Official Luthiers Forum!

Solely owned and operated by Lance Kragenbrink
It is currently Sat May 15, 2021 11:34 am


All times are UTC - 5 hours





Post new topic Reply to topic  [ 12 posts ] 
Author Message
PostPosted: Sun Feb 14, 2021 7:01 am 
Offline
Mahogany
Mahogany

Joined: Mon Apr 01, 2013 3:01 pm
Posts: 76
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


Last edited by pikolo on Mon Feb 15, 2021 10:57 am, edited 1 time in total.

Top
 Profile  
 
PostPosted: Sun Feb 14, 2021 7:51 am 
Offline
Mahogany
Mahogany

Joined: Wed Jan 08, 2020 12:28 pm
Posts: 86
First name: Chuck
Last Name: Skarsaune
City: Butler
State: TN
Country: United States
Focus: Build
Status: Amateur
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



These users thanked the author Skarsaune for the post: pikolo (Sun Feb 14, 2021 9:44 am)
Top
 Profile  
 
PostPosted: Sun Feb 14, 2021 9:45 am 
Offline
Mahogany
Mahogany

Joined: Mon Apr 01, 2013 3:01 pm
Posts: 76
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?


Top
 Profile  
 
PostPosted: Sun Feb 14, 2021 10:35 am 
Offline
Mahogany
Mahogany

Joined: Wed Jan 08, 2020 12:28 pm
Posts: 86
First name: Chuck
Last Name: Skarsaune
City: Butler
State: TN
Country: United States
Focus: Build
Status: Amateur
pikolo wrote:
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.



These users thanked the author Skarsaune for the post: pikolo (Mon Feb 15, 2021 3:45 am)
Top
 Profile  
 
PostPosted: Sun Feb 14, 2021 12:42 pm 
Offline
Cocobolo
Cocobolo
User avatar

Joined: Sat May 02, 2009 2:59 pm
Posts: 463
First name: Marcus
Last Name: Bailie
City: Kirkland
State: WA
Focus: Build
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



These users thanked the author Marcus for the post: pikolo (Mon Feb 15, 2021 3:45 am)
Top
 Profile  
 
PostPosted: Mon Feb 15, 2021 3:47 am 
Offline
Mahogany
Mahogany

Joined: Mon Apr 01, 2013 3:01 pm
Posts: 76
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...


Top
 Profile  
 
PostPosted: Mon Feb 15, 2021 9:55 am 
Offline
Contributing Member
Contributing Member

Joined: Thu Feb 06, 2014 6:19 pm
Posts: 100
First name: Tom
Last Name: Armstrong
City: Suffolk
State: Virginia
Zip/Postal Code: 23432
Country: United States
Have you asked the Vectric Forum for help?



These users thanked the author Gasawdust for the post: pikolo (Mon Feb 15, 2021 10:31 am)
Top
 Profile  
 
PostPosted: Mon Feb 15, 2021 10:21 am 
Offline
Contributing Member
Contributing Member

Joined: Thu Feb 06, 2014 6:19 pm
Posts: 100
First name: Tom
Last Name: Armstrong
City: Suffolk
State: Virginia
Zip/Postal Code: 23432
Country: United States
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



These users thanked the author Gasawdust for the post: pikolo (Mon Feb 15, 2021 10:31 am)
Top
 Profile  
 
PostPosted: Mon Feb 15, 2021 10:58 am 
Offline
Mahogany
Mahogany

Joined: Mon Apr 01, 2013 3:01 pm
Posts: 76
Gasawdust wrote:
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 :)


Top
 Profile  
 
PostPosted: Sun Mar 14, 2021 5:43 am 
Offline
Brazilian Rosewood
Brazilian Rosewood
User avatar

Joined: Tue May 02, 2006 9:02 am
Posts: 2350
Location: Canada
First name: Bob
Last Name: Garrish
City: Toronto
State: Ontario
Country: Canada
Status: Professional
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


Top
 Profile  
 
PostPosted: Sun Mar 14, 2021 9:58 am 
Offline
Koa
Koa
User avatar

Joined: Fri Jun 22, 2007 11:14 am
Posts: 697
Location: Newland, North Carolina
Bob Garrish wrote:
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.


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

Dave


Top
 Profile  
 
PostPosted: Mon Mar 15, 2021 1:15 am 
Offline
Koa
Koa
User avatar

Joined: Mon Nov 24, 2008 12:17 pm
Posts: 1032
City: Escondido
State: CA
Zip/Postal Code: 92029
Country: USA
Focus: Build
Status: Semi-pro
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.


Top
 Profile  
 
Display posts from previous:  Sort by  
Post new topic Reply to topic  [ 12 posts ] 

All times are UTC - 5 hours


Who is online

Users browsing this forum: No registered users and 4 guests


You cannot post new topics in this forum
You cannot reply to topics in this forum
You cannot edit your posts in this forum
You cannot delete your posts in this forum
You cannot post attachments in this forum

Jump to:  
cron
Powered by phpBB® Forum Software © phpBB Group
phpBB customization services by 2by2host.com