HDPE cutting problem

[leaveme]

HDPE was not available in my country so that I was using cutting boards for some time. I use 4 flute (hss) endmill to cut that. Suddenly I found a shop selling different plastic sheets and they claimed that these are HDPE. I bought few of these sheets.

But I'm now having problem to route this material. It is getting mold during milling. I reduced cutter speed, still no improvement. I use a hardware store pot to control the speed of the (air cooled) router. Lowering more speeds means reduced troque so I can't reduce more. I also tried with low IPM i.e. 8. It also didn't help.

Is it that, I'm using a wrong cutter? Any help will be greatly appreciated.

[RomanLini]

If you can't use lower RPM then you could try a 2 flute or 1 flute cutter designed for plastics, and even a fine mist of water from a hand spray bottle can help a lot.

You are probably better off using faster IPM if you can, and take light cuts and keep moving around so there is not as much heat in the one place in the plastic sheet.

[leaveme]

Thanx RomanLini.
What I understood from your suggestion is, I have to do the light cut in increased IPM. Am I right?
I'm going to try the following in Cut2D. Do you think it will work?

[stevespo]

As RomanLini mentioned, you're going to have a lot of trouble with the 4 flute cutter in soft plastic. A mist of air or water will help to cool the cutter and keep the chips out of the way. Without that, you'll have to move that tool very quickly to avoid re-welding.

The standard chip load formulas will work reasonably well, and a feed rate calculator is very helpful.

Assuming a chip load of .005" per flute, a two flute cutter and 8000 RPM, you would need to move a minimum of 80 IPM to keep the cut clear and produce good results.

Cutters designed for soft plastic may recommend a chip load of .010" per flute, and a single flute "O" cutter at 12000 RPM would need to move 120 IPM to produce the recommended chip load.

Both of these examples are in the range of what I use to cut soft and hard plastics. The specialty cutters are really nice for this work, although "standard" 1 or 2-flute (straight) also work pretty well. Two flute spiral end mills can be made to work, but I get good results with straight cutters and less tendency to lift the work.

The depth of cut and step over are more a function of how rigid your machine is and how powerful the router is. My tendency here is to use 50-100% of the tool diameter for DOC, and a 50-80% step over.

Lighter cuts may be helpful, but not always. A deeper cut with a full chip load may actually produce less heat and cut more effectively.

Steve