Milling Guitar Neck Fret Slots

General MeshCAM Questions

Milling Guitar Neck Fret Slots

Postby verhoevc » Tue Jul 26, 2016 1:25 am

Hey guys. Been using MeshCAM for a little while yet and honestly I'm pretty much able to get it to do everything I want to except one thing: Mill fret slots!
I've read up on some of the other threads that deal with this and no one else seems to be having the same issues I am. Optimally I'd just do this with a 3D arc path that my correctly-sized cutter follows. However, as per my discussions with Rob when buying, this 3D-engrave like function is on the to-do list. So in the meantime, I have to find a work around.

I've set up slots to be .024" wide and was assuming the cutter, being .023" diameter, would be able to find and mill them just fine. However, as you can see in the pictures attached, no matter what type of paths I do it just wants to ignore some of the slots, and not cut other fully.
I have also tried making my cutter diameter as small as .021" to hopefully make it find the slot... no luck there either. If I go much smaller I'm just asking for overly-loose slots at that point.
Image
Image
Thoughts?
Chris

While I was writing to post I was trying some parallel finishing... and just broke the bit. Awesome :evil:
verhoevc
 
Posts: 2
Joined: Tue Jul 26, 2016 1:03 am

Re: Milling Guitar Neck Fret Slots

Postby Randy » Tue Jul 26, 2016 11:27 pm

HI Chris, and welcome to the forum. Other than using a smaller cutter and contouring the fret slots (i.e. cutting each face separately) with the waterline and pencil finishing, there is not much you can do. A .5mm bit (.0197") would probably work. Pencil finishing is especially sensitive to machining tolerance, waterline a little less so. If you're not already, use .0001" tolerance. As I often say here, I always use .0001" for final toolpaths. I'll bump up to .001" or sometimes .01" tolerance for a very quick approximate test of machining strategies, but the toolpaths really suffer there. Arc fitting (unfortuantely only in the horizontal X-Y plane) on curved surfaces also seems to improve with the tighter tolerance.

Randy
All opinions in this post are mine alone. I am not a MeshCAM employee, I do not have a financial interest in MeshCAM, nor do I speak for MeshCAM. MeshCAM user since Beta 5 in 2003. viewtopic.php?f=11&t=15333 :ugeek:
Randy
 
Posts: 1812
Joined: Wed May 14, 2008 9:50 am
Location: North Texas, USA

Re: Milling Guitar Neck Fret Slots

Postby verhoevc » Sun Jul 31, 2016 3:12 pm

Guess that is the next step! Which doesn't seem to daunting since I'm seeing .5mm end mills on eBay for WAY cheaper than the fret slotting mills I bought from precise bits!
Best,
Chris
verhoevc
 
Posts: 2
Joined: Tue Jul 26, 2016 1:03 am

Re: Milling Guitar Neck Fret Slots

Postby greg-c » Tue Dec 13, 2016 12:19 am

I tried the cheap .5 & .6 mm bits on ebay and most didn't even make the journey over without breakage, I had drill bits just put into an envelope , pfffft , the others snapped in my hand as i touched the tip. There is no way in the wide world that these will cut hardwood fret boards,

So even though cheap, i wasted weeks waiting for the order, and remember, quality made drill bits from the US are damn cheap if they go the distance,

cheers

GC - australia
greg-c
 
Posts: 14
Joined: Thu Mar 17, 2016 4:23 pm

Re: Milling Guitar Neck Fret Slots

Postby Doug » Wed Dec 14, 2016 11:58 am

The length of the fluted section on these cutters is a problem Greg. Genuine 0.6 mm carbide end mills that I have seen have a flute length of only 1.0 mm. I reckon that 1.5 to 1.75 mm is required to accommodate a fret tang.

You can buy carbide engraving bits with long fluted sections but they're obviously not intended to bear any kind of sideways load and will simply snap off.

I wondered whether it is worth buying ten 0.6 mm engraving bits and just shortening the tips down to 2 or 3 mm; the bare minimum required to cut the slot but still retain a reasonable amount of structural integrity.
Stepcraft 2/840 CNC machine with 4th axis, TurboCAD V19.2 Pro Platinum, MeshCAM, GWizard feeds & speeds calculator, UCCNC. Hobby use: guitar building (luthiery). http://www.facebook.com/DougShortGuitarBlog/
Doug
 
Posts: 55
Joined: Thu Oct 13, 2016 9:56 am

Re: Milling Guitar Neck Fret Slots

Postby larynx » Wed Dec 14, 2016 4:13 pm

Hate to chime in here with no real solution, but you may be better off using a fret saw setup for this and then binding if acoustic or filling the ends if an electric setup. I buy my boards fretted and then final shape them myself.

