Diamond Versus Carbide: Tool Life and Production Trade-Off

Diamond bits last longer, but need to run slower than carbide because of overheating problems. December 2, 2011

I have recently purchased a diamond compression bit for cutting HPL on PBC but tried to cut some melamine with it first. It did very poorly, causing most of the top edge to be chipped. The tool is 1/2" diameter with 2 up flutes and alternating single down flutes. There is one spot where the down angle cutters overlap but the majority of the upper cutting edge is singular. The bottom edge seems to be doing fine with 2 flutes cutting but the top is terrible. I'm turning the tool at 18000 rpm and feeding at 6 to 700 ipm. Also the tool is a 20 degree rake for laminates. Any suggestions?

Forum Responses
(CNC Forum)
From contributor C:
Is this tool a diamond coated compression spiral or PCD tipped? 18,000 RPM is usually too high in either case. But, without knowing more, it's hard to say for sure. Keep those collets changed also.

From contributor A:
Based on the information you provided, the up cut section or the down cut section of the tool is not being used. Depending on material thickness and if you have the board good side up or down, you will get chipping on one side if the up/down part of the tool is not in the right depth.

What's the thickness of the material? What is the tool number and manufacturer? What is the depth the tool is cutting at?

From the original questioner:
The upcut edge is 1/8" on one side and 1/4" or so on the other. The downshear edges are alternating 3/8" or so in length with slightly overlapping ends above and below the 3/4" mark. Since I am cutting 3/4" material the downshear portion is only cutting the top surface with one edge, causing it to chip. The tool is a 1/2" PCD from Carolina Specialty Tool and after talking with the rep this morning, he thought I should keep the RPM at 18k but slow the feed to 400ipm or so, raising it until the cut quality drops. Although I purchased the bit mostly for HPL on PBC, I wanted to try it on melamine also. I hope to get this figured out before we cut the HPL.

From contributor S:
The rep should tell you the chip load. Your tool is probably in actuality a single flute tool because it has staggered flutes. I would start at a chip load of .02". So at 18,000 RPM the feed should be 360 IPM. I would start there and increase IPM.

From contributor G:
A PCD tool with 1/2 diameter cuts great at 200-250 IPM at 18000 RPMs. What you gain in tool life you lose in production versus solid carbide.

Form the original questioner:
I had no idea it would require that slow of speed. What if I turned the tool 21 or even 24k RPM? Am I not in danger of overheating the tool? I know it won't hurt the diamond, but can it soften the weld on the mounting?

From contributor C:
You are correct if you run too high a RPM you can get the tool too hot and the diamond will fall out. On average, if a compression is running 600 IPM, I usually see 300 to 400 IPM. Look at the chips to make sure you are getting chips and not dust and feel them to see if they are warm. This shows the chip is carrying the heat away from the tool correctly.

From contributor G:
As mentioned, we have seen the PCD just fall off because of the heat. When someone asks us about PCD in this application, we provide them with feed speeds. 99.9% of the time they will continue with the solid carbide as the price per part versus cycle time is less with SC.

From contributor C:
Contributor G is correct most (after trying) will go back to solid carbide due to feed rates. Diamond tooling is very application specific still, but in the right application, will outrun carbide easily 10 to 1. I have seen a compression PCD tool run for 2-3 months of standard use, not an all out production shop.