efforts to make installing LinuxCNC simpler, the only place to find that is in the forum. Their web pages are best avoided for installation in my experience (I spent 11 years with Unix so not exactly a newbie to this). There are 3 threads in the forum on Quick and Easy Install (https://forum.linuxcnc.org/9-installing-linuxcnc), one with 320+ posts! Most ppl have success, some do not. Newer hardware seems better although best to avoid parallel ports altogether. Of the gazillion flavours of Linux I must say that Mint is quite friendly. Thankfully that is what Tormach use as well.

I don't consider you closed minded for not using the conversational, it all depends I think on your experience level. I am a relative neophyte with gcode, and for now prefer when my machine starts cutting to focus on speeds and feeds and not breaking tools while still getting mundane tasks completed. I know that I will be hand coding stuff eventually :-) Peter Smid's book is flipped through often in prep for that.

The great thing is that there are choices available, from Mach 3/4 to LinuxCNC with its various gui's and others as well.

Gerrit
Title: Re: Going over to the dark (CNC) side!
Post by: Dave Otto on September 04, 2020, 11:24:33 PM
I run a lathe at work with a conversation control, (Fagor). It is really pretty easy work with, just a bunch of building blocks turn, face, groove, thread etc. It even has a built on CAD window where you can draw a profile and then use it as a tool path. I don't think that I would want to deal with it on the mill but for the lathe it works quite well.
If you think about most lathe parts they usually are not all that complex.

Dave   
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on September 05, 2020, 03:16:08 AM
I never use the PP conversational wizards on my mill as I use CAM for everything.  If it were on my lathe I likely would use it most of the time.

I bought the PP CD from Tormach direct without any problem.  I knew nothing about LinuxCNC and thus had to do a bit of study on how to configure it after the install.  Luckily another use of my machine brand did it first and was able to help a good deal.  I built a new computer from components and added a Mesa card for a total of about $400.  I kept my old control computer and connect its breakout board to the Mesa card via a cable.

I am still running version 1.9 because it's been stable, and I don't want to go to the effort to upgrade to version 2, which mainly implements features I don't need.
Title: Re: Going over to the dark (CNC) side!
Post by: Hugh Currin on September 05, 2020, 04:00:52 AM
Gerrit:

Can't go too far wrong at those prices. I thought it was unobtainable or several hundred dollars. So you're suggesting "PCNC 1100 PathPilot Upgrade Kit - Software & Manual PN: 38706" rather than "PathPilot Software Bootable USB Drive - Recovery Media PN: 38249"? If I can get one I'll start bothering you about which Mesa cards and pin out. But for now which to order. Thanks.

The only downside for Tormach I can see is they'll get more support questions. That could be a problem on their end. Otherwise, win/win.

I confess, I just Google for LinuxCNC questions and end up in the forum more times than not. But it's solid code and free. :-) On my last install I somehow ended up with an old unsupported Ubuntu version which I thought was LinuxCNC's most current release. Works fine until you want to install, say, an editor and all the Repositories are gone. When I get a chance I think I'll upgrade to Mint. Last time around I moved from the parallel port to a Mesa 5I25 card directly connected to my older than old PMDX breakout board.

I tend to be cautious with large scary cnc machines. I use MDI commands and if complex at all CAMBAM. I very seldom hand code G-code, but knowing a little helps at the machine with MDIs. Also handy when modifying post processors. For the mill CAMBAM is, I believe, a good 2 1/2+ CAM package. (I'd like a true 3D package but haven't found one yet.) The CAM packages are pretty good for milling but for lathe work it's a little different. I think there are some good commercial packages for lathe but I can't afford them (and won't use Windows). So, for the lathe I end up doing more hand coding, very carefully. It's a lot easier than a real programming language. A G-code simulator helps with debugging also.

Thanks for the help.
Title: Re: Going over to the dark (CNC) side!
Post by: Hugh Currin on September 05, 2020, 04:07:01 AM
Dave:

I do see how it could be useful. I've not had a chance to use any conversational controllers so not used to it. I do see some things could be useful on the mill if time mattered a lot. Such as bolt circles, countersinks, peck drilling, etc. But for sure on a lathe as CAMBAM won't give lathe boring or threading.

Thanks.

I run a lathe at work with a conversation control, (Fagor). It is really pretty easy work with, just a bunch of building blocks turn, face, groove, thread etc. It even has a built on CAD window where you can draw a profile and then use it as a tool path. I don't think that I would want to deal with it on the mill but for the lathe it works quite well.
If you think about most lathe parts they usually are not all that complex.

Dave
Title: Re: Going over to the dark (CNC) side!
Post by: Hugh Currin on September 05, 2020, 04:08:48 AM
kvom:

Excellent. Someone else to ask about Tormach Mesa cards, pin outs, etc.

Thanks.
Title: Re: Going over to the dark (CNC) side!
Post by: gerritv on September 05, 2020, 09:16:22 AM
Gerrit:

Can't go too far wrong at those prices. I thought it was unobtainable or several hundred dollars. So you're suggesting "PCNC 1100 PathPilot Upgrade Kit - Software & Manual PN: 38706" rather than "PathPilot Software Bootable USB Drive - Recovery Media PN: 38249"? If I can get one I'll start bothering you about which Mesa cards and pin out. But for now which to order. Thanks.

The only downside for Tormach I can see is they'll get more support questions. That could be a problem on their end. Otherwise, win/win.

I confess, I just Google for LinuxCNC questions and end up in the forum more times than not. But it's solid code and free. :-) On my last install I somehow ended up with an old unsupported Ubuntu version which I thought was LinuxCNC's most current release. Works fine until you want to install, say, an editor and all the Repositories are gone. When I get a chance I think I'll upgrade to Mint. Last time around I moved from the parallel port to a Mesa 5I25 card directly connected to my older than old PMDX breakout board.

I tend to be cautious with large scary cnc machines. I use MDI commands and if complex at all CAMBAM. I very seldom hand code G-code, but knowing a little helps at the machine with MDIs. Also handy when modifying post processors. For the mill CAMBAM is, I believe, a good 2 1/2+ CAM package. (I'd like a true 3D package but haven't found one yet.) The CAM packages are pretty good for milling but for lathe work it's a little different. I think there are some good commercial packages for lathe but I can't afford them (and won't use Windows). So, for the lathe I end up doing more hand coding, very carefully. It's a lot easier than a real programming language. A G-code simulator helps with debugging also.

Thanks for the help.
The choice for me was cost, I don't like buying in US and shipping to Canada is extortionate so choose the USB only option. I have a shipping address in NF, NY. (Not much use until next year due to border closure :-() Since my copy is still on 'the other side of the wall', I found a download of the 2.0 version to get on with things.

You have the 5i25 which is directly supported by PathPilot. I went for 7i92 because my Atom PC doesn't have a viable pci slot. The pinout is dictated by which Tormach machine's pinout best matches the PMDX bob. I used jumpers to arrive at the correct match so I avoided editing the HAL files. They get overwritten upon updating PathPilot.

I learned in the early 80's to be OS agnostic, I choose based on what I want/need to do. And for that Windows is far superior to FOSS IMO. I tried Cambam years ago but gave up due to the total absence of the developer for several years. Then came Fusion360 :-) With the Linux subsystem in Windows 10 I can scratch that itch on the rare occassions that I need curl. For Fusion there is also the Mac option although I refuse to spend anything on them :-)

I'll be happy to help once you get to the stage of connecting to the PMDX. I will send you my cable map in a PM, the PMDX-131 should be close to the PMDX-132 that I have.

I am a few weeks away I think from cutting my first chips on this build.

Gerrit
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on September 20, 2020, 05:01:29 PM
With the possible loss of some of the F360 functions I thought I should get a few bits that I already had drawn out run through their CAM and knock them out.

(https://hosting.photobucket.com/images/v156/jasonballamy/DSC03996.JPG)

First up were a couple of simple 2D contouring jobs being the timing bracket and a knob to lock it's position for teh Thompson engine, couple of holes also done on the CNC for the bracket.

(https://hosting.photobucket.com/images/v156/jasonballamy/DSC03995.JPG)

Then the rocker arm for the same engine from steel roughed out with 3D adaptive and then shaped with "steep & Shallow"

(https://hosting.photobucket.com/images/v156/jasonballamy/DSC03994.JPG)

Finally the conrod, a rectangular blank was milled down from some round 2014 and the two holes reamed on the manual mill then these holes were used to hold the blank while the 3D adaptive and Steep & shallow did their thing.

(https://hosting.photobucket.com/images/v156/jasonballamy/20200920_102600.jpg)

(https://hosting.photobucket.com/images/v156/jasonballamy/DSC03993.JPG)
Title: Re: Going over to the dark (CNC) side!
Post by: gerritv on September 20, 2020, 05:51:33 PM
Very good result. Can't wait to get my machine operational.

Gerrit
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on November 02, 2020, 07:02:47 PM
With another stint of pattern making that I can't disclose at the moment out of the way it was time to get back to making metal swarf in the form of the external shaping of a crankcase for a small version of the 36cc Wall 2-stroke.

https://www.youtube.com/watch?v=D76Bwl9F2gc
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on November 07, 2020, 04:59:00 PM
I started this combined inlet and exhaust manifold for the Wall engine yesterday and completed the finish cut on the second side this morning.

