Author Topic: Going over to the dark (CNC) side!  (Read 11025 times)

Offline Muzzer

  • Full Member
  • ****
  • Posts: 22
Re: Going over to the dark (CNC) side!
« Reply #105 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.
« Last Edit: July 05, 2019, 08:18:01 PM by Muzzer »

Offline RonGinger

  • Full Member
  • ****
  • Posts: 247
  • Boothbay Maine USA
    • Pleasant Cove Models
Re: Going over to the dark (CNC) side!
« Reply #106 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.

Offline Muzzer

  • Full Member
  • ****
  • Posts: 22
Re: Going over to the dark (CNC) side!
« Reply #107 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
« Last Edit: July 06, 2019, 01:04:23 PM by Muzzer »

Offline RonGinger

  • Full Member
  • ****
  • Posts: 247
  • Boothbay Maine USA
    • Pleasant Cove Models
Re: Going over to the dark (CNC) side!
« Reply #108 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.

Offline Jasonb

  • Full Member
  • *****
  • Posts: 6769
  • Surrey, UK
Re: Going over to the dark (CNC) side!
« Reply #109 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.



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



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.


Offline vcutajar

  • Full Member
  • ****
  • Posts: 2485
  • Marsascala, MALTA
Re: Going over to the dark (CNC) side!
« Reply #110 on: July 21, 2019, 08:41:48 PM »
Always love to see small CNC machines in action.

Vince

Online Vixen

  • Full Member
  • ****
  • Posts: 1381
  • Hampshire UK
Re: Going over to the dark (CNC) side!
« Reply #111 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
It is the journey that matters, not the destination

Offline Jasonb

  • Full Member
  • *****
  • Posts: 6769
  • Surrey, UK
Re: Going over to the dark (CNC) side!
« Reply #112 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:



Offline Johnmcc69

  • Full Member
  • ****
  • Posts: 530
  • Erie Pa., USA
Re: Going over to the dark (CNC) side!
« Reply #113 on: July 28, 2019, 02:40:01 PM »
 :ThumbsUp:
Very nice Jason!

 John

Offline fumopuc

  • Full Member
  • ****
  • Posts: 2408
  • Munich, Germany, EU
Re: Going over to the dark (CNC) side!
« Reply #114 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.


Kind Regards
Achim

Offline Muzzer

  • Full Member
  • ****
  • Posts: 22
Re: Going over to the dark (CNC) side!
« Reply #115 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.

Offline Jasonb

  • Full Member
  • *****
  • Posts: 6769
  • Surrey, UK
Re: Going over to the dark (CNC) side!
« Reply #116 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

Offline Muzzer

  • Full Member
  • ****
  • Posts: 22
Re: Going over to the dark (CNC) side!
« Reply #117 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 if you are interested / have a few spare minutes.

If you prefer sound and light, John Saunders did a short video on the subject:

Offline Jasonb

  • Full Member
  • *****
  • Posts: 6769
  • Surrey, UK
Re: Going over to the dark (CNC) side!
« Reply #118 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

Offline Muzzer

  • Full Member
  • ****
  • Posts: 22
Re: Going over to the dark (CNC) side!
« Reply #119 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.