Excessive Bit Wear when Cutting HPL

A quarter-inch-diameter bit is too small for working with high-pressure laminate, CNC owners advise. January 4, 2014

I operate a Multicam 3000 router for a small cabinet business. We cut 3/4 inch chipboard with plastic laminate glued to one or both sides. My problem is that after 2 to 3 boards, my 1/4 downspiral compression bit will chip the laminate. I run at 18000 rpm and 500 ipm.

Forum Responses
(CNC Forum)
From contributor J:
I don't know what all you are doing with your tool, but without more info, here is where I would start. Calculate your chip load values, and compare against what the manufacturer recommends. Is your tool burnt? If so you are likely at too slow a feed, or too high rpm. Is there a groove in the tool where it hits the laminate? If so you may have a laminate with an aluminum oxide finish. This is what is used to sharpen carbide tooling, but it is in some laminate finishes, and will destroy your tooling very quickly. If your core material has changed, there is a possibility that could affect it as well. A few thoughts off the top.

From contributor W:
I think you might have better results with a larger diameter bit. We use 3/8 compression with good results.

From contributor B:
I take it you are running what we call 2 sided p-lam (3/4 particle core with 2 sides laminated). We route this a lot but we never would think of using a 1/4" tool. We use a 1/2" compression spiral and at times a 3/8" depending on the geometry. 500ipm at 18000 is too slow. We have found that some carbide is more resistant to wear in the areas where the laminate is. That takes trying several different manufacturers. Go up in tool diameter and speed and try a quality tool.

From contributor S:
500 ipm for a 1/4 double flute compression is not too slow, it's probably too fast. Also, you shouldn't go much deeper than the diameter of your tool in one pass. This can lead to unwanted vibration, poor quality cuts and tool breakage. Using a larger diameter bit of a high quality will help significantly improve your cuts and tool life. Try using a straight double flute cutter, 3/8 or more in diameter, not much more than 1 inch in cutting edge length at 400-600 ipm max, cut in two passes or more. You could cut in two passes, leaving the bottom laminate as a "skin," and then come back and remove the skin using long, shallow lead ins.

From contributor J:
If you are doing outside cuts, a 3/8" tool is good. One pass, 18k rpm, ~700-900 ipm (depending on how rigid your machine is) 2 flute compression. I like the Vortex xp series, 3184xp. I get more than 200 sheets cutting cabinet parts in 3/4 melamine, 4x8 sheets running 900ipm, 18000 rpm. Depending on part size/waste, you could use a 1/2" tool and really push it hard if your router can take it.