Author Topic: Going over to the dark (CNC) side!  (Read 7281 times)

Offline Admiral_dk

  • Full Member
  • ****
  • Posts: 1318
  • Søften - Denmark
Re: Going over to the dark side!
« Reply #15 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:

Offline kvom

  • Full Member
  • ****
  • Posts: 1955
Re: Going over to the dark side!
« Reply #16 on: March 01, 2019, 10:02:33 PM »
I use GWizard for feeds and speeds.  I break very few mills as a result.

Online TobyTetzy

  • Full Member
  • ****
  • Posts: 134
Re: Going over to the dark side!
« Reply #17 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

Offline mikemill

  • Full Member
  • ****
  • Posts: 266
Re: Going over to the dark side!
« Reply #18 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

Offline jadge

  • Full Member
  • ****
  • Posts: 356
  • Cambridge, UK
Re: Going over to the dark side!
« Reply #19 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

Offline RonGinger

  • Full Member
  • ****
  • Posts: 233
  • Boothbay Maine USA
    • Pleasant Cove Models
Re: Going over to the dark side!
« Reply #20 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.

Offline Woodguy

  • Full Member
  • ****
  • Posts: 102
  • Winnipeg, Canada
Re: Going over to the dark side!
« Reply #21 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.

Online Jasonb

  • Full Member
  • *****
  • Posts: 6463
  • Surrey, UK
Re: Going over to the dark side!
« Reply #22 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.






Offline Dave Otto

  • Full Member
  • *****
  • Posts: 3567
  • Boise, Idaho USA
    • Photo Bucket
Re: Going over to the dark side!
« Reply #23 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
« Last Edit: March 02, 2019, 09:24:32 PM by Dave Otto »

Offline kvom

  • Full Member
  • ****
  • Posts: 1955
Re: Going over to the dark side!
« Reply #24 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.

Online Jasonb

  • Full Member
  • *****
  • Posts: 6463
  • Surrey, UK
Re: Going over to the dark (CNC) side!
« Reply #25 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!



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.

Online Jo

  • Administrator
  • Full Member
  • *****
  • Posts: 12405
  • Hampshire, england.
Re: Going over to the dark (CNC) side!
« Reply #26 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
« Last Edit: March 03, 2019, 11:45:54 AM by Jo »
Usus est optimum magister

Offline kvom

  • Full Member
  • ****
  • Posts: 1955
Re: Going over to the dark (CNC) side!
« Reply #27 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.


Online Vixen

  • Full Member
  • ****
  • Posts: 1167
  • Hampshire UK
Re: Going over to the dark (CNC) side!
« Reply #28 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
« Last Edit: March 03, 2019, 12:06:15 PM by Vixen »
It is the journey that matters, not the destination

Offline Muzzer

  • Full Member
  • ****
  • Posts: 11
Re: Going over to the dark (CNC) side!
« Reply #29 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 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 I got one for around £400 but that may be a bit OTT for what you need.

Murray