First side after adaptive clearing which was done with a 5mm 2-flute cutter for Aluminium from Arc's premium range. Run at 5000rpm, 300mm/min feed, 5mm high x 1mm deep cuts to remove most of the waste then it stepped up 1mm at a time to leave a part looking like this.

(https://hosting.photobucket.com/images/v156/jasonballamy/20201106_153712.jpg)

Then a "steep and shallow" finish pass with a 4mm dia 2-flute ball nose cutter for aluminium from APT as they do them with a 4mm shank which I needed to reach down the side of the rectangular flange. This was also run at 5000rpm and 300mm/min feed the scallop spacing was set at 0.25mm which takes a while but gives a nice finish.

(https://hosting.photobucket.com/images/v156/jasonballamy/20201106_174254.jpg)

Then it was basically do it all again for the other side but as the end flanges are different shapes a second setup was used in fusion with the bottom of the work now the top

(https://hosting.photobucket.com/images/v156/jasonballamy/20201107_091214.jpg)

As it will fit onto the side of the engine. Holes were drilled and tapped while it was still a rectangular block on the manual mill and I was happy that the drilled passages did not appear as the external shape was cut.

(https://hosting.photobucket.com/images/v156/jasonballamy/20201107_095758.jpg)
Title: Re: Going over to the dark (CNC) side!
Post by: Chipmaster on November 07, 2020, 07:34:06 PM
That's marvellous Jason.

Andy
Title: Re: Going over to the dark (CNC) side!
Post by: Hugh Currin on November 08, 2020, 03:09:27 AM
Jason:

Marvelous work and part. I need to learn the software to go beyond 2 1/2 D CAM. Such parts push me in that direction. Very nice.

How did you align the two set-ups so well?

The first picture, first roughing pass is cool by itself. It would make an interesting engine to stop there. Kinda an art deco motif.

Thanks.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on November 08, 2020, 07:58:26 AM
It's certainly the type of part where the CNC comes into its own and would mean that all those old aero engine designs that ar eout there with no current source of castings could be made again without needing to spend hours carving manually which I'm sure puts a lot of people off and you have the added bonus of nice material to machine and no chance of finding a defect hiding inside. Makes you wonder if there would be a market for CNC machined "castings" that still left the final machining to the builder?

As for positioning the part. First side was easy as I had machined the block and done the drilling on the manual mill so just set it up on parallels in the vice and located ctr which is what I mostly use a datum and set tool from top of block. For the second side before removing the half machined part I clamped a couple of 1-2-3 blocks in place against the rectangular flange. This then gave me an stop in the X-axis and a vertical face, vice jaw set Y-axis, add a pair of parallels under the two curves and that fixed the parts position.
Title: Re: Going over to the dark (CNC) side!
Post by: nj111 on November 08, 2020, 11:44:12 AM
very nice. Could I ask, can those toolpaths be programmed in the free version of Fusion 360 , or is a higher level required?
Title: Re: Going over to the dark (CNC) side!
Post by: Alyn Foundry on November 08, 2020, 12:04:29 PM
That's marvellous Jason.

Andy

I concur.

 :ThumbsUp:
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on November 08, 2020, 01:25:27 PM
I'm not totally sure about the revised "free" version. You certainly won't get it for free as they have moved the "steep and shallow" to what they call an extension which could be purchased for 1 day or 1 months use but I don't know if you can buy it in the free version or only the next level up. The free one I believe will still do the adaptive clearing and there are other finishing options that would come close.

Funny enough The subject came up on ME when someone asked about the new Alibre "Workshop" which is a 1 off payment for Atom3D and MeshCAM though MeshCAM can be bought separately. I had a quick go at the trial version and although it is more basic as you would expect for  alot less outlay it looks like it would give a reasonable finish.

This is the Alibre simulation
(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/880231.jpg)

And this the MeshCAM simulation, you can see more of a step on the vertical edges in the X direction as it is stepping over in Y rather than stepping along the actual surface.
(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/880232.jpg)

I've since played about with MeshCAM a bit more and can get a slightly better finish, both examples use a similar stepover. It's something I will need to decide on soon as my access to these features on F360 will soon expire so it's a question of first seeing what I can actually still do in F360 with the new "free" version, paying the yearly fee for a program that I am used to and that has a lot of features or go for something like the one off MeshCAM that is less than a years licence of F360. If I get my finger out and finish off another build article for ME mag then that will pay for a few more years of F360 and Alibre which I use for drawing.
Title: Re: Going over to the dark (CNC) side!
Post by: Muzzer on November 08, 2020, 03:55:53 PM
Steep and shallow doesn't allow any particularly unique surfaces to be machined. There are quite a few toolpaths in the free version that can achieve what's being done here (see screenshot) but you'd perhaps need to combine 2 of them.

Most of the other toolpaths tend to be focused on either mostly horizontal or mostly vertical faces. Whilst many of them are capable of machining curved faces, a vertical stepdown or a horizontal stepover isn't best for faces that trasition eg from horizontal to vertical (think a sphere or indeed a horizontal pipe). However, you can tell it to stop when the face reaches a certain inclination. Then you can do the rest with a different, more suitable toolpath. The benefit of steep and shallow is that it achieves a tangential stepover along the surface, so can cope with anything from horizontal to vertical faces. Autodesk consider that enough to command a massive premium.

Looking at Meshcam, I'm guessing the toolpath shown isn't working like SnS - it appears to be running parallel paths. That's one of the simplest of toolpaths and it's one of the many 3D paths in Fusion - if you are doing 3D surfacing, there's not much actually missing in the free version. The main annoyance is the removal of rapids and tool changing (and 4th axis). Having said that, there are already post processor add-ins appearing that get around the rapid and tool change issue.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on November 08, 2020, 04:25:18 PM
Although it may not allow unique surfaces to be machined it is the best for this type of work.

It saves having to do parallel in two directions and on a part like that manifold where the vertical edges are at different heights as ringed you really need to run it the full height, its just a simple case of selecting that option and your scallop spacing and it will do the rest so only two items to do the code for - Adaptive and S&S. Before I discovered S&S I was not getting anywhere near as good a surface. But I guess that's why they want to charge a premium for it.

The other MeshCAM option seems to combine parallel in two different directions which is better but won'tt run around and up/down a curve all at the same time though the simulator is not as good as F360 so you can't really see where the tool is moving as it just shows the toolpath and finished surface

Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on November 12, 2020, 02:39:47 PM
I had an hour to spare so decided to carve out another casting, this time one of the end plates for the Wall engine, turning of the spigot that locates in teh crankcase and boring for the bearing had already been done in the lathe so just the external shape to be done.

After adaptive clearing and pocketing with a 4mm 3-flute Carbide cutter for aluminium at 5000rpm, 300mm/min feed, 4mm high cut x 1mm stepover on teh adaptive and 1mm x 1mm on the pocket ramping down into the recesses.

(https://hosting.photobucket.com/images/v156/jasonballamy/20201112_115509.jpg)

Then steep and Shallow while I still can with the boundary set within the inner diameter of the flange, 4mm ball nose 2-flute carbide at 5000rpm, 300mm/min feed 0.3mm stepover.

(https://hosting.photobucket.com/images/v156/jasonballamy/20201112_122831.jpg)

After that photo I also used the CNC to spot and drill the four 3mm holes. The flange had been left with 0.5mm remaining which I went back to the lathe to turn off.

(https://hosting.photobucket.com/images/v156/jasonballamy/20201112_134205.jpg)

J
Title: Re: Going over to the dark (CNC) side!
Post by: kuhncw on November 12, 2020, 05:16:42 PM
Very nice work,Jason

Thanks for posting the steps you went through in the CNC process.

Chuck

.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on December 31, 2020, 06:55:52 PM
A while ago I asked whether anyone had used the tapered engraving cutters http://www.modelenginemaker.com/index.php/topic,8882.msg223889.html#msg223889

Well I've finally got round to trying out the ones I bought from Sorotec. Although a bit deeper than your average engraving my need was for some letters to apply to the side of a model to represent the cast on wording that would have been done with pattern makers letters. I found a couple of offcuts of soft bending brass which is a bit stickier to machine than the normal harder brasses used for machining and engraving so a good test for the cutters and with a thickness of 1.1mm a lot deeper than you would normally use them at.

