Inkscape Gcodetools plug-in English support forum

[Nick]

Generated Gcode in EMC2

Type	Extension of vector graphics editor Inkscape
Developer	Gcodetools develop team
Written in	Python
OS	Cross-Platform (Windows, Linux, MacOS)
Version	1.6.03
License	GNU GPL
Downloads	7800+

Gcodetools

Gcodetools is a plug-in for Inkscape. It prepares and converts paths from Inkscape to Gcode, using biarc interpolation.

This article is unfinished. You can help cnc-club expanding it.
Screenshots and photos are needed. Please post them at this thread.

Features (для просмотра содержимого нажмите на ссылку)

Features

Preview of the generated Gcode in EMC

Gcodetools area pocketing

Gcodetools lathe

Gcodetools engraving by Rene

Bears by Durachko

Export to Gcode

• Export paths to Gcode
• Using circular (biarc approximation) or straight line interpolation
• Automatic path subdivision to reach defined tolerance
• Multiply tool processing
• Export Gcode in parametric of flat form
• Including personal headers and footers
• Choosing units
• Multi-pass processing
• Numeric suffix is added to generated files to avoid overwriting

Lathe Gcode

• Compute trajectories for lathe
• Fine cut
• Define fine cut's depth
• Define fine rounds
• Two different computation functions for fine cut
• Standard axis remapping

Path's area processing

• Building area paths
• Area paths could be modified

Engraving

• Building trajectory according to the cutter's shape
• Defining different cutter's shapes

Tool's library

• Defining different tool's parameters (diameter, feed, depth step, penetration feed, personal Gcode before/after each path, cutters shape, personal tool's changing Gcode)
• Tools can be managed by Inkscape's standard procedures (copy, delete, assigned to different layer)
• Multiply tools processing

Orientation system

• Applying scale along any axis
• Apply rotate in the ХY plane
• Apply translation along any axis
• Apply transforms according to arbitrary points

Post-processor

• You can create custom post-processor by writing down the commands or choose from the list of default post-processors
• Scale and offset Gcode
• Gcode commands remapping
• Parameterize Gcode
• Round floating point values to specified precision

Verifying tools for the scene

• Select and remove small paths (area artefacts)
• Tool's alignment check
• Cutting order check

Plotter cutting

• Export to Gcode for plotter with tangential knife. Forth axis A is knife's rotation.

License (для просмотра содержимого нажмите на ссылку)

License

Inkscape and Gcodetools are licensed under GNU GPL.

Install (для просмотра содержимого нажмите на ссылку)

Install

Windows
Unpack and copy all the files to the following directory Program Files\Inkscape\share\extensions\ and restart inkscape
Linux
Unpack and copy all the files to the following directory /usr/share/inkscape/extensions/ and restart inkscape

Usage (для просмотра содержимого нажмите на ссылку)

Usage

Spanish manuals and tutorials by txapuzas (También he escrito un pequeño manual de uso en español, está disponible en)
Engraving tutorial by Dormouse
Area cutting tutorial
Making gears using Gcode tools and gear extensions
Export to Gcode from previous tutorial
Version 1.1 manual and tutorial

Screenshots (для просмотра содержимого нажмите на ссылку)

Screenshots

Gcodetools plug-in tutorial (2600*1300 px png ~ 700Kb)

Curve to Gcode result

Preview of the generated Gcode in EMC

Get latest version (для просмотра содержимого нажмите на ссылку)

Get latest versions

Latest stable version Gcodetools 1.7

gcodetools.tar.gz

Gcodetools 1.7

(75.25 КБ) 103133 скачивания

Older versions(ver 1.5)

gcodetools-1.6.tar.gz

Gcodetools 1.6

(56.6 КБ) 15526 скачиваний

(ver 1.5)

gcodetools.tar.gz

Gcodetools 1.5

(21.32 КБ) 11068 скачиваний

(ver 1.4)

gcodetools.tar.gz

(14.72 КБ) 27862 скачивания

(ver 1.2)

extensions.tar.gz

(9.01 КБ) 10876 скачиваний

Dev-version

You can try the newest development version by getting it from github repository https://github.com/cnc-club/gcodetools via web interface or using git clone git@github.com:cnc-club/gcodetools.git .
You'll need to run python create_inx.py to create inx files. After that install procedure is the same with the stable version.

