Official Luthiers Forum!

I finally have my CNC setup and running, with the exception of the t-slot table top for the spoil board to attach to. If you know where I can source the t-slot slats at, I could use the info. The guy I purchased my machine from may not have any available until who knows when.

I am ready to order an assortment of end mills and ball mills. I understand that I want to purchase solid carbide, and mainly 2 flute if I am going to be milling mostly wood. I could use some input from you guys that have experience as to what is really needed. I want to be able to cut just about anything without having to order mills. Here's what I was thinking to purchase:

4 - 1/16" 2 flute end mill
4 - 1/8" 2 flute end mill
2 - 1/4" 2 flute end mill
2 - 1/2" 2 flute end mill

2 - 1/4" 2 flute ball mill
2 - 1/2" 2 flute ball mill

2 - 1/8" drill mill
2 - 1/4" drill mill

I could also use some advise on brands and suppliers. I was going to purchase all my mills from ridiculous carbide, and get all of them as the aluminum cutting mills, but I can't get in touch with them for some reason. I can't get through to their phone, and they don't have an email address listed.

_________________
Jason McGowan
M&S Guitars
_____________________________
United States of America, looks like another silent night
As we're sung to sleep by philosophies that save the trees and kill the children....
Casting Crowns

Hi Jason,

That's not a bad set but, I'm going to give the same recommendation we do to the new luthiers in the main section of the forum when they give a big list of tools asking for feedback before they've even built anything: buy what you need as you need it!

That said here's some thoughts on how I use what you listed:


4 - 1/16" 2 flute end mill - I use these almost exclusively for saddle slots and bridge pin holes. Too big for inlay, too small for most other purposes.
4 - 1/8" 2 flute end mill - also a low use bit.
2 - 1/4" 2 flute end mill - Work horse, I have a number of these on hand at all times. I use both upcut and downcut for different purposes.
2 - 1/2" 2 flute end mill - good ones are pretty expensive so I tend to avoid these when I can. Usually only used when I need a long reach.

2 - 1/4" 2 flute ball mill - also used often for stuff like bridges. Keep a few on hand.
2 - 1/2" 2 flute ball mill - again, good long ones are quite expensive. I use an Amana core box insert bit whenever I can because inserts are only $8 each. Again, used when you need a long reach.

2 - 1/8" drill mill - meh
2 - 1/4" drill mill - and meh. I did recently purchase a 3/16" mill drill for a particular project and it is cool for bridge pin holes because you can drill and chamfer without a tool change. However, you can't use vacuum for obvious reasons.

What you left out was tiny tools for fret slotting and inlay.

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

another alternative is to get coated hss tools. TiN, AlN, or TiCn. here's why:

-cheaper then solid carbide.

-a bit more shock resistant then carbide in the larger sizes. .125 >

-sharper then carbide. yes sharper. hss is a wrought material and as such can obtain and hold a higher degree of edge sharpness, while carbide tools are made from sintered powder. under a microscope you'll see inclusions at the cutting edge. in your hands you can feel the difference.

-the coatings are very wear resistant and wood is abrasive. run dry and tested to destruction on horrible to machine metals like inconel, stainless, titanium, molybdenum, hastelloy, invar, etc.. they are more then a match for simple wood. hss in either t15 or m42 grade can handle a good deal of heat and abrasion and when combined with a coating that is usually rc 72 and higher, makes for an economical combination. in modern cnc programming, using today's high speed milling strategies on aluminum, we'll often rough out the majority of the material with cheap, disposable, offshore coated tools that can take a serious beating then come back in with high end carbide tools to finish with.

-the coatings can help prevent chips from sticking to the tools and provide lubricity at the cutting edge.

when you get down to the smaller sizes under .125 though, then go with carbide for the higher core strength. in either case investigate a coated tool.

your tooling list seems to gravitate towards 2 flute tools. in the smaller sizes, 3 or 4 flute tools have a larger core diameter that can help with tool breakage, but the trade off is decreased chip capacity. also 2 flute tools generate unpleasant harmonics and vibrations in the higher rpm ranges whereas odd numbered flutes cancel each other's vibrations out and can generate a smoother finish on side walls. these harmonics can sometimes be dialed out by dampening the fixturing or by finding the harmonic frequency range of the machine and staying away from that rpm area. a quick and dirty test is to place a indicator point on the rotating spindle and the base to the machine and run through the rpm ranges. look for the rpm the shows the most movement on the dial. write that speed down and avoid that range when programming.

