Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Parallel 3x error string select is out of range 11


Recommended Posts

I modified a generic post for Okuma 3x.  Been running for some time but when I use Parallel and output 3x I get this error:

pst 694 - the value of the string select selection variable is out of range: 11

pst 715 - the value of the string select selection variable is out of range: 11

I have look for some time and cannot find my error.

Thanks,

steve

648060883_posterror.GIF.693226287db99db7bd60d6e8a040db56.GIF

 

 

OKUMA 3X 650.pst

Link to comment
Share on other sites

Right off the bat I'm seeing that both problem lines are using sgcode string variables so I would look at that string select table first. What version of Mastercam did this post originate from? You might need to get the latest version of MPMaster and compare the string select tables for that variable to see if yours needs to be updated. I had the same problem with some of my posts, except it was just for the newer High Speed surface toolpaths, so nothing that would wreck the post, but it was annoying to see them all the time.

Link to comment
Share on other sites

Range = 11 is the prime clue.

5X motion is output as "NCI GCODE 11", which is just point-to-point Vector Moves. The post usually detects this, and sets 'gcode$' back to '1', prior to output. Or, there is somewhere where 'gcode$' is being changed.

The 'sgcode' String Select, uses the Numeric Variable 'gcode$' to control the modal output of motion Gcodes.

  • Like 1
Link to comment
Share on other sites
Collin, it did get rid of the error but did not post past the tool change.  I am unsing mcam 2018.  This program uses the parallel utility transform rotation if that helps.
Thanks guys,
Steve
%
O0000(1159LM41008-11 OP 1 AND 2)
(31-08-18 - 06:18)
( T13 | 3/8 BALL ENDMILL FINISH TOOL  .875LOC 1.CLR | H13 )
G17 G40 G80 G90 G15 H01
( FINISH CORNER RADIUS )
N13 T13 M6
( 3/8 BALL ENDMILL FINISH TOOL  .875LOC 1.CLR | TOOL - 13 | DIA. OFF. - 13 | LEN. - 13 | TOOL DIA. - .375 )
G0 G90 X-.863 Y.6614 S5800 M3
G56 H13 Z1. M8
M5
M9
G00 G90 Z20.
M30
%
Link to comment
Share on other sites

Looks like the 3X Posts might be missing some code to properly process 5X output (in a 3X environment).

Try adding this Post Block (it isn't in your current post), below the 'pmx$' Post Block:

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

 

  • Like 1
Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...