[srl]

I'm using NX7.5 to program a Okuma VTM200YB. On the Okuma, when using cutter comp, it needs a tool offset consisting of three offsets eg: The code would be TL=101010 if I was using tool 10, offset 10 and cuter comp offset 10. If I was using tool 12 it'd be TL=121212 etc. The problem I'm having is when I post process it only comes out with two offsets. I've tried altering it in post builder but I've had no luck thus far.

Any help would be appreciated.

[Buntron]

srl,

I have done something similar using a custom command placed in the operation start sequence. This custom command will automatically set your length and diameter offsets if you have left them at 0 while inside NX. Let me know if you need a hand or if I've made a mistake.

the code I used was:

global mom_tool_number
global mom_cutcom_adjust_register
global mom_tool_adjust_register
global mom_cutcom_status
global nr_tool_adjust_register
global nr_cutcom_adjust_register
global nr_tool_number

set nr_tool_adjust_register $mom_tool_number

if { $mom_tool_adjust_register != 0 } {

set nr_tool_adjust_register $mom_tool_adjust_register

}

# sets your H number automatically

if { $mom_cutcom_status == "UNDEFINED" } { return }
if { $mom_cutcom_status == "OFF" } { return }

set nr_cutcom_adjust_register $mom_tool_number

if { [info exists mom_cutcom_adjust_register ] } {
if { $mom_cutcom_adjust_register != 0 } {
set nr_cutcom_adjust_register $mom_cutcom_adjust_register
}
}

# sets your D number automatically

set nr_tool_number [ expr (10000 * $mom_tool_number ) + ( 100 * nr_tool_adjust_register ) + ( nr_cutcom_adjust_register ) ]

#RENAME YOUR TOOL BLOCK AS $nr_tool_number
#PLACE COMMAND IN OPERATION START SEQUENCE

[nximran]

you have skype id................my id add _nximran