Official Luthiers Forum!

Precisebits suggests " 20 in./min. full plunge cutting (0.100 in. deep) @ 40,000 RPM." with their special fret cutters, but I've still seen too many of them break doing full plunge cuts even at 60,000 RPM. Outside of production, I'd take it really easy on the DOC and put it at 15-20 thou just to mitigate the breakage risk. Digging one of those cutters out of a board, and paying for its replacement, isn't worth a few minutes of time unless you're doing a big run of boards.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Thanks Bob,

I ran a test last night with my DOC set at .028. I programmed it for 10ipm and during the test I upped it to 20ipm using the feed override feature in Mach. It seems like there was a bit of wandering at the higher speeds but possibly that was only when I was increasing the feed rate. There's also a "dot" at the plunge point (which I'm doing at 5ipm) but that should be hidden by the fret and I can't believe that it would have a significant effect on the holding power.

I can do a 3D entry using this machining strategy in VisualMill (engraving) but the 3D path would cut material outside of the fret slot curve. To do differently would require a manually drawn 3D path which is what I assume you do to limit jerk.

I'm using cheaper bits I found on e-bay - Kyocera at $3 a pop but still, digging one out of the slot would be a bear!

After running my test yesterday, I think the bit probably could handle 36ipm but I'm going to leave it around 10 for accuracy's sake. That and I was running in maple so what works in maple might not work in harder woods.

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

Using the Precise Bits fret cutters, I have been running pretty conservatively at 20 ipm and 20 ipm plunge at 18,000 rpm, but only .02 depth per pass. I have done a bunch of ebony fingerboards using only one bit so far, and the shallow passes seem to make it a lot easier to keep the dust from packing in the slot. I know I could cut deeper and make the process faster, but I'm only running a dozen boards at a time so the multiple passes don't really make any difference to me in speed. I'm not breaking bits and they're not getting hot enough to dull.

I do my fingerboards with fret slots that don't quite reach the edge of the board (the built in binding approach) using V-Carve Pro, and don't have any anomalies in the cuts at all. I use Rhino/madCAM for most of what I do, but V-Carve is great for 2D things like most fingerboards. On arched fingerboards, I go back to Rhino/madCAM so the fret slots can be parallel to the fingerboard surface, but most banjo boards are flat....

Dave

I have good luck slotting ebony with .028EM making two passes to get full depth in an arched cut path.
I follow up with two cleanout passes to get rid of the packed in chips.
Oh, I'm running 24K and about 20 IPM.

Thanks guys. Ran another test board, again at a conservative 10ipm, 028 DOC in hard maple and everything went just fine. I also changed my toolpath so that it's only cutting in one direction i.e. it retracts and goes back to the original entry for pass 2.

I might bump it up to 12 or 15 ipm for my next test just to see how it goes. I'm kinda now wishing I had a 24k spindle but what I have is already such overkill for this type of work!

Oh, and I am running an arched path which also seems to work great. The engrave feature on visual mill is under 2.5D but it's actually 3D - whatever path you draw, that's where it cuts.

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

Andy, I'm not at my desk but doesn't the engrave function have a 3D entry along path option or angle entry option?

It does, the problem is that the 3D entry starts outside the engrave path and ends at the start of the engrave path. I'm doing a faux-bound fretboard so the 3D entry would ruin the edge of the fretboard. You can see in the attached screenshot.

Unless there's something I'm missing, I don't think it will work right. You can also see that it doesn't do it for every plunge, just the initial one which is also a bit weird.

I think VM is a "bargain" compared to other full blast CAM packages but in the end, you get what you pay for!

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

Use a straight entry and play with the entry angle. EG 20 degree entry slopes into the cut from the outside of the neck at a 20 degree angle. A 140 degree entry angle slopes in at a 20 degree angle from the center of the neck.

Once you find the angle you like adjust the length so that it starts above the work piece.

You ARE a god among men.... lol.

_________________
"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."

Any way you slice it (or cut it I suppose!) using any path other than vertical, the cutter will touch wood outboard of the saddle slot. I think the only way you could do it is if the plunge was along the path of the fret stlot. e.g. you could start a 1/2" inboard of the stop and cut outward to your plunge depth and then reverse directions.

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

Andy, in most cam software when genning toolpaths you can specify the node that you want as the start point. IF VM has this feature then add a node inside of your slot for this purpose and ramp into that node.

Just an idea.

