Machining UHMW

[bleeth]

Guys: The following is from another thread but I am posting it here as the best machining technique is not something I have experience with for this:

"I cut UHMW & HDPE plastic and some of the cuts could be better. I currently make a 4" roller out of 1.25" UHMW that I have to cut oversize and turn on a lathe because the surface finish is unacceptable it would save me some time if I did not have to finish on a lathe I make 100 of these every 4-5 weeks."

Mike Miller is doing this and is having an issue with machining chatter/finish when cutting. Since they are rollers that is not good. If anyone out there has specific input it would be helpful.(bit/feed/speed/plunge/ramp/allowance/tolerance)

Note he has verified his pinions are good and tight and he is not pushing the limits of the machine. He is using an Onsrud bit designed for soft plastic. I believe the tool is a 4 x 8 PRS standard with a Milwaukee router.

[Brady Watson]

Use a 2-flute spiral-O @ 13,000-15,000 RPM and 1.2 IPS XY speed. Use a spiral plunge taking off no more than 1/8" per pass.

How well is the material being held down?

How well is the router secured?

How tight are the bottom YZ car rollers?

I cut this stuff all the time on my PRT with 7.2:1 Alpha motors - My customers don't accept chatter. We own light machines & have to keep this in mind when cutting certain materials and types of parts.

It could be your are missing something...but I think it is nothing more than cutting a little too fast & maybe taking too big a bite out of the material per revolution of the cutter.

Hard materials sheer off. Soft materials snap back...In your mind's eye, picture what is happening down at the cutter/material boundary. It will teach you things...

-B

[bleeth]

Mike:
Did you try the trammel test on your Z I suggested? After it is dialed in try a sample with Brady's strategy (he suggests cutting the same kind of plunge depth I do on Corian with a 1/4" bit but spinning a little faster) and post a results shot.
Also if I were doing these regularly like you are instead of cleaning up on a lathe I would use a horizontal or verticle belt sander with my parts on a "hub" jig that I could slide into place while the belt was running and just turn the part by hand. You should only need a light touch to clean them pretty good.

My edgebander needs some new rollers and maybe I'll try it myself, but probably with a harder material like Delrin.

[gundog]

I am just seeing this I have tried many things to clean this up even making a final pass but they are still chatter finished. I have use single flute cutters and double flute cutters different speeds and feeds some make the finish slightly better but none leave the finish acceptable. I am cutting 1.7 IPS .375 deep with a .375 cutter the single edge cutter gives the best cut in the climb direction. I use vacuum hold down. The material is 1.25" thick. Parts are machined on both sides. The info on the machine is correct except my PRS has a 3HP Columbo spindle but I had a router on it when I first got it.

Mike

[Brady Watson]

For the heck of it...Try cutting .125" per pass with a spiral lead. .375" per pass is pretty aggressive. Yes the material is soft...and you can machine these quick that way. But...post finishing on the lathe is a pain, costly and not necessary.

Even if you slowed down the cutting speed to .5 IPS, and cut them at .0625" per pass, it would be faster than cutting them .375" per pass @ 1.7 IPS if you then have to reprocess them in the lathe.

-B

[gundog]

For the heck of it...Try cutting .125" per pass with a spiral lead. .375" per pass is pretty aggressive. Yes the material is soft...and you can machine these quick that way. But...post finishing on the lathe is a pain, costly and not necessary.

Even if you slowed down the cutting speed to .5 IPS, and cut them at .0625" per pass, it would be faster than cutting them .375" per pass @ 1.7 IPS if you then have to reprocess them in the lathe.

-B

Actually it is just the oposite The machining time would go through the roof if I machined that slow and took that small a bite. I have also tried slower feeds and it gets worse. I would have to look at the file but it takes at least an hour to cut the 100 4" rollers @ .375" deep per pass @ 1.7" per second. I am doing 100 of these rollers at a time. The process on the lathe is not that bad maybe 45 minutes to turn them to finished size. I have an arbor and turn them in one pass and cut 12 rollers in one pass.

I would like to improve the cut quality in all the plastic I machine. What I find are arcs like rollers or radiused corners are where the edge finish is always the worst. Straight lines look great that is why I think it is a resolution problem and why I asked the questions about these belt drives. I will try and take a picture of what I am talking about but it is hard to show in a picture. The UHMW is always the worst but the HDPE radius corners are always slighly chatter finished I do not cut wood per say so I am not sure about wood or other material. The HDPE finsh is OK and works but it would be nice if it were better.

I ocasionally make cuts with a router mounted in a table using a straight wood cutting bit next to a fence and the finish is perfect. I have been toying with buying some straight flute bits and trying them on the CNC Onsrud even makes a staight O flute I am going to buy some of them and see how they do.

Mike

[bleeth]

Mike:
The straight O's from Onsrud I saw either don't have enough cutting depth for you or are long shanked and designed for air routers. I think you ought to ask Fred to do a 1/4" straight O with a longer cut for you. Your feed and speed should be good numbers (thanks for finally sharing some specifics!!) but the plunge is too deep. If you take 1/2 the plunge you may double your cnc time but cut or eliminate your lathe time and you can always be doing something else while the cnc is running or even drinking coffee and checking out the forum instead of standing at the lathe!

Another thought: Since the main issue is corners and the Arcs it sounds like you may need to change your ramp and/or corner speed so the feed doesn't slow down as much. Brady-You're the ramp/corner speed expert!

I have never gotten a decent finish on any plastic cutting deeper than a 1/4 or so with any bit. Guys with machines a lot heavier than SB's have the same issue.

Thinking outside the box-Why don't you cut a big mold and pour the damned things.

[garyb]

Dave, you missed the 63-700 series
63-785
Gary

[bleeth]

Nope-I was looking at straight O's. 63-785 is upcut. I've found that when cutting smaller plastic parts the upcuts have a good chance of making my part jump when cutting through. The straight flutes just leave it laying there like a pig in a Kansas back yard!!

[Gary Campbell]

Mike...
You say your straight parts have a good finish on the edge. Are they the same size as the round ones? I have noticed that these parts are vibrating as they are cut. Try boring the center holes and adding hold down. Then cut the outline.

[gundog]

Mike...
You say your straight parts have a good finish on the edge. Are they the same size as the round ones? I have noticed that these parts are vibrating as they are cut. Try boring the center holes and adding hold down. Then cut the outline.

Yes the same part such as one of my fillet/Rigging tables have straight sides with 2 corners having a 1" radius the flat sides are anywhere from 24" long to 40" long & 12" to 16" wide. The sides come out smooth and the corners always show more chatter. I hold down with vacuum and cut to a .050" skin and trim the parts out with a laminate trimmer because many of the other parts are much smaller. I usually cut these parts in one pass with a single flute spiral upcut .250" bit ran @ 1.7" per second 18000 RPM. These feeds and speeds as well as the cutter are what is recomended my the plastic manufacturer. Bit is a 63-700 series I am not home right now so I can't remember the last 2 numbers. Material is 1/2" Seaboard HDPE.

If you go to my web site and go to the products page you can see my tables click under the picture of the fillet table and also look at my custom products page for more stuff. The UHMW parts I machine are for my Anchor Locker bracket.

Mike