Follow these simple steps to create a Custom Command in
NX CAM to add to a post processor for header lines to be output from a post processor:
Start Postbuilder.
Select the custom command tab.
Select the Create option.
Right mouse button on the new custom command and rename it. To PB_CMD_header line.
Highlight everything in the right window, as displayed below.
Once everything is highlighted, select the delete key.
Select the lines below:
#=============================================================
proc PB_CMD_header_line { } {
#=============================================================
#This Custom Command will output the header information
#this will output information associated with a program
global mom_oper_program
global mom_part_name
global mom_date
global mom_logname
MOM_output_literal "(PROGRAM NUMBER: $mom_oper_program)"
MOM_output_literal "(PART NAME : $mom_part_name)"
MOM_output_literal "(POSTED DATE : $mom_date)"
MOM_output_literal "(PROGRAMMED BY : $mom_logname)"}
Copy the lines selected above and paste them into the right side of the dialog box. It should appear like this:
Select the Program Tab.
Select the Program Start Sequence.
Select the name of the custom command you just created. In this case it should be the
PB_CMD_header line.
Select the Add block option.
Drag the command after the rewind stop code.
This will add the header lines to the beginning of the CNC program.
Want to learn more about customizing your posts? Get training in NX CAM post processing from Swoosh Technologies. Learn more here!
Written by
Brian Brown
Application Engineer
Swoosh Technologies
