Diamond tooling on laminate

Tool life and feed rates when using diamond tooling to cut laminate. November 7, 2001

Question
Can diamond tooling help with tool life on cutting laminate? I've heard you have to reduce feed rates to use this tooling. Is this true? What feed rates can we get? We're using 1/2" compression bits now.

Forum Responses
Diamond tools will very definitely last many, many times longer than carbide tipped or solid carbide. And don't run them any slower! The geometry of a diamond tool is very similar to that of a compression spiral. Running a bit fast helps to keep it cool, and that helps tool life. Without knowing how fast you go now, I'd suggest you turn the 1/2" bit at 15000 rpm and feed it at 350 ipm (9000mm/min). Increase the feed rate as you feel comfortable. When you get up to 500 ipm, you'll probably want to start turning up the rpm, also.


Diamond tooling will certainly outperform carbide in terms of runtime. But unless you can significantly increase the tool diameter, you'll probably find yourself slowing down. What feed rate are you currently machining at? A 1/2" diameter compression diamond tool will likely be a Z1+1 design, limiting your feed rate to 200-250 inches/min in HPL. A similarly sized Z2+2 carbide tool could easily cut 3-4 times as fast in HPL. But what is worth more to you, faster cutting speeds or longer tool life?

Diamond tooling will outlast carbide in laminate 20 to 50 times depending on your type of laminate. But you can not get anywhere close to the feed rates of a solid carbide compression. We have customers running 1/2" compressions at 1000 ipm 24/7 with great results. A diamond 1/2" router bit will not go more than 300 ipm without snapping off. I have seen many break.

In conclusion, as was stated--speed or long life? Whatever is best for you. My feeling is you cannot sacrifice for speed because your machine time is the most expensive part of the operation. So if you can cut 100 parts/hour with a compression, do you want to go to 30 parts/hour with a diamond? Tooling cost is not much of a factor compared to machine cost, if you look at it that way. The compression is also a lot cheaper and your production is increased.


My experience with diamond was not good. I tried an off-the-shelf compression bit 3/4" OD. This was the manufacturer's recommendation. I'm routing 3/4" melamine and Plam. I followed their instructions as far as feed rate, rpm, etc., and it was chipping in very short order. When they came in and looked at it, they determined that it didn't have enough shear in it and proposed making a custom bit for me.

The bottom line: they wanted somewhere between 700 and 800 bucks for a custom bit. I am currently using 3/8" compression to the tune of 37 bucks apiece, that I get decent life out of. I use them until the cut quality goes south, and throw them away. In my situation it's a no-brainer. Diamond definitely has its place, but it's just not for what I'm doing.

Brian Personett, forum technical advisor



Also cut off pieces that vibrate against the tool. Knock the diamonds off the edge. I tried two and they didn't work for me at all.

PCD vs. solid carbide for panel processing--SC is the way to go. If you run small parts and can't go fast, PCD would be your choice. As a few people have mentioned on .500 dia. machining .750 lam. 250 IPM is max. PCD comes into play when you are profiling an outside or inside detail. Your cost savings would be greater.

I've had a couple of diamond bits. I had to use some Nevermar laminates that would dull a carbide after two parts. They were two flute cheapees, about 280 a piece. (Only one sharpening if the edge is good, but life is shortened after sharpening and $100. These are throwaways.) I was running max feed (472 imp unfortunately) and 17,000 rpm. They worked great for quite a while.

The only problem was a crappy PB core. PB is not always free of foreign objects. I've seen clumps of reddish matter, and I've heard of nuts, screws, sand, dirt and our GM even found a piece of conduit in PB a few years ago. I have seen a few sparks while using carbide in PB cores.

So after a while, the edge of the cutter will chip and leave ridges in the core edge (still cut a good p-lam edge, though). I ran probably 150-200 sheets of 2/s lam until the bander operator said the ridges were a problem (no edge cutter on the bander).

Another possible problem was that I use NBM, chips of laminate in between parts that were not picked up by the dust collector, and trying to re-cut them might also have played a role in the chipping of the tool.

I still use them to cut plywood and other things where the ridges aren't an issue. (Plywood can eat carbide pretty fast, too.)

One more thing: if you cut MDF raw or laminated, go with diamond.


The comments below were added after this Forum discussion was archived as a Knowledge Base article (add your comment).

Comment from contributor K:
I run 1/2" diamond PCD bits on laminated panels - lam on 3/4 core, sometimes both sides. I run it at 18000 rpm and 330 ipm and the edge is perfect and so sharp you could cut tomatoes with it. I have run it at 20000 rpm and 500 ipm with no problems, as well, but usually run it slower just because it is a little easier on the machine.

Related Articles