_________________
I'm outside looking in, just farther from the window than most.

Mike, nothing like that jumped out at me but it may be a possibility. It's not that big an issue though as I ran another board with a slightly different tool path and after going over the slots with a triangle file a touch to get rid of the fuzz, the dots were pretty much gone.

I think to do a 64 second slot job, it's a lot more critical. At my ultra slow 10 ipm, it's o.k. If I have some time, I might do some experiments down the road to see just how fast I can go at my current DOC and still maintain accuracy. Also if I go to the T&T bits, I could probably speed up as well.

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

I understand Andy. I just wanted to give you a possible avenue to look at.
Mike

_________________
I'm outside looking in, just farther from the window than most.

Adding a small chamfer to the fret slot will greatly help when fretting. You can run a .04 - .05 ball down the middle for the first pass and that also removes a little depth material for the delicate end mill which follows. Course....that could be pain without a tool changer....just an idea.

_________________
I read Emerson on the can. A foolish consistency is the hobgoblin of little minds...true...but a consistent reading of Emerson has its uses nevertheless.

StuMusic

That's what I'm talking about.

What benefit do you notice when you changer the slot edge. I've tried with and without and couldn't tell the difference. I've always used a .025" slot though.

You run a wider slot than I do (.023") in hard woods (.022) in softer woods like maple. A .025" slot would be considerably easier to start a fret into...but a .023" groove in cocobolo makes for a pretty hard time getting it started. The chamfer helps right at the intial point of entry. I only do about a .01" chamfer. I use a .04" ball at a .02" depth and that leave a tiny chamfered edge after slotting.

After thinking about it last night though...a better plan might be to use a .03" ball at a depth of .03"-.04" before finsihing off the depths with the .023 cutter. That might help the tang find a straighter path downwards. I'll probably try that next time.

_________________
I read Emerson on the can. A foolish consistency is the hobgoblin of little minds...true...but a consistent reading of Emerson has its uses nevertheless.

StuMusic

What about using like a v-grooving or bit to do the chamfer? It only takes a couple minutes with a triangle file but I could see if you're doing dozens it would be nice to automate it.

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

That would be just as good, imo. In fact, a moderately tapered end mill might be the best call here as long as that cut isn't so deep that it widens the fret slot where the tangs actually grab. Course, I'm not sure I've ever actually seen tapered micromills so maybe that's just a dream.

I think the .03" ball cut to a depth of .04" off the surface probably achieves the best "fret starting effect" with the normal cutters in our generic arsenal. Though I'd study the tang depth issue prior to assuming that .04" depth is valid....to be sure there was an adequate amount of material left for the tang to grip.

_________________
I read Emerson on the can. A foolish consistency is the hobgoblin of little minds...true...but a consistent reading of Emerson has its uses nevertheless.

StuMusic

Yep. I think I could make a macro (either in Solidworks or Rhino) to generate them, but since it's only for production I do them by hand. It's only worth the time if I'm doing 25-50 fretboards.



I think you mean -very- fiscally motivated . It was setting up for a 6000 board/year contract with a Gibson subsidiary that sadly got canned when the recession hit, and I had to beat the price they could get from Asia while charging local hourly rates. Having that one go down in flames, after terms and pricing were agreed to no less, is the biggest sore spot I've got in my entire business career.



Getting the question out there never hurts, though! You can get them here:
http://www.harveytool.com/cat/Miniature-Tapered-End-Mills/Miniature-End-Mills/Products_131.aspx

If you end up trying then, let us know how it goes!

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

I was looking for something else and found these: http://www.stewmac.com/shop/Inlay,_pear ... r_Bit.html

Interesting.

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

Nice but they fit a dremel tool. Now that you have a cnc you will find that you will also need to watch collet sizes. If you are using say a PC router, you can go smaller down to 1/8" from precise bits, otherwise those listed are useless for cnc unless you use a dremel for your spindle, unless again you get specific size collets for your spindle. say if using an R8 or something taper? .

MK

_________________
I'm outside looking in, just farther from the window than most.

Actually, I have a spindle with an ER-20 taper and a full collet set so I can fit just about anything between 3/32 and 1/2"

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

Just wanted to make sure

_________________
I'm outside looking in, just farther from the window than most.

Those look just like dental drills, except the shanks are longer. Back when I was starting out, I asked my dentist for some of his used tools and he gave me a box with about 50 of them in it. I think he switched to diamond tooling or somesuch because he was throwing away all his carbide.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services