To hold the sheet material I soft soldered it onto an off cut of 1/4" brass originally intending to just have a try and then do al the wording from a single piece but as the first letter went well I just squeezed the rest onto two smaller scraps. Taking the 60deg cutter with a 0.5mm flat end and running at 5000rpm and with a modest feed of 60mm/min and ramping down into the work at 2degrees for a max depth per pass of 0.25mm the cutters took it in their stride and seemed to produce a reasonable chip with minimal burrs left on the soft brass so I'm quite pleased with the result. After melting the work from the backing the letters just pushed out with finger pressure and a quick rub on some Emery had them ready for the next step.

https://www.youtube.com/watch?v=MLH2gxh-f7M

I have been upto other CNC things some of which can be found in this thread.

http://www.modelenginemaker.com/index.php/topic,10064.msg229619.html#msg229619

Title: Re: Going over to the dark (CNC) side!
Post by: Alyn Foundry on January 01, 2021, 12:39:01 PM
Your previous attempts went well at the foundry Jason.   :ThumbsUp:
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on January 01, 2021, 01:53:48 PM
Yes they look good with a bit of paint in the recesses, any sign of that flywheel yet?
Title: Re: Going over to the dark (CNC) side!
Post by: Alyn Foundry on January 01, 2021, 02:11:57 PM
No, not as yet.

It's either stuck in the Christmas post backlog or they never sent it. Obviously I can't find out until next Monday at the earliest.

Cheers Graham.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on January 19, 2021, 01:22:05 PM
Well with the post being what it is at the moment I decided to make a couple of Flywheels from Cast Iron, It was a good chance to try out the air coolant setup that I have been meaning to fit for a while. You can see the swarf build up on the ledges during the adaptive cuts as I was not able to manually clear it while taking the various video clips. But if you can bring yourself to watch through to the 5min mark you will see I have finally rigged up some air which is just enough to clear the swarf ahead of the cutter. The first side I stood over the machine clearing swarf more so on the adaptive than the finish but decided I did not want to waste another 3hrs each side. The second side and second flywheel were left unattended except for doing the tool change trusting F360 to have spat out the right code as each side and each flywheel was slightly different and all went well.

Ketan at ARC suggested that I use an air tool lubricator as I did not want to soak the place in coolant as this is what John Stevenson had set up ARCs own machines and his four Sieg CNC mills with. I'll only be using liquid when cutting aluminium but it certainly worked well doing the CI dry. Only a small amount of air is needed - the regulator was almost turned off and the swarf does not get spread all over the place staying in the "trough" that the KX3 comes with. I'll make the fitting a bit more permanent once I have tried it with liquid and then look at getting a quieter compressor as my old Machine Mart one is louder than the mill. The LocLine is acting as a means to position the air only as I have run a 4mm OD PVC line inside that with a small brass outlet drilled 1.5mm to get the velocity up and it will save a build up of fluid in the LocLine before it comes out the end.

https://www.youtube.com/watch?v=Z6IHoHO1yCo
Title: Re: Going over to the dark (CNC) side!
Post by: Steve17 on January 19, 2021, 03:21:12 PM
Jasonb, I like the idea of the tool oiler. What do you use in it? As in white water, cutting oil or any of the liquids designed for minimal quantity use. I purchased the last CNC from John's son last year and there is no sign of any retro fit coolant system.

Steve.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on January 19, 2021, 03:41:04 PM
Ketan says neat cutting fluid but as I'm only going to be adding liquid for aluminium will give it  ago with paraffin first.

If that is the one I saw up for sale then I don't think it was one of the ones from JS's workshop that he used to knock out things like the Myford index plates etc.

I may still have some photos thatKetan sent, will see if I can find them
Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on January 19, 2021, 03:49:16 PM
Jason,

Do you still have diaphragm air-brush compressor that you could try? You dont need a high pressure or even a high flow to blow away the chips. Using a big shop compressor is overkill. The noise on my shop compressor kicking in unexpectedly, when I am doing fine work, always makes me jump.

Another possibility is a small centrifugal fan similar to the fan a blacksmith uses to stoke the forge hearth fire

Mike
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on January 19, 2021, 03:57:37 PM
No chucked that out years ago. Mine is the smallest of the Machine mart ones only 5cfm displacement so more like 3cfm FAD, I would say it's running 30% of the time. Regulator is screwed out as far as it will go, anymore and flow stops and not even registering on the pressure gauges so very little air being used. I would say it's no stronger than I can blow. The biggest problem is it's 95dB so I'm thinking of getting one of the "quiet" ones that are said to be 60-70dB with a larger tank too.

Picks of the setup on the one ARC use

Title: Re: Going over to the dark (CNC) side!
Post by: Muzzer on January 19, 2021, 06:05:29 PM
The compressor on my machine is a Bambi - enough to operate the drawbar and gearbox but barely enough for constant discharge. I can use it to periodically blast chips clear but I need something better that doesn't require manual operation. I managed to break another tool last week due to it recutting (welding) aluminium chips, which is what has broken pretty much all the 3-4 tools I have lost over the last year or so.

I have an HVLP compressor from Screwfix that seems like an alternative approach . Rather than being a reciprocating (piston or diaphragm) compressor, it is a fairly compact centrifugal blower. Perhaps not surprisingly it sounds like a vacuum cleaner. It blows a strong jet of air and may be easier to quieten than a giant compressor, with the possibility of hiding it inside the body of the machine - once you strip away the giant plastic housing, the guts are actually fairly compact. (https://tinyurl.com/y4tex4ju[/url)
Title: Re: Going over to the dark (CNC) side!
Post by: Muzzer on January 19, 2021, 06:08:14 PM
The compressor on my machine is a Bambi - enough to operate the drawbar and gearbox but barely enough for constant discharge. I can use it to periodically blast chips clear but I need something better that doesn't require manual operation. I managed to break another tool last week due to it recutting (welding) aluminium chips, which is what has broken pretty much all the 3-4 tools I have lost over the last year or so.

I have an HVLP compressor from Screwfix that seems like an alternative approach https://tinyurl.com/y4tex4ju (https://tinyurl.com/y4tex4ju). Rather than being a reciprocating (piston or diaphragm) compressor, it is a fairly compact centrifugal blower. Perhaps not surprisingly it sounds like a vacuum cleaner. It blows a strong jet of air and may be easier to quieten than a giant compressor, with the possibility of hiding it inside the body of the machine - once you strip away the giant plastic housing, the guts are actually fairly compact.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on January 19, 2021, 06:42:32 PM
This is what I'm thinking of at the moment, you can get similar cheaper from unknown brands but at least this has a warranty and can be used for other things too.

https://hyundaipowerequipment.co.uk/air-compressors/hyundai-50-litre-air-compressor-1cfm-100psi-oil-free-low-noise-electric-2hp-hy27550/
Title: Re: Going over to the dark (CNC) side!
Post by: Muzzer on January 20, 2021, 01:09:32 PM
They claim 60dBA which is a LOT better than the normal 90-100. Looks as if it perhaps has series diaphragm pumps rather than pistons. 1.5kW should allow you do use actual air tools too, as you say.

By way of comparison, the Bambi claims 40dBA - when it's running, it sounds like a noisy fridge, which is perhaps not surprising when you look at its construction.
Title: Re: Going over to the dark (CNC) side!
Post by: dieselpilot on January 20, 2021, 05:40:21 PM
I have a California Air Tools 10020C which are available in the states. This one is a single 2HP pump. I think initially, all these pumps were made at the same place. The pumps seem reliable as some have run them well beyond the rated 3000Hr. The downfall for noise is they all include a standard pressure switch with an unsilenced unloader valve. Beyond the pump and switch, the rest of the components are cheap as can be. All connections had to be resealed. While the pumps appear to be on isolators there is a solid rod though the middle. Even on a concrete floor after adding real isolators I can feel the machine. My tank leaked at a weld for the motor bracket. CAT did replace the tank just outside the warranty period, but it seems a common failure. I had a very high duty cycle which meant problems with water, so I added an aftercooler. For unloader noise, I added a solenoid valve with a silencer. Cheap compressors are ,well, cheap. Unfortunately, the next step is a huge investment.

Maybe a Hyundai is better? I'd wait from some reviews if not in a hurry.

HVLP turbine is certainly less than 10 psi, cheap units probably below 5.

Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 25, 2021, 06:29:52 PM
With the Stuart Victoria out of the way it was time to turn the lights off and get back to the dark side and do some more work on the 11cc Wall engine.

I'll do a full write up at some time but this shows some of the work on the cylinder.  Starting with manual work on the lathe to bore undersize and cut the fins which was quite complex as each fin is a different diameter so the tapered sides vary on each.

Then onto the CNC to first rough out and finish the bottom flange and also add the screw holes at the same time. With that done the cylinder was repositioned onto it's side to cut out a shaped pocket to accept the manifold flange (there is a simpler one on the other side too) Then some 30mm round bar was shaped to fit the cut outs, I found they were a little tight so tweaked the CAM by entering the tool diameter as 5.95mm rather than 6.0mm so it took off a fraction more material which allowed the bosses to be tapped in with a small copper hammer.

Finally back to the manual machines to curve the inner faces of the bosses before silver soldering it all together after which it was finish machined. Last job was a quick sandblast to clean it up as my well used pickling acid tends to leave the steel with a copper coating.

https://www.youtube.com/watch?v=bBaRjJ4Tlh0
Title: Re: Going over to the dark (CNC) side!
Post by: Hugh Currin on April 25, 2021, 07:04:08 PM
Mike, et al:

Old thread, but I thought my experience may be of interest.

