Official Luthiers Forum!

Hi folks

I have a Cnc router 8 tools auto change etc, and wish to retrofit a saw for fret slotting

Has anyone on this forum already done it, I don't want my mods to be permanent, just a local quick attachment

Ideas

I've never slotted a fretboard on a CNC but if I was going to I don't think a saw would be my first choice. A tiny end mill would be my preference. Especially on a router. I don't see how you would have the Z axis travel for that.

a 90 deg head would work. never seem one for a cnc router though....

a good coated (diamond esp.) endmill and an air blaster would be my choice. program your toolpath to follow the curvature of the fretboard radius for better contact with the fret if you want. having a saw blade whizzing at typical router speeds would be "exciting" imo.

these people make some of the finest small diameter tooling available:
http://www.harveytool.com/

this thread might offer some insight:
viewtopic.php?f=10106&t=31933

did some searching for 90 deg heads and found these from Techniks:

http://www.techniksusa.com/aggregate/OilVario.htm

don't know what your "capital equipment" budget is nor your type of machine either, but they look interesting...

Yeah that would be exciting for sure! I just dont see how the extra cost and set up would be worth it? Seems like a real pain to do it that way when you can just cut it with an endmill with no trouble at all. Plus with and endmill you could do the faux binding too, if you like that sort of thing.

Thankyou arie, thats exactly what Im looking for, Ive emailed them for a pricing and availability

I have a 9kw spindle on my machine which can be speed controlled.

Yes I can cut fret slots with an end mill, but its just too slow, its the same as profiling a fretboard yes you can do it on the cnc, but it takes 10-15minutes and leaves ridges, I can use the jig on the belt sander and have it done in a minute.

The next thing is working out a way to adapt that to my machine

Steve

10 to 15 minutes to radius a fretboard!! thats a little slow isnt it? I admit i dont cut wood on my cnc's but that seems like waaaayyyyy to long. I could cut one out of titanium in that amount of time.

Yes.

Well I see comments here on this forum about the speeds that people are profiling and machining fretboards and fretslots etc, on there home made machines and I cannot seem to duplicate them on a commerical unit.

My machine for info costs 125k, driven by servos and runs on 415 volts with 8 tools loaded into the change rack for auto changing, it can move the cutter at a speed of 3ft a second with an accuracy of 0.0005", but it still breaks cutters if I attempt to machine at the speed people hear post at. The Z axis has a travel of 12 inches

So I take some posts with a pinch of salt.

To radius a fretboard for me, I would run a roughing tool over the whole blank, takes about 4-5minutes and then a finishing tool ballnose would take another 10 minutes, you are still left with small ridges from where the ball nose ran. Its easier to attach it to the jig above the belt sander and do a couple of swings and wolla its perfect with no further dressing required until after fitment.

Some of the feed rates in question were likely mine, which were definitely -not- on a home made machine. My machining times were on a Fadal VMC retrofitted with a KFLOP controller (amazing control, let me more than double factory acceleration) and a 90,000 RPM air turbine spindle. I think Andy Birko is on to me, for the most part, but the toolpath for those slots also had to be drawn by hand to keep all the cutter stresses under control.

I'd recommend you get yourself an Air Turbine Tools spindle. They can come with a 3/4" shank, so you can put them in a tool holder, and you get crazy high RPMs in exchange for 2HP worth of air and a tiny fraction of the cost of an aggregate head. Also remember that you're going to have to replace that aggregate head, or pay for an expensive rebuild, sooner than you think. At Taylor guitars they (used to, at least) cook them within a couple months.

So far as the fretboard is concerned, you can go straight to the finishing ballnose. With a one inch ball, you can get a fretboard finish that'll take two zips with 220 to clear the compression marks off of in six minutes with a 10K spindle. You're likely running an 18K spindle, so you should be able to do better by a good margin. If you're going for production quantities then a shaped cutter is the way to go: much faster and leaves a shiny planed finish. You can also cut right through shell if you've got the cutting edge moving fast enough. Oh...or get one of those button cutters Sheldon Dingwall got, those things are choice.