Translations

Gcodetools is included into Inkscape v 0.49 so it will have native translations as other Inkscape's extensions. Until it is released you can use some self made translation packs:

• Spanish translation: http://dl.dropbox.com/u/23923366/gcodetools_es_00.zip

Credits (для просмотра содержимого нажмите на ссылку)

Credits

Developers:

• Nick Drobchenko (Nick)
• Vladimir Kalyaev (Dormouse)
• Henry Nicolas (Alfcnc)
• Chris Lusby Taylor (ChrisInNewbury)

Translators:

• John Brooker (greybeard from cnczone.com)

Develop (для просмотра содержимого нажмите на ссылку)

Develop

At the moment following features are being developed:

• Plasma cutter extension
• Turning lathe extension
• Plotter extension

You can help us improve Gcodetools in several ways

• Writing a report / bug report
• Improve help and manuals
• Publish G-codes / SVGs / other code
• Publish photos / videos
• Make a bug report
• Help develop new features
• Suggest a new feature

Tested on (для просмотра содержимого нажмите на ссылку)

Tested on

Linux
Ubuntu 9.10 14.04 + inkscape 0.48 (older Gcodetools versions also work with 0.46, 0.47)
Windows
Windows XP, Windows Vista, Windows 7 + inkscape 0.46, inkscape 0.47
MacOS
There are some reports on successful work on MacOs.

[Nick]

Wow awesome!
Will include that for sure!

By the way, I can include you into Gcodetools-team so you will be able to update the code dirrctly.

PS Hmmm... I'm thinking of moving the code to github...

[bartg]

Hallo everyone! I'm new on the forum.

First of all I must congratulate you Nick really usefull software you've developed.

But I have some troubles, I'm not shure if it works properly. When I do Path for Gcode options i fill G00 Z save over blank with 20, and I receive g code without any move in Z axis at all! Every path I selected and G00 pathes between them are on the same level at Z zero.

I've no idea what cause the problem, furthermore I was generating propper g codes with G00 moves safe height before.

[Nick]

Can you attach your svg and ngc so I'll be able to check them.
PS what version are you using?

[bartg]

Here are svg file and generated g-code:
https://drive.google.com/folderview?id= ... sp=sharing
Of course I selected only colored pathes, gray ones are for real elements after cutting. I use 1.7 version and as I said before I was able to generate propper tracks several times, but never as complex (and never open pathes, may be it's a reason?).

Thanks for quick response!

[Nick]

Hmmm just tested your svg everything seems to be fine...
Where do you set Z safe distance, (in Path-to-Gcode -> Preferences)?
Can you attach a screenshot of that window?

[bartg]

Yes, I set it on that tab. Here's the screanshot you asked for:

https://drive.google.com/file/d/0B1Ug7J ... sp=sharing

I tried it again, but with the same result:/

May be a piece of code I've just generated would help:

M3
(Header end.)
G21 (All units in mm)

(Start cutting path id: path4032)
(Change tool to Default tool)

G00 Z0.000000
G00 X791.977310 Y50.824528

G01 Z0.000000 F400.0(Penetrate)
G01 X790.442699 Y44.130556 Z0.000000 F1600.000000
G01 X759.945088 Y44.130556 Z0.000000
G01 X759.945088 Y46.935167 Z0.000000
G01 X760.744793 Y46.935167 Z0.000000
G01 X757.982317 Y46.935167 Z0.000000
G01 X758.736810 Y46.935167 Z0.000000
G01 X758.736810 Y44.130556 Z0.000000
G01 X729.615004 Y44.130556 Z0.000000
G01 X728.080421 Y50.824528 Z0.000000
G00 Z0.000000

(Change tool to Default tool)

G00 Z0.000000
G00 X727.401310 Y53.823139

G01 Z0.000000 F400.0(Penetrate)
G01 X725.866754 Y60.525917 Z0.000000 F1600.000000
G01 X794.190977 Y60.525917 Z0.000000
G01 X792.656394 Y53.823139 Z0.000000
G00 Z0.000000

Edited: And have you generated it succesfully?

[bartg]

My fault. I didn't notice 0.00 Z scale in Options tab. I changed it to 1 and everything's fine. I'll cut my work as soon as I get 2mm collet. I'm sorry for mess.

Keep going!

[bricofoy]

Hi there

This is my first post here, so I will explain a bit what I do.

But first, a LOT of thanks and congratulations for the job done making this plugin It was something really missing to the open-source CNC world.

I use linuxCNC on my router for gluing solarpanels at work, and when work is done, I pretty often unscrew the glue pump from the machine, put a spindle on it, and play with gcodetools... And here is my Xmas gift of this year : a little bird's house. To be cut in a 800x600x10mm wood panel with a 6mm cylindrical tool, glue/nails-free assembly, suitable for chidren.

Here are the svg and the ngc files for those who want to try it :

ok_COMPLET_trous_larges_1passe_0001.ngc

(187.74 КБ) 1297 скачиваний

chemins -3mm, calepinage 800x600, chemins, trous larges.svg

(59.2 КБ) 1079 скачиваний

Should look like this at the end :

I would like to help you making this wonderful tool, but I understand mostly nothing to python... So as I'm french, I propose to help for french translation if needed.

Have a good day

Yann

[Nick]

Wow cool! Birds should like it .

As of the translation... Gcodetools is included into Inkscape, so all translations are to be made inside inkscape's POT files.
But I've heard that they plan to put translations of the extensions outside, so probably we will be able to make our own translations without pushing the code into inkscape...

