Please check the file Working_with_OOTB_MACH_Simulation_Examples.pdf and search for G28
in NX11.0.2 it is chapter 9.3
Here it is described where the position of G28 is defined
I tried to set G28 sim simulation on sim15_millturn_9ax, but it does not work on that. I copied the home position definition to the INI file, but the axes will not move in the simulation. Need to set something up for this simulation?
Is the sim looking for G28 X Y Z (and you are outputting G28 U V W?)
Try outputting (use INSERT UDE if you have to) a "G28 X0 Y0 Z0", and see if that works.
If that works, but UVW doesn't, then the issue is mapping the UVW words correctly.
If XYZ doesn't work either, then it is something else.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled
Not even G28 X0 Y0 Z0 works. I tried it at sim13_turn_4ax and there it also does not work. I've tried everything, but none of them. At sim12_turn_2ax I have tried G28 X0Y0Z0 and G28 U0 V0 W0 and both work. I also went through CSE settings and it's the same.
the OOTB G28 implementation in the Fanuc.CCF are working for single channel machine tool or I need to say for machine tools with axis names like X,Y,Z.
These axis names and related axis numbers are used (hard coded) inside the method GMe_GoToReferencePosition
To adopt it to other machine tools like sim15 with X1 Y1 Z1 etc, it is needed to copy the method into the MCF and change it. Search for hard coded axis names like e.g. "X"
The OOTB sim15 Fanuc will not use G28 as it is.
Im Having a problem with G28 as well.
Initial machine point (offset from Machine zero point) is defined in ini file.
But these values wont register. N1240P1R550 this is for X axis offset used in GMe_GoToReferencePosition.
But reading it in CSE simulation it show 0.
INI file is registered and it is correct file.
in Sim_10 G28 works and getArrayElement("AxisData", 1240, getJointNumber("X"))/GVe_dFactor shows 660 witch is correct.
So problem is narrowed down to my setup, is there any known issue that could cause this?