Inkscape Gcodetools plug-in English support forum

Nick · Сообщение **Nick** » 10 дек 2009, 10:28

: 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)

License (для просмотра содержимого нажмите на ссылку)

Install (для просмотра содержимого нажмите на ссылку)

Usage (для просмотра содержимого нажмите на ссылку)

Screenshots (для просмотра содержимого нажмите на ссылку)

Get latest version (для просмотра содержимого нажмите на ссылку)

Credits (для просмотра содержимого нажмите на ссылку)

Develop (для просмотра содержимого нажмите на ссылку)

Tested on (для просмотра содержимого нажмите на ссылку)

Nick · Сообщение **Nick** » 18 ноя 2011, 21:38

What do you mean by engrave? Could you attach a sample svg?

Basically, when you use Path to Gcode function you'll get trajectory which goes exactly trough middle line of the path. Like if you adjust 0.01 mm stroke width. When you'll make the cut, it's width will be the same with the tool's diameter. It's not necessary to set up tool's width if you are using Path to Gcode.

Engraving from Gcodetools is a little bit more complicated. For that engraving you'll got to have shaped mill bit. For example V shaped bit. And Gcodetools will try to cut the interior of the path by non constant penetration depth. (The deeper gets mill's bit the thicker becomes the cut.) It's not to easy to start with this function, and better try Path to gcode first.

About 5mm=5px, all depends of Orientation points. If there's no orientation points when exporting the path, Gcodetools will add them automatically, or you cat do it yourself using Extensions->Gcodetools->Orientation points. Once the points are added, they define scaling, rotation, and zero points. By default 1mm=1mm~3.453px~2.835pt~0.0394in.

EtchnSketch · Сообщение **EtchnSketch** » 18 ноя 2011, 22:23

I have not made the file yet, since I will make it for this extension. It is not really engraving, more like plotting, since it is 2 dimensional. The Z is just to drop to the surface. I think stroke and tool width is clear now.

I think you mean 1mm = 3.543px, since my 100.0 point is at 354.3px. I presume this is because of Inkscape, so the best thing is simply to set the document to mm, and not pay attention to pixels? If I wish to work in the xml editor (which is always in pixels for paths for some reason), I have to set 100.0 to 28.22 (well, do the math out more decimal places) so that a pixel is .1 mm... or can I move the second point in the editor to 1000.0 pixels and leave it 100.0, so that I can draw or edit xml with pixels?

Thanks!

Nick · Сообщение **Nick** » 18 ноя 2011, 23:06

EtchnSketch писал(а):I think you mean 1mm = 3.543px, since my 100.0 point is at 354.3px. I presume this is because of Inkscape, so the best thing is simply to set the document to mm, and not pay attention to pixels? If I wish to work in the xml editor (which is always in pixels for paths for some reason), I have to set 100.0 to 28.22 (well, do the math out more decimal places) so that a pixel is .1 mm... or can I move the second point in the editor to 1000.0 pixels and leave it 100.0, so that I can draw or edit xml with pixels?

You can can do what ever you want

. Yes you can move second orientation point to any place, but try not to ungroup them (use double click to get into the group). Or you can just edit it's coordinates written inside () using text tool.

The bes practice for me is to use mm for all the units in Inkscape. But I'm not using XML editor to often.

Why do you need XML editor? Is there any problem with drawing? Attach approximate sample drawing, probably I can tell you about some "secret" techniques

.

EtchnSketch · Сообщение **EtchnSketch** » 18 ноя 2011, 23:55

I want to use the xml editor because it is faster than drawing to make sure certain lines are one path instead of cloning shapes that touch each other and double checking, mergin, etc. (this is just because glass has special properties I want to respect). I also use drawing (or I wouldn't need Inkscape) for more complicated things. I understand now about the orientation points, and I hope to write back with my success story soon!

Thanks again, it is really great to see more complicated projects like this that people are devoting time to (I opened up the .py, and realized it is a lot more complicated than I thought it was).

