CNC feed rates for melamine

Concerns on purchasing a CNC router and software for cutting melamine. August 12, 2001

We manufacture cabinets using mostly melamine. I am on the verge of purchasing our first CNC router and software for NBM. I am a little concerned about the quality of cuts and the hold-down capacity with universal vacuum when using melamine. What kind of feed rates can I expect and how much time can I expect from tooling before I get chipping when cutting mostly 1/2" melamine?

Forum Responses
From contributor L:
Presently, we are running our 1/2" melamine at 2000 inches/minute. Average tool life is 150-200 sheets, per sharpening. Keep in mind that two sharpenings is all you are going to get before the bit diameter gets to the point where your cabinets are changing sizes.

The quality of cut using a router is second to none--no more scoring line, edgebander does a better job, etc.

You will get part movement on some small parts. Don't skimp on vacuum. 600 CFM is the minimum these days. Make sure you get a demonstration with melamine at a minimum feed rate of 1600 inches/minute.

From contributor B:
You mention the cut quality being second to none. I'm curious as to what board you are using. With domestics, I see a little fuzzing or pulling out of the center core. It seems to be worse with the Canadian boards. Can anyone address this issue?

From contributor L:
For the bulk of our production, we are using Panval #555 white melamine. I have witnessed some "fuzzing" from time to time, but nothing serious.

Currently, our feed rate is limited by our available vacuum (lesson: more vac is better; careful when listening to salesman!). Cut quality is great. Generally, the faster you run, the longer the bit life. Slow feed speeds and high RPM increase heat, which dulls bits very fast. It's still amazing to me how well the compression spirals work.

From contributor G:
A 1/2" up/down tool will do the job. Our tool will achieve approximately 2400 IPM at 30000 RPMs, with 40 HP vacuum pumps. The tool can be serviced up to four times, but you are required to use the tool offset as the service reduces the diameter. Depending on your part size, the feed speeds must be reduced as well as the RPMs. The tool should be creating a chip (not dust--this will cause premature dulling).

From contributor E:
Am I correct in calculating a 0.040" chip load per flute for your example? That seems high for melamine on chipboard. I will have to give it a try when the time comes.

I also would like to confirm that you are working off chip load independent of RPM. Thus, for a 20,000 RPM spindle, the feed rate would be 1600 ipm?

If you buy a solid machine, good cut quality will be relatively easy to come by with the right tool selections. Yes, compression is the way to go, as it is the industry standard. The vacuum system should be matched to the machine. Make sure the pumps have enough HP and CFM to hold the parts relative to part size and table size. As previously noted, more CFM is better!

Note also the diameter of hoses from the pump to the table. The larger, the better. 4" is ideal. You may find yourself using the CNC for things you never thought of. We have upgraded our pumps three times for in-house material testing and still would like a little more CFM. If only we had more room!

P.S. I believe contributor G is using a 3-edge compression and that he forgot to mention the number of cutting edges. That would equal a chip load of 0.027", which would make more sense for the 1/2 diameter that he noted. I'm unaware of a double edge tool that would withstand that kind of cutting pressure, unless it had a chipbreaker design.

2000 IPM?! I'm running Onsrud solid carbide, 2 flute, 3/8" diameter, at 600-800! Can I go that fast or do I need to change tools? The router can do it; can the tool?

From contributor R:
No, I would not run a DE 3/8 compression at 2000 IPM. It will fail. 600-800 IPM is a good range for that tool. I'm assuming you're at 18000 RPM and most likely in 3/4" material.

Most of the time, tooling alone will not be the only driving force in reaching that kind of speed. As mentioned above, machine issues like part hold-down, chip removal, RPM range, spindle HP and part size come into play.

We do carry a 3-edge 3/8 compression that will get you to the next level (900-1500 IPM), but the core type will most likely be the limiting factor. IE MDF typically runs slower than chipboard. If you are not opposed to moving up to 1/2 diameter, we can push into the 2000-3000 IPM range. But, programmed feed does not always equal actual. You have to take your part size and the speed of the control, as well as programming techniques into consideration.

From contributor P:
To contributors R and G: When we look at the formula for chip load, and calculate using the number of flutes, feed speed, and spindle speed, does the bit diameter not matter at all? Other than the fact that a 1\4 diameter bit will break at 1200 inches per minute, is chip load the same for a 1\4, 3\8 and 1\2 diameter, two-flute compression bit, spinning at 18000 RPMs, cutting at 1200 inches per minute? I would think that diameter has to figure into the equation somehow other than more heat to dissipate in a smaller area.

From contributor R:
Yes, obviously the tool's diameter matters, as well as the depth of cut and material type. It's all too easy for us to throw out excessive feed rates and forget to mention the complete parameters that the tool ran under, like tool diameter, cutting edge length, OAl length, # of flutes, material thickness, core types, etc.

Yes, the chip load has to be reduced in smaller diameter tooling. By how much will matter on too many variables to list. In general, a reduction of 40% for 1/4" diameter and 20% for 3/8" diameter will be a good starting point. Then increase your feed rate until part finish becomes unacceptable and back it off by 10%. Then start reducing your spindle speed until, again, part finish is unacceptable, and increase it by 5%.

This will maximize the chip load on your tool, giving you the best tool life for your application. In the end, we are all looking for the same thing--the fastest cycle times with an acceptable part finish, and the longest tool life. Note: most of the time we compromise one or more of these because of factors we can not control.

From contributor L:
To contributor G: You mention tool offset. Do you change the offset in your nesting program? Or on the controller at your machine?

From contributor E:
Controller! The operator knows what tool is in the machine, and should know the tool's actual diameter. The programmer may not, and should not have to deal with that issue. Of course, if your controller does not support cutter comp, then you will have to deal with it on the CAD side.

To elaborate on the above point, the controller generally has the tool offset table, but the program that produces the tool path must call out the compensation. So the real answer is both. If you are nesting parts that are already tool pathed, then each drawing must have this callout. CV and CW also contain the means to accomplish this.