Showing results for 
Search instead for 
Do you mean 
Reply
Solved! Go to solution

mom_fixture_offset_value error after add PB_CMD_init_tool_list

Dear All:

I have a problem in NX CAM post builder.

I want to set tool list all in program head,and i want to set fixture_offset_value (ex:G54~G59).

But when i set tool list ,offset_value is error.

Why this post is falut?

 

13 REPLIES

Re: mom_fixture_offset_value error after add PB_CMD_init_tool_list

I'm not sure if it is causing your problem, however

"PB_CMD_init_tool_list" does not need to be added to the start of program, and certainly not after "PB_CMD_create_tool_list"

 

from the tool list procs

 

#=============================================================
proc PB_CMD_init_tool_list { } {
#=============================================================
#  This command will be executed automatically at the "Start of Program" to
#  prepare for the tool list generation.

Create tool list cycles the operations and builds the list then outputs the list before carrying on to outputting the operation code.

ie. it posts "twice" and makes it slower and creates problems like this.

 

I either output the tool list at the end.

Or output tool and other information to a second file while posting and then append it to the top of the program at the end.

Re: mom_fixture_offset_value error after add PB_CMD_init_tool_list

I have downloaded your postprocessor. Open my prt and postprocess my operation. NO ANY PROBLEMS.

POSTPROCESSORPOSTPROCESSOR

 

 

Re: mom_fixture_offset_value error after add PB_CMD_init_tool_list

I set Fixture Offset to 2 and:

 

O1234

(PART NO.: model7.prt )

(DATE: 2016/08/17 11:24:35 )

(User = Юрий)

(T 0 D16T 16.0 0.0 H= 0 D= 0 )

G90 G80 G49 G40 G21 G00

/ G10 L2 P1 X0. Y0. Z0.

/ G10 L2 P2 X0. Y0. Z0.

/ G10 L2 P3 X0. Y0. Z0.

/ G10 L2 P4 X0. Y0. Z0.

/ G10 L2 P5 X0. Y0. Z0.

/ G10 L2 P6 X0. Y0. Z0.

G91 G28 Z0.0

N1 ( T0 D16T H0 D0)

T0 M6

G0 G90 G55 X-21.653 Y151.283

G43 Z46. H0 M3 S123

/ M8

G1 F1234.

Z16. F250.

Y-21.528

X-7.171 Y-21.533

 

 

Whats wrong?

 

Re: mom_fixture_offset_value error after add PB_CMD_init_tool_list

Set Fixture Offset as 1, 2, 3 - integer values.

 

I think - you set as "G54"

Re: mom_fixture_offset_value error after add PB_CMD_init_tool_list

G54.png

 

 

Re: mom_fixture_offset_value error after add PB_CMD_init_tool_list

Sorry!

This file attachment is correct.

I forgot adjusted.

Re: mom_fixture_offset_value error after add PB_CMD_init_tool_list

You can output this again....

 

 

O1234
(PART NO.: TEST.prt )
(DATE: 2016/08/18 08:48:38 )
(User = hueim)
(T 1 ED10_L50 10.0 0.0 H= 1 D= 1 )
(T 3 BR3_L50 6.0 3.0 H= 3 D= 3 )
(T 2 ED6_L50 6.0 0.0 H= 2 D= 2 )
(T 4 DR6 6.0 118.0 H= 4 D= 0 )
G90 G80 G49 G40 G21 G00
/ G10 L2 P1 X0. Y0. Z0.
/ G10 L2 P2 X0. Y0. Z0.
/ G10 L2 P3 X0. Y0. Z0.
/ G10 L2 P4 X0. Y0. Z0.
/ G10 L2 P5 X0. Y0. Z0.
/ G10 L2 P6 X0. Y0. Z0.
G91 G28 Z0.0
N1 ( T1 ED10_L50 H1 D1)
T1 M6
G0 G90 G57 X23.924 Y32.933 T3            (Should be G54)
G43 Z10. H1 M3 S3000
/ M8
Z3.
G3 X23.924 Y32.933 Z-3.734 I-3.424 J2.067 F1000.
X20.5 Y39. Z-6. I-3.424 J2.067
G1 Y35.
Y20.5
X27.739
G2 X24.5 Y28.5 I8.261 J8.
G1 Y41.5
G2 X27.739 Y49.5 I11.5 J0.0
G1 X20.5

Re: mom_fixture_offset_value error after add PB_CMD_init_tool_list

Hi Agrivas

Becouse my guest want to show for factory CNC operating workers.

So need to show TOOL Information all in program head.

I update my files in the next post,you can try it!

Solution
Solution
Accepted by topic author cadex04
‎08-22-2016 01:03 AM

Re: mom_fixture_offset_value error after add PB_CMD_init_tool_list

In PB_CMD_save_active_oper_tool_data

 

add following line to the lappend list

 

    lappend mom_sys_oper_tool_attr_list  mom_fixture_offset_value

Updated post attached.

 

I have also removed the PB_CMD_init_tool_list from "Start of Program" as it is not required there

Learn online





Solution Information