Official Luthiers Forum!

Ya...it is.

I was thinking about an electric spindle motor in a cat 40 holder.

I guess making a holding brackett and mounting it on the side of the main spindle wouldn't be the end of the world. I'm thinking about setups being a chore but figuring out a quick mount system wouldn't be the hardest thing I ever did.

_________________
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

Air Turbine tools makes that CAT40 air spindle. They also make them with a stub to mount in a tool holder for under $1K. They take a boat load of clean air though.

Here's what you're describing Stuart. http://www.nskamericacorp.com/prod_machineTool_hes.aspx

I think they're about $5K but dead quiet.

I picked up a rebuilt spindle speeder on eBay. It's nominal working speed is only 18k RPM so not that impressive for fret slots. We'll see how durable the gears are. May just use an air spindle.

I didn't realize you were following the cutter with the air jet. What about two nozzles on either side?

I have...lemme think...I think I have three 602JS air turbine spindles with 3/4" shanks on them. Two 90K and one 65K. Might be four...man, I really haven't spent enough time in the shop in the last two years since I've been back in school!

I'm not doing much production anymore, and they're older models, but if you want one then I'm selling a heckuva lot cheaper than the dealers are

Andy:
So far as my 'secret sauce', it does indeed require cutting in two directions. The 'reset' would slow the process down quite a bit if cutting in one direction only.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Bob,

I think I have a pretty good idea of what you're doing I currently have a table driven model for my fretboards in SW and what I haven't tried to figure out yet is how to make a model in SW that would automatically update that sort of toolpath with changes in the model but....as I'm writing this message I'm actually getting a few ideas.

I suppose if I ever go after volume orders I may just have to do a little work!

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

There must be a half a dozen cam modules that plug into Solidworks...Camworks and Mastercam....probably GibbsCam too. They would all certainly work in that context....make a model change...hit a button to make a new toolpath.

I got to thinking it would be nice it to offer custom neck contours. Embedded cam software would go a long ways toward that.....but I can draw the basic files with that in mind and just switch out surfaces in MasterCam easily enough....little hassle....so what.

_________________
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

Just saw this high-speed spindle on Keling's new sight. 60K RPM and air cooled.

http://www.automationtechnologiesinc.co ... ng-spindle

Looks like it would not be difficult to mount this little guy next to his big brother and have the best of both worlds
Would it be practical to have one VFD, with enough capacity for the largest spindle, drive both spindles via switching?

At the PBG Arroyo Grande shop, they changed from a speed multiplier tool holder to this right angle blade. Works Great!

You can see the other one in the tool changer: It still gets used for some things:

It sounds perfectly feasible to switch between two spindles with one VFD but, you'd obviously need relays or switches that can handle that sort of current and, you also need a 1000Hz VFD. VFD's commonly have a max output freq. of 400Hz which is only good for 24000 RPM.

The bigger issue as I see it is that you'd need either a second z axis (which is actually rather common) or a special fixture or some other method to make sure that both spindles can get to the fretboard and not collide with stuff it's not supposed to!

I think it's actually not a bad idea to do the switch to save money on the VFD but, I think that designing the machine with dual Z-axes would be the best way to handle it. A friend of mine (Ger21 on the zone) is currently designing and building just such a beast that will hold 2 PC routers. Still works out much much cheaper than a tool changer!

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

Andy, you're probably right on the second Z axis. I was thinking that it could be handled with tool and fixture offsets but I see the concern with fixture collision.

I think it could be handled that way but, you'd be sort of committed to that all the time.

Let's say you put it so that the difference between the tool tip on the low speed and high speed was like 3", you could elevate your fixture around 3.5" to make sure you won't hit the table and you could mount your high speed so that it's maybe 4" +y in relation to the big spindle. That would probably allow you to do what you're after. However your work envelope for the high speed spindle is now pretty restricted compared to that of the big spindle, you've taken away from your Z travel, you've got to worry about collisions when working on other stuff etc.

One method of dealing with that would be to make a repeatable quick mount for the high speed but now you've got to deal with tool changes again.

One of these days I'm going to add an 3D print head extrusion thing to my machine and my plan is to simply make something that bolts on to the spindle to do so. It will sit lower than the spindle to avoid collisions.

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

On our old machine we use two independent Z's. You have to manually edit the code to switch from one to the other but it allows two tool files.

Keling sells a 1000 Hz VFD.

Has anyone used a high helix cutter on wood? I assume since I've never seen one intended for wood there's a reason not to use one but it seems like these bits would do a better job of clearing the cut. Tool guys care to comment?

http://www.harveytool.com/prod/Harvey-T ... ls_58.aspx

High helix cutters are designed for very small chips, and the clog very quickly in wood or aluminum. A regular spiral cutter throws the chips out quite effectively. I've had to use a high helix on wood before, because I'm dumb like that and ran out of 1/8" end mills, and it was a very smokey experience unless I blew 90PSI directly at the cutter to dislodge the clogged chips. Even then, the feed rate had to be very slow because there's nowhere for the chips to go.

Once upon a time I was really excited that I could get six flute cutters and really get cooking on feeds and speeds in wood, but after trying it I know (and smelled) why it isn't done

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

I think that a high helix would tend to pull up and cause rougher top edges than standard cutters. Maybe high rpm machines make that moot but I've never had a high rpm machine really. I've used high helix cutters on aluminum but always shyed away from using them on wood for that reason. Fact is: on a lot of cuts, a straight flute or down spiral cutter provides a better top edge.

