Official Luthiers Forum!

Apologies if this has been addressed before but I wanted to ask how sensitive the kerf tolerances have to be when fretting a fingerboard.

The reason I bring up this question, is that a co-worker here has offered to mill my fingerboard for me using his Roland MDX-500, only thing is that his smallest bit has a .028" dia. which is 0.005" more than what seems to be the standard kerf width used with fret wire. The fret wire I am planning to use has a tang width of .020" and a stud width of .032". My main concern is that there will be enough meat for the studs to bite into when being set.

Now another thing that I was curious is, if having kerf is not all that bad in the first place? I have heard about the the fret barber tool from stewmac that is used to shave down the studs a bit so it doesn't warp the fingerboard as much when being installed. Maybe having a slightly larger kerf may be beneficial if this is the case. I'm also not opposed to gluing in the frets either if that would help. I've read in a few threads that some luthiers do that as well.

The wood being used if that is a factor is African Ebony. I think its a wonderful opportunity for me to have it milled, I built the 3d model already with fret distances accurate to a millionth of an inch, so it would be a shame not to make use of model I made. I don't think I could manage tolerances that accurate on my own even with a commercially available fret template.

Thanks,
Greg

The ideal thing would be to have your co-worker mill some random slots in a scrap piece of ebony, pound some frets into it and see how they bite in.

_________________
Jordan Aceto
Ithaca, NY

By stud width I assume you mean barb width.

If the barb width is .032" and the slot is .028" that means tht each barb has an interference fir of .002" at each side of the tang. this is just less than half the typical barb interferance expected and it does not take ANY runout tolerance for the bit into consideration. This is way too loose as it is in my books before accounting for any runout or push-off in the bit. And believe me he will have some runout and or push-off and you will have some extrusion toerance in the fretwire to deal with as well. material will build up between the bit and the piece jsut a bit quicker tha the bit can clear it, so my guess is that when he actually cuts a slot the slot will be closer to.030-.031 wide

Yeah barb is what I meant, just seems that a few sites refer to it as "stud width" in there diagrams.

But what your saying about runout tolerances is what I guess my primary concern was. since I am not to familiar with the process or how ebony takes to machining, but I know that when dealing with wood or materials that have the tendency to expand, contract or compress, that there would be subtle issues like that. My co-worker is pretty confident in the precision of the milling machine as he's done optics with it and very fine passes with it. However what he's not too sure about is the ebony itself. What type of bit to use, e.g. carbide, 2-flute or 4-flute, what rpm to use and XY feed rate, if a upstroke pass or contour cut is recommended or not.

Since I am having this milled I figure have it done right, so I wanted to make sure all the variables are considered. If we need to order a smaller bit to do the kerfs, than thats just something we can do. I think we can get one as thin as .015, if need be which should be capable of creating the kerf lines. I guess what my next move is to find someone who's done this before and see if their willing to share any specifics and advice on the matter.

the tolerances i refer to are machining tolerances. While the material will have an influance on the machining tolerances most of the toleraces comes from push off of the bit as it is forced incontact with the material it is cut. if your coworker is a machinest he can explain this to you. There will be a tolerance factored into the final width of the cut caused by run-out of the mill and psh off of the bit. no machine runs with absolute Zero runout or push off. every machine has some. It may be .0001" or less. It may be .005" or more.

.028" is too big. A .023" carbide end mill costs about $10.

"I built the 3d model already with fret distances accurate to a millionth of an inch, so it would be a shame not to make use of model I made."

that's overkill by a factor of about 1000.

_________________
Howard Klepper
http://www.klepperguitars.com

When all else fails, clean the shop.

As mentioned above, bits having 0.023 can be bought (www.precisebits.com).

You could also glue the frets in, for example by weeping crazy glue after the frets are pressed (or hammered) in.

My 2 cents...

yeah I noticed on that website they have a bit designed precisely for cutting kerfs in cross-grained ebony and rosewood. I am sure that would be the ideal bit to use. However its rated speed seems a little fast for the MDX-500 that he has. Using the high speed spindle the max rpm of is around 20K which seems to be the slowest rpm certified for the bit. From what I gather, my co-worker wants to refrain from operating the unit at rpms that high. So he's curious if a slower speed can be used.