fwiw, true aluminum specific tools generally have a high helix, 35 deg and up. this is the amount of spiraling that the flute has ground on the tool. they are designed this way for fast chip evacuation, high feed rates, and a high rate of shear in side milling applications with non-ferrous metals. the down side is that they have significant "pull". meaning that if your part isn't fixtured down firmly you run the risk of lifting it off the table and throwing it, or pulling the tool out of the collet, or on a less then sturdy diy machine pulling the head downward. this would be something to consider when pocketing pick ups, tremolo pockets, neck pockets, or full depth cuts on the outside body contours in a solid body electric for example. but not a big issue in shallow depth of cut or open surfacing projects like bridges, the backs of necks, fingerboard surfaces, etc...

for inlay pocketing i'd look for reverse spiral tools. yes you can drive chips down to the floor of the pocket and get some re-cutting going on, but the advantage of a clean pocket lip is worth it imo.

btw, what kind of machine do you have?

sorry for the wall of text but as an mfg engineer i get fired up about cutting tools and machining!

My workhorse bits are a 1/8" spiral upcut and downcut bits by Whiteside, which I usually buy at Woodcraft or online. I also use their 1/4" upcut quite a bit. Other than that, I use a bunch of smaller bits for inlay, and larger carbide endmills for other work. I get my ball end mills from American Carbide, but there are plenty of places that are inexpensive for this stuff. I also use a large diameter bottom cleaning bit from grizzly for spoilboards and truing up surfaces of vacuum fixtures.

_________________
"I want to know what kind of pickups Vince Gill uses in his Tele, because if I had those, as good of a player as I am, I'm sure I could make it sound like that.
Only badly."

Andy, top notch advise as usual! I think I'll go through that list and carve it down some on the least used bits, and then add some for inlay.



The main reason I was going to purchase these is I plan to do some aluminum cutting, lilke parts for my cnc and whatnot, which will need chamfered. Maybe I could get away with just an 1/8" one?

_________________
Jason McGowan
M&S Guitars
_____________________________
United States of America, looks like another silent night
As we're sung to sleep by philosophies that save the trees and kill the children....
Casting Crowns

You know, I've seen people mention HSS tools here and there, but I thought carbide was superior so I never even thought twice about it. I will most definitely be looking into it now. This is why I love this site. So, as far as tool life goes.. Will the coated hss tools last as long, and stay as sharp as the carbide? Also, you said that you guys do a majority of the stock removal with the coated hss tools and do final passed with the carbide.. So, would I need to do that with my wood cutting as well? In a production setting, if I can ever get there, a tool change takes time and $$..



I have an Xzero Raptor with a 60"x40" bed and a 2kw Teknomotor spindle. I've been working on getting all of my parts together, and getting the machine built since February. Now its almost time to start cutting.



It is all good! I love all the info.. Exactly the kind of stuff I'm looking for. Keep it coming.

_________________
Jason McGowan
M&S Guitars
_____________________________
United States of America, looks like another silent night
As we're sung to sleep by philosophies that save the trees and kill the children....
Casting Crowns

Hey Don, is that a mortise bit? Grizzly seems to be out of them, but whiteside has an 1-1/4" mortise bit (part #1304) that isn't much more expensive. I wonder if it would do a good job.

_________________
Jason McGowan
M&S Guitars
_____________________________
United States of America, looks like another silent night
As we're sung to sleep by philosophies that save the trees and kill the children....
Casting Crowns

Andy,

What are your most used sizes for this stuff? At Burchet Tool, the smallest endmill is 1/32"

_________________
Jason McGowan
M&S Guitars
_____________________________
United States of America, looks like another silent night
As we're sung to sleep by philosophies that save the trees and kill the children....
Casting Crowns

My most used sizes are 1/32" when I can get away with it. 1/32 is a pretty stout bit that you can get aggressive with. If the corner radiuses are too big, I'll go down to a 1/64" bit. I've not used anything smaller than that yet.

For fret slotting, I use a .024" bit and that seems to work well.

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