I followed this thinking and obtained a Grip Rite G100 compressor for the small shop. Specifically to run a mist coolant system. It's speced at 0.6CFM at 90psi. It was small and I thought any compressor would be OK for this job. Well, it didn't come close to running the mister. I can't find solid numbers but I'm now thinking 3-4CFM for a mister. Anyone have better numbers here? I may try a California Air Tools 4620AC (4 gal, 2HP, 5CFM) mainly because it fits my space.

So, a small compressor should work, but not too small.

Thanks all.

Jason,

Do you still have diaphragm air-brush compressor that you could try? You dont need a high pressure or even a high flow to blow away the chips. Using a big shop compressor is overkill. The noise on my shop compressor kicking in unexpectedly, when I am doing fine work, always makes me jump.

Another possibility is a small centrifugal fan similar to the fan a blacksmith uses to stoke the forge hearth fire

Mike
Title: Re: Going over to the dark (CNC) side!
Post by: gerritv on April 25, 2021, 08:29:46 PM
Hugh can you refresh us on which mister you have? A fog buster style will happily run from an airbrush compressor. The suction/venturi effect ones need a lot more.

I can supply plans for a usable fog-buster clone, a few holes and a needle valve in a block.

Gerrit
Title: Re: Going over to the dark (CNC) side!
Post by: kuhncw on April 25, 2021, 09:50:26 PM
Jason,

It's good to see you back on the dark side.  Thanks for posting the video showing the sequence of operations. 

Chuck
Title: Re: Going over to the dark (CNC) side!
Post by: Hugh Currin on April 25, 2021, 11:32:11 PM
Gerrit:

I've tried both. The Fog Buster type was described here (https://www.modelenginemaker.com/index.php/topic,9930.msg225136.html#msg225136) and is very similar to yours. I also have two siphon based misters that I've tried with this compressor. I've used the settings you all suggested, but my experience was I needed more flow that 0.6 cfm.

p.s. I do like your design. Thanks.

Hugh can you refresh us on which mister you have? A fog buster style will happily run from an airbrush compressor. The suction/venturi effect ones need a lot more.

I can supply plans for a usable fog-buster clone, a few holes and a needle valve in a block.

Gerrit
Title: Re: Going over to the dark (CNC) side!
Post by: Hugh Currin on April 25, 2021, 11:35:27 PM
Jason:

It sounds to me like you need a cnc lathe.

I look forward to the full write-up. Thanks.

I'll do a full write up at some time but this shows some of the work on the cylinder.  Starting with manual work on the lathe to bore undersize and cut the fins which was quite complex as each fin is a different diameter so the tapered sides vary on each.
Title: Re: Going over to the dark (CNC) side!
Post by: gerritv on April 26, 2021, 12:01:15 AM
Gerrit:

I've tried both. The Fog Buster type was described here (https://www.modelenginemaker.com/index.php/topic,9930.msg225136.html#msg225136) and is very similar to yours. I also have two siphon based misters that I've tried with this compressor. I've used the settings you all suggested, but my experience was I needed more flow that 0.6 cfm.

p.s. I do like your design. Thanks.

One other thing that I don't recall seeing in the other thread: the tank should be near on-level with the mister. At the pressure used there isn't much oomph left over to push fluid uphill. OTOH  you also then need to watch out for syphoning, ask me how I know that.

As my gantry CNC mill is finally almost ready to use, I am looking at building a END CNC version using a persaltic pump for fluid control. Sebastian included pins for an air and fluid solenoid as a bonus. Trying at present to find out if he will ship to Canada, his site only allows EU.

Gerrit
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 26, 2021, 07:22:42 AM
I quite enjoy Sebastian's videos and that's a nice home made mill he has.

Having tried the air tool lubricator as a means of supplying a small amount of liquid it has not worked that well as that too seems to need a high flow of air to draw up the liquid even though the height is only 25mm. So will have a look at something else for when I'm cutting aluminium, rest can be done dry with just air to clear the chips.
Title: Re: Going over to the dark (CNC) side!
Post by: Muzzer on April 26, 2021, 07:45:45 AM

Finally back to the manual machines to curve the inner faces of the bosses before silver soldering it all together....


Nice result, Jason but I'm a little confused. At around 5:00 you are creating a flat surface for the manifold boss to mate with, yet at 8:00 you are putting a cylindrical face on the boss itself. Is there some sort of filler piece between them when you fit them together? Or is this the boss for the other side?

Your silver soldering is very neat (skillful!) and effective looking. Never tried it myself but it seems to be ideal for this kind of fabrication!
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 26, 2021, 08:52:48 AM
There is an easy answer to that one, not wanting to bore people with an overlong video I just showed part of the pocket being cut and edited out the rest. It carried on doing a couple more passes at 3mm deep each time until the hole went all the way through.

I could have left the end of the boss flat but just put the rough concave cut on to make for a smoother cut when doing the final boring out rather than having an interrupted cut. It also slightly reduces the bulk of metal that needs to be heated when it comes to silver soldering

(https://hosting.photobucket.com/images/v156/jasonballamy/20210411_142324(1).jpg)
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on May 23, 2021, 07:32:26 PM
This mornings effort was the conrod for the 11cc Wall engine I have been working on, some manual work had already been done machining up the two halves bolting together which also entailed reducing the rod width so that counterbored could be drilled for the cap head screws which have to go in from the small end and the two holes had also been drilled and reamed.

When doing the CAM I also picked up on the two diameters and used them to locate some holes to drill the scrap used to hold the part at the correct spacing and subsequently tapped these by hand with a 3mm spiral flute tap. Using some top hat bushes the blank was secured ready for machining.

First an adaptive (Peel) to remove the majority of the waste then a contour to finish the outer shape. Followed this with a radius corner cutter to form the two bosses and then a 3mm ball nose for the recess in the side of the rod. At 6.08 in you can hear the sound of the cut change as a bit of ali welded onto the tool as it took a full width cut so a quick reduction in feed and a dab more paraffin just managed to save the day, the other side cut fine using the slower rate from the start. Full details of cutters/feeds/DOC etc in video description.

https://www.youtube.com/watch?v=IG5Ypx77y68

Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on October 27, 2021, 04:36:45 PM
Following the trail adaptive feed rates for aluminium that I posted about in Achim's thread

https://www.modelenginemaker.com/index.php/topic,10535.msg242572.html#msg242572

I had a pressing little job for another forum member that needed cutting from some 20mm thick EN3 steel so thought I would have a play. The cutter is once again a 6mm 3-flute carbide one this time made by New Century which is YG-!'s Chinese factory and it has had quite a lot of previous use on steel and iron. I have attached their speed and feed chart but as the first set of figure sis for carbon and alloyed steels upto 1000Nm and I was only cutting a low carbon steel I upped the spindle speed to 5000rpm and also increased Ae (sideways feed) to 0.1D or 0.6mm. Ap (height of cut) was 5.5mm which suited the 20mm thick workpiece giving 4 passes with the tool finishing below the bottom of the work piece.

First pass was at 300mm/min, then using the override which goes up in steps of 10% 450mm/min, then 510mm/min which gave a Fz (chip load) of 0.034mm which it seemed more than happy with and I should think 600mm/min x 6.0mm Ap quite possible but that can be tested on some scrap. At then end of each piece there was no noticable increase in the temperature of the work and what heat was in the tool was only slight and likely to have come from the spindle rather than the cutting end so looks like the chips were carrying away all the heat as they should.

The adaptive cuts were set to leave 0.2mm stock which was removed with a finish pass at 200/min, You can see that the first 5-6mm of the tool that had been worn is leaving a dull finish but as the less used upper flutes make contact they are giving a brighter finish. This is only visual as I can't feel any difference

https://www.youtube.com/watch?v=HkNxBHIelUI

Can you tell what it is yet?

Title: Re: Going over to the dark (CNC) side!
Post by: Admiral_dk on October 27, 2021, 07:26:05 PM
Looks and sounds like your Tools where more than happy to work under these conditions  :ThumbsUp:

Nice result  :cheers:     ..... and No, I haven't got a clue so far   :headscratch:
Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on October 27, 2021, 08:22:14 PM
Well done Jason,

Another interesting experimental result. Last week we all thought we were doing well machining aluminium with low Ae (sideways feed) and highish Ap (height of cut) values. Now you have shown the low carbon steel can be machined at much the same feed and speed rates using carbide tooling. The only difference being your spindle's 5000 RPM max limit was well below optimum speed for the aluminium but absolutely spot on correct for the steel.

I have been looking around and have found a usefull (free to download) feed and speed calculator called FS Wizard. (Google it). FS Wizard offers a wide range of materials, cutter types, shapes and sizes. including HSS, Carbide, Cobolt and PCD (diamond).

Based on the adaptive, deep hole pocketing I did on my cam gear covers last week; I ran some comparisons in FS Wizard to see the effect of increasing the Ae (sideways feed) 0.1D, 0.2D, 0.3D while maintaining Ap (height of cut) constant at 9.7 mm Ap =1.4D. My spindle is limited to 5300 RPM max. It was surprising to find the Fz (chip load) and feed rates remained unchanged as did the spindle dispite the wider cuts.

