What end mills for plastics?

[TMaster]

I going to start milling ABS and delrin for the first time, I was wondering is the standard carbide 2 flute end mills will work, like for aluminum. Or do i need to find some special endmills? I need to have smooth finished work. My max rpm on the spindle is 10,000 and my IPM is 25. Benchtop mill.

[Geof]

We use two flute 45 degree helix 1/4". 3/8 and 1/2" diameter cutters intended for aluminum on both ABS and Delrin and get a very good finish using flood coolant running at 10,000 rpm and up to 200 ipm feed, 0.01" per tooth chipload. It is important to use new cutters because the plastics cut best with a nice sharp edge. Also the feedrate needs to be kept high to reduce rubbing and carry away the cutting heat with the chip. With a limited feed rate it may be necessary to back off on the rpm to keep the chipload high.

One thing we have found is that firm and even clamping is needed especially on sheet material. A tool with a large positive rake wants to dive into Delrin and if things are not rigid bits of Delrin go everywhere. Also when the speed is reduced to accommodate low feed rates sometimes the depth of cut has to be kept small to prevent breaking out chunks.

[TMaster]

Thanks for the info. Im going to try 3/16" and 1/4" end mills on some delrin and ABs this week. I don't have coolent unless I get a squirt bottle and spray some soapy water on the cutter/material. Since my travel is pretty limited at 25ipm max; what do you recomend for the rpm of the spindle, ipm, and depths of the cuts or chip load? With or without coolent.

I was drilling some gray pvc today and it seemed like it was getting to warm. I had 2800rpm at 4 ipm drilling. It was kind of a almost scraped look, not too great. I'm learning!!!

[sdantonio]

One suggestion I would add is that the end mill should be upspiral to facilitate chip clearance.

Steven

[Geof]

Originally Posted by TMaster Thanks for the info. Im going to try 3/16" and 1/4" end mills on some delrin and ABs this week. I don't have coolent unless I get a squirt bottle and spray some soapy water on the cutter/material. Since my travel is pretty limited at 25ipm max; what do you recomend for the rpm of the spindle, ipm, and depths of the cuts or chip load? With or without coolent. I was drilling some gray pvc today and it seemed like it was getting to warm. I had 2800rpm at 4 ipm drilling. It was kind of a almost scraped look, not too great. I'm learning!!!

Soapy water is a good choice. I would keep the speed in the 2500 to 3000 region. Experiment a bit and you will soon see what your limits are.

For drilling the pvc your speed was much too high, drop it to 1000 or even less. Again a good sharp drill is needed, you have to clamp the work firmly and go in fast; maybe even increase your feed.

When drilling the big problem is the chips in the flutes rubbing against the side of the hole. Soapy water is a good lubricant/coolant but if your are doing deep holes sometimes you have to stop and clear the flutes.

[brownandsharp]

i machine delrin alot and don't use any coolant just blast it with 2 air nozzles about 90-110 psi.

sharp cutters cannot be emphasized enough when cutting plastics.

2800 rpm is too much rpm for only 4 ipm. your material was gumming up

[TMaster]

Air sounds like a good idea. I was going to rig up a vacuum; but maybe I can blow air on it also. I bumped up to 8 ipm to try with the 2800 rpms, I'll figure out a good combo eventually. Waiting on some endmills to try. I'd like find the fastest rpm I can do with the ipm i have avaliable. Time is money!!!

[brownandsharp]

if you are adamant on sticking with 2800 rpm. go 20-25. ipm. on that drill.

don't worry it wont break.

what you can do is give it a tighter tip angle .. and make sure it is SHARP!!

[TMaster]

Solid carbide uncoated 2 and 4 flutes.

[sdantonio]

Originally Posted by brownandsharp 2800 rpm is too much rpm for only 4 ipm. your material was gumming up

Great for mills, but for those of us with routers, if we dial them down much klower than 8000rpm the torque drops off to practically nothing.

Joe, one of the guys here in a different thread, has had great luck milling plastics at (if I remember right) 16000rpm, 60-70 ipm feed rate, 0.25in solid cobalt, upspiral bit with no coolant, (don't remember depth of cut, but I suspect that it is around .100 inch).

Steven

[brownandsharp]

I only use upspiral endmills for acrylics. for delrin, nylon, and abs. i use hi helix hss with great results.

typically for a 1/2 cutter, .5 doc 40% tool dia. i'll feed 160 ipm @ 7000 rpm

also he has a benchtop mill and his max feed is 25 ipm.

theres no need to use all his rpm's if all he has is 25 ipm.

[TMaster]

Here are all the end mills I have; two are shear for aluminum can you guess which 2? All are carbide except the 3 on the left.

My ipm is limited from my computer cpu speed. I could have up to 50 or 60 ipm if i would get faster computer on the mill.