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** » 24 июн 2014, 08:53

peanutty420 писал(а):It happens with anything i create. it will add orientation points, but when i try to add tool and path to gcode it returns this same error.

Can you post error's text once again...

narvf · Сообщение **narvf** » 22 июл 2014, 11:47

Hello. First of all thank you for wonderful inkscape extension!

I have question about cutting objects. I is hard to explain in english, but i will try.
I know how to create some simple gcode, and run linux cnc with this code to cut rectangle or a letter for example. But how to make a rectangle to not be smaller my diameter of my tool? I can manually make rectalne biggger for exmaple by 6 mm(my drill actually) but its more complicated in letters or non regular shapes. How to cut things "outside" of path and some holes in my shape "inside" of a path? Is this can be done with inkscape or linuxcnc? I don't want to make all letters bigger by 6 mm in inkscape.

I hope you can understand me

Nick · Сообщение **Nick** » 22 июл 2014, 12:24

two ways:

1. offset paths in the inkscape. Ctrl+J and adjust offset in xml editor (Ctrl+Shift+X all sizes there are usually in px). Can be some artifacts while offseting some times you will have to fix them manually. (second way using inkscape - define Steps in preferences and then use Ctrl+( or Ctrl+) )
2. add G42 offset to Gcode. But it wont work on complex paths because sometimes offset totally changes the path. You will be warned if this situation occurs.

narvf · Сообщение **narvf** » 22 июл 2014, 12:31

Thank you very much. Will check when i will be at home

F3rr31r4 · Сообщение **F3rr31r4** » 07 авг 2014, 19:10

good afternoon
I am using the code for my cnc, and presiso generate a file from a drawing of three meters, however this design will have to be divided in half to be able to cut the first part, put the machine on pause and move the sheet manually cut the second part of the file. Someone has already done it the idea of how to do?
grateful

Leandro

narvf · Сообщение **narvf** » 08 авг 2014, 11:42

Hello.
I think you have to cut your project into 2 parts, and first cut one part, then move your material and then import second part of project and set beginning point in the same place like before without homing axes - i don't know how to exactly write this in english.

HTH

narvf · Сообщение **narvf** » 14 авг 2014, 11:44

#459 Сообщение Nick » 10 янв 2014, 16:08
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...

Can you show an example how to do this? Or point me where i can see how to do this?

bricofoy · Сообщение **bricofoy** » 14 авг 2014, 15:17

some details on G41/42 in linuxcnc :

http://www.linuxcnc.org/docs/2.4/html/g ... mpensation

narvf · Сообщение **narvf** » 14 авг 2014, 15:32

Thank you, but i have no idea how can i use it? Do i have to edit file manually after exporting path to gcode or i can use file in gcodetools "Tool's change Gcode" and type someting there?

bricofoy · Сообщение **bricofoy** » 14 авг 2014, 20:26

I use it by adding it manually to the gcode file. The fact is you need to choose between G41 and G42 depending on the design of your work. If you want to have a look at the attached files, I used it to cut some protective panel for electrical box. You will see here I needed to use only G42. But in some cases you will need both.

What I do to make sure the resulting path is ok is to run the file one time without adding G41/42 in a linuxcnc simulation install, and then I make the changes and I re-run the file without cleaning axis display, so I get the two pathes displayed : the original one wich in fact is the part outline, and the tool conpensated one, so I can check if I use the right command : if the new path is on the wrong side of the part outline, then I need to change between G41 and 42.

narvf · Сообщение **narvf** » 15 авг 2014, 01:06

Thank you very much! That explains a lot and example file was helpful. But can you show me your linux cnc tool table screenshot? I am getting error about tool compensation and don't know why, i guess i will have to ask on linuxcncs forum... When i will succesfully cut something i will paste photo.

bricofoy · Сообщение **bricofoy** » 15 авг 2014, 01:42

what is the error you got ? I can't send you my tool table right now because the cnc computer is at my workplace. but it was nothing special, only a 6mm cylindrical endmill.

narvf · Сообщение **narvf** » 15 авг 2014, 01:51

I think it was ""Length of cutter compensation entry move is not greater than the tool radius" I am not sure if it has something to do with table tool even.

My table - i use 6mm drill

Error:

Sample file from inkscape:
https://dl.dropboxusercontent.com/u/396 ... t_0001.ngc

SVG file:
https://dl.dropboxusercontent.com/u/3960024/test.svg

How do you set size of orientation points? I have always 100 - do i have to change this manually?

bricofoy · Сообщение **bricofoy** » 15 авг 2014, 03:58

no, this has nothing to do with the tool table. in fact gcodetools generates a tool path wich starts and ends at the exact same place, right on the part edge. but for G41/G42 to work, you need an entry move that starts away of that part edge, and that is longer than the tool radius. You can check on my ngc file, and with my svg file : try generating the ngc file, and compare with mine to see how and where I added manually some moves.

some good explanations here : http://www.linuxcnc.org/docs/2.4/html/g ... Entry-Move

narvf · Сообщение **narvf** » 15 авг 2014, 19:29

I'm still searching - when i generate file, it is a little different. It doesn't have "G01 X[661.519941*#10+#6] Y[439.565468*#10+#7] Z[-8.000000*#11+#8] F [#21]" and first few lines with this things. And what about orientation points, how it's made to be like 675 in yours file? Do you chaneged it manually?

bricofoy · Сообщение **bricofoy** » 15 авг 2014, 19:38

yes, I canged manually the value to fit my design

the #10 #6 is because i selected "generate prametric Gcode" or somethink like that. Try with the different options.
but anyway, that doesn't matter for see the movements I added manually for the entry points in each cut.

narvf · Сообщение **narvf** » 17 авг 2014, 23:02

Actually i gave up - i have to read more about gcodes... I will just make obejcts bigger by diamenter of my tool.

bricofoy · Сообщение **bricofoy** » 18 авг 2014, 00:43

well, the explanation for entry moves on the linuxCNC website is pretty clear. I d'on't see where you are stuck ?

narvf · Сообщение **narvf** » 18 авг 2014, 11:17

I couldn't find lines that you added - i think i have to experiment with very simple gcode and then try. I think i understand instruction about entry point but don't know how to add this point for rectangle in example. Maybe on my vacation i will have more free time to read more about gcodes.

narvf · Сообщение **narvf** » 18 авг 2014, 16:51

Im sorry for making offtopic here

With this example:

Код: Выделить всё

%
(Header)
(Generated by gcodetools from Inkscape.)
(Using default header. To add your own header create file "header" in the output dir.)
(tool 6mm in linuxcnc table)
T1 M6
M3
(Header end.)
G21 (All units in mm)

(Start cutting path id: rect2987)
(Change tool to Cylindrical cutter)

G00 X-10 Y60
G41
G00 Z5.000000
G00 X0.000000 Y50.000000

G01 Z-1.000000 F100.0(Penetrate)
G01 X49.999999 Y50.000000 Z-1.000000 F400.000000
G01 X49.999999 Y0.000001 Z-1.000000
G01 X0.000000 Y0.000001 Z-1.000000
G01 X0.000000 Y50.000000 Z-1.000000
G00 Z5.000000

G40

(End cutting path id: rect2987)

(Footer)

M5
G00 X0.0000 Y0.0000
M2

(Using default footer. To add your own footer create file "footer" in the output dir.)

(end)

%

I move to x-10 and y 60 and i still get message about "Length of cutter compensation entry move is...." with x-3 and y53 it's still not working.

cnc-club.ru