From left to right Ae 0.1D, Ae 0.2D and Ae 0.3D         Ap was 1.4D throughout

(https://lister-engine.com/coppermine/albums/userpics/10013/FS_WIZsmall.JPG)


FC Wizard also calculates MMR (metal removal rates), spindle power (suprisingly low) and cutting force on the tool and many other parameters. The MMR, power, and cutting force all increase as the Ae (sideways feed) is increased.  No surprises there. The cutting force is an interesting parameter. Because, depending on the tool diameter and stick out length the tool will eventuall break if too much (bending) force is applied. This is a limiting factor in high machining rates. FC Wizard offers additional features, with a yearly subscription, one of these additions, calculates just how close to tool breakage you are working.

We may need to consider cutting force more, because of the long thin cutters often used by model engineers. There is a good case to use larger diameter cutters.

Mike

PS. I know what you are making....... An iron smiley  :) :)


Title: Re: Going over to the dark (CNC) side!
Post by: fumopuc on October 28, 2021, 07:34:53 AM
Seems to be a tool for pressing a special shape.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on October 28, 2021, 08:25:01 AM
Yes it seemed quite happy at those sort of rates so will try something a little faster next time, as I'm on the free version of F360 which uses the feed speed as the rapid any increase in feed is worth while. You may also have spotted that I have the stay down set longer than default and at 70% which combined with being able to set the non engaged feed rate helps that is why you can see the feeds on the screen change eg 510 cutting and 800 return.

Thanks for the screen shots Mike I'll download it and have a play. I'm not sure on out machines what will give up first as the load goes up, the cutter, get excess chatter or something else breaks.

Yes it's a press tool and Mike is close, just the wrong part of the face ;)  I'll leave it to Graham if he wants to say what it is at the moment.
Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on October 28, 2021, 12:13:36 PM

Yes it's a press tool and Mike is close, just the wrong part of the face ;)  I'll leave it to Graham if he wants to say what it is at the moment.

OK, Iwill try again. It's a press tool for making mustache curling tongs.  :help:

FS Wizard is a very comprehensive feed/ speeds calculater. To appreciate what it can do, You need to play around with the inputs and observe the calculated result. What it does not do is to tell you when you are asking too much or if something will break. You may need to buy the Pro version for that.  Alternatively: start with a low feedrate (25% ??) and creep up from there.

Mike
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on October 28, 2021, 12:53:48 PM
You are getting closer.

I did not see mention of coolant or air on those screen shots which may also make a difference.
Title: Re: Going over to the dark (CNC) side!
Post by: Alyn Foundry on October 28, 2021, 02:40:32 PM
Eye cannot put a face on the current project Jason. My lips are sealed. Obviously you nose what it’s for, I presume I’ll be ear ring from you soon?  :)
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on October 28, 2021, 03:03:22 PM
It's all crystal clear to me  :-X

Should be in the post tomorrow.
Title: Re: Going over to the dark (CNC) side!
Post by: crueby on October 28, 2021, 03:51:41 PM
Eye cannot put a face on the current project Jason. My lips are sealed. Obviously you nose what it’s for, I presume I’ll be ear ring from you soon?  :)
Hmmm.... You are building a mechanical Capt. Jack Sparrow! 
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on October 29, 2021, 10:18:09 AM
Width of cut is not a factor in chip load, so no surprise that the three calculations are the same.

Endmills for aluminum typically have at most 3 flutes to provide chip clearance, hence are weaker than endmills with the same diameter and more flutes.  For steel my default tool is 1/2" 4 flute.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on October 29, 2021, 10:46:14 AM
I would have though the effect of chip thinning would mean the actual true chip load increases as the width of cut goes up. For example the thickness of chip as the cutting edge exits at 0.1D will be a lot less than at say 0.3D. And it is not until you get to 0.5D that the thickness of the chip cut is the actual feed per tooth.
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on October 29, 2021, 03:01:47 PM
Chip load is rather theoretical as it's just a function of RPM, feed rate, and flute count.

What you want to optimize is material removal rate while respecting SFM.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on November 27, 2021, 07:12:43 PM
A bit more peeling steel this week.

Started with a 2" dia piece of EN1A (230M07) steel and did most of the work on the CNC. The initial adaptive and contour around the main shape was done with an over length 8mm dia 3 flute cutter as that was the smallest I could find with 30mm long flutes as the sides are 27mm tall. With the whole part being 32mm I also had to feed a bit slower due to 35mm of tool stickout from the collet to stop any chatter.

Then change to a 4mm 3-flute to do a second adaptive around the spigots as the gap was too small for anything larger and then the same tool to contour the spigots.

A couple of ctr drill holes to clock in when boring on the lathe and while I was at it 2.1mm tapping holes for the M2.5 fixings that will hold it to te entablature (part is being machined upside down)

https://www.youtube.com/watch?v=hiJNyflwKdA

Then I did the Entablature from some 5mm thick EN3. Adaptive with a 6mm 3-flute then contours with a 4mm 3-flute to get into the corners.

https://www.youtube.com/watch?v=GH23zia1M58

Before removing the part from the machine I tried the cylinder, it felt like it would be a press fit which was a bit tighter than I wanted so I tweaked the contour to think it was using a 3.98mm dia cutter and ran it again, this effectively took 0.01mm off the face of the two holes and that was just enough to make it a push fit that assembles by hand yet won't drop off.

I also did the cam while I was at it but did not bother to film that.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on December 21, 2021, 03:58:56 PM
I finally had reason to use the engraving cutters I bought almost 18months back see this post

https://www.modelenginemaker.com/index.php/topic,8882.msg224230.html#msg224230

A good friend who is into building model ships finally finished one and as well as asking me to make the display cabinet also mentioned a plaque to go with it and I said I would see what I could do.

Size was to be no more than 80mm which dictated the font size which ended up being 2.5mm high for the lower two lines and 4mm for the top one. I used the pointed single flute 60degree cutter and as the width of the lines meant it was not going in much deeper than 0.12mm the actual largest diameter was in the region of 0.1mm which meant a fairly slow feed of 50mm/min with it spinning at my max of 5000rpm to try and not damage the cutter.

As the DOC was so shallow I took a 0.2mm skim off the top of the plate first with a 63mm face mill fitted with inserts intended for non ferrous to ensure the cuts were all the same depth from the top of the work.

I'm quite pleased with how it came out, run time was a bit slow as using the free F360 combined with a slow feed rate meant the rapids were rather sluggish too but I was able to leave the machine to it and get on with other things while it did it's stuff.

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/902237.jpg)

I also did a bed plate for the next engine from a block of cast iron at the weekend, adaptive with a 6mm di a cutter 6mm x 0.6mm cuts and finish 3D contour with a 4mm dia cutter with 1mm corner radius, 0.2mm stepdown as all the verticals have 3deg "draft" angle. Finish is good enough  to go straight to paint.

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/902178.jpg)
Title: Re: Going over to the dark (CNC) side!
Post by: Alyn Foundry on January 02, 2022, 03:21:51 PM
With the excesses of Christmas and the new year over and done, I ventured out to the workshop.
Armed with the little package that Jason had very kindly sent me a month or so ago. I’m guessing it took me way less time to make my parts than it did to make the tools.

Some Silver soldering, pickling, and polishing later and behold…. A “ highly “ styalised “ Eye of Ra “

Made from 2 mm 316 Stainless Steel, which still needs to be polished further it forms an integral part for my latest “ top secret “ project.

Thanks again Jason.  :ThumbsUp:
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on January 02, 2022, 03:52:43 PM
That looks to have turned out well, now get a move on with the rest so I don't have to worry about letting the secret out :-X :-X :-X

Middle photo has certainly replicated Ra's eye well
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 24, 2022, 07:39:20 AM
Bit more into the dark brown side yesterday

To avoid the F360 simulation screen turning red with so many collision markers I had to set quite a bit of stick out for the 4mm ball ended cutter, 115mm to be exact :o

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/907079.jpg)

But I managed to get the machining done without breaking any tools. Quite a marathon session starting at 8.30 in the morning and finishing about 6.00pm. Luckily I could just leave the machine to it and get on with other things, just popping back into the workshop when another tool path needed to be started or tool changed from roughing to finishing.

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/907078.jpg)

Core box is next on the list so the casting comes out hollow and with some windows in it.

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/906812.jpg)

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/906809.jpg)
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 28, 2022, 08:24:11 PM
Both halves of the core box are now done along with the bearing caps, hopefully on their way to the foundry tomorrow

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/907206.jpg)
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 30, 2022, 07:31:02 AM
nice to see the results of your labours, I posted about this pattern back in post number 253 (https://www.modelenginemaker.com/index.php/topic,8882.msg224793.html#msg224793) and have just seen the casting, hopefully will get a more detailed image once it has been offloaded from the lorry

Title: Re: Going over to the dark (CNC) side!
Post by: Alyn Foundry on April 30, 2022, 02:28:26 PM
nice to see the results of your labours, I posted about this pattern back in post number 253 (https://www.modelenginemaker.com/index.php/topic,8882.msg224793.html#msg224793) and have just seen the casting, hopefully will get a more detailed image once it has been offloaded from the lorry

More yours on the final stretch Jason, many, many thanks.

