[ecl66]

Dear All,

I am pretty new in CNC milling and now facing a finishing issue with HDPE.

I am using a good brand (T&O) carbure end mill 6mm 1z for profiling, at 25,000RPM (Kress 1050) and 2400 mm/min feedrate, with conventional milling direction.

Attached is a photo of the resulting finishing - could someone provide me with some clues about why I get this strange not nice looking surface pattern and some burs? I have already tried to change RPM and feedrate but couldn't see any improvement.

Many thanks in advance.

Emmanuelhttp://www.cnczone.com/forums/attach...d=320980&stc=1http://www.cnczone.com/forums/attach...d=320982&stc=1

[A1CNC]

I see a couple things going on. Looks like chatter (Either machine or cutter flex) and Chip re-welding. I would also use climb milling but it depends on your machine also. The part you show looks like the edge was milled by profile milling not Face milling.

What kind of machine are you using? I am guessing a router with that spindle speed. Sometimes you need an air-blast to clear the chips while you are cutting.

[bhurts]

This may also be caused by improper part clamping. If the part is vibrating or being pulled up by the cutter. Hdpe is one of the most easily machined and forgiving plastics to work with. What is your cutting strategy? Are you making multiple depth passes and a finishing cut or just trying all in one pass?

Ben

[ecl66]

Thank you Ben and A1CNC for your suggestions. Material is very well clamped and I am using 2mm passes. Strategy was profiling/waterlines. I have switched to BlenderCam and forced climb milling - result was absolutely perfect. I was previously using MeshCam that is OK but does not allow for choosing the milling direction with the waterline strategy (only conventional). Also, movement is much smoother with BlenderCam (adjusted to 50um resolution) than it was with MeshCam (same resolution) - CNC is being controlled with Mach3.

Thanks again for your help!
Cheers,
Emmanuel

[Jon.N.CNC]

This may also be caused by improper part clamping. If the part is vibrating or being pulled up by the cutter. Hdpe is one of the most easily machined and forgiving plastics to work with. What is your cutting strategy? Are you making multiple depth passes and a finishing cut or just trying all in one pass?

Ben

Not sure I agree, hdpe is easy to machine as its soft but to get a finish is far from easy without correct feed & speed. I find the best finish I get is with a stretched cut, ie slow rpm fast feed. 24000 is far too fast. 8000 at 4m/min with single flute would be the rates I'd start at. Try a test contour without finishing pass, if the finish is reasonable then try with finishing pass. If the test finish is poor its down to feed and speed and there's no point trying to polish it with finishing passes as it simply won't improve things.

Good luck

[Jon.N.CNC]

Missed last post, glad you got it sorted.

[ecl66]

Hi Jon,

Thanks a lot. Indeed, I also reduced RPM which helps improving the final results. So thanks for this valuable clue!

[kiwibrick]

Bit late to the party, but I cut a lot of HDPE sheet.
I generally use either 6 or 8mm 2 flute bits, 3mm depth of cut running around 10k rpm(kress spindle too with a superPID for rpm adjustment) and between 2500 to 3000mm/min feed rate, I get similar marks when I get a bit of chatter sometimes.
This is cutting slots and pockets

[Jon.N.CNC]

Bit late to the party, but I cut a lot of HDPE sheet.
I generally use either 6 or 8mm 2 flute bits, 3mm depth of cut running around 10k rpm(kress spindle too with a superPID for rpm adjustment) and between 2500 to 3000mm/min feed rate, I get similar marks when I get a bit of chatter sometimes.
This is cutting slots and pockets

Still a little to many rpms for the feed i would imagine if you still get chatter.. Though i find its very sensitive to drops in velocity so trying to maintain the velocity helps, i ramp up the acceleration but inevitably there will be places where it cant be maintained.