Talk to Jeff Silver at Jescar and see if he can supply you with fretwire of the appropriate tang and barb width to suit your manufacturing process.

I know they produce EVO for Gibson that has a .028 tang. I've got some that was sent by mistake.

_________________

------------------------------------------------------
Bob Connor
Geelong, Australia

I went ahead and ordered a couple fo fret cutting bits from precisebits.com, both the .022" and .023". I figure bits that are designed specifically for machining cross-grained ebony or rosewood is probably my best bet. We are going to run a few tests on some scrap ebony to determine which will be the best application for cutting the kerfs as well as what will be the optimal feed rate and infeed rate for the bits running at a slower rpm. After the fact though, we went over to the other building where I work at and in the milling stations they had there, they had bits as small as .005" in dia. But regardless, I figure the bit made for it will be the best bet.

I would have thought a Roland MDX-500 was some kind of keyboard with digital sampling. But I guess it's some kind of cnc mill? Is it capable of running a slotting saw? .023" saw blades are also readily available, and you wouldn't need nearly as high a spindle speed.

_________________
Howard Klepper
http://www.klepperguitars.com

When all else fails, clean the shop.

yeah that what my co-worker thinks, even though the end-mill bits that are designed for cutting the kerfs are CNC certified between 20-100K RPM we can probably get away with running at 11K so long as we don't take as much material off each pass.

Filippo, just to give you a reason for my madness, I am a visual effects artist by trade. So that kind of stuff is easy for me to do. Granted that kind of precision is not necessary for film, but I have done some rapid prototype modeling for practical props and costumes for film. Some of the tolerances I was dealing with were down to the thousands so that the milled pieces formed nicely against the support substructure. When it comes to 3D with computers, its just second nature to me.

Besides if your going to have a piece milled from a CNC machine, one that is pretty much capable of such precision, than why not?

OH yeah, the Roland MDX-500 is a 3-axis rapid prototype milling machine. Its pretty, precise with what it can do. The guy who has it in his office has milled out lenses from plexiglass that had a glass like finish and he said, he didn't even have to polish it. No tooling marks whats so ever, a perfectly smooth surfaces. He's optimistic that I won't even have to sand the fingerboard when I am finished. Which personally I'll believe it when I see it. I do expect to see some faceting because I didn't go too insane with the polycount, only 600K polygons to make up the fingerboard.

http://www.3dprint.no/images/3D%20scan/mdx500.pdf
Interesting machine!
Greg--The accuracy with which the part is modeled on the computer doesn't guarantee by any means that the machine can cut it to that accuracy.
Also running the bit at slower than it's rated speed is certainly no problem. Just slow the feedrate accordingly so that the chip load per tooth per revolution is about the same. It's also a good idea to program "cleanout" passes when cutting ebony with this small diameter bit. Cut the fretslot to about half depth in first pass then a second pass at same depth to clear out the chips before doing the final cut depth. The ebony is really bad about packing shavings in the slot to where even an air blast may not clean them out. Running multiple passes at progressive depths also minimizes the side deflection on the endmill for better slot accuracy.
I have good luck running 25K RPM at about 20 IPM (inches per minute) feedrate in ebony with a .028 diameter.
Nelson palen

Well of course, I don't expect it to, even though my co-worker is pretty much is pitching its accuracy like a used car salesman. However, for me like I said anything for me 3D is second nature, and it was a neglidgeable amount of time spent putting that accuracy in my model. Plus my OCD engineering characteristics wouldn't have it any other way However I am pretty sure there is going to be a certain level of ± with what the machine will be able to do in the final outcome, especially with runout and pushoff that could occur when dealing with such a small bit and a dense medium.

I'll ask my co-worker about the cleanout passes, and let him know about the shavings issue? He was curious when milling ebony, if a upstroke cut could be used or a contour cut. It sounds like he doesn't really want to push much past 15K if he has to on the rpm band just to preserve the life of the machine. So the plan is to take off small amounts of material with a slower feed rate, so it doesn't stress the machine as much and reduces the amount of deflection that would occur.