I see now you are near Saint Petersburg. This is the one city I most want to see in the world right now. The Hermitage must be truly beautiful.

Nick · Сообщение **Nick** » 19 ноя 2011, 00:18

Usually for exact drawing I use fixed increments that can be defined in Inkscape Properties + Different snaps + (most important) BB calculated from geometry, not visible path. And some modifiers like Ctrl+moving/rotating. Sometimes I use transform dialog which allows to enter transform values manually, and sometimes clone patterns.

Hope to see your story of success soon

!

PS Some times I think that Saint-Pertsburg is better for visit for 10-20 day than living for the life time. Now it's November, lots of clouds and almost no sun. It makes me depressive

.

Nick · Сообщение **Nick** » 19 ноя 2011, 00:33

Man, you are living in 50 kilometers from Surfing spot

and still want to go to Saint-Peterburg...

But yes Hermitage is beautiful and it's only the small part of sightseeing in SPb

.

EtchnSketch · Сообщение **EtchnSketch** » 20 ноя 2011, 06:06

I am just learning about transforms and their pitfalls right now on the Inkscape forum! Since my sizes are determined by things outside of the drawing (material specifications, etc.), I have avoided snaps. I will look into custom snaps in preferences to learn if that is useful. Thanks for the great tips.

Surfing is great, but we need both great nature and great culture. I am sure you are right about it being dreary in winter! Even here it can be too much fog. I think I would go to the tanning salon for UV in winter if I lived so far north (it keeps you happy, not for color). My family is close to your longitude in Scandinavia, and it is surreal for me, since I am not from there. Summer is quite interesting, since the sun never really sets!

Nick · Сообщение **Nick** » 20 ноя 2011, 12:52

EtchnSketch писал(а):Since my sizes are determined by things outside of the drawing (material specifications, etc.)

I'm not suer that got you right... Your sizes are depend of material, not drawing?

EtchnSketch · Сообщение **EtchnSketch** » 21 ноя 2011, 05:11

Some things don't come from cnc, so the cnc must use their sizes. I can't just make everything nice and simple

.

bill.french · Сообщение **bill.french** » 29 ноя 2011, 03:59

Hello! In the earlier screenshots, there is a preference for setting the tool diameter, for offsets I imagine; that option is gone now? How do I set the tool diameter now?

Thank you!

(I am planning to use this with a laser cutter)

Nick · Сообщение **Nick** » 29 ноя 2011, 10:21

Tool's diameter was used not for offseting, but for filling the area to make pocketing. Offset itself is a really hard procedure, and it does not work properly on every path.

There are 3 options now how can you do the offset:

Use inkspape's offsets:
1. configure the steps in Properties dialog (Ctrl+Shift+P) and use Ctrl+( or Ctrl+), could be buggish, more or less depending on the Inkscape's version.
2. use dynamic offset and set exact value in XML editor (select object, Ctrl+Shift+X, change offset diameter to needed value in px), could have buggs, not to handy.
3. assign stroke width equal to 2 x needed offset radius, then Ctrl+Alt+C to Convert Stroke to path, Ctrl+Shift+K to break path appart, and finally delete inside path, not to handy again.
Use one of G41 or G42 Gcodes to compensate tool's radius, it's a good solution, giving very clean path, but some times it can give an error if the tool can not reach every path piece. For smaller radiuses this error can appear rarely.
Use Gcodetools offset function - it has more bugs that Inkscape's offset so not reccomended

PS in the dev version there's a function for plasma cutters that can add entering/exiting paths and special corner processing to make cut cleaner, but I do not know if it is actually needed in laser cutting. I'm only building my first laser cutting machine.

bill.french · Сообщение **bill.french** » 01 дек 2011, 00:42

I haven't worked on offsets yet, but I have got it working in general very well with my laser cutter and EMC2.

Right now, I'm running a "search and replace" on the following lines to turn the laser on and off:

G01 Z-0.125000 F100.0(Penetrate) becomes: M64 P0
G00 Z5.000000 becomes: M65 P0

What would you suggest would be the easiest way for this to happen automatically through the plugin?

