Gcode went wrong

Today my first gcode program went wrong. I wanted to mill a simple rectangle contour by using the tool radius compensation.
The raw material dimensions were 57mm x 25mm and i wanted to mill it to 56mm x 24mm.
The path from point 2 to 3 to 4 went wrong, but i do not understand why. In the tool table i added a 10mm tool.
Tanks for any hint.

Gcode:
G21 G17 G64 G90
F56
G0 Z5
G0 X-2 Y-2
G41 T10
Z-10
G1 X0.5 Y0.5
G1 X0.5 Y24.5
G1 X56.5 Y24.5
G1 X56.5 Y0.5
G1 X0.5 Y0.5

My quick guess would be that you've called the T10 tool load after the G41 compensation has been turned on:


Cutter compensation uses the currently loaded tool to determine the correct offset from the intended path. By loading the tool after the compensation has been turned on the compensation may not 'know' what the new tool is and assumes it is whatever diameter was used up to the point it was turned on (in your case no tool was defined beforehand, so tool diameter would be zero).

Try calling tool T10 before calling G41 and see if that corrects the issue. Alternatively it looks like you can use G41 D10 as well. The D variable forces the compensation to use tool number 10 for every subsequent compensated move. More info here;

linuxcnc.org/docs/2.6/html/gcode/gcode.html#sec:G41-G42

Isn't that what G41 does? From the manual:

To start cutter compensation to the left of the part profile, use G41. G41 starts cutter compensation to the left of the programmed line as viewed from the positive end of the axis perpendicular to the plane.

Based on the OPs picture it looks like his code started at point 1 and went clockwise around the part, G41 should have placed the cutter to the left as it went around the perimeter.

Edit: not so sure any more. The diagrams on this page make me think G42 might have been required rather than G41.

I don' t think cutter compensation is active and that the coordinate system is a bit off. G0 X-2 Y-2 would make a big dent in the corner with a 10mm tool before compensation is switched on. Not sure why compensation didn't activate, maybe lack of M6?

If a 10MM tool is loaded that program should have failed with an entry move error.
Axis shows the loaded tool at the bottom of the screen, I am not sure how the other interfaces display that information.

If you look at the sketch, there must have been a crash at X-2 Y-2 with the G0 Z-10 move, without cutter compensation. There was no report about. Probably touch off was done with the tool to sides of the block. T without M6 only prepares tool.
Since cutter compensation in linuxcnc is kind of ¿?¿ ,it`s good advice to read this part of the manual.

Thanks to all your comments. I thought it´s easier to run a simple program. I will check all suggestions in the next days.
Merry Christmas.
Mane

Here's an attached png to clarify what I posted earlier.
The red is your file with no tool loaded and no D in the G41 line. You need one or the other for linuxcnc to read the tool table.
The white is a compensated path with a lead-in, notice how it rolls around corners.

It's not hard programming if you follow the rules.
Merry Christmas to you as well.

I changed line 5 to G41 D10 and did not use the tool table. Homed the machine and touched left lower corner of the workpiece with G54. Then i loaded the program below with error "Length of cutter compensation entry move is not greater than the tool radius".
To have no problem with tool cutter entry i added line 4 to be far away from the corner. But this does not help.
The error comes right after loading the program, in the status line bottom i have no tool loaded. And G54 DRO view does not change the values when i jog around the axis by keyboard.