[dwomble]

Hello Everyone,

I have a question about milling ABS material. Does anyone know the feed rates, speed, and depth of cut that should be taken with a 0.031" end mill (square) in ABS. I need to make a lot of small features in a key fob case that I am milling out. I have set up all the operations in Camworks already but the cuts that I have taken so far are really shallow so I don't break the end mill. I just wanted to see if anyone would know what depth and the speed and feeds to use to cut with this material.


Tooling Info:
I have 0.031" HSS 2&4 flute mills
spindle can reach speeds of 6,000 rpm
feed rates up to 40 ipm

Here are some pics of a key fob case similar to the one that I am attempting to mill out.
Thanks!

[Dylwad]

There's nothing really set in stone for small bit plastic milling feeds and speeds as far as I know.

I do know the spindle max speed is going to be an issue, 6000 rpm is very slow on a 1/32" bit, so your feedrates will have to be slower as well.

I would ditch the hss and 4 flute right off the bat and go with a carbide 2 flute. ABS is harder on bits compared to other plastics, at least that's been my experience. It also has a low melting point, so one flute packed with melted plastic will ruin the job and break the bit as it starts melting. 4 flutes don't have enough room between the flutes for proper chip evacuation on abs at the chip load you need to run to get the heat out in the chip, and not put it into the bit and material.


I run quite a few different parts from abs sheet and 1/32" bits, up to 1/8" thick.

For 1/32" thick sheet I run 18000 rpm, 6 ipm plunge, 20 ipm feed, .033" full depth cut through the sheet.

1/8" thick sheet is 18000 rpm, 6 plunge, 25 ipm feed, .034 depth of cut

On an older, more conservative file in 1/16" thick sheet I run 24000 rpm, 2 ipm plunge, 18 ipm feed and .0315" depth of cut.

I have cut thousands of each part and never broken a bit. I have good dust extraction around the bit too.

I use Kyocera bits from drillman1 on Ebay.

Sent from tapatalk

[dwomble]

Awesome! Thank you.

I tried your settings and they worked perfectly.

[dwomble]

Oh... I forgot to mention on the last post that I had forgotten that my spindle had a reducer on it which made it go 6000 rpm. Without it I am able to reach speeds of 25000 rpm.

Since this worked great I was wondering what speeds, feeds, and depth of cut do you use for 1/8" end mill or 3/16". Maybe I could improve on what I am currently doing...

Thanks again!

[Dylwad]

It's been a while since I have done any abs milling with an 1/8" bit, before I actually knew what rpm I was running. I haven't cut abs with anything bigger than 1/8" bits.

I did use a single flute carbide bit though, which helped. I'll see if I can dig up some old code for you.

The single flute bit would shrink (wear) a bit after 8-10 hours of cutting, making the pockets undersized just enough to notice. (was cutting 1/4" abs with a two depth pocket and outside contour, one pocket accepted a printed circuit board that sat flush, deeper pocket was for thru hole and wire clearance)

Sent from tapatalk

[Dylwad]

Took a bit of digging but found my last working file on a jump drive.


Rpm 14000 estimated. 20 ipm plunge, 70 ipm feed, .085" depth of cut. Was fairly aggressive.




Sent from tapatalk

[dwomble]

I tried to get as close as possible to these settings but my feed rate could only reach 40 ipm so, it didn't work too well. I will try and play with my settings and see what I come up with. Thanks again for your help

[Dylwad]

lower the rpm if you can't match the feedrate.

I snuck up on these settings, going by sound and the size/shape of the chips, and did short runs checking the bit temperature, it should stay relatively cool.

Sent from tapatalk