The problem G90 and G02,G03

[Dima_Savenko]

I want to switch to UCCNC with Mach3, and there is one problem in the absolute coordinate system (G90) and circular interpolation (G02, G03)



In Mach3, there is no such problem when you put IJ Mode: Absolute

What should I do?

I attach Gcode: test .txt

The problem is visible in the pictures:

[ger21]

G90 is absolute distance mode, and is not the same as Absolute IJ mode.

UCCNC does not support absolute IJ mode, so you'll need to change your code to use Incremental IJ mode. Virtually all CAM software uses Incremental IJ mode.

[Dima_Savenko]

I often have to delete parts already cut out on the plasma from gcode so that I can continue working after shutting down the CNC, and I cannot in this case use the g91 system

[ger21]

G90/G91 have nothing to do with the IJ mode.

You can still use incremental IJ mode with G90.

[cncdrive]

You can ofcourse use G90/G91 absolute/incremental distance modes.
The arcs absolute/incremental IJ mode is 90.1/G91.1 which is a non-standard g-code and is not supported by the UCCNC, but this has nothing to do with G90/G91.
The UCCNC always interprets the arcs in incremental IJ mode, absolute IJ mode is not supported.

You should switch your CAM post processor to output incremental IJ code, that is understood by both the UCCNC and Mach3.

[Dima_Savenko]

Unfortunately, my postprocessor Pronest can only work on the G90 or G91 system, and it does not have a separate Arc center incremental support, I hope in the next versions you will add Arc center Absolute support, as done in Mach 3 and Mach 4.

I really like your program, and I would like to replace my Mach3 with UCCNC.
But this problem with the ARC center does not give me that opportunity.

[Robertspark]

That is a weird bit of gcode as the tool offset won't work given it has no tool number and therefore offset value

[Robertspark]

Pronest is hypertherms own cad cam package (which I did not know) for industrial plasma cutters

It seems from reading various posts on cnczone that you cannot create a postprocessor for pronest... but have to ask hypertherm to create one for you .....

[cncdrive]

I think you did not fully understand my description.
The UCCNC can work with both G90 and G91 systems.

What it does not support is absolute IJ for arcs which is G90.1.
the UCCNC always work in G91.1 which is incremental IJ mode.
Honestly I have never seen a CAM program which only supported absolute IJ for arcs, so maybe your software also supports it, you just don't know what setting to change.
Also check if your CAM software supports R code format instead of IJ, because there is no G90.1/G91.1 difference for that, because then the radius is defined instead of center point, so if your CAM software can do that then it does not matter if it is not supporting G91.1, because then R code format will still work fine with the UCCNC.

[Dima_Savenko]

All perfectly!
The absolute coordinates of the G90
Everything worked as it should, replaced the postprocessor with another one.
Thanks for the advice!!!