Nick · Сообщение **Nick** » 01 дек 2011, 10:26

Sure:
1. To turn on/of the laser you can use Gcode before/after path from Tools definition (just add M65(4) P0 to them).
2. If you still need to remove Z moves use post processor "remove z moves" from the Preferences tab.

PS Are you using "search and replace" from Gcodetools post-processor or from another external editor?
PSS Gcodetools "remove Z" post-processor uses it's regex replace postprocessor

.

bill.french · Сообщение **bill.french** » 01 дек 2011, 15:23

Are these options in the development version? In the version I have (1.7 i think?) I honestly can not figure out the tools definition and I don't have an option to remove z moves under the post-processors on preferences tab.

And yes, I was just doing search and replace in a text editor.

Nick · Сообщение **Nick** » 01 дек 2011, 15:46

Probably Remove Z is only in dev version, try to use this as custom post-processor:
regexp("G0?(0|1)\s*Z\s*[\-0-9\,\.]+.*", "(removed Z)");
It should change all strings starting with G01 Z ... .

bill.french писал(а): I honestly can not figure out the tools definition

When you do Path to Gcode you can notice that some new elements are added to the drawing - at least Orientation points and Tool's definition. You can change tool's parameters using text tool (F8). So edit them and do path to Gcode once again.
You can add you Tools definition manually using Gcodetools->Tools library. And I recommend to create working template that will contain default tool and orientation points for your machine and optionally some schematic picture figuring your machine to get easier to orientate in your drawing. After that you can save the template to Inkscape's template dir and use File->New->Your template every time you need something to cut

.

bill.french · Сообщение **bill.french** » 01 дек 2011, 18:32

Wow, that's great! I did not realize you could simply edit the stuff in the green box.

OK -- how about this: any capacity to change tools? Really what I want to do is be able to have different speeds for different objects, so that my laser might quickly engrave some text, but then slowly cut out an object, in the same drawing.

Nick · Сообщение **Nick** » 01 дек 2011, 21:41

No question about it

Create two layers and add a tool to each. Only one tool can be in each layer. And tool will interference on the same layer and all layers above (or below, hmmm I do not actually remember

).

bill.french · Сообщение **bill.french** » 09 дек 2011, 22:57

Thanks for your help, I am making great progress with the laser cutter, inkscape, and gcodetools. I will have more questions!!

The boxes were made using the "Tabbed Box Inkscape Plugin" at http://twot.eu/

Nick · Сообщение **Nick** » 09 дек 2011, 23:40

Wow nice job! Glad you have posted the photos! THANKS A LOT! Some times it's really hard to get any photos or feedback from the users

!

So anyway, can I use those pictures at the main page? And why have not you posted it to the forum directly? If you want to promote your site it's ok. You can put your avd in separate theme (only if it concerns the cnc theme)!

Thanks for the link!!! I'll try to get in touch with Tabbed Box developer! Probably it'll lead to great cooperation

!

PS If you your own site I appreciate if you'll post a link to Gcodetools, it'll lead to popularize open source software and our forum of course

.
PSS If you get any questions, we'll be glad to help

!

bill.french · Сообщение **bill.french** » 10 дек 2011, 04:41

Sure, use the images however you'd like. I'm not interesting in promoting my site, this is all just for fun, for me. I just host the pictures at my web host because it's easy for me to do.
You can see some more photos at http://fubarlabs.org (my local hackerspace which has the laser cutter), there's one with me at the computer working with inkscape, you can see the gcodetools tool definitions in the background.
... and my build log at: http://www.buildlog.net/forum/viewtopic.php?f=16&t=913 -- buildlog.net tons of open source info on laser cutters. I'll also have more info at my blog at http://stopreinventingthewheel.com.

Once I get my workflow ironed out, i plan to share it as widely as possible, hopefully it helps someone. My dream would be to get it on hackaday.com.

So, here's a question: how do I create a post-processor? I want to use the "remove z motion" stuff mentioned earlier, but I'm not sure how to do it.

cnc-club.ru