Good morning,
I am looking for suggestions and sources for the tiny bits needed to cut peghead inlays with. I run a shopbot buddy, and have collets for 3/32 and 1/8 shanks.
Thanks, Graham
Good morning,
I am looking for suggestions and sources for the tiny bits needed to cut peghead inlays with. I run a shopbot buddy, and have collets for 3/32 and 1/8 shanks.
Thanks, Graham
Blues Creek Guitars.
http://www.bluescreekguitars.com/sho...v8LNbHumGIkKR0
"It's comparable to playing a cheese slicer."
--M. Stillion
"Bargain instruments are no bargains if you can't play them"
--J. Garber
Thanks Mike. Just ordered some.
I found some even smaller at Bits&Bits.
Graham
I get .016" and .020" bits with 1/8" shanks from drillbits unlimited.
Last edited by Jimmy Kittle; Oct-30-2017 at 10:42am. Reason: typing error
I get all mine from Precisebits.com. Great selection and very helpful. There's tons of useful info on the site too, if you're new to this kind of thing. They have endmills down to 0.01", which can be useful for getting into tight spots, as long as you don't break them
Andrew Mowry
Mowry Stringed Instruments
http://mowrystrings.com
Also visit me on Facebook to see work in progress and other updates.
Thanks guys.
Another thumbs up for Precisebits here. And for buying extras. You might want to consider the precision collets that they sell. They are really important if you're going to be cutting with the little tiny bits.
Dale Ludewig
http://www.ludewigmandolins.com
I use to cut with 12 thou bits (.3mm), got sick of them breaking, went 20 thou bits (.5mm) modified my files to suit and have not broken one since, average 40hrs of cutting per bit before they go too blunt.
My point, just don’t go too small, they break really easy at .3mm
Steve
d
Do any of you folks have a suggested speed to turn them? How slow do you cnc guys move the spindle when using these tiny bits?
Thanks, Graham
I have a dedicated machine for cutting pearl and shell, pass depths .1mm a a time, spindle speed 10k
Pics, bottom of this linked page
http://www.mirwa.com.au/Our_Facility.html
Precise Bits has a great table for speed settings for each size bit and type of material.
Steve
Thanks again. Mirwa, that is one very impressive shop.
Graham
Steve. Just went through 100$ worth of bits in 2 days. Thought I had it fixed. Just looked at the chart. Thanks.
Thanks James
Ouch, that hurts, what width?
Steve
.0156. 3 flute end mill. Precise Bits #MM318-0156-006F.
Would you like advice on feeds and speeds? With a .015" end mill, I would be running at your max rpm, 24000-30000, and cutting 0.010" depth of cut at 10 inches a minute. That's overly conservative but should work on anyone's setup unless something is really wrong.
Some things to help you keep from breaking cutters:
Start .010" above your inlay and go .10" below your inlay.
Fixture your part really rigidly. Super glue onto PCB board or something and then use acetone to separate, sometimes you can pop them off with a really sharp chisel
Oil your collets and keep them in good condition. Runout will destroy cutters.
Use good CAM to generate your paths.
Unnecessarily conservative ramps can break cutters. Ramp in at the same speed you plan to cut, and at about a 10 degree angle.
Zero your cutter accurately. Use a good quality tool setter or built-in probe if possible. If not, use a continuity mode on a volt meter and connect it to the cutter, then to a 1-2-3 block. That will get you very accurate (within the intrinsic error of your CNC setup) tool zero with minimal cost.
And, one post by Marty shows how much I don’t know about any of this.
I know what those words mean individually but not when they are put together in that order. :^ p
Pete Braccio
"The Rules: Play nice and don't run with scissors"
http://www.braccio.me
Check out my web site for:
Jack Tottle music files
BBC Virtual Session files
O'Neill's PDFs
ITM Tunebooks, and more
Thanks Marty
All great info from Marty, as always. The one thing I would add that I also do is slow down the acceleration on my machine when I'm cutting inlay (I think it's around 2"/s^2), so it's not jerking the end mill around too much. For zeroing my Z I use a 1/8" calibration blank on the phenolic backer, so I'm consistently cutting a bit into the backer, regardless of shell thickness.
I plan on breaking at least one of those 0.0156" cutters when I'm cutting a batch of inlays for five or six instruments, because there's only so much stress those tiny cutters can handle. It hurts the pocketbook, but it sure beats sucking pearl dust for days on end
Andrew Mowry
Mowry Stringed Instruments
http://mowrystrings.com
Also visit me on Facebook to see work in progress and other updates.
Typo. Start .010" above your inlay and go 0.010" below your inlay.
Another important point is to surface the thing you're using to hold down your parts. A perfectly flat surface to place the inlay on will improve the accuracy of the resulting parts.
It will also prevent broken cutters, since a non-level surface is likely to cause your bit to break.
PreciseBits recommends 20in/s^2 for tiny bits in soft media. With shell, that 2"/s^2 is probably giving you some benefit, and the stuff is so small it's not really slowing anything down.
The only thing I would warn about is if you set the accel too low on a stepper-driven machine running Mach3, you will actually end up not following the path, and it might be worse than keeping it at its recommended accel. With your fancy encoder-equipped machine, of course Andrew, you can get away with whatever accel setting you want. But there are still people out there running Mach3, so just wanted to say that slower is not always better.
Andrew Mowry
Mowry Stringed Instruments
http://mowrystrings.com
Also visit me on Facebook to see work in progress and other updates.
What does ^ represent?
Bookmarks