• I want to thank all the members that have upgraded your accounts. I truly appreciate your support of the site monetarily. Supporting the site keeps this site up and running as a lot of work daily goes on behind the scenes. Click to Support Signs101 ...

Cutting HDPE Plastic on a CNC Router

ExecuPrintGS

ExecuPrintGS

New Member
We just recently got a cnc router, we ran a number of tests before cutting into a good sheet of HDPE for our client and everything looked great on the foam.
When we cut the plastic we ran into a few issues. Seems like the cut depth liked to vary a little occasionally, the bit seemed to melt the plastic and not "chip away" like we were told it would.
We tried slowing the bit down as was suggested to us but nothing seemed to work.
In the end we ran the job, and have a decent looking sign, just needs a ton of clean up work around the edges that doesnt seem right.

We used a 2 flute up cut, 1/8" end mill bit.
Photos show the result, if anyone has a different suggestion for bits to use for this material that would be greatly appreciated, or any other suggestions.
We have a few other customers that would love to get some of these signs and would like to reduce the labor on the back end with less clean up work if possible.

Thanks
 

Attachments

  • photo 1.jpg
    photo 1.jpg
    40.6 KB · Views: 2,564
  • photo 2.jpg
    photo 2.jpg
    66.3 KB · Views: 2,044
C

CanuckSigns

Active Member
ExecuPrintGS said:
We just recently got a cnc router, we ran a number of tests before cutting into a good sheet of HDPE for our client and everything looked great on the foam.
When we cut the plastic we ran into a few issues. Seems like the cut depth liked to vary a little occasionally, the bit seemed to melt the plastic and not "chip away" like we were told it would.
We tried slowing the bit down as was suggested to us but nothing seemed to work.
In the end we ran the job, and have a decent looking sign, just needs a ton of clean up work around the edges that doesnt seem right.

We used a 2 flute up cut, 1/8" end mill bit.
Photos show the result, if anyone has a different suggestion for bits to use for this material that would be greatly appreciated, or any other suggestions.
We have a few other customers that would love to get some of these signs and would like to reduce the labor on the back end with less clean up work if possible.

Thanks
Click to expand...

I think the up cut bit is your problem, while it's cutting, it's pulling the material up, causing uneven depths, try a down cut bit, it should help with the material fraying along the cut as well
 
S

synergy_jim

New Member
1/4" double spiral downcut on hdpe runs around 18,000 rpm's at 350inch per minute - this is assuming you are only taking 1/2" bit diameter deep.

1/8" single spiral downcut - hdpe cuts around 200 IPM @ 18,000 rpms. on 1/8" bit you should be cutting 1/16" of material per pass

Upcut bits are always a pain.


use downcuts.
 
SebastienL

SebastienL

New Member
Material melting: slow the rpm down or increase cutting speed. Up or downcut, just make sure you have a proper bit for the material. Not all bits are good in all materials, some are specific to aluminum, some to plastics and some to wood. Consider making a rough and finishing pass.

Uneven depth: My guess is the material is not laying flat on your table... or maybe some "melted" material sticks to the bottom. Again, consider doing it in 2 passes leaving .005" to .025" for the finishing pass.

If you can do it in 2 passes, use an upcut bit for roughing to evacuate the chips and an downcut bit for the finishing pass. Downcut will leave a cleaner edge.

If all else fail... just run the finishing pass twice ;)
 
E

Eric H

New Member
Your hold down may be a bigger problem the bottom of the cut should be smooth. We Just ran about 130 colorcore signs all cleaned out out with 2 flute 1/8" gerber gold upcut spiral. 19000 rpm 150 ipm .1 cut depth. I will say all bits are not the same I tried about 3 different upcut spirals before I found one that cut really clean. We also use straight flute bits sometimes, they work well to. Didn't need more than a blast of air to clean them up.
 
ExecuPrintGS

ExecuPrintGS

New Member
Thank you all for the input, we are going to look at a few different blade options and play with speeds next week.
I will let you know how it goes.
 
skyhigh

skyhigh

New Member
How thick is your HDPE material....and.....are you using vacuum hold-down?
My first thought, is that you are warping the material from the heat, thus the difference in depth.

