Cutting Melamine for cabinet parts

[ZamcoLaser]

Hello all. I've been running my CNCRP 48x96 for a little over a year and I couldn't be more happy with it. I've been building arcade machines a lot lately and have really been spending money on bits and trying to figure out the right feed and speeds to get the best results with cutting melamine.

Does anyone here have any experience with this stuff? I'm cutting 3/4" with It seems to really be a bit hog and I'm only getting 2 sheets or so out of a 1/4" compression bit (24,000 at 75ipm) The cost of bits is eating into my profits on these things. I've tried the fancy 1/2" three spiral compression bits and I'm getting about the same results.

any tips or help is appreciated!

Z

Similar Threads:

• Very Weird Cutting Problem Melamine MDF
• Cutting 1/4" thick melamine with MDF core
• CRP4896 for cabinet parts
• Cutting Melamine
• cutting cabinet parts

[ger21]

How fast is your machine, and what size spindle do you have?
You're cutting too slow, at too many rpm's.

A 1/2" 3 flute compression bit needs to cut at about 1200ipm and 16,000 rpm for maximum tool life. You can probably get 100 sheets from one bit, but you'd need a $75,000 machine to do that.

I'd use a 3/8" bit, at about 13,000 rpm and 200-300ipm, if your machine can do it.

With a 1/4" bit, I'd try doing it in two passes, at maybe 18,000 rpm and 200-300ipm.

I've cut thousands of sheets of melamine, but on a much bigger machine. Normally at 700-800ipm with either 3/8 or 1/2" tools.

[Inverted CNC]

Hello all. I've been running my CNCRP 48x96 for a little over a year and I couldn't be more happy with it. I've been building arcade machines a lot lately and have really been spending money on bits and trying to figure out the right feed and speeds to get the best results with cutting melamine.

Does anyone here have any experience with this stuff? I'm cutting 3/4" with It seems to really be a bit hog and I'm only getting 2 sheets or so out of a 1/4" compression bit (24,000 at 75ipm) The cost of bits is eating into my profits on these things. I've tried the fancy 1/2" three spiral compression bits and I'm getting about the same results.

any tips or help is appreciated!

Z

Hello all. I've been running my CNCRP 48x96 for a little over a year and I couldn't be more happy with it. I've been building arcade machines a lot lately and have really been spending money on bits and trying to figure out the right feed and speeds to get the best results with cutting melamine.

Does anyone here have any experience with this stuff? I'm cutting 3/4" with It seems to really be a bit hog and I'm only getting 2 sheets or so out of a 1/4" compression bit (24,000 at 75ipm) The cost of bits is eating into my profits on these things. I've tried the fancy 1/2" three spiral compression bits and I'm getting about the same results.

any tips or help is appreciated!

Z

I had similar problems with horrible bit wear all though with different materials. Was able to track it down to a lack of rigidity that allowed the entire z carriage to wobble in the y direction. For how much mass this machine has (an older pro 24x48) and how substantial its construction the y hardened rails flex between the mounts. I doubled up the mounts then even tripled the number with incremental improvements but never entirely was able to stop the flex. A tiny amount of flex in those rails gets hugely magnified by the time you reach the tip of the endmill. Unfortunately I moved on from that machine as a result.

[jon8949]

Not knowing your machine it looks like your feed rate is too low, which gives you a low chip load. Are you running a spindle or router?

[ZamcoLaser]

wow you guys are fast at replying. Thanks!

I'm using a 2.2kw spindle with the CNCRP Pro machine.

So I need to try speeding up the cut and using less rpm? I'll give that a shot and see what happens. I can get fine cuts with the regular mdf or plastics and die bond materials, I've just been having issues with this melamine stuff.

[Tigerflyer]

cutting a bigger chip is what pulls heat away from the cutter. Heat is what reduces the cutter life more than anything else.

I would increase the feed rates if you can... if you are running near the top of your machines capability... reduce the rpm.

There is some trade off where you are flexing the bit too much and your cut quality will suffer... but you want to push as close to that as you can while you still get a good quality cut. Something to play with.

I run my 1/4" 2 flute bit at 15,000 RPM and 160-200 ipm in MDF

[Andrew22]

Hello all. I've been running my CNCRP 48x96 for a little over a year and I couldn't be more happy with it. I've been building arcade machines a lot lately and have really been spending money on bits and trying to figure out the right feed and speeds to get the best results with cutting melamine.

Does anyone here have any experience with this stuff? I'm cutting 3/4" with It seems to really be a bit hog and I'm only getting 2 sheets or so out of a 1/4" compression bit (24,000 at 75ipm) The cost of bits is eating into my profits on these things. I've tried the fancy 1/2" three spiral compression bits and I'm getting about the same results.

any tips or help is appreciated!

Z

You're cutting really slow which isn't going to help your bit life. Check what your ideal chip load per tooth should be, I typically go between .003" to .005" to get a good quality cut on mdf


Sent from my iPhone using Tapatalk

[ZamcoLaser]

so I updated some settings on my drawings and boy where you guys right. I feel kinda dumb. haha!

This melamine is cutting great, and a hell of a lot faster than it was. So thank you for your help! I should have asked this sooner.

[dgage]

What settings were you running and what did you switch to?