Official Luthiers Forum!

hi there! I am trying to fret slott with a cnc machine. I use a tiny bit and aspire vectric. The problem i have is that the cnc cuts one pass (the fret slot)0.1 mm and then it lifts up and goes again to the begining to cut the 0.2 cut depth. I would like to make it cut left to right and then right to left till it cuts the slot to the end...it is very time consuming the way it cuts now....is there any solution? i have found a video that shows what i want to achieve https://youtu.be/hRuM4Z8pQfE?t=3 . Can someon eplease help me? i also upload the gcode sample...


( Profile 1 )
( File created: Sunday February 14 2021 - 01:22 PM)
( for Mach2/3 from Vectric )
( Material Size)
( X= 600.000, Y= 600.000, Z= 6.000)
()
(Toolpaths used in this file:)
(Profile 1)
(Tools used in this file: )
(1 = End Mill {0.4 mm})
N100G00G21G17G90G40G49G80
N110G71G91.1
N120T1M06
N130 (End Mill {0.4 mm})
N140G00G43Z20.320H1
N150S12000M03
N160(Toolpath:- Profile 1)
N170()
N180G94
N190X0.000Y0.000F250.0
N200G00X281.508Y36.546Z5.080
N210G1Z-0.100F250.0
N220G1X318.492Y36.546
N230G00Z5.080
N240G00X281.508Y36.546
N250G1Z-0.200F250.0
N260G1X318.492Y36.546
N270G00Z5.080

Vectric doesn't make the most efficient toolpaths. Even with the advanced options on a 2D profile toolpath, what you describe is what it does. It will get the job done but when time is money, it's not the quickest.

The easiest option to me (but I've spent years programming CNCs) is to manually edit your file. If you're not familiar with G code, it may be a bit intimidating.

Here's an example. This is the first pass -
N190X0.000Y0.000F250.0 - Move to part zero
N200G00X281.508Y36.546Z5.080 - Rapid move (G0) to location of first slot
N210G1Z-0.100F250.0 - Feed move (G1) to first cut depth, -.1
N220G1X318.492Y36.546 - Feed move (G1) to end of cut. Move is a straight pass in X, Y doesn't change.
N230G00Z5.080 - Rapid up (G0) to Z clearance plane
N240G00X281.508Y36.546 - Return to beginning of slot
N250G1Z-0.200F250.0 - Feed move to second depth, Z-.2
N260G1X318.492Y36.546 - Make the second cut

This repeats for each cut depth, and each slot. So yes, a lot of time in the air, not as much in the cut.
An edited version -

N190X0.000Y0.000F250.0 - Move to part zero
N200G00X281.508Y36.546Z5.080 - Rapid move (G0) to location of first slot
N210G1Z-0.100F250.0 - Feed move (G1) to first cut depth, -.1
N220G1X318.492Y36.546 - Feed move (G1) to end of cut. Move is a straight pass in X, Y doesn't change.

(deleted lines 230 and 240)

N250G1Z-0.200F250.0 - Feed move to second depth, Z-.2
N260G1X281.50Y36.546 - Make the second cut . Note X value is changed in this line, to the beginning of the cut position.

This can be repeated for all depths, and the same method applied for each slot.

Doing this manually can be a little nervewracking, and editing 20+ fret slots at 4 or 5 cut depths will take a while, but if you're cutting many fretboards, the hours invested will get paid back pretty quickly. If you're not comfortable with the manual editing, find some one who will do it for you.

Hope this helps.

Chuck

Thanks for the reply!!I dont knoq qnythibg about g xode so maybe there is a chance to learn. Is there any cam program that makes this kind of stuff?

If you mean, are there any CAM programs that will generate the tool path the way you want, I’m pretty sure I could do it in MasterCAM, which is what we use at work & school.

But it’s about $10,000 / seat per year.
There may be other CAM solutions that will do it, I’m just not familiar with them.

Fusion 360 has the ability to machine a path both ways. It has a free version you can download. It messes with your toolpath in the free version, but it just makes the rapid move way slow.

_________________
-Marcus
http://www.bailieguitars.com
Instagram | YouTube

I have tried fusion 360 and i find it really hard to findout the toolpaths and stuff....well i must learn to do it cause i spent more time with the cnc than doing it by hand...

Have you asked the Vectric Forum for help?

Here is a link to a topic in the Vectric Forum about a gadget for allowing variable inputs to produce a fretboard of any scale, both imperial and metric. Also any width, any radius, and any fret tang size.

This should afford you to experiment without actually cutting a piece of wood as Vectric products do a virtual representation of the cutting as well as computes “runtime” projections in minutes and seconds.

There are quite a few luthiers on the Vectric Forum that could provide answers to you but I suggest to NOT post the entirety of your g-code.

https://forum.vectric.com/viewtopic.php?f=51&t=32949

Sorry for that. I edited it. I will try and see what i get

A lot of CAM software has an option to machine along a curve. I used to draw my fret slotting toolpaths in Rhino and just have MasterCAM follow the 3D curve. Fusion360 probably has something similar.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

That's what I do with Rhino/MadCAM too. Works very well.

Dave

Yes, Fusion does the same called "Project". "Axial Offset" tells it how deep into the fretboard and "Axial Offset Passes" if you don't want to take it all in one pass. Just cut a fretboard today. I use Jesscar wire with .020 tang. Much easier to find .020 bits compared to .023 bits; but they are even more delicate.

FWIW, I also am doing 2mm deep slots but in three passes at 250mm/min@30000rpm. I could probably cut it in two passes, but it wastes more time to order bits than to baby them. After all, I'm not a production shop.