As for the rough cut/cleanup....
My first inclination would be to use an up-cut bit. Also, I agree with Sebastian.....slow the rpm's down. I would slow it way down, and use a new bit. The HDPE is pretty soft material (although I haven't cut any myself, I have used it), so I would imagine it would melt very easily. If you're melting the material (which you are), then your rpm's are too high, or you're cutting too slow....or both.
 
omgsideburns

omgsideburns

New Member
I'm not expert in this area, we don't have this type of equipment in my shop, I am just a hobbyist.
I cut 1/2" HDPE material on my DIY CNC that was using a dremel as a spindle with an 1/8" two flute upcut bit. 40ipm, 1/10" per pass. RPMs were probably holding at half of what the dremel turns at so maybe 12-18k. It cut fairly clean, picture below. I was making mounts for a bigger spindle. :Big Laugh

IMG_0889.jpg
 
SebastienL

SebastienL

New Member
omgsideburns said:
I'm not expert in this area, we don't have this type of equipment in my shop, I am just a hobbyist.
I cut 1/2" HDPE material on my DIY CNC that was using a dremel as a spindle with an 1/8" two flute upcut bit. 40ipm, 1/10" per pass. RPMs were probably holding at half of what the dremel turns at so maybe 12-18k. It cut fairly clean, picture below. I was making mounts for a bigger spindle. :Big Laugh

View attachment 94051
Click to expand...


:thumb: If this forum had a "Like" button... I'd click it!
 
skyhigh

skyhigh

New Member
Pretty cool OMGsideburns!!! (got pictures?)

I was mistaken..... I guess king colorcore is HDPE. My wife just cut this sign out of 3/4" material (8ft long). She said she used 2 flute upcut bits (flatbottom). She used a combination of 1/16, 1/8 & 1/4" bits. Ran the job at 3ips @ 14000. At first the material was coming off in chips that resembled skinny/mini pieces of rice (or elongated mouse droppings....LOL) As the bit got hotter, then it started to melt a tiny bit. She increased the feed rate, which solved the problem. Total depth was 1/4" in 2 pass. (edit: also cooled the bit with air during part of the process)

I'll see if she can send me a couple pics of the finished job, and post them up.
 

Attachments

  • Untitled.jpg
    Untitled.jpg
    30.1 KB · Views: 2,074
omgsideburns

omgsideburns

New Member
skyhigh said:
Pretty cool OMGsideburns!!! (got pictures?)
At first the material was coming off in chips that resembled skinny/mini pieces of rice (or elongated mouse droppings....LOL)
Click to expand...

Yes, when it's chipping off bits like rice seems to be when it cuts the cleanest. Easier to clean up the mess too, they vacuum right up.

So not to thread jack let's not discuss it in this thead, but here's my build thread on another forum. http://www.shapeoko.com/forum/viewtopic.php?f=5&t=1838
 
Joe Crumley

Joe Crumley

New Member
Choosing the right cutting tools

On any materials I'm not familiar with I go to my trusty tool supply to get the right bit, feed and speed rates. Gary at Beckwithdecor has a wealth of knowledge on router bits since he's an Onsrud dealer. Hell get you going in nothing flat. HDPE is a dream to cut.
 
Joe Crumley

Joe Crumley

New Member
Jim's correct about Onsrud having a feed and speed manual. It list all substrate materials and spells out exactly what you need to do the job. The only quirk is, that manual isn't very accurate if your not using their bits. It's close but sometimes doesn't seem to work. My best effort is to call my Onsrud dealer, Gary Beckwith, and get his advice. He's routing everyday on just about everything so his advice is good. Check out his website to see what he's up to. www.beckwithdecor.com

Joe Crumley
 
A

axis

New Member
I've cut a ton of coextruded HDPE. Best results were with a 1/4" straight double flute. With materials prone to melting, I've had good luck with a single straight flute. It effectively reduces your tool rpm by half. A dull bit will leave "feathers" too.

I've always been disappointed with Gerber bits but I've had great results with Freud and Whiteside bits.
 
ExecuPrintGS

ExecuPrintGS

New Member
Just as an update, no photos sadly but we did get that job finished, had to do some clean up work but we did do another recently and found that we had the (feed) direction the wrong way. A few tests and we are getting a lot cleaner of a cut. In the end i will end up cleaning it up a little bit still but much much better.
We appreciate all of the input you guys helped a ton! :rock-n-roll:
 
You must log in or register to reply here.
Top