Cutting Solid Phenolic with CNC Equipment
Pros discuss bit choice, feed rates, RPMs, and more. October 26, 2005
Question
Does anybody have any experience cutting 3/4" solid Phenolic material (in this case made by Trespa USA)? What I'm interested in is feed speeds, tool type and speed and depth of cut - all 3/4" in one pass. Is it possible to do more than one?
Forum Responses
(CNC Forum)
From contributor K:
I have very little experience cutting solid Phenolic, but recently I cut some 5/16 Penolic with a 1/2" 3 flute low helix upshear at 14000rpm and 300ipm. I did not have to cut very many pieces, but the quality of the cut was excellent. Based on my only run, I would figure tooling and feed speeds to be similar to solid surface.
From contributor M:
I run 6mm Phenolic constantly with a profile on the edge. What I do is rough cut with a 1/4" solid carbide bit at 300ipm/18000ipm and then put the profile on with a 5/8" diamond bit at 325 ipm/18000rpm. The cut quality is great.
From contributor E:
You can do this in one pass. Use a 1/2" slow helix ruffer and then a 3 flute compression. Feed speeds with these tools for 3/4" material 1/2 ruffer are 650IPM @16000 rpm. Leave .125 for the compression 1/2" tool at same feed speed.
From contributor L:
I cut a lot of Phenolic, from 1/2 to 1" thick. I am using Onsrud 3 flute ruffers followed by a low helix finisher. We are cutting full 1" in a single pass. Cutting at a high feed/lower rpm will put more of the heat into the chips and not the bit. Far greater bit life can be expected.
From contributor G:
I'm pretty amazed at some of the speeds that the Phenolic sheet is being cut. Do these feeds apply to canvas or linen Phenolic sheets also? I've been cutting C or CE Phenelic for years and have been cutting about 100 IPM with 4 - 5 passes in 3/4" thick material. Ramping into the middle of a sheet scares me a bit. About a year ago an operator went into a thick piece of Phenolic (single pass) and my cooling fan inside the motor (columbo) blew up and I had to replace the whole spindle. You can see my reservations about trying these speeds especially with a single pass. Any more insight is appreciated.
From contributor E:
Many firms have purchased tools meant for another piece of material. Clearance angles, relief angles and the type of carbide a firm uses, determine the quality and longevity of a cutting tool. Even though firms supplying the tools today are learning what type of tools to sell for a certain material, most just want to sell something and hope it works. We also keep track of competitors and a few a have a number of selections in there product mix, otherwise we also would not offer 1000 plus tools for a specific material.
From contributor L:
We cut a lot of 5/16 canvas Phenolic, but these pieces are very small. There are 120 pieces in a 3x4 foot sheet. I am using a 5mm single flute down spiral and I leave .015 onion skin for the final pass.
From contributor J:
Most people cutting Phenolics and solid surface materials on their CNC Routers find they have to run at slower speeds and lower rpm’s than desired. The primary problem is that these sheets want to slide or shift due to the shear force of the cutting tools.
From contributor U:
I cut 1" Trespa all the time. I use a 3flute corn cob rougher. I used to do it in 1 pass 500ipm at 18k, but after a while the tool changer would jam up so I just went two eq at the same feed/speed and just avoid the jamming hassle. I finish with a 3flute up shear at 400ipm @ 17k, and the finish was as smooth as butter.
Keep in mind that if your speeds and feeds are wrong it will leave a burn mark on the material if it pauses for a second - especially with large roundover bits. So lead-in and lead-outs may factor in depending on the complexity of your parts.
The comments below were added after this Forum discussion was archived as a Knowledge Base article (add your comment).
Comment from contributor A:
Depending on the shape that you are cutting, if the router doesn't get to the desired feed rate you will have to adjust your RPM. I had RPM’s at 12,000 running at 250ipm, but was leaving a burn mark on the bit. Now I am running at 6250 RPM with a feed rate of 150. It seems to help considerably. Before I was getting a burn mark at the end of the bit, however that was after cutting a 5x12 3/4" phenolic sheet.