Yea!!! Some one does understand that the programming accuracy of the machine is not the same as the manufacturing tolerance capability while under load. There is tool push off (which can change due to speed of bit and movement), tool wear, resistance of material, movement of material under load (deflection). These and other factors go into determining the actual manufacturing tolerance capabilities for each part. Not just programming accuracy of the machine.

.001 = one thousandth
.0001 = one ten thousandth
.00001 = 0ne one hundred thousandth
.000001 = one millionth
WOW thats close

_________________
Say what you do, Do what you say.

I have been in precision machine manufacturing for 35 years there is no machinist gauge tools that can come close to measuring .00001” more less .000001” to measure those kind of dimensions requires an electron microscope. A tolerance of .0005”+/- is considered an exceptionally tight tolerance to manufacture to. .0001” +/- is considered extremely tight.

Anyone that says they can machine to .00001”+/- tolerance is going to have to get out their calipers and prove it to me. (good luck with that ) Anyone that says the can machine to .000001”+/- tolerance is just plain loonie toons

Sounds like I got in when you got out michael
On a good day if the moon is in the right phase, the winds out of the right direction, I part my hair on the right side and hold my tongue just right I can hold +/- .0001

_________________
Say what you do, Do what you say.

Michael is quite correct about the difference between software and hardware. Despite the software claiming accuracy numbers which are very small (easy to do...you can always add more digits in software) the actual hardware accuracy spec is only 0.004" with no load, and it's going to be worse under load. That's in contrast to a mill where the accuracy is 0.0002" (and something close is achievable).

That said, this is woodworking. You should get a usable slot with the Precisebits cutters, and they can be run at least as low as 10K RPM though they do tend to work better at higher speeds. Chip load becomes less important than edge speed when you're talking tiny cutters as the game changes down there. If you're going through all this effort then you're not in a giant hurry so I'd say just do the safe thing and take a lot of small passes.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

You're already talking in crazy terms, too! Just for reference, a machine like a Fadal or a Haas can only pull off 0.0005" in very controlled, careful conditions, with expert programming, setup, and operation. A machine that can pull off 0.0001" in a cutting operation is a machine that very few machinists or engineers will ever get the chance to see or touch in their working lives.
(In milling, of course...when it comes to turning and grinding it's a bit easier to pull off tighter tolerances as you're dealing with fewer axes)

In 'real world' 0.005" is what a lot of stuff is made to and 0.001" is considered precision machining. In the real world, on most projects, it's a real hassle to get a CNC mill to hold 0.001" over a whole part and it's an equal hassle to get a CNC router to hold 0.005" over a whole part.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Ask the guys at NASA, I am sure with the hubble telescope, they were hitting tolerances that close with the mirrors, if not more so.

But yes it is loony for that kind of tolerance when dealing with this application. I just wanted to see how accurate my software can get, since its 3D animation software and not CAD/CAM software. All my measurements are actually within the thousands so for a kerf width I am using .023" not .022999" or .023001", all very unnecessary, but I was having fun modeling the fingerboard in 3d, so what ever. If its off by a couple thousandths, I'm not going to loose any sleep over it. Besides the smallest step that the MDX-500 can do is a .000039" so its incapable of that level of accuracy.

I am sure with wood the tolerance is looser. But with steel we mill and lath turn parts with in +/-.0005" day in and day out. But you are right 90% of our precision parts are more like +/- .005" and common machined parts are +/-.010”

Thats the plan, rough pass with a larger bit, rough pass with smaller bit, fine pass with the smaller bit which will cut the kerfs with a boat load of passes.

Didn't Hubble not work at first and require a space walk or two to repair it?

Sheesh, now I wish I never opened my mouth about my measurements.
indeed, it was because it was 2.3 micrometers off from the required shape, which is a little over 90 millionths of an inch. So yeah you got me on that one Hesh!
Side not my grandpa worked on that project, I don't know exactly what his contribution was. It was unfortunate he lost his eyesight before the first pictures came back from the hubble.