Feed Rate and Cut Depth for Melamine on the CNC Router

A discussion of CNC settings that work well for machining cabinet parts from 3/4-inch melamine. June 23, 2014

Question (WOODWEB Member) :
With all of the questions and answers on cutting melamine I was wondering if everyone is cutting the whole 3/4" in one pass depth-wise?

Forum Responses
(CNC Forum)
From Contributor B:
We use a 3/8" compression spiral and do it in two passes. A company I used to work for used a 1/2" compression spiral and we would do it in one pass. That is for large pieces. For the small pieces we do an onion skin so it is actually three passes with the 3/8" bit.

From contributor Y:
I use a 3/8 Vortex 3185 viper one pass on 3/4 in. melamine and pre-finished maple vc plywood. All cabinet parts are at 18,000 rpm at 300 ipm. I've cut many hundreds of sheets with this setup (not the same bit) and usually get 60 to 80 sheets between sharpening.

From Contributor E:
The Vortex chip loading chart suggests a 3/8" two flute running 18,000 should be moving around 600/650 ipm. One pass on all but the smaller parts.

From contributor Y:
I also spindle drill my 5mm and 4 mm holes at 18,000 rpm, plunged at 300ipm with solid carbide drills with 10mm shanks. Tens of thousands of shelf and construction holes, been doing it like this for ten plus years. Most all of my CNC tooling is from and sharpened by Vortex.

From contributor M:
I use 3/8 compression, 18,000 rpm, 850 inches per minute, cutting the full thickness in one pass is my set-up. I also get 70-80 sheets before sharpening.

From contributor J:
U use 3/4" melamine, one pass (except very small parts which get onion skin), 18,000, 600ipm, vortex 3184xp (I have not been happy with any vortex bit outside of the xp line) 200 plus sheets and throw the tool away. I don't re-sharpen (not worth the hassle, time, postage, offsets, etc.). I use a CNT motion machine. The same for plywood, but I don't cut enough of that to have a good sheet count number.

If you are running a two flute 3/8" compression at 18k, 300 ipm, you will get longer tool life if you increase feed-rate. I would speculate that your tools are very black on the end. Heat is the enemy of carbide. When I ran 'big-iron' CNC's with very fast acceleration, I could push 1200ipm with the same tool (Onsrud 'mw' series when sharp, but 900ipm seemed best.

From contributor D:
We use1/2" 2 flute compression. 18k rpm, 600 imp. One pass on all parts except small about two square feet or fewer leaves. We use Meisenhiemer bits and get 45-60 sheets. We are cutting mostly 12-16" deep material so there are more cuts than bigger cabinets.

From contributor T:
We have an Onsrud 5x12 panel pro router. We are using Onsrud 1/2" compression bits to cut 3/4" melamine in one pass. Our machine is running at 18,000rpm and 600ipm. We are only getting eight-ten sheets of nested cabinet parts per sharpening. We get about the same number of sheets with a new bit. I see others are getting 40-80 sheets per sharpening. What are we doing wrong?

From contributor J:
If you are running standard (not aluminum oxide finish) melamine, I don't know what to tell you other than try my tooling and speeds listed above. I don't' have a feed chart handy, but 600 ipm on that machine is very slow even if you are only using a two flute tool. If you are using a three flute, you are very slow, probably burning your bits really badly. In my opinion, 1/2" tool is overkill for cutting 3/4 melamine, and you just have more dust, and more expensive tooling. If you are cutting melamine that has an aluminum oxide finish, you need to use a different bit (not carbide).