Yes having patterns made to such a high standard makes a huge difference to the castings. This was something that Roger “ the pattern “ used to say about them being of 110% to get 100% finished.

Attached are a couple of pictures of the castings.

Having had many complaints about over fettling of castings I make sure that mine are just blasted, as you can see.

Cheers Graham.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on April 30, 2022, 03:19:10 PM
Good to see a few more images Graham. The second attempt at the main casting looks to have come out very well. What about a group shot of the rough assembly with the beam as well :stickpoke:
Title: Re: Going over to the dark (CNC) side!
Post by: Alyn Foundry on April 30, 2022, 03:34:49 PM
Good to see a few more images Graham. The second attempt at the main casting looks to have come out very well. What about a group shot of the rough assembly with the beam as well :stickpoke:

LOL….

Once the beam yoke and bearings come out from the four jaw then yes….
Title: Re: Going over to the dark (CNC) side!
Post by: Johnmcc69 on April 30, 2022, 11:23:29 PM
 :ThumbsUp:
 Great work gentlemen! The patterns & parts look very good.
 What's the material & shrink factor(s)? What do you find works as draft angles?
 I'm only familiar with die cast design of aluminum & zinc, so I find this very interesting.
  :popcorn:

 John
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on May 01, 2022, 06:59:05 AM
They are all iron castings.

Mostly 3degrees of draft on the patterns I made with 1% shrinkage allowance
Title: Re: Going over to the dark (CNC) side!
Post by: Alyn Foundry on May 02, 2022, 06:40:03 PM
Although I’ve been an amateur pattern maker for the best part of my adult life, these machine made patterns surpass anything I’ve used to date. The accuracy of fit is truly amazing.

Closeup of the Brayton beam yoke after line boring the main bearing caps. The whole engine as a partial mock-up with the cylinder that was finished about 15 years ago.

I can’t wait to see the results of Jason’s latest endeavours coming back from the foundry. 😉
Title: Re: Going over to the dark (CNC) side!
Post by: Alyn Foundry on May 14, 2022, 02:08:21 PM
Taken from The Shining….

Here’s Otto….  ;)
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on May 14, 2022, 03:54:09 PM
Not too shabby, what's the writing like?

3mm off top and bottom and 2mm of the bearing split line.
Title: Re: Going over to the dark (CNC) side!
Post by: Alyn Foundry on May 14, 2022, 04:02:52 PM
Not too shabby, what's the writing like?

3mm off top and bottom and 2mm of the bearing split line.

Plain enough to read and discreet enough for use ! 😉

Off to the Le Blonde.

 :cheers:  Graham.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on May 19, 2022, 02:40:21 PM
My castings turned up today and I'm quite pleased with how they came out particularly as it was my first pattern with a core. External surface finish could have been a little smoother but I think that is one of the problems with airset as they don't seem to sieve any fine sand on first and just ram it up in one thick layer which can leave the sand surface a bit porous so the iron replicates that. These are the bits from my patterns

(https://hosting.photobucket.com/images/v156/jasonballamy/20220519_130038(1).jpg)

The bit of writing that  was a last minute addition turned out quite well, easily read yet out of sight for most that will view the model.

(https://hosting.photobucket.com/images/v156/jasonballamy/(edited)_20220519_130249(1).jpg)

(https://hosting.photobucket.com/images/v156/jasonballamy/20220519_130349(1).jpg)

And here is the rest of the "set" including the scotch yoke which is a brass casting and the spun brass piston which will give it a thin wall and light weight which should help with running. There is also a flywheel casting which I forgot to include in the photo.

(https://hosting.photobucket.com/images/v156/jasonballamy/20220519_130202(1).jpg)

I just need to catch up with Graham now who is posting good progress over on his Facebook Page (https://www.facebook.com/groups/ALYNFOUNDRYMODELS/)
Title: Re: Going over to the dark (CNC) side!
Post by: Alyn Foundry on May 19, 2022, 03:52:29 PM
Pleased to read that your castings arrived safely Jason.   :ThumbsUp:

For those that might be interested here’s the inspiration behind what will become known as “ Little Otto “

N A Otto, famous for the four stroke cycle was dabbling with atmospheric designs prior to his momentous discovery. The original engine that lived in the Deutz museum went “ missing “ many moons ago. A member of our group decided to make a full scale replica of which I immediately fell in love with.

 :cheers: Graham.
Title: Re: Going over to the dark (CNC) side!
Post by: Admiral_dk on May 19, 2022, 04:49:46 PM
Thanks for the history Graham  :ThumbsUp:

I can see why you both are very pleased with the result  :cheers:

Per
Title: Re: Going over to the dark (CNC) side!
Post by: Dave Otto on May 19, 2022, 07:42:11 PM
Nice work guys! :ThumbsUp:

Dave
Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on May 19, 2022, 08:56:41 PM
Congratulations are due to both Jason B and Graham C,  :ThumbsUp: :ThumbsUp: :ThumbsUp:

Some very nice patterns and fine iron casting. That's a nice touch to include the names of those involved, hidden away inside the casting

Mike
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on May 20, 2022, 07:02:26 AM
Thanks for all the comments. I'll probably start a new thread for any more work on this one as the swarf starts to be produced. Though as I type this I have just thought of something on the engine that the CNC would be the ideal tool for :)
Title: Re: Going over to the dark (CNC) side!
Post by: Zephyrin on May 20, 2022, 09:24:40 AM
this is a great project !
looking at the variable crank, I seems to me that the piston move faster on the downward stroke to minimize heat transfer before its expansion, a very clever design by Otto...in 1873 !
this is certainly a model to do, simply out of respect for the thoughts that gave rise to this engine !



 
Title: Re: Going over to the dark (CNC) side!
Post by: Roger B on May 20, 2022, 07:33:36 PM
Another interesting project to follow along  :)  :)  :ThumbsUp:  :ThumbsUp: 
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on July 24, 2022, 06:58:47 PM
A bit more pattern making completed today. The aim was to try and produce a flywheel pattern that had a similar look to the curved spoke flywheels used on National Gas Engines

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/911728.jpg)

Quite pleased with how it turned out

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/911727.jpg)

More details in the video

https://www.youtube.com/watch?v=AloAsKTpV4I

I was the first time I used the peristatic pump fed fog buster in anger and very pleaed with how it performed giving just enough liquid to wet the tool and stop tip build up and meant I could leave the machine running unattended. I used about 40mls over the six hours of machining which did not leave me with a dripping pile of swarf.
Title: Re: Going over to the dark (CNC) side!
Post by: Admiral_dk on July 24, 2022, 11:16:37 PM
Great result Jason - and I can only agree, that you got the Fog-Buster dialed in perfectly  :ThumbsUp:
But still surpriced how tiny an amount you used for that session  :o

Per
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on July 25, 2022, 07:02:22 AM
I did turn it down quite a lot from what can be seen in the video for the finish cuts as they remove such a small amount of metal and that was about half the cutting time.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on March 20, 2023, 04:15:45 PM
Well it's been a while but a couple of castings from the patterns above arrived today. Look to be quite good with little flash and the two halves seem to line up well. hopefully they will have soft centres.

I did have to get them out of the unexpectedly heavy parcel quickly to avoid the risk of cross contamination from the other well maturted castings with that special coating that made up the other 80% of the contents :naughty:

Title: Re: Going over to the dark (CNC) side!
Post by: Alyn Foundry on March 20, 2023, 05:52:57 PM
Great to read that they arrived safely Jason.   :ThumbsUp:

Have no fear, the foundry have altered their Iron recipe slightly with the addition of a little extra Copper. I found the flywheel quite easy to machine and managed the whole operation in under 20 minutes.

The casting was so symmetrical I was able use the boss initially to clean out an inner rim. Once clean I then expanded the 3 jaws into it and then do the usual, all faces and boss in one operation.

 :cheers:  Graham.
Title: Re: Going over to the dark (CNC) side!
Post by: Twizseven on March 20, 2023, 08:06:37 PM
That looks really nice Graham.  Between you both you have done a very good job.
Colin
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on May 11, 2023, 01:06:59 PM
I've been wanting to try thread milling for a while and the need finally came up so time for a new adventure.

The part in question is a gland nut that fits onto the end of a steam engine cylinder to seal the piston rather than it having piston rings. The lower lip just needs to clear the 19mm dia piston and the thread I chose was M22 x 0.5mm and needs to go as close as possible to the lip.

(https://www.model-engineer.co.uk/sites/7/images/member_albums/44290/924272.jpg)
 

I made use of a bar end of 1" brass and milled the top flat enough using the jog function as a glorified power feed control and then use the CAM in F360 to produce the code to firstly rough out the two bores leaving 0.3mm of material which was then taken to finished size in to passes of 0.2 and then 0.3mm.

A change of tool to a single tooth,5 flute thread mill took care of the thread, I ha dread of possible tool deflection so took light 0.1mm steps and a spring pass.