You can mill them, it will take a lot of time. If you wish to use a roughing pass with a small bit, followed by parallel and pencil then you will need tight tolerances and it can be made to work - I did it before as a test, but did not save anything - it turned out to be a waste of time and materials for me. Tolerances tight, almost no "extra milling" in the rough. In fact, if I remember correctly, I ended up with separate cut files, using a parallel cut as my roughing/finish pass - allowed me to not have to fool with the cutter "extra mill" stuff, but set the milling depth and speeds very low to not break bits - depends on hard or soft, types of wood too. I believe I set up:
----------------------------------
1. USING include region dxfs

2. ROUGHING: use parallel path finish with very low feed speeds and plunge rates/depth of cut use the biggest bit that will fit, overlap will be an easy pass and cool down for the cutter, first new depth pass will be strenuous on the bit - go slow. Still have a good vacuum or air jet to clear debris - or follow once every so often depths with hand vac slots while cutting, have your fingerboard setup at a right angle [the closer to right angle to your cutter travel the less "arc" interpolation or sideways movement of the head necessary to follow the slot - I am anal and attempt to minimize unwarranted movements] it will never be perfect it seems but it is easier to setup in the beginning

3. FINISH: did nothing else, the parallel does it, did not use pencil either. If this is not satisfactory after a cut like this, perhaps you have other issues - not with meshcam but the machine?
----------------------------------
You CAD file must be precise, your stl precise, and I suggest creating "include" region surface dxfs for the area to machine based on the outlines of your slots - and extend those outside of the board by two bit diameters at least. This will add some "air cutting" but allows for cleaning of the slot and cooling of the bit too.

It does appear, although I am still assuming, that you are "arcs" were stated and the paths displayed, attempting to arc the slot bottoms and slot not extending through the edge of the board as in a bound slot without binding. You will need really good vacuum or air blowing debris from the slot to clear the cutting and dust so as to not further bind you cutter.

I cut my necks, internals, jigs.......but not my fingerboards. Like I said, too wasteful use or resources/time/cash for me all the way around when full binding the neck anyway. You may have non-standard spacing or other, that's a different issue when having you boards pre-slotted to non available scale lengths.

Like I said, no real solution for you is given, just perhaps some suggestions, perhaps something will click.

But why listen to me when I can never seem to even get the "list" text to work on the forum?
I am not aligned with nor do I have any relationship with MeshCAM or its staff other than being a user [that sounds a little like I have a dependency problem]
larynx
 
Posts: 74
Joined: Thu Oct 29, 2015 2:56 am
Location: East Central Florida

Re: Milling Guitar Neck Fret Slots

Postby Doug » Tue Dec 20, 2016 4:16 pm

Agree with larynx. I concluded that it would be more trouble than just doing it manually which I invested a lot of money buying StewMac tools for.

When you have a CNC machine, the temptation is to set it to work doing clever things just for an intellectual challenge even if it brings little benefit in terms of cost or time saved.

I will be sticking to CNC for radiusing and outline shaping the fretboard only.

Doug
Stepcraft 2/840 CNC machine with 4th axis, TurboCAD V19.2 Pro Platinum, MeshCAM, GWizard feeds & speeds calculator, UCCNC. Hobby use: guitar building (luthiery). http://www.facebook.com/DougShortGuitarBlog/
Doug
 
Posts: 55
Joined: Thu Oct 13, 2016 9:56 am

Re: Milling Guitar Neck Fret Slots

Postby Doug » Sun Jan 07, 2018 12:05 pm

My goal is to be able to make a fully shaped, radiused, dotted and slotted guitar fretboard in one CNC session. I recently slotted a fretboard manually and unfortunately the slots I cut using StewMac fret slotting miter box and Japanese fret slotting saw were slightly offset (by about 0.5 mm) compared to the dots. I therefore revisited a previous attempt to cut fret slots using G02/G03 CW & CCW arcs in the XZ plane wth the G18 command. I asked for assistance with this on the following thread "G Code for Arc Cuts (G02, G03)":

viewtopic.php?f=3&t=15748

I bought a Kyocera 0.6 mm diameter solid carbide flat nose end mill with 1.8 mm flute length to try this. The GCode construct is given below for the zero fret only for the fret positions on a 24" scale Brian May Red Special guitar with a 7.25" radius/14.5" diameter curve fretboard. Zero position is the centre of the fretboard. To keep the code simple, the cutter describes arcs from X = -26.5 mm to +26.5 mm which is slightly beyond the widest part of the fretboard that I have previously cut to shape and fine radiused with a 6 mm ball nose end mill to 1/4" (6.35 mm) thick at the crown.