What make/model of machine is it? Sounds like a fancy Thermwood or a Komo, but there's no such beast as a CNC router (or mill, or anything) for 125K that'll hold five tenths at 2160 IPM.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

that'll hold five tenths at 2160 IPM.

I dont understand the question.

Our machine will under G01 control travel at a speed of 2160 IPM, it also travels at 2160IPM at G0 command, and it can stop with pin point accuracy, according to the machine interface when I manually command it by typing direct into the controller, I can command it to move 0.001 of a mm, in reality I cannot see that but the machine will move to that point of accuracy .

My point is just because it can move and run at that speed does not mean I can cut at that speed, Im incredibly intrigued by those that fretslot a fretboard in a minute, to do a 1.5mm (60" approx) deep fret slot I need to do two - three passes at .6mm a pass and at a speed of 16IPM, faster than that and the tip snaps, deeper than that and the tips snap,

So lets assume 1.2mm will be deep enough as that equates to just two passes, a 21 fret slot board not adding in machine repositioning for each fretslot, retractions, plunges etc, fret 1 42mm wide fret 21 70mm wide so lets average them all out to 55mm cuts by 21 = 1155mm of travel or for those imperial minded about 45 inches of fret slotting, at 16 IPM and having to cut twice = 90 inches divide that by 16 and you have a minimum of 5.6 minutes and remember this has no allowance for machine repositioning plunging etc, add into this retraction / plunging repositioning etc and this easily blows out to 10 minutes plus, any faster and I break a tool tip any deeper and I break a tool tip.

So my setup is not capable of going faster or deeper, I was under the impression from some of the posts Ive read, peoples home made units are machining deeper and faster than my commercial unit.

That aside.

For the reasons above I wish to attach a circular blade somehow.

Five tenths at 2160 IPM, means .0005" at 2160 inches per minute. Most machinists in the US use .001" as standard measurement so .0005" is five tenths of a thousandth, or for short five tenths. I think he was saying he doesn't know of any router that can hold an accuracy of .0005" while traveling at 2160 inches per minute. You have to keep in mind that just because a machine is rated to move those speeds and can move very accurately they tend to lose a lot of tht accuracy at high speeds.

What sort of RPM are you running your fret slotting mill at? Also what tools are you using. And are you using air to blow the chips from the slots while cutting? These things can all effect your cut time significantly.

Cool. I now understand the five tenths statement, never seen one written like that before.

Most of my work is in thou, so even though Im in a metric country I understand and use imperial daily.

My cnc router is 3metres long by 2metres wide (9ft by 6ft), and there are a lot of jigs custom made and fitted into the vac table (whole surface is a vac table).

The accuracy is achieved with 415volt feedback servo motors which not only go to a location but also feedback exactly where they are during the travel.

The unit is a auto changing spindle, and fitted out with bt30 tool holders, trust me a 0.023" end mill is tiny in one of these. The machine requires air to be fed to do the auto changing and it also provides clearing air on the job for removal of debris. The rpm is 10,000 on fret slotting and inlaying

To say its fast is an understatement. We left a circular saw (makita 10 1/4) sitting on the bench one day and didnt notice it on startup, when we did the first tool change we spotted the circular saw, I could not run fast enough to get it of the bench and it was crushed as the x gantry went over it and the machine didnt miss a beat, changed tool and headed of to its first job.

But fret slotting takes too long, circular saw would be such an improvement, we make guitar kits for local music stores, and supply most of the local builders with the raw products and pre-machined for them to finish

Something is definitely funny because I can assure you that my semi-home made machine can cut a full depth slot of .080" at 22ipm, 18krpm using "Bob's Secret Sauce Toolpath". At least I have in some test runs to see if I'd be snapping bits or not. I haven't modified my "production model" to the new toolpaths yet.

