[cnczoner]

I've been trying different combinations of endmills (2 and 4-flute) and different DOC's, speeds, etc, but still can't get clean cuts in HDPE. I've not yet tried sandwiching it with a sacrificial sheet of wood on top (there's one as a base-plate on the bottom), but before I try that, I'm wondering if anyone here has a recommendation for getting burr-free cuts.

The piece on the right has been deburred manually with a utility knife.

Thanks,
-Neil.

[HuFlungDung]

Use high helix endmills. Plain uncoated high helix (for aluminum) HSS works well, perhaps even best because some coatings may round over the edge to a miniscule degree.

Climb mill and take a fairly decent chip in the finish cut wherever possible. Light finish cuts do not work well.

I think some burr is unavoidable, but a proper procedure makes a very light burr that is easy to remove with a sharp deburring tool.

[RICHARD ZASTROW]

Did you try right hand cut, left hand helix? Pulls the chip down to the bottom of the cut.

Might help, try it.

Dick Z

[Geof]

Very sharp cutters. As Hu suggests high helix because this increases the effective top rake and HDPE needs a good top rake. High helix micrograin carbide cutters will probably work fine but they must have never touched metal.

[AppEng]

Sharp, sharp, sharp! Are you using coolant? Try a mist or a light flood. It's only plastic, but it's heat and cutting pressure that's forming those "leftovers." Mist always worked well for me- light lubricant, and air pressure to blow chips away. Open geometry is important on the flutes to get those chips out fast and keep them from rubbing or getting drug back in. I've machined that stuff before, manually & cnc. RPM's up, 2-flute tool- high quality, fine sharp edge. Unless you buy a high-end uncoated micrograin carbide end mill, HSS will give you better edge definition and will definitely be cheaper.

[Mattyvdv]

hey mate.

i work in a relatively small plastics engineering and polyurethane shop.

We get success by using a 10-12mm HSS slot drill. no coolant, relatively fast feeds if possible.

[cnczoner]

Hmmm... my mill only does 1500rpm, so I cut relatively slow. The pieces above were done at 10-ipm with a regular Atrax 2-flute 1/8" endmill. (I broke my last 4-flute 1/8" endmill). I used 3 passes of .09" DOC each, climb milled. No finishing cuts. No coolant, as I found that the bits are relatively cool (to the touch) after cutting these pieces, but I can try that.

These endmills have never seen aluminum, but they have seen a bunch of acrylic and ABS plastic. That's 90% of what I cut. I'm guessing acrylic would dull the cutters pretty quickly.

i keep planning to pick up some high-helix endmills such as this, but I will now, as I want to try those on aluminum also.

What about straight-flute endmills -- I have a couple of those (Melin 1/8"), but haven't tried them yet.

Bigger question -- I've heard of right hand cut, left hand helix endmills, but haven't seen them at any of the usual sources (MSC, Enco, etc). Any pointers to where I can get these?

BTW, what is a "slot drill"?

Thanks,
-Neil.

[HuFlungDung]

A slot drill is a 2 flute center-cutting endmill. It can plunge (at a reduced feedrate) into solid material and still evacuate the material something like a drill. However, because the tip is square, and the edges sharp, it can wobble around a bit as it drills its way down. The corners are easily damaged in harder materials. Then its kind of useless unless you can resharpen the end.

The left hand helix (used with CW spindle rotation) tool might work okay for a light finish cut. However, bear in mind that it needs a place to 'push the chip' to, so a heavier roughing cut in full cutter diameter engagement is probably not going to work all that well.

For a part like your samples shown in your first post, I think you'd make better time roughing that out with a 1/4" tool at a higher feedrate and 1/4" deep, then go back and finish what needs it with the 1/8 later. That way you can use the 1/8 tool for it full flute length.

[cnczoner]

Updates...

Above 1/8", the only known very-sharp endmills I have is 1/2", but I ordered some other sizes. For the left-helix, CW-cutting EM, I could cut a clearance "trench" into the sacrificial wood base, but still can't locate any.

In the meanwhile, I tried a 1/8" straight-flute EM and got noticeably better results. I cut a couple more pieces with a regular 1/8" 2-flute EM (as before) so that I could compare the same speed/feed/doc with both of these. The straigh-flute cuts were much nicer (in terms of burrs/frayed edges). But I noticed that with the regular 1/8" EM, that the leftover material has a really clean cut. So perhaps the answer is to reverse the path. Currently I am cutting clockwise around the part, with the spindle turning clockwise, so that is climb milling. I haven't check the underside of the leftover material, so I'll do that tomorrow. In the meanwhile, I'll reverse some g-code for tomorrow's experiments.

Cheers,
-Neil.

[chollopeter]

Another thought, try using router "wood" bits. The finer edge should clean up the cut quite a bit. I've used woodworking bits on both nylon and delrin with good results. Much less deburring than with either carbide or HSS endmills.
Good Luck
Carl