PVC Machining Tips
Advice on bit choice, speeds, and RPMs for cutting PVC sheet goods with a small, low-powered CNC router. December 8, 2010
Question
I've been routing 3mm and 6mm PVC sheets, all different colors. I have had terrible trouble with the white sheets. It is supplied to me and I'm not sure if it's Komatex, Sintra, or some other brand. It seems more rigid and doesn't like to be routed as smooth, and it re-welds like crazy.
Any specific bits I should look at? I've tried up/down/straight flute from Onsrud. Okay results from up and straight O flute, but thin profiles want to lift too much, and still get subpar edge quality. Need 1/16", 1/8", and 1/4" bits that I can trust every time. Other colors machine much better.
Forum Responses
(CNC Forum)
From contributor G:
Use the Onsrud O flutes. There is no way you should be rewelding. Your tool diameter really should be twice the thickness of material, but I see you are using smaller. Conventional cuts. Make sure your cutters have never been used on wood (including your spoilboard). Upspirals will clear out a chip quite well, but you will need to put some time into your vacuum hold down technique. Change cutters way more often than you would cutting wood.
3mm EPVC can be cut with a 1/4" cutter 18000 rpms at 400-600 ipm with a buttery smooth edge. Experiment from there. I cut this stuff day in, day out.
From contributor D:
I can't run as fast as contributor G because I'm on a machine with a home built flat table fitted on top of pods and using only a 12hp vacuum pump. I get good results with single o flute, 16k at 100-220 ipm. Chips pack into the groove tight and help hold parts. Any slower, chips get recut and heat up here and there, but snap off with your fingers. Any faster and small parts start moving around. This is a downshear.
From contributor G:
I run with a 10 hp pump 60" x 120" table, but I also take extensive time to vacuum out and gasket a lot of my spoil boards. People think it's a pain to do so, but I can never argue with my results. Keep the cutters fresh and away from wood. Drop the cutter down a bit once it's worn and then toss it away (or recycle). I have not found anyone who can resharpen an O flute to my satisfaction.
From the original questioner:
Thanks for the info. I picked up a Belin 1/8" upspiral single O-flute the other day, since they had them at the local plastics house. It seems just like the ones in the Onsrud catalog, so I'll give it a shot.
The other day (when I was having trouble) I was cutting some 11x17 full frames that were only .5" wide, out of 1/8" thick material. My vacuum table works pretty well, but obviously there's not much there to hold onto. I cut through all but .01 of the inside and outside profile, then finished off. My CAM has tabs I can use, but they are straight up and down, as opposed to 3d (hump shaped) tabs, so they tend to leave a slight tool mark where it raises. I'm hoping they will update this behavior soon.
From contributor D:
I couldn't make a cut half inch away from another cut with an upspiral. Granted, my CFM is limited to 4mm air lines in rails versus your flat table's massive hoses, but still I have to use a downspiral or the narrow sections will start to lift. Sometimes I can only get one or two grids for large windows on a sheet of $40 PVC. One boogered spot and the whole thing is trash.
From the original questioner:
I'll have to get some straight O-flutes if parts like that lift, I guess. The guy at the plastics place did have a good suggestion. He said some shops will put app tape over the backside of the sheets, then just cut down to the tape. You don't lose vacuum that way, I guess. I cut for a sign company, so if they send another project like that, I'll have to see if they can put some on to help hold everything.
From the original questioner:
Yesterday I used an Onsrud 1/16" upspiral O-flute on 3mm Komatex. Everything cut really well. I actually cut down to .01" on the first cuts, then came back around and went .002 into the spoilboard. No rewelding at all. Had to tab some really small parts. Ran it at 80 ipm, about 19,000 rpm. Did not use my dust collector, as I was afraid some of the untabbed smaller parts might lift. Next time I might use the DC on the first pass and cut it off for the cut-through pass.