Even with my old toolpaths though, it still only takes about Edit: 13 minutes to slot a board doing 3 passes @ .030-ish with just a simple plunge entry. With the "BSSTP" I imagine that will go down by more than half. One thing I should add is that I do blow air at the cutter to clear the chips.

I doubt profiling on the CNC will ever be faster than a dedicated sander but like Bob said, you're probably over thinking things. I have a small spindle so my largest tool is a 1/2" ball nose. Using that with a .010 stepover running at 390ipm it again takes about EDIT: 11 minutes to radius a board and like Bob said, a few wipes with 320 and all the marks are gone. No need for any roughing with just a .010 stepover. If my machine could go faster, I'd probably cut those at about 800ipm.

With the size of your machine, is it a cantilevered gantry machine? A friend of mine runs one of those at a cabinet shop and although the thing is stupid fast and accelerates pretty darn fast, he's found that if he's not careful with the tool path, he can get the gantry to vibrate when changing directions - in spite of the fact that it's about 1000lbs or more of cast iron!

In particular, he once programmed a corner with a small arc to try and keep things moving quickly but it turns out that the machines acceleration was so fierce that going around the corner without slowing down caused the gantry to vibrate. He learned that in that case, programming a "square" corner worked better because the controls slowed things down enough to avoid the vibration.

p.s. - I edited because my numbers weren't adding up to my total time so I checked my records. Fret slotting takes me about 14minutes with the slow toolpath and radiusing about 11minutes. With the new tool path for fret slotting, it should go down to about 5 or 6min.

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

I believe that you should increase your spindle speeds for fret slotting. It would allow you to increase your feed rated. Like Andy said he is running 18,000 rpm for slotting the fingerboard. By increasing your speed you can proportionally increase your feed without an increase in chip load. As long as you have air blasting the chips out I see no reason why you couldn't go significantly faster.

Not the best photos but

ah! now that we see the beast things are much clearer. i don't think that you're going to be able to mount nearly any angled head (compound or otherwise) on that thing esp. with a tiny bt30 spindle and expect decent repeatability due to the weight and overhang -or you're going to have to dampen your toolpaths down to minimize accel/decel velocities. i'd suggest an air turbine or an electric hi-frequency spindle. nsk and ibag make a whole bunch of them. tiny, quiet, and usually around 5~7k usd. (for an NSK HES510)


i have used many of these and can testify:
http://www.nskamericacorp.com/prod_machineTool.aspx


good rep but I haven't personally used them:
http://www.ibagna.com/spindles.htm

good luck!

All servo motors feed back their position, that's the definition of a servo motor. And all full scale machines use servos. There's no question that the motor knows its own position perfectly well at any instant in time, the problem is that between the motor and the cutting edge there is error introduced by: servo following error, motor to screw coupling, ballscrew lead error (or, worse, rack and pinion), linear rail error, thermal expansion and contraction, axis misalignment error, flex in axes, spindle runout, and tool runout / diameter error. Just as an example, your machine will expand in length by 0.0016" with a one degree Celsius change in temperature at your shop.

I cut fret slots at 105 IPM and 90,000 RPM, which scales pretty accurately to what Andy's doing. Or his cuts scale to mine since I was doing it first . For cutting with small mills, you need edge speed. 10,000 RPM doesn't get the edges of a 0.025" end mill moving fast enough to cut efficiently. I found this out the expensive way when my turbine spindles were all down and I needed to ship a critical order; even at half of the scaled feed rate (1/18th of the 90,000 RPM feed) I was losing cutters left and right.

You can get an air turbine spindle from Air Turbine Tools for something like $750 new. 601JS is the model you want. I'd recommend getting the 65,000 RPM one rather than the 90,000 RPM one unless you're going to buy two or three to have a backup when the bearings are shot. The 90K spindles really cook through bearings. Besides fret slots, you'll also be able to cut inlay pockets and shell much more quickly and with almost no cutter losses at 65,000+ RPM.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

I do understand this bob. I wrote this as many people dont understand the difference between a servo and a stepper, as I have no idea who I am dealing with, I state IMO the obvious.