_________________
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

Thanks Bob. I knew there had to be a reason.

I've learned so much from this thread and am now trying to cut some slots on my K2.
I've taken my basic 2d fingerboard drawing in Rhino, and added a surface for the radius. I'm able to cut everything out, but the engraving path I'm using does not follow the contour of the FB. It does a simple straight line. I have to deepen the slots at the edges with a handsaw after removing the boards from the machine.
How do I get it to follow the contours of the fingerboard radius?
I'm using Rhino-VisualMill-MACH3

thanks! Here's what it looks like so far:

Saul, one way of doing it and certainly not the best way: draw an arc of the fingerboard radius minus the depth of the fretslot with a length to mill the longest slot in the board and, maybe, a quarter inch lead-in and lead-out. Program the arc with simple CAM which will output the radius in the X & Y axes. Then use G17, G18, or G19 , whichever is applicable in your case, to cut the arc. Use a text editor to generate the rest of the program by repeating the arc after moving over the correct distance between slots. The arc can be repeated for several depths of cut or the whole program repeated for final depth and cleanout pass(es). It's amazing what can be done with a simple text editor such as word pad and or Excel type software.
I'm sure others will have ideas on how to program the slots also.
Nelson

Although it's in the 2D toolpath strategy section of VisualMill, engraving is actually a full 3D strategy.

Here's what I do - I have a sketch that draws straight lines the length of the fret slots on a plane just above the fretboard. I then project that down onto the fretboard to make little arcs. Select those projected arcs (they're actually elliptical on a compound radius fretboard) for an engraving toolpath and Bob's your uncle. DOC is set in visual mill.

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

Thanks guys!
I'll try each way.I don't understand the G17,18, and 19 plane selection commands yet. But I'll try to figure it out. I'm still doing doing tiny baby steps, pussy footing around. If it were a new language, I can now count to ten and ask where the bathroom is and order another beer. But I'm not quite ready for a solo trip to that new country.
Luckily I can dabble around and ask questions. I appreciate your help. You are my tourguides.

After the machine sat in my shop for a couple years as the worlds most expensive shelf, I'm starting to make it do things. Having fun with it, and actually making real parts! It is an exponential journey. Every new thing I learn prompts a hundred more ideas and questions.

Cheers,
Saul

Hey Saul, missed you in Montreal.

Great strategy Andy. I like that a lot.

HELP! Please help..... I'm at my wits end.....my CNC is breaking 23 mil bits and I don't know why.

I have the fret slots all curved nicely and can generate the tool path file nicely (from Rhino/MadCAM), and even though I have the X/Y/Z move speeds all set to only 1 ips, and am only taking a 10 mil pass depth, the darned bits break on the first pass!!!

All I can think of is that I set the ramp angle to 90 degrees thinking this would be best for the bit (which breaks easily in shear). The bit seems to break after it has been plunged to the cutting depth right at the point the head starts to move to cut the slot - there doesn't seem to be any time between the plunge and the move.

Also, bit is going at 6000rpm....too slow?

Any ideas from anyone muchly appreciated!!

Cheers,
Dave F.

_________________
Cambrian Guitars

"There goes Mister Tic-Tac out the back with some bric-brac from the knick-knack rack"

hmmm...

6000 seems very slow to me. I run at 18k but would run at 24 if my bearings could handle it. That said, if you go 3 times slower than I do all should be well.

If I recall correctly, I'm running at about 20ipm also with a vertical plunge and I'll cut up to .030 depth per pass. Perhaps you're going too slowly and the bit's getting too hot?

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

Thanks Andy!

The second bit I broke was going at 10 ips 16Krpm, same thing....

My test wood is coco, but I tried a piece of Alder (fairly soft) early on.....that broke a bit too.

I'll give it a go at 16Krpm (I think that's the fastest my 4HP spindle will go) and 1ips tonight.
I'm also thinking of hand editing the code to put in some short pauses after the plunges and before the moves - couldn't hurt, right?

Cheers,
Dave F.

_________________
Cambrian Guitars

"There goes Mister Tic-Tac out the back with some bric-brac from the knick-knack rack"

Perhaps it's excessive runout? What is your spindle setup?

Router or spindle? If it's a router, are you using a precise bits collet? Have you measured the runout on your setup?

Edit: Just saw you have a spindle.

One other idea is instead of plunging at 90 degrees, plunge at 45 degrees along the path in the opposite direction of your tool path. This will limit the jerk on your cutter if your controller isn't already doing it. Definitely run at your highest spindle speed with such a tiny bit.

What controller are you using on your machine? If you do an air cut, is the motion jerky or nice and smooth?

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

OK, I've got it mastered!! Thanks very much for your help Andy

There's no measurable runout on my 4HP spindle I only broke 3 bits to get there....not too bad I suppose

The problem was the bit rotation speed I guess. Once I made a toolpath with a 15 mil step size and a 45 deg ramp, and ran the bit at 3 ips x/y and 1 ips z, at 18,000 rpm, everything behaved beautifully!

I should be able to make my first real (usable) CNC fretboard tomorrow night, yay!
It will be the one I use on my ESJ2 guitar for the OLF Challenge part 2.

Thanks again Andy! If it weren't for great fellows like you, lots of us would be in a bind!!

Cheers,
Dave F.

_________________
Cambrian Guitars

"There goes Mister Tic-Tac out the back with some bric-brac from the knick-knack rack"