Fadal tlngno$ in post

[Bill]

I am using the mpfadal.pst and I was wondering if I can place or if there is such a thing as a wildcard in the post.

 

This is what the post looks like...

 

ptllncomp # Tool length compensation

if tlngno$ = 0, tlngno$ = t$ # If NOT set, default to same as tool number

if tlcomp = 1, *tlngno$ # Tool LENGTH offset number (FORCED OUT)

if tlcomp = 2, tlngno$ # Tool LENGTH offset number (IF Changed)

tlcomp = 0

 

A guy on the floor went to reuse a tool in an operation and the length offset was set to 4. The tool number was 1. Needless to say the H4 posted with T1.

 

I have a tool library with all l offsets set to zero but apparently this tool he created and failed to change the length offset the second time through.

 

Is there a way to set the post overlook tlngno and post the H value = to the T#?

 

Thanks for any help I may get.

[john316]

.

 

This will override any machine defs. or control defs.

 

In your post at this location

 

# --------------------------------------------------------------------------

# Additional General Output Settings

# --------------------------------------------------------------------------

nobrk$ : no$ #Omit breakup of x, y & z rapid moves

progname$ : 1 #Use uppercase for program name (sprogname)

sub_level$ : 1 #Enable automatic subprogram support

sub_seq_typ$ : 1 #Enable subprogram sequence number reset at sub call

arccheck$ : 1 #Check for small arcs, convert to linear

atol$ : 0.01 #Angularity tolerance for arccheck

ltol$ : 0.002 #Length tolerance for arccheck

vtol$ : 0.0001 #System tolerance

mtol$ : 0.000001 #Internal rounding for 4 dec output

met_ltol$ : 0.05 #Length tolerance for arccheck, metric

vtol_m : 0.0025 #System tolerance, metric

met_mtol$ : 0.00001 #Internal rounding for 3 dec output

tooltable$ : 1 #Read for tool table and pwrtt - use tool_table to disable

 

Add these at the end

 

tloffno$ = t$

tlngno$ = t$

 

.

[john316]

.

 

Make sure you have a number in the "Dia. offest number" and the "Length offset number" or it won't work right. When I create new tools I usually put a "1" for both parameters. When you post it the "D" and "H" numbers will be the same as the tool number.

 

.

[Bill]

Very good.

 

Thanks a lot.

 

Haven't had to deal with Mcam or post issues in almost two years.

 

Glad the forum is here. And you too John316

[Bill]

I tried that John but couldn't get it to work right.

 

What I ended up doing is...

 

ptllncomp # Tool length compensation

if tlngno$ <=>0 , tlngno$ = t$ # If NOT set, default to same as tool number

if tlcomp = 1, *tlngno$ # Tool LENGTH offset number (FORCED OUT)

if tlcomp = 2, tlngno$ # Tool LENGTH offset number (IF Changed)

tlcomp = 0

 

<=> 0and checked it with length offsets at 150,235, and 250. The NC file came back with all H# equaling T#

[john316]

.

 

I'll have to check my post to see if I forgot something. Either way you're working and that's what matters.

 

.