Milling PVC

Hi all, I'm trying to mill 1.7" thick PVC on a 5 axis router. I am not able to dial in the speeds and feeds for high speed steel cutters. I've searched and all I keep finding is sharp tools, slow rpm's and high feeds. That's great but doesn't really give me a starting point. Can somebody help me out with some actual numbers (SFM, IPT, etc.)? I'm using .625 dia. 3 flute high speed steel endmills and the cuts involve basic 2D contours and some 5 axis milling. Using suction and a few screws to hold the work piece and have a 20,000 RPM spindle. Any help would be appreciated. Thanks in advance.

I think it's going to vary a lot depending on your setup. You'll be material limited, not cutter limited. That's to say the cutter will be happy at max RPM and feed, but your material will likely melt and stick to the tool, unless you have enough airflow to keep it cool. So what you'll be able to get away with will depend on how deep you're cutting and how much air you can get into the cut to cool it off. Only solution is to try something and adjust.

If your cutting dry, try a starting point of 600sfm, and .005"/tooth then increase feed until either finish is unacceptable or stuff starts moving. a simple mist setup will be helpful to you. I prefer uncoated Aluminum specific carbide endmills they will keep a sharp edge longer in pvc than Hss. Watch out if plunging if you get any chip wrap stuck on the endmill it will melt up the top of your cut. Beware Pvc fumes are not good for breathing. And the chips can build a static charge in a dust collector if you use one.

If your cutting dry, try a starting point of 600sfm, and .005"/tooth

Click to expand...

I haven't played with PVC in quite a while, but I'd be starting around 200-250sfm and
.010" a tooth.

Plastics always amaze me at how much of a chipload you can take. My "metal" brain
is thinking .005 a tooth and then my "plastic" brain has to kick in and I realize
I can take .040" a tooth. I was drilling some LDPE with a 1" twisty drill a while
back and started at .020" a rev. Kept playing with it, and at .200" a rev it started
overrunning the relief on the end of the drill, so I ran it at .150 a rev. The endmill
on that job was just a 3/8" 2 fluter. Ramping in at 30 degrees and .025" a tooth.

Looks like you are working with a piece of PVC plate if holding by vacuum table. Razor sharp tooling is a must, so is air blast. And beware if you sink that .625 full diameter deep you will need to use the air blast to keep chips out of the cut. PVC swarf does not like to be re cut. The chips are already hot and even the slightest melting will turn your cut into Friction Stir Welding. If that happens your work holding may not be stout enough. Screws fail and get hit by the bit. Sparks fly into the dust extraction system and there is an explosion and fire with deadly fumes. Neighborhood is evacuated and soon helicopters are flying overhead. Teams of men in full hazmat attire roaming around.

Pvc really needs coolant, partly for chip evacuation and partly for the finish.

With coolant, I generally start with maybe 1-1.5 chip per tooth as aluminum recommendation.

Ditch the hss. Use a single flute plastic cutter from onsrud or harvey where possible. I have decent luck with maritool aluminum cutters, but for surface finish, the single flute cutters do the best. The biggest trouble with single flute cutters is that they don't slot cut real well. If you don't have coolant, set up some type of air blast to get the chips out of the hole.

For reference, I run 1/2" tooling at 10k rpm and up to 100-150ipm depending on cutter type. With coolant of course. Especially with high helix aluminum tools you want to remember possible uplift of the part.

PVC is quite similar to ABS, perhaps a tad softer. Both are fairly abrasive to machine so your HSS will lose its sharpness quickly. On an ABS production job I ran a 3/4" carbide mill at 3k and around 120-150 ipm profiling and pocketing. I would start around 2k spindle and 50 ipm and go up from there. Increase the feed until the surface finish is too rough before increasing the spindle speed. As others have said don't think about chip load, soft plastic is totally different to machine. Use a very free cutting mill, aluminum types are ok but those specialty routers for plastic from Onsrud are several levels above aluminum type mills for plastic. Kind of like going from mills for steel to aluminum specific for machining aluminum, a real eye opener. I use 2 fluters vs 1 flute and have had no issues. The only downside of the Onsrud tools is the surface finish on pocket floors is poor. Harvey makes the plastic specific routers too but they are twice the price.

Plastic is usually difficult to hold so that maybe your limiting factor.

I find I can machine plastic twice as fast with flood coolant vs air so prefer flood. Burning plastic is bad for your health, nothing special about PVC in this regard. If you were molding it then it is special, if left in the barrel too long it can go boom.

Run flood coolant and use uncoated 2 or 3 flute carbide endmills. Dont use anything TiAln coated, it will stick to the cutter.

We use this tool: Harvey Tool

8000 RPM (machine max ) and around .020 IPT at full slot. You can drill with G00 on a Haas, no sweat.

You know you're feeding crazy fast when you get scallops in a slot.