Milling UHMW - what am I doing wrong?

[Jay C]

I'm trying to mill some small parts from .53" thick UHMW sheet. As you can see in the photos, the finish is awful. Even in the lathe the plastic stretchs rather than cuts.

The bit is a carbide TiN coated 1/8" 2-flute. Feed on the one on the right was 26ipm at 16K RPM and a .07" DOC. I've read where people love this stuff but I am not feeling the love

I am using a vacuum clamp to hold the sheet and the gauge reads 26" Hg. the portion I'm cutting is overhanging the clamp to allow me to cut through.

Thanks,
Jay

[A1CNC]

Hi Jay,
I mill UHMW alot.
Ditch the Endmill. Go with a single flute or 2 flute cutter made for plastic. I use either an Onsrud O-flute on a micro 100 made for plastic. I frequently cut (1 flute 1/2" cutter) .25" deep 60"/min 6000 rpm.
For Uhmw you need a razor sharp cutter.

Eric

[Geof]

Yes for UHMW you need a razor sharp cutter; coated carbide does not have a really sharp edge.

As suggested a cutter intended for plastic may be the best but you can get good results with uncoated micrograin carbide cutters intended for aluminum.

In the lathe use HSS tools and sharpen them with a large top rake, something like 15 degrees or more; with UHMW you have to 'slice' it off rather than chipping it off.

[Jay C]

Thanks guys. Would I see the same issue with acetal using the same bit?

[Geof]

Acetal is very different to machine than UHMW. Whereas UHMW needs a good top rake acetal can be machined with zero top rake; something like brass.

Regular new carbide tools will work quite well on acetal and the micrograin carbide tools will also work well even though they often have top rake. The important thing with acetal, and UHMW, is holding the part. They are both slippery and the helix on a milling cutter can pull them out of a vise if a heavy cut is attempted. It is best if you can clamp them down or bolt them down rathetr than relying on friction in vise jaws.

[A1CNC]

Another good way to hold these materials is a vacuum holddown.
I have to plane 1-1/2" thick material down to 1.3". I use a 6" dia. face-mill and take off .1" deep per pass the full 6" width and have no trouble with the material moving, unless the vac pump shuts down then things get interesting!
I Generate literally trash bags full of shreaded UHMW per job.

Also not cutting fast enough for the chips to evacuate the heat from cutting will cause the material to "swell". This makes holding dimensions on your parts interesting. Feel your part after you are done, if it is warm or hot you are not taking the heat out with the chips. Plastic grows with heat.

Eric

[Jay C]

Yeah, so my router is spinning too fast, my feed is too slow, and my tool is not sharp enough.

Can I improve the situation by using the slowest speed of 10K RPM, using a single flute uncoated endmill, and changing my DOC? Should I try to take deeper cuts or lighter ones? The Onsrud are pricey and this is just a personal project so I'd like to "get by" with the end mills I have.

[CNCRim]

HSS is your answer, cheap and work great.

[naytep]

We specialize in plastics. What most of the guys say is correct. Speed up your feed and slow down your spindle. At 10k rpm I would be running 150ipm. HSS works better most of the time. If you have to use carbide because you dont know how to sharpen a tool then use the polished aluminum inserts from Korloy. There are plenty of other manufactureres but Korloy is cheep and wear or chipping isnt an issue. I use a high positive on all plastics. Threading, turning, milling. The only time I use a 0 or negative is when i am step drilling. most plastics tend to "suck" the bit in if not. Dont take small cuts unless absolutly required, especially in UHMWPE, HDPE, PP, PE. It has tendencay to burn and stick. The heavy chip gets the heat out, and its heavy enough to weigh itself down so that it doesnt wrap.
Good Luck