[nagjames]

I'm trying to cut UHMW with a 1/8 cutter. This is the first time I'm trying to cut this material. It's not too bad but the top of the part is far from clean cut.
I'm cutting it with a brand new 1/8 2 flute carbide cutter DOC is .125 4400RPM , 40IPM lot's of coolant. I started from 25IPM and gradually increased the feed while 4400RPM remained constant.
I don't dare to push it further I hate breaking tools...
My Mill is a Tormach max IPM65 max RPM 4500

Thanks,
James

[DSL PWR]

You need to push the feed higher. You probably will need to take a shallower doc so you can clear the chips. Go to a .05" doc and max feed, then lower the rpm until you have a better finish. I know this is counter intuitive, but uhmw is a funny beast.

[black_taco]

Can you take a slower finish cut around the contours to clean the ragid edge? Although capable of being cut at high speeds UHMW is not always cooperative when doing so.

[nagjames]

I’ve read somewhere that UHMW is best cut at full depth or even 2x depth. Maybe it was for a different cutter. I could decrease the RPM or increase the IPM but then I’d increase the chipload and it’s already .0045 per tooth. GARR suggests .002 for plastic for carbide 1/8.
I don’t quite understand. I forget to mention that I profile slotmill and I do have a finishing cut . I leave .02” for finishing. I’ll try to decrease the finishing RPM for start. But I still don’t get why GARR ( and Niagara cutter) suggests .002 for plastic. Maybe the term “plastic” is too wide and not applicable for UHMW?

[rounsy222]

Uhmw has give to it as well so if you push it too much you will find your diminsions will vary. The main thing is to keep your cutter clean and cool otherwise you run into other issues. Better to to take faster lighter passes than slower heavy passes. Rigidity will make a diference on how much you can take as well. Good luck.

[fatal-exception]

I machine UHMW all the time, and have not had any problems with cutters down to 1/16" diameter. I think DSL is correct when saying you need to take a heavier cut.

Make sure that the cutter is making 'real' chips. Stop the spindle and clean off any strings that are whipping around. Also, carbide and UHMW have never seemed to get along for me. Now I only use 4 flute, hss cutters, and I usually knock the square corners off the flutes so that overlapping toolpaths are smooth, and burrless. 2 swipes with a fine diamond hone is usually enough.

Paul

[nagjames]

I did a bit more experimenting and found that 200SFM and 4x chipload increase (compared to aluminum for example from .001 -> .004 ,1/8 carbide) works best. What did make a huge difference when I switched from climb to conventional milling.

4 flute cutter? really interesting I thought that 4 flute and plastics do not mix well that's why they sell even 1 flute cutters. What DOC are you milling with a 4 flute cutter . 1/2DOC 1xDOC?


Thanks,
James

[fatal-exception]

Hey James,

Well, most of the stuff I do I can use 1/4" 4f em's, and for roughing passes some of my programs take up to .35" deep. This is only when there is alot of stiffness to the part being machined. As the part dwindles, I take less of DOC, with the minimum being 1/8".

As a generalism, the swirl marks on the part are about .025 apart with the 1/4" end mill, which would suggest ~ .0065"/flute @ 2500rpm. I don't know how this fits into the sfpm formula, but it works...consistently.

Some uhmw is much more abrasive than other batches I've received. Some batches, I can run 15 cycles/tool, other batches, it may be as low as 6. Depending on the product I'm making, I can sometimes start honing the tool between parts and the parts will stay within tolerance.

All my programs for uhmw are climb cutting, but they are all tuned to make the correct size of features. I don't notice a difference between climb and conventional milling.

I think the big thing is figure out what works all the time. I've tried carbide 2 flute end mill and they didn't agree, maybe they are too stiff for my machine, on the other hand, hss just sizzles through the material like nothing and spits out consistent chips at 50ipm with no problems. If it's not milling properly, my tendancy is to lower the spindle rpm until it is working properly. (to a point)

Paul