Machining soft plastics UHMW & HDPE

[gundog]

I have asked questions before on machining UHMW & HDPE, are any of the rest of you machining this stuff on a Shopbot?

The parts I make are cut from 1.25" and .5" material. The round parts are coming out with a poor finish and I am forced to clean up the edges on the lathe and it is time consuming.

I have machined this stuff with a hand router using straight flute bits and got a much better finish than I am getting now. I am using some Onsrud spiral up cut bits designed just for this material now. I am thinking I may try the straight plunge type bits and see how that works they worked good in the hand held router.

I have tried different speeds and feeds it does not seem to change the result. I am running at step 5 or 6 on my 3.5 HP Milwaukee router I am not sure what speed that is. I am only plunging .375” with .5” bit @ 1.5-1.7 IPS.

I have tried a clean up pass of just .015” and it helps a little but still looks pretty bad. I am going to try some more experimenting. I may do the hogging with the spiral bit then try a final pass with a straight bit. I am just wondering if anyone else has figured this out yet.
Mike

[Gary Campbell]

Michael..
I just cut a couple of mounting blocks from 1.25 Black Delrin using a 1/4" O Flute. 12K rpm 1.5ips 3 passes. No cleanup pass. I did a 2.85" pocket 1/2" deep, 2.1 thru hole, and OS profile on 4.1" square. Cut quality was very good. You may want to try one of those. They come in spiral up, down and straight.

I was surprised how much harder Delrin was than HPDE or UHMW. I had to use vacuum on a 12" square piece along with clamps to keep vibration down. I threw some platic chips on the top of the material during a test cut and watched them dance off the piece. Then I added the clamps.

Another thing you might want to check for is runout or machine flex. To check, warm up router, remove bit, place dial indicator against collet nut, put finger pressure against other side of nut. See how much movement about 10# of force gets you. Then move up to base of router, repeat, and see what you get for a reading.

Many routers have .008 to .015 play in lower bearings. Add a few thousanths flex from the machines moving parts to another ten from vibration and you have poor cut quality. Power at lower rpm and much less runout are the reasons to use a spindle for machining materials that are harder than wood.
Gary

[jerry_stanek]

I was just at John Forney's cap and the Jennifer From Onsrud gave a session and sad to look at the scrap if it has a better cut the reverse your travel

[paco]

UHMW is a little trickier. Maybe you could post pictures about your issue.

[bearcat]

How are you holding down the HDPE / cut part? I've found that cut edge quality is directly related to a solid hold down.

Which Onsrud up spiral bit are you using? The 63-775 family is a good choice for HDPE.

Ed

[gundog]

I have been busy sorry it took so long but her are the pictures. The first picture shows the left roller turned on the lathe the other two that are stacked are the ones with the rough finish.

One of the problems that I am having is that Partworks for some reason makes the machine do a bunch of plunge cuts like drilling a bunch of holes then comes back and starts making passes. The funny thing is the holes are random and not all of the rollers get these plunge holes in the profile the ones that do it leave a line and that just makes the finish worse.

http://img.photobucket.com/albums/v292/millnut/DSC05155.jpg

Here is an issue I ran into today for some reason the chosen vectors did not cut all the way around the parts you can see that here. These are rectangular parts for some reason the toolpathing did not cut all the way around.

http://img.photobucket.com/albums/v292/millnut/DSC05153.jpg

[wayne_walker]

Michael,

I think your problem with the rectangular parts is not having the proper spacing between the parts. I would run the file in preview and see what it looks like.

Hope this helps.

Wayne

[gundog]

I think you are right Wayne I made the spacing 1/2" to match the bit size to conserve material. I don't know why it would cut it partially though. I had to go back and make a new tool path I just chose every other one and ran that and it finished the cuts. The preview did show exacty what it did.

When I cut the rollers from sheet stock I just don't understand the plunge cuts and why it makes those. I have made several different files to cut those parts and each one has a different amount of those plunge cuts it does not do it on the whole sheet.

For hold down I am screwing down to plywood. I set up a mounting drill patern and the bot drills those holes first the holes all land in the waist portion of the material. I use screws in the center areas of the material and the perimeter. I leave .100 skin in the material to keep it stiff and trim it out with a laminate trimmer.
Mike

[paco]

If you could post the file, we could then make appropriate recommendations...

On another note, I wouldn't expect the Bot to give me the same result as a lathe.

[scottcox]

Michael,

There has been previous discussion about the Vectric programs not recognizing a pocket that's "exactly" the same size as the bit.

When you're designing your parts, leave your pockets "larger" than your bit, even by 0.001".

That should correct that problem.

[kerrazy]

TO Add to Scott's comment, You could trick your tool library as well, by entering a duplicate cutter with a .001 under the half inch. You of course use your half cutter, but now your software will fill the pocket.

[gundog]

I don't expect to get the same finish with the Bot as I do with the lathe but it has to be better than what I am getting. I can't upload my files I don't know what I am doing wrong. The files are in a folder but they are saved as a Vcarve file and the uploader won't find them what do I need to do?

[Call-Tech]

Use winzip or winrar to compress file. These are known formats that the message board should accept.