NX Displaying On-Machine Probe Motion in a Simulation Machine Kit

An out-of-the-box Fanuc machine kit cannot simulate a Probe Cycle when running Machine Code Simulate. The tool does not move when the probing macro is executed and an error is displayed stating that the probing cycle was not found. How can this code be simulated?

Solution

Adding an empty PRG macro file to the cse_driver -> fanuc -> subprog folder will stop the error messages but still the probe will not move during simulation. This PRG file is a text file created in Notepad whose extension was changed from TXT to PRG. The name of the file needs to begin with the letter O followed by the macro call  number. Adding the text seen below to the PRG file will cause the probe macro to read the X, Y and Z values from the probe macro call and then move to that point . More complicated probe motion can be created. The NX supplied G73, G81, etc. drill macros and the ToolChange macro file can be used as examples. The value of different probe macro words can be read using the # variables seen below.

O9821 
N1 G1 X[#24] Y[#25] Z[#26] F50.
M99


O9810 
N1 G1 X[#24] Y[#25] Z[#26] F50. 
M99

Notes and References

Please be aware that any code provided by NX CAM Support is intended to be used for sample purposes only. It is the user's responsibility to determine whether the code is suitable for the purpose.

Hardware/Software Configuration

Platform: all
OS: n/a
OS Version: n/a
Product: NX
Application: CAM
Version: V1946
Function: ISV

Ref: 001-9926449