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) 27861 скачивание

(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]

Dear all

I'm great fan of cnc-club and milled several projects so far. Yesterday I experienced a problem. The code seemed to be finde on EMC2 (Ubuntu 10.04). But when milling, it follows on a huge radius, when I understand the G-code, see picture and see what I mean. (I tried two fonts, Comics Sans / Tlwg Typist)
...

It appears that EMC2 threat G02 and G03 commands as a full circle if start and end points of the arc are closer than 0.0001 and probably if |start-end|<10^-5*R.
Thanks to psha from linuxcnc.org : http://www.linuxcnc.org/component/optio ... lish/#6787 !


I've got this bug fixed at Gcodetools-dev revision 174. You can get that version throught bazaar ("bzr branch lp:gcodetools") or throught web interface from http://www.launchpad.net/gcodetools .

Once again thanks for the bug report !

[Bartelime]

Hi root
I just tested the improved engraving and I see perfect result! I appreciate your help and your time you invest in this great plugin.
Again, thanks very much !
Regards
Bartelime

[Nick]

You are welcome !

By the way do you have any photos to post in this forum?

[geekinesis]

Hi

The code works great. The only problem I have is the scale of the output. The gcode, when imported into emc appears to be at about 20 percent of the size of the original inkscape drawing?

[Nick]

What units do you use in the inkscape?

Post here an svg file and generated ngc, and I'll try to get your problem solved///

[roteng]

problem with Z depth:

This morning I used inkscape .48 with your entension to generate gcode using mm and z axis parameters 5 mm safe, surface 0.0, and depth -0.01 it generated top portion shown below:

Header)
(Generated by gcodetools from Inkscape.)
(Using default header. To add your own header create file "header" in the output dir.)
M3
(Header end.)
G21 (All units in mm)

G00 Z5.000000
G00 X5.766556 Y-8.309251

G01 Z-0.010000 F100.0
G03 X5.801289 Y-7.860250 Z-0.010000 I-21.541572 J1.892197 F400.000000
G03 X5.827190 Y-7.402779 Z-0.010000 I-22.343967 J1.494543
Mach3 read file, objects egraved very well.

Then tried same object with some added objects using the same z axis parameters 5 mm safe, surface 0.0, and depth -0.01 it generated top portion shown below:

(Header)
(Generated by gcodetools from Inkscape.)
(Using default header. To add your own header create file "header" in the output dir.)
M3
(Header end.)
G21 (All units in mm)

G00 Z5.000000
G00 X20.257776 Y32.258771

G01 Z-10.000000 F100.0
G01 X20.201933 Y32.234045 Z-10.000000 F400.000000
G03 X20.152934 Y32.153001 Z-10.000000 I0.182507 J-0.165678
G03 X20.112459 Y31.923775 Z-10.000000 I0.625309 J-0.228600

The z won't show up as -0.01 it shows up as -10 as seen above. The text in the origin that the extension adds, shows (100.0;0.0;-0.099999) which looks like the right z depth, but why does it only create -10 as the zdepth?

[Nick]

Attach your svg file please. I'll got to check it.
It's a strange behavior...

[roteng]

attached is the inscape file both before the extension and after running the extension. I had to remove a few converted text elements that were paths to make it more generic, this version still generates the -10 on the Z axis.

[Nick]

I thought that you've got problem with "Path to gcode". That's why svg is important .

Now to the point.
It seems that there's something wrong with the default tool. Try go to Gcodetools->Tools Library and add an cone cutter definition. It worked for me.

By the way what cutter's bit are you planing to use to engrave it?

[roteng]

I usually use either a half round or a profile on an old 3 axis hermes vanguard 3400 on aluminum.

I admit I am unsure which tool type for the roatry engraver.

Can you explain what the difference between pressing apply from the engraver tab vs pressing apply from the gcode tab? If I add a cone as you suggest and use the gcode tab, I get the desired result, but if I use the engraver tab, the result in terms of the z depth is different.

Thanks,

Lee

[Nick]

Engraving makes a trajectory inside the path. And edges of machined trajectory should fit the original path. Z depth of the trajectory will be different for different parts of the path and it depends on the cutter's shape and path's "width" at that part.

Path-to-gcode converts the path into gcode trajectory. And cut it at the defined depth.

So here's a small illustration:

Here's an engraving example:

And Path to Gcode: Notice the letters

[inizul]

First of all, thanks for your program.
It works great, it's fantastic!

I am doing a G-Code file viewer program, and I use files made with your program to check it.

