What's new
What's new

Tooling for milling UHMW

Ukraine Train

Cast Iron
Joined
Feb 10, 2014
Location
Ohio
I rarely run anything besides steel so I'm not sure what the best approach is with this. I need to hog out a bunch of material in UHMW plastic, about 2" deep. My first thought was to use a square shoulder inserted shell mill making 1/4" deep passes, but I also have some 1" HSS end mills that I could run at full depth. Or maybe a fly cutter? What's the best way to go? I'm not sure if carbide inserts will "weld" to the plastic if the speed is too high?
 
I rarely run anything besides steel so I'm not sure what the best approach is with this. I need to hog out a bunch of material in UHMW plastic, about 2" deep. My first thought was to use a square shoulder inserted shell mill making 1/4" deep passes, but I also have some 1" HSS end mills that I could run at full depth. Or maybe a fly cutter? What's the best way to go? I'm not sure if carbide inserts will "weld" to the plastic if the speed is too high?
.
i have used a roughing end mill the corncob wavy teeth type. use a sharp one and watch for plastic melting. but often 1" dia will just plow right through it if you can hold the plastic
 
You can cut it really fast, use sharp HSS bits and keep them cool, and the chips evacuated. Dont melt it. IIRC I cut it at 3k rpm at 24 ipm on a proto trak.
 
It cuts REALLY easy, so use a brand new HSS endmill or a 2 flute carbide endmill.
There are 2 things you need to watch out for when cutting UHMW:

1) the part WILL change size overnight
2) UHMW is so slippery and flexible that too much cutting force will make it squeeze out of the vise, so make sure you take that into account. Maybe use more holdins stock than normal.
 
What the others said about cutters and keep the speed down & feed up - don't even think of running high ALU speeds.

X2 on clamping, UHMWPE isn't known as poor mans PTFE for nothing.

Also watch for high helix EM's they have a stronger lifting action.

If your 1'' EM's are sharp, as in never been used for anything else 10X glass type sharp, they will be OK.

FWIWQ, The only viable insert cutter I know for soft plastics is the Korloy Ripper mill as done by Curtis here RIPPER MILLS
 
Thanks guys. I'll have 2" of stock to clamp onto in the vice so it shouldn't move. For the open pockets I'll try a nice sharp HSS end mill. I'm taking material off the top too and I think I'll try my 2" Coromill with aluminum inserts there.

Edit: Does 150sfm and .010IPT sound reasonable?
 
Last time I ran uhmw I was at 4000 and 150 ipm. 2"x.100 wide with solid carbide 3/4. It is slick in the jaws so make sure you have plenty to hold on which it sounds like your fine. Also make sure the cutter you use has never touched steel tomake sure it is sharp.
 
I've lined the jaws of my vise with self adhesive sandpaper for milling UHMW. It gives you a better grip with less squeeze :D

I would typically just do it dry, with a new high helix endmill. HSS will be fine for it, depending on how many hours of tool life you expect to get.
 
Thanks guys. I'll have 2" of stock to clamp onto in the vice so it shouldn't move.

Ya'd think, but you might be wrong.. The crap is slippery and squishy. And it seems to melt and leave
horrible burrs at anything over body temperature.


For the open pockets I'll try a nice sharp HSS end mill. I'm taking material off the top too and I think I'll try my 2" Coromill with aluminum inserts there.

Edit: Does 150sfm and .010IPT sound reasonable?

When folks say low speed and high feed, they aren't kidding. My last adventure with UHMW, mostly drilling, I was running 3/8 drill around
90sfm and .040 a rev.. That low speed with flood coolant still left a HUGE burr on the backside, so I had to let it cool down and come
back at about 20sfm for the breakout to keep from getting a nasty melted burr..

Drilled a ton of HDPE (or was it LDPE) a while back, and just screwing around was able to punch a 1" drill at .200 a rev, that left a
bit of a burr because I was out running the relief, did just fine at .150 a rev.. On that same part, running 3/8" 2 flute endmills, feeding
around .040 a rev and ramping at 30 degrees..

Just pointing out that its NOT METAL... You CAN and SHOULD feed the ever livin' hell out of it. FEED before speed..

My METAL working brain would want to start around .010.. But then the PLASTIC working brain would kick in and you'll probably
end up at well over .020, I wouldn't be surprised if you could easily pull .030 to .060 a tooth..

Fresh, un-used HSS is a good choice.
 
We run a fair number of UHMW parts and have been having excellent results with the YG Alu-Power uncoated end mills. Even after using them in aluminum. They're stupid sharp and seem to stay that way under moderate use. Far fewer burrs than with the ZrN end mills we were using before and no lift issues as the material seems to shear very well with them.

Been facing with a Mitsubishi 3" AXD4000 face mill at 10000 RPM and 300 IPM also with good results. I suspect the ripper mills would work the same as they use the same or very similar type of ground and polished inserts.
 
When I run plastics, I use a set of steel knife jaws with teeth milled into them. Basically just dovetail jaws with a serration milled into them. Use a regular vise handle and work the teeth in to bite. Then back off and Clamp using a torque wrench. 40-50 in. Lbs will do it.
 
If this is going to be a recurring order/project/etc., you will want to invest in a plastic router bit from Onsruud. For pockets you want a single or double flute upcut.
 
Plastic routers have a low helix, 5 -10 degrees, for a reason. If you use that 1" mill I would use the sandpaper on the vise jaws, run the spindle around 1000-2000 rpm and chip loads up to .04" with lots of coolant keeping in mind the part could come out of the vise at any moment. The more experience you get the more you will worry about the part pulling up. If you are making very many parts get a 2 flute router or 2 from Onsrud. The difference between them and aluminum end mills is more than you can imagine. If the plastic is has any recycled content your tool life with HSS may be dismal.
 
At a shop I used to work it was the carpenter that did all the machining of UHMW with the same machines he did his wood with
That went really fast
I immitated that once when at another shop I had to make some long chain guides
Just pushed it through a opening I had created and a 100mmHSS facemill I ran it at max speed 2000rpm
Did 40mtr or so of the stuff within less then a hour

Peter
 
This is applicable for most plastics:

Remember that plastics are weak. So, you can feed the hell out BUT the part must withstand the cutting stress.

I.e when squaring material, the last corner may break off when width of cut is too large.

Dammit, if somebody understand please translate it to more fluent english :)
 
This is applicable for most plastics:

Remember that plastics are weak. So, you can feed the hell out BUT the part must withstand the cutting stress.

I.e when squaring material, the last corner may break off when width of cut is too large.

Dammit, if somebody understand please translate it to more fluent english :)
Your not going to break the corners off on UHMW by feeding too hard.

Depends on the plastic how you work with it but UHMW can be fun to machine if you can hold onto it. You run your feedrates as high as the machine can go and slow the spindle down as much as you can. Drilling you can just about rapid instead of feed. I have done it by accident and it worked just fine. Dealing with the burrs is the second worst part. Doing this on the machine works best. Sharp cutters and a very free cutting chamfer mill can do most if not all of the deburring much easier than by hand.
 








 
Back
Top