Cutting UHMW and delrin

[tverdin]

I am having trouble cutting 2 different materials. UHMW is the one im having the most trouble with. and delrin is the next. the thickness is anywhere from 3/8 to 3/4" I need to use an 1/8" bit. any suggestions on what bit to use and router and move speeds to cut at?

[Brady Watson]

Both materials are relatively easy to cut.

What bit are you using? (is it new?)

What RPM?

What Move Speed?

-B

[tverdin]

The bit im using may be the problem, I just used a bit i had and its not new. Its a 2 flute upcut spiral. I was cutting at a slower RPM at about 13,000 and MS at 2.5 a sec. I started at a higher RPM with slower MS but read online to do the opp. what do you recom?

[gundog]

I cut a lot of UHMW with my PRS standard and I have not found a cutter that gives a smooth finish. I have used Onsrud bits designed for plastic I have used 63-XXX series single spiral up flute and 50-XXX 2 flute spiral up flute bits. I get the best results with a 3/8 single flute bit 1.7 IPS 19000 RPM. I am cutting 1.25" thick parts.

I make a roller and I cut the rollers over size by .150" and turn them to size on a lathe. The lathe makes them look great. I built a mandrel and turn 12 of the rollers at a time.

I have a CNC knee mill and using the same bits it will cut with a good finish but the mill is very rigid and weighs 4000# and has servo motors rather than stepper motors. The router table has a 96"x48" table the mill only has a 31"x17" work envelope they each have there pluses and minuses.

Mike

[knight_toolworks]

Yep it cuts easily but not cleanly. Plus holding the parts in place can be fun. I was pocketing out a sheet of acetel for these tile molds. it warped worse then mdf. I nailed it down along the edges came back the next day and the nails were pulled out of the table.

[tverdin]

Im able to cut it just needing a better finish than im getting. Im wanting to cut the parts on the router to save time. I will be cutting alot of them so if i have to clean them all up on a different machine, I would be working backwards. anyone else have any ideas on getting a better finish. I cut delrin yesterday with the same 2 flute up spiral at 13,000 rpm and 1.5 MS and it cut like a charm. no problems and clean as it gets. no clean up at all. so now if i can figure this UHMW out I have it whipped.

[Brady Watson]

The problem with UHMW is that it will show any little vibration etc in the cut/edge. I believe this has to do with harmonics more than anything else, plus the fact that the cutter is essentially grabbing the chip & then that chip sort of 'snaps back'. If it snaps back, it doesn't always completely cut off of the part and this is where you get hairs left behind in the cut. The only remedy for this is to change your tooling selection (buy a bit made for plastics - a single, double or triple O-flute from Onsrud) and crank up the RPM, which essentially reduces the chipload, or the size of the bite taken off by each flute of the cutter. If the parts are hairy - you need more dwell time - which means a smaller chip - lower move speed & higher RPM. You'll only find the right range by experimentation and it will be a range that gives you a nice cut without melting.

If you find that the scrap edge looks better than the finished part, you need to change direction. Instead of climb milling, do conventional or vice versa. The key to machining ANY plastic is - Steady as she goes...avoid abrupt changes and get the tool to move as smoothly as possible. This may mean lowering your Slow Corner Speed down to 40 in the VR command to soften up direction changes (in SB3). Also, you may or may not find it beneficial to do your profile passes with allowance (cut the part big) leaving .03 or so on the sides of the part and bottom to clean off in a FULL DEPTH cleanup pass that wipes away all stepdown/waterline marks with little resistance to the bit, diminishing cutter deflection. Do the profile with allowance stepping down 1/8 to 1/4" per pass (essentially offset to the outside .03") and limit the depth so that you leave an 'onion skin' holding the part at the bottom. The come back with ZERO allowance in one full pass and shave off the allowance & onion skin you left on the previous toolpath.

While you have your single, double and triple O flutes on order, you may want to try a regular old 2-flute straight. When cutting plastics I would recommend a 3/8" cutter over a 1/4" if you can get away with it. It is much stiffer than a 1/4 and this makes a big difference in certain plastics. Keep the cutting edge length of the tool as short as possible - ALWAYS use the shortest cutter to get the job done, no matter what you are cutting.

Now that I am thinking about it...I'm pretty sure that Delrin/Acetal likes to be climb milled.

-B

[tverdin]

Wow, thanks, lots of great info there. I will give all that a try and let you know my results. thanks again