NOTE:
I downloaded the file gnu.ngc on this page and do not have the GNU !!
only the text shown in the picture.

https://picasaweb.google.com/lh/photo/f ... directlink

Thanks again

[Nick]

OMG you are right!

The GNU is missing !!!

I'll fix that bug !

[alfcnc]

Hi !
I'd like to have an option on the offset function that's make a new layer with the offset path create by the offset function.
This doing won some time when generate the pre-process for cutting path with multiple zone with different order of cutting...
This give the ability to d'ont have to select all the path between the offset and the original one when doing path to gcode
but just have to select all path on visible layer that were the one generate by offset function....

I hope you understand me...
Have a nice day.

[Nick]

Which offset function do you mean? The one from the Gcodetools (it only appears in the dev version), or Inkscape's offset functions?

Usually all paths that are made by Gcodetools are put in the separate group. You can easily push them to another layer by Ctrl+PageUp/PageDown.

[alfcnc]

Yes i think about the Offset function of Gcodetools-dev...
For now i do it like you say Ctrl+PageUp/PageDown.
But when having many path that were offset it's long after each offset to set them to a layer...if Gcodetools have an option to done this directly i found that's were faster to work with don't you ?

Have a nice day.

[alfcnc]

Hi !
Ill try to test new dev release of gcodetools , first the lathe extension but nothing work.
And after just the path to gcode and same problem ??? Inkscape 0.48 on Debian.
The svg is just a spriral , Two orientation point set with gcotools dev 1.6 last rev 173.
And standard tool... and i have nothing done and no errors...if I'll set the option direct viewing and then I have :

Traceback (most recent call last):
File "gcodetools-dev.py", line 5396, in <module>
e.affect()
File "/usr/local/share/inkscape/extensions/inkex.py", line 211, in affect
self.parse()
File "/usr/local/share/inkscape/extensions/inkex.py", line 139, in parse
self.document = etree.parse(stream)
File "lxml.etree.pyx", line 2706, in lxml.etree.parse (src/lxml/lxml.etree.c:49958)
File "parser.pxi", line 1522, in lxml.etree._parseDocument (src/lxml/lxml.etree.c:72015)
File "parser.pxi", line 1552, in lxml.etree._parseFilelikeDocument (src/lxml/lxml.etree.c:72325)
File "parser.pxi", line 1435, in lxml.etree._parseDocFromFilelike (src/lxml/lxml.etree.c:71240)
File "parser.pxi", line 997, in lxml.etree._BaseParser._parseDocFromFilelike (src/lxml/lxml.etree.c:68381)
File "parser.pxi", line 539, in lxml.etree._ParserContext._handleParseResultDoc (src/lxml/lxml.etree.c:64257)
File "parser.pxi", line 625, in lxml.etree._handleParseResult (src/lxml/lxml.etree.c:65178)
File "parser.pxi", line 565, in lxml.etree._raiseParseError (src/lxml/lxml.etree.c:64521)
lxml.etree.XMLSyntaxError: Document is empty, line 1, column 1

Thanks !

I have always the problem on this computer.. I have try to update... search difference between others computer...and I found that this computer
is in utf8 not the others... the bug should probably be this one....

http://comments.gmane.org/gmane.comp.py ... devel/1852
excuse me to reload this post but If someone have the same problem this make win some time.... when i have time i'll test to change encoding to see if this correct the problem...

[alfcnc]

Hi !
I'll try to test the Stable version , on top of this thread... v 6.0.4 is write.
But after download and install the help tab of gcodetools says ver: 1.6.01...

Not a drama...

[alfcnc]

Hi !
I have the path show under this was design from Qcad in dxf...
This give me on inkscape this with just stroke activate...

If setting fill the form become this....

If I do Area with Gcodetools this give me the area of the shape from the fill shape not the stroke....
bad for me....and curious results...

here the svg...

test_area.svg

(13.96 КБ) 894 скачивания

The alone solution i have found...
Is Stroke to path Ctrl+alt+c
Union Ctrl++
Apply Close Curve to have clean curve...
And then Area...
But this give me twice path were I have one ....
And When doing Area this make Inside outside offset path were I require just the In or Out...???
Then i can do path to gcode and then take just the path in or out from path to gcode and then apply
path to gcode to the inside or outside path but very complex...
If you have a better solution....

Thanks ! nice day to you.

[alfcnc]

Hum I reply me...for give more accurate..
Because it is possible too use the method on the tutorial of this post...with Boolean operation...
But I'd like to stay with the original path to don't have distorsion of it's size...
Because when doing Stroke to path it have the with of the Stroke adding to the size...