Quite happy with how it came out so will be using it again particularly as one cutter can do several pitches and almost unlimited diameters both internal and external

https://www.youtube.com/watch?v=5Y58fe95IFw

Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on May 11, 2023, 01:53:47 PM
Hello Jason,

Nice work.  :ThumbsUp: Thread milling will produce near perfect internal and matching external threads over a wide range of diameters and materials.

I usually go for full thread depth in one pass followed by a spring pass. I have had good success using a single tooth thread mill made by grinding all but one teeth from a standard tap. That worked well over a range of thread pitches and diameters, but eventually the single tooth cutter becomes dull requiring a new cutter to be made.

(https://listerengine.com/coppermine/albums/userpics/10013/P1060569.JPG)



I know commercial thread milling cutters are available, the ones I have found are very expensive and way above my pay grade. I would be interested to know just where you sourced your 5 flute cutter and how much your 5 flute thread mill cost.

Cheers

Mike
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on May 11, 2023, 02:26:50 PM
Thanks Mike, I do wonder if some of what I read regarding tool flex applies more to the multi tooth cutters that will do the whole vertical depth of the thread in one helical revolution and obviously harder materials than brass.

I seem to get most of my carbide ( and inserts for that matter) cutters from APT, still a bit pricy and not something you would want to snap on the first attempt so may be a bit bolder next time. But compared with what it would cost for a few taps and dies if you had to do it by traditional means and it saves having to play about with change wheels when you get to the larger diameters so it's not a bad investment.

This is the one I got which does 0.5 to 1.0mm pitch

https://www.shop-apt.co.uk/single-tooth-thread-mills-for-general-use-internal-60-partial-profile/internal-partial-profile-60-thread-mill-05-10mm-pitch.html
Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on May 11, 2023, 03:20:35 PM
Hello Jason,

I have seen those APT thread mills before; not exactly inexpensive. The 0.5 to 1.0mm pitch [24 to 56 TPI] milling cutter you chose seems like it will cover most of our model engineering needs and offers the best value for money. It is probably the only one we would need. I can understand your cautious approach to the first attempt, however you should be safe for a full thread depth single pass. as it's only a shallow thread.

I have thread milled in aluminium alloy, brass and mild steel using mist coolant. Tool flex did not seem a problem but I cut at a slower feed rate than your video: nice and gentle. Could be a different story with some of the harder steels

I suffered from some cold welding last time I thread milled aluminium. Probably due to my single point tap cutter becoming dull (it's done a lot of work!!). I applied some Trafelux tapping paste inside the hole and that seemed to help.

When I milled the four threads in the cylinder heads, the first turn of each of the four threads started in exactly the same angular position; beautifully regimented.

Cheers

Mike

Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on May 11, 2023, 03:38:19 PM
Hello Jason,

Thread milling gives the finest finish from climb milling. This means internal threads should be cut from the bottom, upwards and external threads from the top, downwards. Your Fusion 360 probably does that by default.

Cheers

Mike
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on May 11, 2023, 04:31:13 PM
Yes Fusion tends to default to climb milling and I stick with that for just about everything as the machine and tool sounds happier with that.

Out chip loads are probably similar as with 5-flutes my feed of 500mm would be similar to a 100mm feed with your single point cutter

Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on May 11, 2023, 04:56:08 PM
Hello Jason,

Feed rate needs to be looked at carefully and adjusted if necessary. Your 500mm rate for a M6 thread will appear so much faster than for a M30 tread. I always slow down for the smaller diameter threads.

Mike
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on May 11, 2023, 07:14:25 PM
Yes on the M22 the rate at the cutting edge is about 40% more than at the ctr of the tool which is where the rate is picked up from.

I'd usually be running a 3 flute cutter at 5-600mm/min so chip load is still lower with the 5 flute thread mill, 0.02mm in this case if it were going in a straight line. Actual chip load at the 22mm dia is 0.028mm but there is a considerable amount of chip thinning with such a low engagement  It would be happier running faster but I don't like to push it too fast and am limited by my 5000rpm spindle.

In fact that 6mm cutter doing the initial adaptive is actually cutting at something like 1500mm/min around the 11.7mm dia as it starts to open out after the initial helical entry cut :)
Title: Re: Going over to the dark (CNC) side!
Post by: Admiral_dk on May 11, 2023, 09:29:22 PM
I've seen single point thread cut before - but this is first time I see it done 'from Fusion360 free version'  :)

I will agree with your usual statement about us amateurs not needing the optimized code/speed and likewise Mikes comment about deeper cuts – but like you, my first will be tried with caution  :old:

Thank you for sharing Jason   :cheers:

Per
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on May 12, 2023, 06:40:58 PM
The female thread was only half the part and I really needed the male to make sure it all went together so I threaded a short length of bar with a test thread on the lathe and it screwed on very nicely. I made use of that test thread to hold the part while the remaining turning was done. Using one wheel only of teh diamond knurl gives a reasonable looking "rope" knurl

(https://hosting.photobucket.com/images/v156/jasonballamy/20230512_141812_wHgfP9AwFz6viSjsxPSu62.jpg)

Happy with that I cut the thread proper on the piece of thick wall tube that will become the engine's cylinder. I'm running in reverse and cutting from the run out in groove towards the right which allows cutting at a decent speed.

(https://hosting.photobucket.com/images/v156/jasonballamy/20230512_144845_433qb1iq66erU1TbLBQomE.jpg)

And how it goes together with the cylinder support plate, I'll bore it out tomorrow and the thread will be nice and concentric to the bore.

(https://hosting.photobucket.com/images/v156/jasonballamy/20230512_143941_xdL1DgDn63gQxrWhY8rCte.jpg)


Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on May 12, 2023, 07:00:10 PM
Nice work Jason  :ThumbsUp:

Mike
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on July 05, 2023, 02:43:31 PM
Those that have seen the last instalment of my Nattie thread https://www.modelenginemaker.com/index.php/topic,11475.msg269215.html#msg269215 will have seen that I CNC cut the nameplate and was asked for some details on that which is what this post is about.

One of the main issues with cutting raised letters is being able to get the tool to fit around and within the individual letters, particularly ones like "S" and "G" and "A" which depending on the font and height can have very little space so you end up needing a very small diameter cutter. There are a couple of downsides to this the main one is the cutter becomes very delicate and secondly you can only run very small chip loads so run times become quite long particularly if you don't have a high speed (20K rpm approx) spindle. So some time at teh design and CAM stages is needed to tweak things as best you can.

For the Nattie nameplate I had to go to a 42mm x 32mm size oval which was a bit larger than I really wanted but anything smaller I was not getting room for the cutter. Alibre does not currently have the ability to place text along a curve but it is coming in the next update so each letter was angled and positioned individually, the inner ones being 3.5mm high and the outer 4mm. Once I had a layout that worked it was exported to F360, actually I had to do it a few times as the CAM showed up what would not work so back to Alibre to alter the layout and export again.

(https://hosting.photobucket.com/images/v156/jasonballamy/nat5.JPG)

One way to avoid having a very delicate 0.5mm (20thou) diameter cutter is to use a V shaped engraving cutter, this also had the advantage of giving some draft angle to what probably would have been a cast nameplate on a full size engine. The disadvantage is that you can't cut that deep as the diameter increases the deeper you go and as they are only single flute feed rate is low. I went with a 60deg Vee with a flat 0.3mm end

In F360 I found that using an adaptive type tool path with zero stock to leave worked best cutting the full 0.25mm (10thou) depth in one go with a 0.1mm stepover. In hindsight the stepover could have been 0.2mm but I did not wish to risk the cutter and was also working with softer bending brass rather than the usual harder types. I split the job up into areas so I did not have to do all in one go. The carbide cutter was run at my maximum of 5000rpm and fed at 150mm/min. Total machining time for each plate was 2hrs 43mins according to F360 but closer to 3hrs actual.

First the "Alyn Foundry"

(https://hosting.photobucket.com/images/v156/jasonballamy/nat1.JPG)

Then the "Nattie Gas Engine"

(https://hosting.photobucket.com/images/v156/jasonballamy/nat_2.JPG)

The As had to be done a bit shallower as the recess was very small

(https://hosting.photobucket.com/images/v156/jasonballamy/nat3.JPG)

The last bit was the "stamped" engine number which was done using an engraving tool path and that actually used th efull width of teh cutter though I did slow the feed a bit just in case

(https://hosting.photobucket.com/images/v156/jasonballamy/nat4.JPG)

A scrap of aluminium was skimmed flat and the workpiece fixed to that using the two layers of tape and superglue method, after drying with a weight on top for an hour cutting started. Once the engraving was done I also used the CNC to drill the two holes which were then used for added security while the oval shape was cut out with a 2mm 3-flute cutter using a basic contour path. Looks like I got my depths about right as I cut the top layer of tape but not the bottom

(https://hosting.photobucket.com/images/v156/jasonballamy/20230407_145651.jpg)

https://www.youtube.com/watch?v=CU6RDN2-Lzs

After cutting I bead blasted the plates to give a more uniform look. Mine then got a quick spray og etch primer followed by a heavy one of satin black. Once dry the face was rubbed on some 1000g wet & dry to clean up the raised letters

(https://hosting.photobucket.com/images/v156/jasonballamy/20230411_143207.jpg)

(https://hosting.photobucket.com/images/v156/jasonballamy/20230411_143207.jpg)

Title: Re: Going over to the dark (CNC) side!
Post by: Dave Otto on July 05, 2023, 05:30:48 PM
The plates turned out very nice Jason, Kind of reminds me when I did the little Powram Base for my Morrison & Marvin Model Builders vise.

