I need help with CNC chipping
Its happen just on top part .
I'm using 3/8 chip-breaker bit.
I ready change bit to new one and switch collet and tool holder and clean.
Attached is pictures of part and tool setting
Any idea ?
My other bits make clear cuts

View higher quality, full size image (3264 X 2448)

View higher quality, full size image (498 X 572)

This is picture of bit i using

View higher quality, full size image (1632 X 1224)

I would use a PCD bit on any PB that is laminated. Chipbreaker is not ideal for a smooth finish cut.

Either the tool bit is done or your first pass is too shallow.

PCD is a bad idea on melamine. The ones I've tried do what you have here.

I have 3 flute 3/8 compression bit
but i just check PCD bit is just 1 flute and i think i will need to slow down speed of cutting

What feed rate on the 3 flute? Anything slower than 900IPM at 16K RPM and you're killing the bit.

Here is my setting for 3 flute 3/8 compression bit

View higher quality, full size image (498 X 572)

it could or could not be the bit
we have ran some melamine that
the finish is real brittle & no matter what u use the finish chips like what urs has.
so if u have some older stock u could try a small cut out on it & see if it is eliminated.
then u will know if cutter or finish is the culprit.

I was thinking about that but my regular down-cut bits make still clean cut without any chipping . this is happen just with 3/8 compression bit

If I understand your speeds properly, it looks like your running the 3 flute at 429 IPM. Way too slow.

I also agree about the melamine supplier. I refuse to run certain material for just this reason.

Bob,

That picture does not look like a chipbreaker tool. The biggest problem I see also are feed rates are way too slow. You will have better results with a 2+2, If you are not running a high feed rate a 3+3 is over kill.

Hope this helps,

Do you have any recommendation for settings ?

Bob,

Do you want to stay with the 3+3 or move to the 2+2 (recommended)?

I ready have 3 new extra bits. I like to stay with 3 flute for now

I noticed your pass depth is 9.2 so you need to use 3 passes for 19mm material? What model of router do you have that needs to make 3 passes? I agree 400 in min is way to slow for that tool. I start out at 12,000 rpm 30meters min one pass. If you have a light machine maybe you can not do this and need to go to either a 2 flute or even single flute tool.

As for these panels they look like it may be just the finish that is the problem. If you are using multiple passes and the first one is definitely deep enough to get into down sheer, what does the cut look like after first pass?

Bob,

You are going to have to increase your feed rate a lot then. I would start @ 700 IPM and work up quickly from there on feed rate. Keep in mind collets, machine condition, and hold down comes in to the formula also. But, keep in mind that material maybe holding you back also.

Hi dustmaker1 .
I just change setting that is cut in single pass plus onion skin . My CNC is omnitech seleex pal.
Cut looks much better now. and i think that is problem in bit up-cut partion ( i just put new bit) and my gues that is material too . I just order material from new supply . ( material supplier is UNIBOARD )

Uniboard is one of the better melamines to cut.

I would bet that you are cutting the top surface on first pass with the bottom of the tools using up-cut wings.

Now that your cut is better and you are going deep enough, you might consider going to a standard compression bit when cutting 3/4 or 5/8 melamine instead of the mortise compression. The mortise compression will work but the small amount of up-shear means that the kerf is not well evacuated. That means more re cutting of chips, more heat and less tool life.
Some make this sacrifice so they can cut 1/2 inch and 3/4 with the same tool as well as all 1/4 inch dadoes. Just a choice between versatility and tool life.