NX Altering code output without editing the post processor

Is it possible to add lines of code to a tool path to handle special situations without making edits to the post processor?  In this case, the user has had issues where the Y axis of a 4-axis lathe is not on center for drilling, so he uses an offset.  He would like to manually insert code into the tool path to force a Y0 output line without editing the post.  e.g.

( Path Name  : CENTERLINE_DRILLING_8.2 )

N0020 ( SAFTEY LINE BELOW )

N0030 G00G54G18G40G80G97G99

( Tool Number: 7 )

( Tool Name  : UGT0301_004  Tool Diameter: 8.000 )

N0040 T0707

N0050 G54

N0060 G00 Z25.

N0070 X0.

Y0.   <<  how to add/insert this line to the tool path?

N0080 G00 Z3.

This can be done using the tool path editor:

 - right click the operation in the navigator and choose Tool Path; Edit.  The Tool Path Editor dialog appears.

 - either graphically or in the list of events, select the event right before where you want to insert the new line.  Choose the Add New Path Event button at the top right:

The Create Subop dialog appears. 

 - in the Move Type list, choose Machine Control

 - in the Events Available list, choose Insert.  You can either double click the Insert choice, or highlight it and hit the Add New Event button:

 - enter the desired new line of code exactly as you want it to appear when post processed, and OK out of the dialog.  This will populate the Events Used list with your entry.  For example:

 - Ok back out to the Tool Path Editor dialog and you will see the new event in the operation list:

 - Ok out to NX and note that the operation will now be flagged with a wrench in the Path column of the navigator to indicate that it was manually edited:

You can now post process and see the extra output in the code:

Bear in mind that if you regenerate the operation, all edits will be thrown away.  This is how NX 'undoes' hand edits.  After generating the operation, you'll need to add any edits in again.  Once you are satisfied with the operation, you can lock it to prevent accidental generation.  Right click the operation and choose Tool Path; Lock.

Full documentation on the Tool Path Editor can be found here:

https://docs.sw.siemens.com/en-US/doc/209349590/PL20220512394070742.mfggeneral/opt_navtool_ont_mb3_options_toolpath