Tool list in NC File problem

[ICT_Outkast]

I am having a problem with the tool list in the NC file created by v9 and x. I am sure it is something simple that I am overlooking in the post. Can someone tell me what to look for? When I post the program the tool list is fine, up to the last tool. It outputs the last tool twice, then goes on. It is looking like this:

 

%

O6669

(PROGRAM NAME - 6669 )

( POST DATE: 31-08-07 )

( TIME: - 11:35 )

( = )

( PART NUMBER - 114-810048-3 )

( MACHINE - SKT250SY )

( CNC OPERATION - DRILL AND SLOT )

( = )

( STOCK SIZE - PREVIOUSLY MACHINED PART )

( FIXTURE - CHUCK )

( PROGRAMMER - JWN )

( PROGRAM REVISION - "NEW" )

( = )

( G54 )

( -Z- ZERO - FRONT EDGE OF PART )

( = )

( C-AXIS CROSS DRILL )

(TOOL - 1 OFFSET - 1)

(#3 CENTERDRILL)

(TOOL - 2 OFFSET - 2)

( 1/4 DRILL)

(TOOL - 3 OFFSET - 3)

(6.0 DIA X .281 WIDE VALENITE WHEEL CUTTER)

(TOOL - 3 OFFSET - 3)

(6.0 DIA X .281 WIDE VALENITE WHEEL CUTTER)

(TOOL - 1 OFFSET - 1)

(#3 CENTERDRILL)

G0 T0101

G19

M43

 

Thanks in advance,

 

Jerry

[mtnflyr]

The problem may be in your operations manager. If you have more than one operation with Tool 3 check to see if you have force tool change turned on after the first operation.

 

HTH

[Roger Martin from CNC Software]

Jerry,

 

What does the code in the pwrtt$ postblock look like in your PST?

[Don S at Barefoot CNC South]

Roger ver 9 post here that also does it.

 

code:

---

 pwrtt           #Buffer toolchange information, tooltable = 3 calls on 1003

if gcode = 1001, psetup

pcut_cctyp

if opcode=104 | opcode=105 | opcode=three | opcode=16, cc_pos = zero

if gcode <> 1001, plast_recd

pcur_recd

if gcode <> 1003, cc_pos = zero

!opcode, !tool_op

if gcode = 1003,

[

size1 = rbuf (one, zero)

rc1 = one

if rc1 < size1, preadcur_nxt

if cc_1013 = zero, cc_pos = zero

]

 

# Write tool table, scans entire file, null tools are negative

tnote = t

strtool = ucase(strtool)

if t >= 0, "(", tnote, "-", strtool, ") "

if t >= 0, tcnt = tcnt + 1

---

[Roger Martin from CNC Software]

Try this change...

I not tested this, but it'll only take a second of so for you to see if this makes a (positive) difference.

 

if gcode = 1003,

[

size1 = rbuf (one, zero)

rc1 = one

if rc1 < size1, preadcur_nxt

if cc_1013 = zero, cc_pos = zero

]

 

else

[

# Write tool table, scans entire file, null tools are negative

tnote = t

strtool = ucase(strtool)

if t >= 0, "(", tnote, "-", strtool, ") "

if t >= 0, tcnt = tcnt + 1

]

[ICT_Outkast]

Mine is as follows...

 

pwrtt #Buffer toolchange information, tooltable = 3 calls on 1003

if gcode = 1001, psetup

pcut_cctyp

if opcode=104 | opcode=105 | opcode=three | opcode=16, cc_pos = zero

if gcode <> 1001, plast_recd

pcur_recd

if gcode <> 1003, cc_pos = zero

!opcode, !tool_op

if gcode = 1003,

[

size1 = rbuf (one, zero)

rc1 = one

if rc1 < size1, preadcur_nxt

if cc_1013 = zero, cc_pos = zero

]

 

 

if t > 0, ptoolcomment

 

I tried adding what you posted and got an error.

[ICT_Outkast]

mntflyr,

 

No on the force tool change, and only one T3 in operations manager. Thanks tho.

 

Respects,

 

Jerry

[Roger Martin from CNC Software]

@*$^#$!

 

Sorry,

 

I forgot the "," (comma) after the else,

[ICT_Outkast]

Now I get an error on this line

 

if t >= 0, tcnt = tcnt + 1

 

Getting there, I think.

[Roger Martin from CNC Software]

quote:

---

Now I get an error on this line

 

if t >= 0, tcnt = tcnt + 1

---

D'oh!

 

I see the problem.

I gave you a "try this" based on Don's code sample, not your pwrtt code.

 

Try adding this additional test-> & gcode$ <> 1003 in the 'if' logic test that ultimately calls 'ptoolcomment'

 

pwrtt #Buffer toolchange information, tooltable = 3 calls on 1003

if gcode = 1001, psetup

pcut_cctyp

if opcode=104 | opcode=105 | opcode=three | opcode=16, cc_pos = zero

if gcode <> 1001, plast_recd

pcur_recd

if gcode <> 1003, cc_pos = zero

!opcode, !tool_op

if gcode = 1003,

[

size1 = rbuf (one, zero)

rc1 = one

if rc1 < size1, preadcur_nxt

if cc_1013 = zero, cc_pos = zero

]

 

if t > 0 & gcode$ <> 1003, ptoolcomment

 

[ 09-05-2007, 01:46 PM: Message edited by: Roger Martin from CNC Software ]