endmill specs for foam milling ?

[swagman]

i use these to cut patterns for vac forming. we use poly styrene foam. we use epoxy resin and mat for the actual former. i cut at 4000 rpm with up to 500 mm per minute feed. they do exelant job.

[thinkntink]

When you are cutting plastic foam, a great deal depends on the rigidity of the material being cut. High rigidity (like styrene and HDU) allows a cutter to develop high cutting shear at modest chiploads. Spongy, flexible foams need MUCH higher feedrates to achieve clean cutting.

Generally speaking, burrs do not have enough flute volume to allow debris evacuation at high chiploads. High rake 2-flute or 1 flute end-mills are by far the most effective tools for 3D foam carving.

Let's say you are carving a fairly large model so that you can use a 1/4" (6.35mm) dia ball cutter (picture attached). Also assume that you are plunging 20mm on each pass. If your spindle can turn 10KRPM you should cut styrene or HDU (high-density-urethane) foam at approx. 5 meters/minute. Anything much below this may melt the material to the bit and damage your model.

If you are cutting a more compliant material like ethafoam (polyethylene foam) or die ejection rubber foam with the same cutting parameters, you would want to use a feed rate of 10 to 12 meters/minute.

In any case, a VERY high shear cutter is called for.

It is pretty easy to determine the best feedrate to use with any soft material (not stone or metal). Go to:

http://www.precisebits.com/tutorials...s_n_speeds.htm

Generally speaking, it is better to feed too fast than to feed too slow when cutting any thermoplastic material. For a case study on cutting a material similar to sheet styrene, go to:

http://www.precisebits.com/tutorials...moplastics.htm

[shrthang]

I've been custom cutting foam for over 10 yrs now and there is no question experience is the best guideline. For every material I cut, I've done trial runs to experiment with different feed rates and plunge depths. EPS is the common foam I use and I've run my 1" dia x 12" long 4 flute custom bit at 100% stepover at 6" deep, sometimes deeper. When you're manufacturing, cutting time is important. Hogging away as much material as you can with a large dia tool and then finishing with smaller tool is the way to go.

The two flute bits that thinkntink shows work great, but when you get into larger cuts, getting custom made bits designed for foam cutting is the smartest thing you can do.

If you want to see some interesting foam cuts, check out my site at www.revolutionaryminds.com.

If anyone has questions on hotwire cutting, I'm also very experienced in that department.

[shrthang]

Rotary burs do work great as well for providing a very nice finish. Having a good vaccum system is very important when cutting foam, especially with rotarty burs because of the fine offcut particulate that will build up on your gantry and spindle because of the static build up. Ensuring that your table is excessively ground is a good idea. Foam can build up a tremendous amount of static when being cut and can cause your system to crash or even scrambles the program and can make your machine do some crazy and dangerous things.

When I first started cutting foam on a large custom built CNC table, it did some crazy things. It would race across the table and dive down through the bed. I was just lucky the custom bits were 1" dia and very durable. Once I got the grounding issue dealt with, I never had problem again. Foam building up on the gantry can be bad, because if it get into the teath for the cog and continually compressed, it turns to a hard plastic and keeps building up and puts torque onto the cog and it will eventually snap off.

[thinkntink]

To Shrthang

Very nice models in your gallery. What feedrate and RPM (or chipload) are you using when doing deep hogging?

[shrthang]

The feed rate when using the 1" dia 12" long 4 flute custom bit, was approx. 6000 rpm and the feed rate would be between 100 and 200 inchs per minute. If I dropped down to a 1/2" dia bit, I'd increase the rpms to 12,000 and the feed to 200 in/m.