position changes in G-code

[leotse]

Hey machinists everywhere,

I have written a relative work-intense G-code a while ago and now need one of the milled pockets to move to a different position within the XY coordinates. I first tried to implement a G92 command to simply add an offset to the position, but neither my CAM (Filou) nor my CNC controller software (WinPC NC) can handle the G92 command. But I anyway would rather change the values in the G-code directly than adding an offset, because in my world this can only lead to a lot of new problems....

So what I search for is a software where I can put in a set of G-code and tell it:
1. Search for the letter X (or Y)
2. add the value "A" to the number after the letter
3. search on

So e.g. the program gets:
N1 G1 X13 Y20
N2 G1 X14 Y30

and if I choose the X axis and "A" is -2 it returns:
N1 G1 X11 Y20
N2 G1 X12 Y30

Does anybody see a solution for this?

I do something similar when I want to change the Z height of an engraving. I copy the code into Microsoft Wordpad and use the "replace" command to change the Z-height for a set of G1 commands.



But this only works because all Z values are identical. I would like to find a similar primitive-but-fast solution for a large number of commands with changing values after X or Y.

thanks in advance from Germany
Leotse

Similar Threads:

• Check Position M6 Tool Change Code
• Biesse Parking Position Code
• Need Help!- How to transform a G code into a XYZ position?
• Need Help!- Code moving to z position before xy
• Need Help!- DYNAPATH 20, WHEN E-CODE IS ENTERED, POSITION DISPLAY DOES NOT UPDATE.

[Heavy_Metal]

Hey,

You can use G54 - G59 or shift offset by G52 ( X - Y - Z ).
If you can find Cimco Edit or an other good nc-code editor they can do the job for you.
Cimco Edit has the [ Simple Math Function ] see picture.

[mactec54]

Hey machinists everywhere,

I have written a relative work-intense G-code a while ago and now need one of the milled pockets to move to a different position within the XY coordinates. I first tried to implement a G92 command to simply add an offset to the position, but neither my CAM (Filou) nor my CNC controller software (WinPC NC) can handle the G92 command. But I anyway would rather change the values in the G-code directly than adding an offset, because in my world this can only lead to a lot of new problems....

So what I search for is a software where I can put in a set of G-code and tell it:
1. Search for the letter X (or Y)
2. add the value "A" to the number after the letter
3. search on

So e.g. the program gets:
N1 G1 X13 Y20
N2 G1 X14 Y30

and if I choose the X axis and "A" is -2 it returns:
N1 G1 X11 Y20
N2 G1 X12 Y30

Does anybody see a solution for this?

I do something similar when I want to change the Z height of an engraving. I copy the code into Microsoft Wordpad and use the "replace" command to change the Z-height for a set of G1 commands.



But this only works because all Z values are identical. I would like to find a similar primitive-but-fast solution for a large number of commands with changing values after X or Y.

thanks in advance from Germany
Leotse

You can just use a simpleG1 X------ Y--------F---. move to where you want the pocket to be, or use another work offset G55 G0X----Y-----

[machinehop5]

...write the Pocket/Program in Incremental G91 XY coordinates... then minor Editing to shift with G90 to move pocket anywhere you need possibility.

[lucaswalker]

In my opinion one of the reply above are cleaner, but if you really need the job to be done, use Notepad++

Then :

1) Install Python Script plugin from the Plugin Manager or from the official website.

2) Then go to Plugins > Python Script > New Script. Choose a filename for your new file (eg add_numbers.py) and copy the code that follows:

dx = 100.0
dy = 100.0
dz = 100.0

def AddNumberToX(match):
return 'X%s' % (str(float(match.group(1))+dx))

def AddNumberToY(match):
return 'Y%s' % (str(float(match.group(1))+dy))

def AddNumberToZ(match):
return 'Z%s' % (str(float(match.group(1))+dz))

editor.rereplace('X([+-]?[0-9.]+)', AddNumberToX)
editor.rereplace('Y([+-]?[0-9.]+)', AddNumberToY)
editor.rereplace('Z([+-]?[0-9.]+)', AddNumberToZ)

3) Run Plugins > Python Script > Scripts > add_numbers.py

You may need to manage I and J for arc centers if they are not defined as relative to starting point !

[leotse]

Awesome, thanks a lot for all the suggestions. I try to figure that out.

"machinehop5" : I tried the G91 incremental commands and it makes sense. I would not have access to the automated CAM functions in Filou as these use mostly G1-G3 commands. But for easy jobs and for my lathe this hint will be very helpful in the future, thanks.

" Heavy_Metal" & " mactec54" : I tried to use the G52 and G54 commands but my CAM software can`t handle them, so I cannot see the results in my simulation, this seems to risky to me. Now I see WinPC-NC also can handle these, but in a newer version than I have....

The Cimco simple-math-function editor is exactly what I imagined in my wildest dreams, but the software is quiet expensive. I will try the demo now, it surely has a lot of other things to offer.

"lucaswalker" Wow, thanks for that. I did all that and now have the Python script. I didn't find out, how to process my G-code with the script. I put it into another txt file and let the script run as you said, but nothing happened...



Can you give me a hint what I am doing wrong?

"You may need to manage I and J for arc centers if they are not defined as relative to starting point !" Luckily my program uses I and J relative to the start point. e.g.: N1 G2 X52.5 Y154 I-5 J0

thanks
Leotse

[lucaswalker]

Awesome, thanks a lot for all the suggestions. I try to figure that out.

"machinehop5" : I tried the G91 incremental commands and it makes sense. I would not have access to the automated CAM functions in Filou as these use mostly G1-G3 commands. But for easy jobs and for my lathe this hint will be very helpful in the future, thanks.

" Heavy_Metal" & " mactec54" : I tried to use the G52 and G54 commands but my CAM software can`t handle them, so I cannot see the results in my simulation, this seems to risky to me. Now I see WinPC-NC also can handle these, but in a newer version than I have....

The Cimco simple-math-function editor is exactly what I imagined in my wildest dreams, but the software is quiet expensive. I will try the demo now, it surely has a lot of other things to offer.

"lucaswalker" Wow, thanks for that. I did all that and now have the Python script. I didn't find out, how to process my G-code with the script. I put it into another txt file and let the script run as you said, but nothing happened...



Can you give me a hint what I am doing wrong?

"You may need to manage I and J for arc centers if they are not defined as relative to starting point !" Luckily my program uses I and J relative to the start point. e.g.: N1 G2 X52.5 Y154 I-5 J0

thanks
Leotse

Normally you just have to open your Gcode and then run the script :

[leotse]

I found the Python console and it returned this error message:

Python 2.7.18 (v2.7.18:8d21aa21f2, Apr 20 2020, 13:19:08) [MSC v.1500 32 bit (Intel)]
Initialisation took 172ms
Ready.
File "C:\Users\LeoBuero\AppData\Roaming\Notepad++\plugi ns\Config\PythonScript\scripts\Leo adds numbers to XY coordinates.py", line 6
return 'X%s' % (str(float(match.group(1))+dx))
^
IndentationError: expected an indented block

I searched the web and could solve this by adding a "space" in front all three "return... lines, then it looked like this:


And now it works, this is awesome. My pocket and the copied one with added X and Y values:

Worktime: under one minute

Thank you very much, this made my day and surely someone else can use this in the future. Have a great autumn.
Leotse

[lucaswalker]

Oops, it lost identation when I copy/paste the code I guess, sorry for that.
Im glad you have your solution !

[leotse]

I attach the python script file