Official Luthiers Forum!

Sorry for not being around earlier to answer this one, but you can bet your foot that it was jerk breaking the cutter. Even when machines look like they're moving pretty smoothly, servos with coarse feedback or stepper systems especially tend to be very jerky at the start of motion. In the case of fret slots, a ramp motion is definitely the easiest way to correct this.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

You might want to look at your setup and see if something is loose or out of alignment or something.. I finally got around to making a test run of a ramped entry but did something backward and the first slot plunged at 5ipm and cut a full depth slot, .080", at 5ipm with no broken bit. I then fixed my toolpath and got it up to 22ipm at full depth (in rosewood) still without breaking a bit. I'm using a 2 flute carbide cutter.

I just need to implement this on my fretboard model - it will shave a crapton of time off of my fretboards.

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

Ran my first fingerboard this evening from black locust. Just used tape to hold it down. 20ipm and .020" DOC and 20k rpm. Based on how easily it cut, I think I could have taken deeper passes or amped up the feed. Pretty cool though to have the machine radius, profile, slot, and cut inlay pockets. I like it!

Ken

_________________
http://www.casperguitar.com

Ken,

Congratulations!

Like you I'm still learning and figuring out how to do this. I know exactly that great feeling when it all comes together.
I was just telling a friend how I had been making fingerboards and all the jigs necessary to manually do it.
Process lumber to a blank, thickness the blank, slot it, taper it, radius it, cut inlays, etc.
So many jig, so many tools, etc. So much room for mistake.

Now I can start by jointing one side of a fingerboard blank and (at this point) tape it down to the table of my machine, press start and walk away for a sandwich....

I love it!

Or a slice!

Ken had asked me about my FB fixture via PM but I figured I'd post it here.

I use vacuum and locating pins to keep the FB from squirming while cutting. I did an experiment the other day and with the right approach path, I was able to cut at 22ipm @ .080 depth...not bad. It's going to take a little work on my model to get the tool paths to update but with this new approach, I should be able to cut about 5 minutes off of my machining time.

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

Finally got around to testing slotting today. Precisebits .025" bit, Depth of cut 1X diameter X 4 passes to get .1" max depth. 18,000 RPM spindle speeder, Feedrate from GWizard of 26 ipm. Wenge cut like butter. Really happy with the results. May try doubling the DOC to cut down the time a bit. Air spindle is next but need to hook up new compressor and air dryer first.

That looks good Andy...again, I like to comment you on the great work you are doing with your CNC machine.....

One Question: What type of gasket are you using, and where are you sourcing it from? I am in the process of creating a bunch of new vacuum fixtures, primarily out of HDPE for the moment, to see how they will come out, and I wanted to use some better gasket material....

_________________
-CyborgCNC
http://www.cncguitar.com
https://www.facebook.com/CncGuitar

Thanks,

Couple of things - I've given up on using HDPE for vacuum fixtures. The one in the post works but when it's not bolted to the table it warps like mad. I'm in the process of switching over to the General Plastics Tooling board recommended by Stuart.

Gasket - I use this stuff from McMaster Carr: http://www.mcmaster.com/#8605K42 for the most part but also have some stuff from All Star Gaskets. I haven't used the all star stuff yet but it looks like it will be even nicer for dedicated fixtures. The All Star has self adhesive on the back while the McMaster is just a round section cord. http://www.allstaradhesives.com/prod_dedicated.php

Something else to consider (forgive the shameless plug ) - I'm now distributing a "needle plate" that sits in your fixture to keep workpieces from squirming about while machining: http://www.birkonium.com/product-catego ... omponents/ These have these little needles that dig into the workpiece under vacuum to keep it from squirming. I'm working on some video now to show how it works. I'd recommend the 1mm plates for "normal" hardwoods but for really hard stuff like Ebony go for the .5mm plates

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

Cool website Andy, and good luck! How big are those needle plates? They look pretty interesting.

Dave

Ask and ye shall receive

They're 20mm x 20mm x 3.5mm (made in Italy). If you click on the 1mm needle product there's a print that you can look at as well. The holes they leave are very small.

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

I use the stuff from All Star Adhesives, round cord. The roll I have now might not be from them, actually, might be from a local place but either way it's just closed cell neoprene foam cord. I used to use the adhesive and rectangular cross-section stuff, but I found the cord easier to use and it produces a better seal. Cut a flat-bottomed channel for it just over half the diameter of the cord.

The one issue I had with the rectangular stuff besides any rough edge making a bad seal and kinking at corners was 'roll over' on the edges of the channel. I had to chamfer the channels I put it in to be sure it went down into the channel reliably when compressed. I also originally suspected the flat stuff would make a better seal than the round stuff, but that turned out to be false.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Have you tried round bottom too? I've been using the 1/4" stuff from McMaster in a round bottom and it seems to work well. If flat-bottomed works just as well I'll just go ahead and do that instead.