Dave
Title: Re: Going over to the dark (CNC) side!
Post by: RonGinger on July 05, 2023, 10:01:50 PM
Very nice, thank you for the detail. I guess my problem is II now cannot even see cutters that small, and I cannot imagine running a job for 3 hours.

Very nice work.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on July 06, 2023, 07:14:54 AM
Dave did you post about that at the time ? Looks like you had the added complication of needing a lot of tool stick out to avoid the raised central section

Ron, as someone who has just started to need glasses for reading and close up I know how they have improved things.

As for the time it is not as though you really need to be there, I find if something is going to go wrong it is usually in the first 60seconds due to a setup error. Also one of the reasons I broke it down into sections so if I needed to take a break there were places where I could. In fact after the first one having it in sections probably cost me time as I did not always get back to the machine to start the next section straight away. But as I was doing something else anyway it was not really wasted time.
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on July 06, 2023, 01:22:06 PM
Feeds and speeds for thread mills should be adjusted depending on outside vs. inside.  If you calculate the linear feedrate based on material and SFM, then:

Adj Internal Feed = [(Major Thread Dia - Cutter Dia) / Major Thread Dia] x Linear Feed

Adj External Feed = [(Major Thread Dia + Cutter Dia) / Major Thread Dia] x Linear Feed

Above courtesy of Harvey Tool

I found that the cutter diameter of thread mills was often off by several thou, so I would make several passes increasing the depth of cut until the thread would work given the mating thread.
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on October 13, 2023, 08:33:36 PM
Without giving away to much that will allow you to guess what the next engine is  ;) I've been playing about with some letters. This name plate measures 50mm x 32mm and the letters stand 0.4mm above the surface with the font being 3.5mm high. All except the contour around the outside was cut with a 60 degree engraving cutter with 0.3mm wide end using a 0.2mm stepover and it took a little under 4 hours to run. The tool marks that can be seen but not felt in the first image soon become invisible once lightly sandblasted, some black stove paint will take care of the rest. More details when I get round to doing the build thread for the engine.

(https://hosting.photobucket.com/images/v156/jasonballamy/20231003_150606.jpg)

The square base of the fabrication with it's integral feet, rounded edges and draft angle was also a CNC job

(https://hosting.photobucket.com/images/v156/jasonballamy/20231008_144337.jpg)
Title: Re: Going over to the dark (CNC) side!
Post by: Dave Otto on October 13, 2023, 11:00:15 PM
Nicely done!

Dave
Title: Re: Going over to the dark (CNC) side!
Post by: Art K on October 14, 2023, 02:57:33 AM
Jason I have to agree with you here.
Quote
As for the time it is not as though you really need to be there, I find if something is going to go wrong it is usually in the first 60seconds due to a setup error.
One of the reasons I ditched Mach 3 on my Tormach is that it had a nasty tendency to loose the Z axis zero point at the most inopportune times. I have a scrap head for my Val engine to prove it.
Art
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on October 14, 2023, 06:51:39 AM
I have had that happen a couple of times Art, luckily in both cases the tool has ended up too high and just not cut for the rest of the job.

What do you run now?
Title: Re: Going over to the dark (CNC) side!
Post by: Vixen on October 14, 2023, 08:23:03 PM
I have had that happen a couple of times Art, luckily in both cases the tool has ended up too high and just not cut for the rest of the job.

What do you run now?

Personally, I would recommend LinuxCNC. I have been running it now for about fifteen years and I don't believe it has missed a beat (or lost it's place) in all that time.

Mike
Title: Re: Going over to the dark (CNC) side!
Post by: kvom on October 15, 2023, 01:08:04 PM
PathPilot is the obvious solution for Tormach.  I used it on my non-Tormach mill and it was a big improvement over Mach3.
Title: Re: Going over to the dark (CNC) side!
Post by: Alex on October 17, 2023, 12:39:06 AM
Of course, PathPilot and LinuxCNC are tied at the hip. Tormach helped fund some work on LinuxCNC (trajectory planner?? it's been a while) and of course they have their own GUI and call it PathPilot.  If you go back through the EMC mailing lists on Archive.org, you'll see a guy called Art Fennerty asking if he could use the code and port it to Windows.

Of interest with LinuxCNC is that one can import a jpg, and have it "raster scan" a photo, I've used that to replicate cast letters, worked well, and a lot less work than with Jason's (great, BTW) recent work above. Maybe not quite as smooth as with Jason's example?? Something to try, if you are running LinuxCNC.

Another vote for LinuxCNC here! JohnS.
Title: Re: Going over to the dark (CNC) side!
Post by: Hugh Currin on October 20, 2023, 03:20:07 AM
I'm still off making pool cues, but I've been wanting to post my new machine tools. I wanted to engrave on a pool cue, a cylinder. This led to a simple fourth axis and a high speed spindle.

(https://lister-engine.com/coppermine/albums/userpics/10011/fourth-axis-3.jpg)

The 4th axis is a Sherline spindle connected to a stepper motor thru a 3:1 timing belt drive. I figured with the Gecko micro stepping it would be OK. The spindle is mounted to the milling table on the aluminum "posts" shown. It's lined up with a Sherline bed for tailstock support. The high speed spindle is a lower powered water cooled job from China. Both have worked well so far.

But, wait for CNC content, this led to needing engraving software and 4th axis conversion along with converting pixel (*.jpg) drawings to CNC G-code. I work in Linux and found these readily available.

I found that Inkscape can export *.dxf files. It looks like a powerful piece of software but I've only used it for this conversion. Once it's in *.dxf form it can be imported to CadCam (or Fusion). But for engraving I found another program called F-Engrave from Scorch Works. I believe it will run a tool around the lines of a *.dxf but haven't done this. What I've used is the V-carve function. This uses a conic tool, I've used a 60 deg pointed tool. The program raises and lowers the tool to give different width "lines". It will also calculate the tool path for an end mill to clear the internal islands. Nice program and works well. Finally, I found "G-Code-Ripper", also from Scorch Works, which will wrap G-code around a cylinder. I mapped the Y axis to the A axis. Easy peasy.

(https://lister-engine.com/coppermine/albums/userpics/10011/gecko-3.jpg)

Once the cavity is there I filled in using crushed malachite using super glue. Build the fill up over the surface then cut back using the Sherline lathe and high speed spindle with carbide router bit. In the pic below the diameter needs to come down a little to thin some of the gecko. Here the toes are pretty fat.

(https://lister-engine.com/coppermine/albums/userpics/10011/gecko-7.jpg)

After finishing the butt of the cue looks like this:

(https://lister-engine.com/coppermine/albums/userpics/10011/gecko-8.jpg)[

I used the same process to engrave (V-Carve) initials into the plastic butt cap. This was filled with blackened epoxy and turned down.

(https://lister-engine.com/coppermine/albums/userpics/10011/normal_HC.jpg)

It all came out, to my eye, well. But I thought some of you may be interested in my new tooling and the software used.

Thanks. Glad to answer any questions.





Title: Re: Going over to the dark (CNC) side!
Post by: crueby on October 20, 2023, 03:47:36 AM
Wow, Hugh, that works great!   :ThumbsUp:
Title: Re: Going over to the dark (CNC) side!
Post by: Kim on October 20, 2023, 05:39:11 AM
Very cool, Hugh!  :ThumbsUp:  ;D

Kim
Title: Re: Going over to the dark (CNC) side!
Post by: Admiral_dk on October 20, 2023, 08:28:57 AM
Great result Hugh - love it  :praise2:

Per      :cheers:
Title: Re: Going over to the dark (CNC) side!
Post by: Jasonb on October 20, 2023, 09:20:32 AM
That came out well

Not tried 4th axis yet though the KX3 has all the drivers ready installed.

High speed spindle will be higher up the list as the single flute type engraving tools can't be fed that fast when limited to my 5000rpm spindle.
Title: Re: Going over to the dark (CNC) side!
Post by: Dave Otto on October 20, 2023, 01:46:27 PM
Nice work Hugh!

Dave
Title: Re: Going over to the dark (CNC) side!
Post by: Hugh Currin on October 21, 2023, 01:34:42 AM
Thanks all. I've wanted a high speed spindle and fourth axis for a very long time. Have several designs kicking around in the computer. But this is the first job that really needed both. The fourth axis is under powered and I question it's holding ability. But for this job it worked well.

The spindle is VERY quiet. Its noise is overpowered by the VFD fan. Haven't checked run out nor used it on metal yet, but it should work well with small cutters.

It wouldn't have been possible without Inkscape and the two Scorch Works programs. Recommended.

Thanks again.
SimplePortal 2.3.5 © 2008-2012, SimplePortal