posts MASTERCAM 2022 POST GETTING ERROR IN MASTERCAM 2023 / DEBURR TOOLPATH USING A LOLLIPOP ENDMILL

[EdgarMachines]

Hey guys,

I never had a problem with this post ( Generic Fanuc 3X Post) when used in Mastercam 2022 but now that I am using it in 2023 I'm getting this error. I pinpointed it to a deburr toolpath with a lollipop mill. Thank you in advance for any help!

[gcode]

I moved your post to the Post thread where it will get more eyeballs

 

I believe this error is your older post not recognizing the new deburr toolpath

The simplest way to fix this would be to download the 2023 3X post fro0m the Tech Exchange

 

[eltklas]

The error is for because a string value is out of the list. 

I had some similar error and it was the problem.

You must find wich one, but I would start for sgcode and sgabsinc

Or some misc value can be too

Good Luck.

[Colin Gilchrist]

On the error line, it tells you the "value of the string selector variable", which is "11". This is because the 5-Axis Toolpaths produce "NCI G-code 11 - Vector Moves". Something in the Post is not resetting the 'gcode$' to '0' (for rapid motion) or '1' (for feed motion). 

Your post is probably missing the following "pre-process" block:

#Pre-process rotary motion control flags
pmx0$            #5 axis gcode setup
      if drillcur$ = zero,
        [
        if fr$ = -2, gcode$ = zero
        else, gcode$ = one
        ]

[Colin Gilchrist]

This checks to see if a Drill Cycle is not-active. (drillcur$ = 1, means active, when drillcur$ = zero, means not-active).

When we are "not drilling", this block then converts the current value of 'gcode$' (11, for a 5-Axis path), to either Zero (rapid) or One (feed), based on the 'internal flag variable 'fr$'. The value is signed '-2' when we are in rapid mode, otherwise '-1' means "unchanged" (same feed value repeats). For "regular feed output", 'fr$' will be a positive decimal value, that contains the actual Feedrate unit, in either inches per minute, or millimeters per minute.

[Colin Gilchrist]

#Pre-process rotary motion control flags
pmx0$            #5 axis gcode setup
      if drillcur$ = zero,
        [
        if fr$ = -2, gcode$ = zero
        else, gcode$ = one
        ]

I rinsed the code through Notepad, so the color formatting is removed. This may help with readability.