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

Yeah, only for the first one, though. Cutting round bottom slots in aluminum is really annoying, and that was enough push that I did the flat bottom experiment right away. Flat bottom works just fine; I cut at like 0.150 for quarter inch cord.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Bob, were your fretslotting paths in both directions (zig zag) or just one (zig)?

I tried my air spindle today and had to hold it down to 50 ipm @ 65KRPM, .025" depth of cut, or the bit would deflect too much and widen the top of the slot by a couple of thou. I was cutting in both directions which I guess doubles the deflection error. Seems like rapiding up and over to keep the passes in a single direction would be a waste of time.

Thanks.

The collets on air turbine spindles aren't so great sometimes, it's worth checking them for runout when you put in a new cutter. I've had bad ones that were putting up to 2.5 thou of runout in my cuts, which made the fret slots way too wide. I always did zig-zag cuts.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Thanks Bob. Checked the runout just above the flutes and it was .0005". I'll use a dowel pin to test closer to where the tip would be. The slots taper in width. Wider at the top. On spec at the bottom.

Noticed something yesterday. Slot width varied over the length of the FB. Tight in the middle section where our frets are perpendicular to the centerline, sloppier where the frets are at an angle. Switched to single direction passes and problem solved. I assume the angled grain deflected the bit more than the perpendicular grain.

Backlash

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

dang, I didn't think of that. I'll break out the manual and figure it how to measure that. Thanks Bob.

My standard is to put a dial indicator in, turn spindle lock on, and run the spindle to the left (G1 X-5.0). Then put a gage block on the table and nudge it over until you get a reading of a few thou on the indicator and put a drop or two of CA on it so it won't slide around. Now do a turnaround move (G1 X-10.0, G1 X-5.0) and see what you get. Having an indicator that reads in tenths tends to help a lot for this, since you're going to be getting a pretty small number unless things really went sideways with your machine.

The screws on the machines tend to be pretty good unless they've really been run hard, backlash is usually in the motor coupling or thrust-bearing. If it's a '94 or later machine, with metric ballscrews, then the screws are really good. If it's a '93 or earlier then they were using cheaper screws. You can tell which it is by the max feedrate: a '94 machine has a max feed of 400IPM at 100% feed (rapid 600) where a pre-94 machine has a max feed of 250IPM at 100% feed.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

So being very lazy...I just finally cut my first fretboard using Bob's super secret fret slot slotting path and have to say it was pretty impressive. Went from about 15 minutes to slot a board down to about 5 minutes. And, I wasn't feeling that aggressive so I slowed my feedrate down to 18ipm where I've tested this out at 22ipm (in rosewood anyway, this was ebony)

I've been debating adding another small Z-axis to the side of my spindle to add a 60k spindle which theoretically should be able to get me under 2 minutes to slot a board .

I've also updated my fretboard fixture so I thought I'd include a shot. I was going to make a 4-up fixture but I didn't feel like spending the cash on all the vacuum valves quite yet. Maybe down the road. The brass plates have little needles protruding up to keep the stock from squirming - no need for locating pins (though I still use them if I'm doing an inlay as sometimes I've had to go back to fix something)

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

Hiya All,
I would like to thank you for all the information in this thread, I managed to rout fretslots under 10min thanks to you all.
It used to take me over 45min
Respect!
BTW here is a wee crappy movie I shot during the machining...

_________________
FB Page

I think our bearings are going on our air spindle. We just can't maintain RPM at a reasonable feed rate. Obviously torque has become a limiting factor. This made me think of Stuart's method of using the mill spindle.

The air spindle had to be so babied that we were taking almost 30 minutes to slot a 5-string board. Running the machine spindle at 9K RPM and taking deeper passes to compensate allowed us to slot a 5-string board in just over 10 minutes. The width tolerance of the slots is better and I'm confident that our bit life will be better too.

I'm using a 50K air spindle setup and do 3 passes to a consistent depth of .090 cutting blind slots in compound radius boards with a 2 flute .023 upcut.
Takes a couple minutes at about 100 IPM.
Not many blades can do that.

Unfortunately I bought 4 2FL carbide bits so may take a while before I break them and move to 3FL which should allow an increase in feed rate. Plus 3FL tools are a little more robust.
Usually there is some chip packing that needs to be cleaned out but haven't had breakage since the first one. I'm expecting tools to break when they dull.

What are you using for an air spindle Pete? I'm not so sure 3 flutes are tougher. I've got some singles on order to compare to them. We've been breaking 3 flutes way too often.