CNC cutting inlay trouble

robbycar

robbycar

Registered
I have a 6090 cnc router which I use for profiling and for cutting inlays and pockets.

I am having a lot of trouble cutting point inlays, today I broke 6 cutters! I'm cutting .5mm depth (.019") at 75mm(3")/min, so it takes a long time!

I am using a .5mm (.019"). The only cutters I can get are 10mm long, and I only need 4mm, so they are a bit flimsy.

Should I not worry so much about sharp points and use a bigger cutter?

Or should I be taking shallower cuts at a faster speed?

Would be grateful for any advice I can get.

TIA!
 
Rob, what material are you cutting for your inlays?
Also, a lot of bits at that size are drills and not actual endmills / cutters, hence they have little cutting ability on the sides.
Is that a possibility?
You don't give the rpm you are running your spindle at. What is the runout on your spindle? Obviously, at that cutter diameter, a little bit of runout will result in a lot of wobble at the bit, and that alone will break bits.
Sorry for all the questions and no answers, but more info is needed to help you figure out this problem.
Gary
 
Thanks Gary, appreciate the reply.

I’m running the spindle at 30,000 rpm and the cutters are endmills mounted in a precision collet. I did not consider runout so will check that tomorrow.
 
We cut in a few smaller passes instead of cutting full depth at once and cut many parts without breaking bits.
 
You will have to cut to full depth in several passes, sounds like you might be feeding too fast. Checking runout as you mention is key, If things doesn't spin true that tends to decrease the lifespan of the end mills.
 
You cuemakers rock. i've always got my ear to the road. Thanks for the info and thank you guys for helping out someone trying
 
Use a much larger tool for roughing, and only use the smaller ones for finishing inside corners. .020" and under does not like plunging at all. If you are forced to use tools this small, you'll have to set up depth cuts.
 
10 mm sounds like an awful long bit of .5 mm diameter. If that is accurate it's no wonder they break.

Here are some that are 3.5mm .139" that I use for inlaying my logo and rarely break one without user error.

drillbitsunlimited.com

.020" 0.50mm x .118" LOC Chip Breaker Carbide Router - Drill Point Tip

Get precision .020" 0.50mm chip‑breaker carbide router bits R148: Chip Breaker Flutes, drill‑point tip for PCB laminates, carbon‑fiber composites, fiberglass panels, and phenolic boards. In‑stock—order now for fast shipping!
drillbitsunlimited.com

Sheldon is correct though you need to be using a roughing bit.
 
I would cut the parts out with 1mm or 1.5mm and hog the pockets out with larger bit then clean the edge up with .5mm if MM sizes are what you use. I also would not plunge full depth in one pass.
 
Here are some really basic pockets being cut. .05 for roughing and .02 for finish.
I like to gradually (depth cuts) cut the corners out. Straight cuts into the corners first, then a tiny pocket a couple thousandths shy of finish. The idea being to never fully bury the tool, always come in from a previously cut area. Then do a final pass all the way around at full depth. With no inside corners on the male pieces, you can easily cut them out with almost any size cutter. I would use a .050.

UeuMcMq.png
 
Last edited:
You must log in or register to reply here.
Back
Top