how to use a 1/32" bit

[ks2]

Hello
I need to use a long reach 1/32" end mil to cut some smaller letters out of some 1/4" thick pine. The questions are, does anyone have a suggestion for durable brand name to purchase from and had used personally and are there any tool path strategies that any one could recommend.
I did buy a bit and it was cutting fine until it plunged straight down at one of the corners and snapped off.
I was cutting a simple profile with a depth of.09 per pass, no ramps or the such was used.

Any thoughts?

Thanks
Ken

[Adrian]

The smallest I've used is a 1/16" and I would never cut with that without using a ramp. I found the best strategy for me (although I was using plexi rather than pine) was to use a spiral ramp with a 1/8" pass depth.

Do you really need a bit that small? The letters must be tiny.

[mezalick]

Ken,
Can you post the file ?
I would look at the toolpath, ( you know, the blue lines that show the cutting pattern ) and rotate the 3-D image, or look close at where the bit plunges.
If it's the program, you will see that effect.
It may be a different issue.
Michael

[sailfl]

I have cut with some 1/16 and 1/32 bits. I buy the cheapest I can because in my experience they are going to break. You have to go slow on every thing. I cut some PVC material with the small bits but not much wood. Take your time.

[ks2]

Hello
The letters aren't necessarily tiny, but I thought that using that size would give me the greatest detail in the inside/outside corners.
I did think that some kind of ramping would help. I can cut with the stubs all day without breaking. Just the longer necks on the long reach don't fare so well.

Thanks

[sailfl]

If you can use an 1/8" bit without problems, I would use it.

[FixitMike]

If you must use a 1/32" bit, first do a roughing cut with a 1/8" bit. For sharp inside corners use the V-Carve toolpath with a V bit. I like to use a 60 degree V bit.

[Leo]

Richards Micro Tool
Harvey Tool

These Guys do tiny tools ONLY

Criterion has small tools too.

Pine huh? Sometimes those softer materials are more difficult to cut than harder materials like Maple.

I have cut brass successfully with a 1/32 end mill

Sometimes it is just easier to "finish" the job off the machine.

A good SHARP chisel - or a SHARP gouge, or a knife.

I will often make a special tool out of a piece of oak with 220 sandpaper glued on.

[dond52]

I use Harvey Tools quite often.
I machine a lot of 360 Brass.
I rough the outside contours with a 1/16 " dia. endmill offset .005 " to .010"
Then follow up with a 1/32 " dia. endmill.
I cut through .150" depth. I have the cutter set to .010 depth of cut at 4 ipm and use a spiral ramp.
I have also found that conventional milling works much better for this than climb milling.
The tool number I use from Harvey Tool is #34631
It is an 8x meaning it's reach of cut is 8 x's the diameter.
They also make them with a longer reach as well , up to .775 overall reach
The tools have a .046 length of cut.

[Paul Kierstead]

Disclaimer: I am total CNC n00b. However, I'm not a router/wood n00b.

On plunge into wood, bits can deflect quite a bit. I'd suggest you look at lowering your plunge rate, since that seems to be where it broke.

[ChrisInEstes]

Your 0.090 pass depth seems awful deep for a 0.0313 Dia. bit in wood. My general rule of depth-per-pass in wood is 1:1... So, if I had to use a 1/32" Dia. bit, I'd go 1/32" deep per pass.

Chris