X not posting work offset numbers

[Jeremy Grigsby Excelsior Marking]

In 9.1 my post would put the g54's in the nc file at the tool change, now it looks like its putting g28's What do i need to change?

Also when you make a new tool, can it still default to having the length and dia offset set to the tool number without typing them in the edit tool dialog?

 

%

O0

( MACHINE_GROUP_1 )

(DATE=DD-MM-YY - 11-08-05 TIME=HH:MM - 15:06 )

N1 G20

N2 G0 G17 G40 G49 G80 G90

/ N3 G91 G28 Z0.

/ N4 G28 X0. Y0.

/ N5 G92 X10. Y10. Z10.

( ) ( TOOL - 1 DIA. OFF. - 0 LEN. - 0 DIA. - .25 )

N6 T1 M6

N7 G0 G90 X.5179 Y-.1551 S14500 M3

N8 G43 H0 Z.25

N9 Z.1

N10 G1 Z-.25 F50.

[crazy^millman]

Do you have workoffset checked in the planes dialog box?

 

Do you have the Control Def set to the workoffsets to use workoffsets in the Work System? There are 4 options here.

 

HTH

[Ke Wang CNC Software]

Did you check your misc values? Usually the misc interger 1 controls g54/g92.

[Kelly Burns]

Look down the screen at "Anyone know how to access the Post". We talked to CNC Software on this earlier today.

[Carl Hessig]

Had the same problem with my makino post.

Goto the machine type menue above toolbar

select control defintions > misc. int/real values

& in the Work coordinates box put a 2 & in the real

values I think it #3 not sure but if its got 118.0

change it to 0.0 Also make sure at the bottom

to check (from these settings) to intialize toolpath operation.

Also while in the control defintions > operation

defaults you need to go into each toolpath operation & in the parameters for each toolpath

in misc. values put a check mark to auto set to post values when posting.

It takes time but it should work.

 

Carl Hessig

DJ/NYPRO

[Carl Hessig]

Just so you know the 118.0 in the real values causes

/ N3 G91 G28 Z0.

/ N4 G28 X0. Y0.

/ N5 G92 X10. Y10. Z10.

to be output in my code I think that is part of what you wanted to get rid of.

 

Carl Hessig

DJ/NYPRO