Post Process from a script

[Inventthis]

Hello,
Please help.
I am using FC 0.18 and I just need a script to post process the path since I am writing a macro to save G Code to a file.
I am using linuxcnc as a post processor and I have used the following without success

import linuxcnc_post
linuxcnc_post.export (ObjectName,"C:/Documents/FreeCAD-Gcode/outputFile.cnc", " ")

What ObjectName should I referenced from the screenshot below ?
I have tried many combinations without success.

If there is another way to do it, please share as the script should be able to save without dialog box confirmation

I am able to manually post process the "Profile_Edges" path
Thanks

[dubstar-04]

Could explain a bit more about the goal and the required outcome?

Post processing the path job will write GCode to a file using the selected post (linux_cnc for example)

Does this not achieve what you require?

Note that each operation contains generic gcode. A rough example (There are much better ways to do this using the Path.Utils):

job = App.ActiveDocument.getObject('Job') # Get the path 'job' from the current document
ops = job.Operations.Group # Get the operations group from the job
op = ops[0] # Get first operation from the job group
commands = op.Path.Commands # Get the commands from the operation

Thanks,

Dan

[Inventthis]

Thanks for replying

I would like the script to post process the file using the linuxcnc post processor (saved in the C:\Program Files\FreeCAD 0.18\Mod\Path\PathScripts\post) and save it without further intervention to a file on my computer so I can just use it to machine the part

I am trying to save the Path to a file so I get an output like this:

(Exported by FreeCAD)
(Post Processor: linuxcnc_post)
(Output Time:2020-04-18 23:24:07.240089)
(begin preamble)
G21
G90
G17
G40
G80
G21
(begin operation: Default Tool)
(machine: not set, mm/min)
(Default Tool)
M6 T1
M3 S15000
(finish operation: Default Tool)
(begin operation: Profile_Edges)
(machine: not set, mm/min)
(Profile_Edges)
(Uncompensated Tool Path)
G00 Z14.000
G00 X780.000 Y950.000
G00 Z6.000
G01 X780.000 Y950.000 Z-5.000 F600.000
G01 X780.000 Y150.000 Z-5.000 F1200.000
G01 X120.000 Y150.000 Z-5.000 F1200.000
G01 X120.000 Y950.000 Z-5.000 F1200.000
G01 X780.000 Y950.000 Z-5.000 F1200.000
G01 X780.000 Y950.000 Z-10.000 F600.000
G01 X780.000 Y150.000 Z-10.000 F1200.000
G01 X120.000 Y150.000 Z-10.000 F1200.000
G01 X120.000 Y950.000 Z-10.000 F1200.000
G01 X780.000 Y950.000 Z-10.000 F1200.000
G01 X780.000 Y950.000 Z-15.000 F600.000
G01 X780.000 Y150.000 Z-15.000 F1200.000
G01 X120.000 Y150.000 Z-15.000 F1200.000
G01 X120.000 Y950.000 Z-15.000 F1200.000
G01 X780.000 Y950.000 Z-15.000 F1200.000
G00 Z14.000
(finish operation: Profile_Edges)
(begin postamble)
G0 X0.000 Y0.000
M05
G17 G54 G90 G80 G40
M2

[dubstar-04]

Its a bit hacky but if you're not looking to do anything special then you should be able to do something like:

import PathScripts.PathPost
myPost = PathScripts.PathPost.CommandPathPost()
myPost.Activated()

This will require the output policy to be set to overwite or append unique ID in the preference or you could so it in python. See PathPreferences.py.

DeepinScreenshot_select-area_20200420214352.png (106.75 KiB) Viewed 1396 times

Thanks,

Dan

[Inventthis]

Thanks again for your input. I am trying to learn Python as I am getting better at FreeCad as well.

I have tried your suggestion but I get an error message and I am not sure that I will achieve the expected result.
On FreeCad 018, the path preferences as shown in your picture has changed.

I am just wanted to write the G-Code output to an external file using the post processor file linuxcnc_post.py

The following code is from the wiki page

import linuxcnc_post
linuxcnc_post.export (ObjectName,"C:/Documents/FreeCAD-Gcode/outputFile.cnc", " ")

What ObjectName should I referenced to be able to write the G- code path to an external file using the linuxcnc_post ?

Thanks.

[dubstar-04]

import linuxcnc_post
linuxcnc_post.export (ObjectName,"C:/Documents/FreeCAD-Gcode/outputFile.cnc", " ")

What ObjectName should I referenced to be able to write the G- code path to an external file using the linuxcnc_post ?

Thanks.

The objectName should be a list of the objects to be post processed. using this method will only process the gcode from each object you pass.

An example of posting all the ops from the operations group:

Code: Select all

from PathScripts.post import linuxcnc_post as pp
obj = App.ActiveDocument.getObject("Operations").Group
pp.export(obj, 'C:/Documents/FreeCAD-Gcode/outputFile.cnc', '')

I hope that helps.

Thanks,

Dan

[chrisb]

Thanks! Bookmarked this one!

[Inventthis]

Thank you so much Dan, it worked. I just have to disable the Input box that pops up for validation [ok] and [cancel] since from the script running I do not wish any more user interaction.

[Inventthis]

Hello Dan
I found the argument in linuxcnc_post to get rid of the validation box

pp.export(obj, 'C:/Documents/FreeCAD-Gcode/outputFile.cnc', '--no-show-editor')

Thanks again for your help

[Inventthis]

import linuxcnc_post
linuxcnc_post.export (ObjectName,"C:/Documents/FreeCAD-Gcode/outputFile.cnc", " ")

What ObjectName should I referenced to be able to write the G- code path to an external file using the linuxcnc_post ?

Thanks.

The objectName should be a list of the objects to be post processed. using this method will only process the gcode from each object you pass.

An example of posting all the ops from the operations group:

Code: Select all

from PathScripts.post import linuxcnc_post as pp
obj = App.ActiveDocument.getObject("Operations").Group
pp.export(obj, 'C:/Documents/FreeCAD-Gcode/outputFile.cnc', '')

I hope that helps.

Thanks,

Dan

Hello Dan,
You are correct , I just found out that the information from the "Default tool" is not in the G-code such as:
(Default Tool)
M6 T1
M3 S15000

Do you know how to add that to the post processor script?
Thanks