I thank you on the expansion information, but as a side note, I have a background qualif and certification in Mech / Aero Engineering, you were not to know this, so again thank you.

I appreciate the info people have relayed, but from what I am understanding no one is using a circular saw. The link supplied by arie on the aggregate head appears to be the quickest solution and I am awaiting a reply from the manufacturer. This solution will also allow us to retain our machine in current configuration and capability.

The cnc machine on your website bob is almost identical to our other cnc milling centre. However we dont machine wood on it, just aluminium and steel.

We currently have a saw blade that attaches to our milling machine, the machine has a DRO, so we can manually fret slot, for Info this is faster than doing it by our cnc.

Steve

Oh no an engineer

That's all I'll say about engineers. Mom always said "if you can't say anything nice then don't say anything at all". Abiding by that rule I cannot discuss engineers. Hahaha

In all seriousness I can't see how spending several thousands of dollars on an aggregate head would be a worthwhile investment for slotting fingerboards. There are just much more cost effective ways of doing it I can't see how to justify the cost. But hey everyone likes to do things their own way. Frankly I could build a machine capable of cutting all the slots in one go, probably cut 2-4 fingerboards a minute, for less than the cost of an aggregate head (unless you are getting some awesome deal).

You could do it with a table saw just as fast. (Well...almost)

We use (I should say they use) a saw for slots on the HAAS at Gene Baker's shop to cut fret slots.
It is so much better (faster) for us in a production situation.
We still use the tiny endmills for stopped cuts, but for the full width slots, the saw blade works great!
You can see the thing in the ATC here:


Here it is in use:


On my personal smaller K2 machine I'm using the .024's from Precise bits. It's an awful lot slower, and at about $20 a pop, can get expensive.

Engineering is simply knowledge, some use that knowledge some dont.

I left engineering to work on Musical Instruments as thats what I enjoy, having an engineering background merely allows me to understand something before I do it.

But real learning happens when you do it yourself.

My first cnc router I built myself, my first cnc lathe I built myself, and we are talking using milling machines and lathes to create them with. However I learnt that I cannot make something as good or as cheap as someone that does it for a commercial living


Saul.....

Thanks, thats exactly what Im making enquiries about at the moment, appreciate the photo. I notice the two tool stations around it are no longer used, makes sense regarding clearance for the blade

Engineering is simply knowledge, some use that knowledge some dont.

I left engineering to work on Musical Instruments as thats what I enjoy, having an engineering background merely allows me to understand something before I do it.

But real learning happens when you do it yourself.

My first cnc router I built myself, my first cnc lathe I built myself, and we are talking using milling machines and lathes to create them with. However I learnt that I cannot make something as good or as cheap as someone that does it for a commercial living


Saul.....

Thanks, thats exactly what Im making enquiries about at the moment, appreciate the photo. I notice the two tool stations around it are no longer used, makes sense regarding clearance for the blade

Yes, yes and yes! You can have all the "book knowledge" in the world but with no real world experience of manufacturing it does no good. That's my main issue with all these "engineers" these days. They go to school an get a piece of paper and then they go around "designing" things with no clue how things are made. I personally believe that all engineers should be required to spend a minimum of 2 years in a manufacturing environment. Just because something works on paper does not make it work in real life.

Anyhow about the saw I wish you te best of luck with that endeavor. And regarding the spaces open on both sides of it on the tool changer, haas has implemented a cool feature in the newer model machines. You can designate a tool as large in the tool offsets page and it will automatically keep an empty slot on both sides of it in the tool changer. Pretty cool and very handy of you ask me. It keeps you from having to program around it and prevents any mishaps from someone not thinking about what teu are doing when loading tools.

To totally digress but, there's room for all types of engineers. Just because manufacturing says it can't be done doesn't mean it's necessarily so. Some times you just need to push them a bit and they'll surprise themselves.

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