Official Luthiers Forum!

I'm having a terrible time getting dialed in on shell cutting using these bits from precise bits:

MS3I8-0100-006F 0.0100 in. (0.254 mm) 3-flute optimized natural shell cutter, 0.020 in EFL, 0.060 in. max reach

I have followed the recommended feeds and speeds they posted on their site - depth of pass .005, RPM 24000, Feed Rate 1.5 IPM (they recommended 4) and still I'm breaking the bit after a very short time. I'm wondering if I should invest in a higher speed spindle rather than the router for this, or is there something fundamental I'm missing? I've already RTFM over and over to see if I missed something, but I'm stacking up bits like cord wood now and need to resolve this....

Suggestions? thoughts?

Thanks in advance....

_________________
Mitch

Have you tried the 4 ipm @ .005?
If you go too slow you can pack the cut full of shell dust and overload the cutter as it cant clear the dust fast enough.

_________________
Jim Watts
http://jameswattsguitars.com

I tried 3 ipm and it snapped halfway through the first letter, that's when I backed it off to 1.5 - Seems like it cuts ok until it gets deep into the cut (shell is right at .60) and then it gives up its ghost. I may try some thinner shell to see if that makes a difference....

_________________
Mitch

What spindle or router. Run out might be the culprit.


Sent from my iPhone using Tapatalk

_________________
Ken

Hitachi MV12 Router

_________________
Mitch

I use their .025 shell cutting bit, and have never had a problem with their recommended speeds and feeds. I'm actually kind of impressed with how much I've cut and not dulled the bit!

I was warned by someone on this forum (Don Williams if I recall correctly) to be careful of tir so I measured my router and wound up switching it out for a dewalt which has very low TIR runout. (I do use the precision bits collets as well).

I also use an air chuck or canned air to blow out the paths as it cuts,
Mike

Definitely run out. This could be a problem right from the factory, a worn out collet or spindle taper, dust or dirt in the taper, the grooves of the collet or up inside the nut.

If you want cutters at that scale to survive, you're either going to run so slowly that there's virtually no load on the cutter...really, really, really slowly. And it's going to get chewed up by abrasion and wear really quickly doing this. Or you need to decrease your run-out to tiny, tiny numbers.

Ten thou at a sixty thou depth of cut is a very high profile cutter combined with being insanely tiny. If you've got more than a tenth of run-out then you're absolutely battering it, and you're not going to get less than a tenth of run-out with a router. It's hard to make those cutters survive long even with the right equipment (very high RPMs, 40-60-90K, and very low runout). They also take forever to cut anything, so I always charged accordingly when customers wanted that level of detail.

That 0.01" cutter is 1/40th as stiff as the 0.025" cutter. It's even only 1/5 as stiff as a 0.0156" cutter. Those ratios also more or less correspond to your margin of error with any operating parameters. I'd say try the 0.0156" cutters first and get your bearings and then go to the tiny ones.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

I'm not sure if anyone has pointed this out. I cut shell all the time by hand with a dremel in one pass. You got to have very short cutting shank. No more than 1/16" I use the Best Carbide 531-20312 But then again I use somthing I call a poormans CNC. I don't cut in multiple passes. Just cut on through in one shot. Thinking about get a CNC

_________________
Michael F Smith
Goat Rock Ukulele
http://goatrockukulele.com

Michael there's a huge huge difference in strength between a .032 bit and a .010 bit. The smallest I'll use is a .015. A 1/32" bit is down right durable compared to .010. No way a .010 bit is making it through .060" of shell in one pass by hand and possibly never with CNC either.

Runout is critical for small tool survival and if you want to do it right, needs to be dialed in each time you use the tool.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

Isn't the general rule not to plunge more than 1/4 the thickness of the tool in 1 pass? At .01 it would take 3 passes to cut a human hair..

Ok not really.... but.... you know...

No, that's definitely not the rule. 1xd (diameter) is usually no problem and often we'll do 3x and even 5xd depending on the job. Obviously feeds have to be reduced for this to work. I routinely run my .024" fret slot cutters at .080 doc with no problems. I just have a hard time believing a .010 will do .060 DOC in shell as I know that a .015" cutter won't!

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com