[torriem]

Great work on this extension! It's the only g-code generator I've seen that can generate lead-ins and lead-outs for plasma cutting. I am using the version 1.7, linked to on the first post. I assume this is the latest version?

Two questions though:
1. Is it possible to control the order of the cut paths? Right now if I have a hollow drawing object (say a circle with another circle removed from the inside of it), the generated g-code cuts the outer path first, before the inner path. This is not correct. The inner paths should always be cut first with a plasma cutter (well most 2-d cutters I imagine, such as vinyl).

2. Is it possible to change the direction of the paths? For plasma cutting the current generated directions are backwards. Outer cuts should always be clockwise and inner cuts should be counter-clockwise because of the way the plasma jet swirls. I understand that this is backwards of the direction rotary cutters are typically moved.

I can hack the python code easily enough, if I am pointed in the right direction.

[Nick]

1. Is it possible to control the order of the cut paths? Right now if I have a hollow drawing object (say a circle with another circle removed from the inside of it), the generated g-code cuts the outer path first, before the inner path. This is not correct. The inner paths should always be cut first with a plasma cutter (well most 2-d cutters I imagine, such as vinyl).

Right now you can control order by moving paths up/down along imaginary Z axis. I.e. the paths that are above others will be cut firstly.
(and you will probably need to uncheck auto sort paths to reduce rapid moves).

2. Is it possible to change the direction of the paths? For plasma cutting the current generated directions are backwards. Outer cuts should always be clockwise and inner cuts should be counter-clockwise because of the way the plasma jet swirls. I understand that this is backwards of the direction rotary cutters are typically moved.

In Inkscape - Path - Reverse path.

[torriem]

Thanks, Nick! That sounds like it should work out. When you say move the path up the Z axis, do you mean I do something in Inkscape once the plasma paths have been created but before I generate the G-code? I'll give it a go.

[bricofoy]

yes, you have to play with the objects position. With inkscape (or other vector drawing tool, for what i know) you can define objects (here, your pathes) to be in front of others. So the path in front will be cut before the path in back.

[torriem]

Got it. Many thanks! Looks very good! I just had to break my paths apart so that I could manipulate the inner path separately from the outer.

Is there any provision for setting a tool width so that the cut is always outside the shape instead of right on the line? Or do I just need to take that into account when drawing things up?

[bricofoy]

This is what I do myself : I draw my path right where it should be, and then I use the inkscape command "inset" or "outset" from the "Path" menu, Ctrl+( or Ctrl+)

Buuuuuuut....... I look into inkscape to see the exact english menu name to tell you... and there is a big problem, inkscape should ask for the amount of units you want to inset or outset the path... so you can move your path for half your tool size and it's ok. And now with the newest version I have, the amout of move is defaulted to 2px and I can't find any way to change this. Documentation just says the default is 2px. Looks like they changed a very usefull feature to a totally pointless one
Does anyone know if there is a way to change that value ?

EDIT : ok I found out one solution, it's explained into the "gears" tutorial here : http://www.cnc-club.ru/forum/viewtopic. ... rt=20#p194
you should use "dynamic offset" and do some boring xml editing to adjust the value. But at least you can do it.

[Nick]

inkscape should ask for the amount of units you want to inset or outset the path... so you can move your path for half your tool size and it's ok. And now with the newest version I have, the amout of move is defaulted to 2px and I can't find any way to change this.

There are two ways either Path - Dynamyc offset (Ctrl+J) and edit amount in XML editor (Ctrl+Shift+X), or you can define offset's step in Preferences- File-Preferences-Steps.

The bad thing that offset is really complicated procedure and it changes the path from time to time, i.e. offset can be not accurate.

[bricofoy]

Thanks for the tip ! Why the hell is this not mentionned in inkscape documentation ?

Can we imagine a future version of gcodetools can have an option to use G41/G42 for tool radius compensation when using path-to-gcode ? http://linuxcnc.org/docs/html/gcode/gco ... 41_1-G42_1
So we can draw the exact path, set a tool to use, and the rest is automatic...

Problem in that case can be for determining if it should use left or right compensation, but I think you can select this with the color asigned to the path stroke, e.g. green for right and red for left.

Or with the path direction, maybe ?

[Nick]

You can try to add G41/G42 into Tool's change Gcode.
But! If there are small segments in the sharp angles which can not be reached with defined tool's radius LinuxCNC will raise an error that those segments can not be reached and will refuse to execute the code.
As I've said offset is really complicated procedure... so even linuxcnc can not do it for every path...

[billt]

I have used the engrave tool on the path shown, however it produces extra engraving paths at the upper "T" and the lower "d". Is this a problem with my settings, or could it be an issue with the gcode program? svg and ngc files are attached as well. Thanks - BillT

[billt]

I eventually figured this one out.
There were duplicate path points that caused the engraving path problems.
After removing the duplicate points, the engraving path is now fixed.

For some reason the engraving is now offset from the original path.
I am not sure what causes this issue.
All of the paths have been combined prior to running the engrave operation.
Any help would be appreciated.

Thanks - BillT