You can see this code in action 'milling air' in the short (2m 30s) YouTube video below:

https://www.youtube.com/watch?v=ncJCqhZCJhE

I have not tried this yet but I have kept the feeds ultra conservative. In the video I run at an XY feed rate of 750 mm/min but I have reduced this to 600 mm/min in the code below. Z plunge rate is 120 mm/min. As you will see, I cut at -0.25 mm depth increments down to -1.75 mm. I might stop this at -1.5 mm in case there is any variation on the cut stock thickness to leave me a little more margin to the maximum flute length of 1.80 mm.

(Zero Fret)
G00 X-26.5000 Y230.9687 Z2.0000
G01 F120.0 Z-2.1667
G18 F600
G03 X26.5000 Y230.9687 Z-2.1667 I26.5000 J0.000 K-181.9833
G01 F120.0 X26.5000 Y230.9687 Z-2.4167
G18 F600
G02 X-26.5000 Y230.9687 Z-2.4167 I-26.5000 J0.000 K-181.7333
G01 F120.0 X-26.5000 Y230.9687 Z-2.6667
G18 F600
G03 X26.5000 Y230.9687 Z-2.6667 I26.5000 J0.000 K-181.4833
G01 F120.0 X26.5000 Y230.9687 Z-2.9167
G18 F600
G02 X-26.5000 Y230.9687 Z-2.9167 I-26.5000 J0.000 K-181.2333
G01 F120.0 X-26.5000 Y230.9687 Z-3.1667
G18 F600
G03 X26.5000 Y230.9687 Z-3.1667 I26.5000 J0.000 K-180.9833
G01 F120.0 X26.5000 Y230.9687 Z-3.4167
G18 F600
G02 X-26.5000 Y230.9687 Z-3.4167 I-26.5000 J0.000 K-180.7333
G01 F120.0 X-26.5000 Y230.9687 Z-3.6667
G18 F600
G03 X26.5000 Y230.9687 Z-3.6667 I26.5000 J0.000 K-180.4833
G00 Z2.0000

If anybody is interested, I came up with the following G Code to cut the holes for the 1/4" (6.35 mm) diameter circular mother-of-pearl fretboard marker dots. I cut at 6.45 mm diameter to allow a good fit and -0.5 mm Z depth increments in this case.

(3rd fret, centerline at Y = 149.2195 mm)
G00 X0.0000 Y148.9945 Z2.000

G01 F90.0 Z-0.5000
G02 F2000.0 X0.0000Y148.9945 Z0.000 I0.0000 J0.2250
G01 F90.0 Z-1.0000
G02 F2000.0 X0.0000Y148.9945 Z0.000 I0.0000 J0.2250
G01 F90.0 Z-1.5000
G02 F2000.0 X0.0000Y148.9945 Z0.000 I0.0000 J0.2250
G01 F90.0 Z-2.0000
G02 F2000.0 X0.0000 Y148.9945 Z0.000 I0.0000 J0.2250
G00 Z2.000
Last edited by Doug on Mon Jan 15, 2018 2:00 pm, edited 1 time in total.
Stepcraft 2/840 CNC machine with 4th axis, TurboCAD V19.2 Pro Platinum, MeshCAM, GWizard feeds & speeds calculator, UCCNC. Hobby use: guitar building (luthiery). http://www.facebook.com/DougShortGuitarBlog/
Doug
 
Posts: 55
Joined: Thu Oct 13, 2016 9:56 am

Re: Milling Guitar Neck Fret Slots

Postby Doug » Sun Jan 14, 2018 12:44 pm

Last night I successfully managed to cut 1.5 mm deep, 0.6 mm wide pure arc slots for the frets in a guitar fretboard I am making using the G18 (arc in XZ plane) command in conjunction with the G02 and G03 CW & CCW arc commands.

I wrote the GCode for this myself as per the previous pot. The YouTube video below (filmed with my iPhone, hand held) illustrates the process. I used a 0.6 mm diameter, Kyocera solid carbide two flute end mill cutting in 0.25 mm depths per pass. The system parameters were extremely conservative to avoid breaking the fragile end mill. Spindle speed 10,000 rpm, XY feed rate 600 mm/min, Z plunge rate 120 mm/min but all Z movements were done outside the line of the stock. This is a test/validation cut on spruce tonewood. The final cuts will be done on European oak.

https://www.youtube.com/watch?v=hRuM4Z8pQfE

The fretboard is for a Brian May Red Special replica, so 24 frets cut at a radius of 7.25".

Doug
Stepcraft 2/840 CNC machine with 4th axis, TurboCAD V19.2 Pro Platinum, MeshCAM, GWizard feeds & speeds calculator, UCCNC. Hobby use: guitar building (luthiery). http://www.facebook.com/DougShortGuitarBlog/
Doug
 
Posts: 55
Joined: Thu Oct 13, 2016 9:56 am


Return to General