Cancel
Showing results for 
Search instead for 
Did you mean: 

Re: Suggestion for Cam Improvement

Pioneer
Pioneer

Maybe I'm missing something here.  We output a separate program for each tool.  So we separate operations in NX into separate program groups per tool.  In postbuilder check option to "generate group output."  I highlight the master program folder at the top and post just one time, and get a separate program for each folder.  Could you do something similar to get your desired result?

 

1.png2.png3.png

Re: Suggestion for Cam Improvement

Siemens Phenom Siemens Phenom
Siemens Phenom

Hello @Patel

I understand this requirment as I have had to do for other customers in the past.

This is possible by adding the the custom command pb_cmd_tape_utils.tcl to your post.

It will output a seperate cnc file for each operation from the group you select to post. Very easy to do.

Regards

Paul

#=============================================================
    proc PB_CMD_output_tape_per_operation { } {
    #=============================================================
    #
    #  This procedure can be used to output an N/C tape with each operation.
    #  Place this custom command at the VERY begining of the Start of Operation
    #  event marker.
    #
    #  This proc will also delete the initial program tape and rename it to
    #  {operation_name}{sequence number}{extension}.
    #  Any N/C code output with the Program Start sequence will be lost.
    #
       global ptp_file_name
       global mom_output_file_directory
       global mom_operation_name
       global mom_output_file_basename
       global mom_sys_output_file_suffix
   
    #
    # Remove next two lines of code if you don't want the original nc tape
    # with the start of program info to be deleted.
    #
       set fn ${mom_output_file_directory}${mom_output_file_basename}.${mom_sys_output_file_suffix}
       if [file exists $fn] {MOM_remove_file $fn}
   
       MOM_close_output_file $ptp_file_name
   
       set ptp_file_name "${mom_output_file_directory}${mom_operation_name}.${mom_sys_output_file_suffix}"
       MOM_remove_file $ptp_file_name
       MOM_open_output_file $ptp_file_name
    }

 

Re: Suggestion for Cam Improvement

Pioneer
Pioneer
ok , i'll try this
i hope this is work for me..
thanks

Re: Suggestion for Cam Improvement

Valued Contributor
Valued Contributor

Have you tried the Batch Processing?

In Command Finder type Batch and then click search.

 

It is located in Operations Group.

 

Another is the Parallel Generate Tool Path. This will generate tool paths in the back ground while continueing the work session. Also located in the Operations Group.

EDS UG V3 -UG V15 UNIX; UGS UG V6 -UG V19 - NX-NX5 UNIX/MS; Siemens NX6-NX11 MS

Re: Suggestion for Cam Improvement

Pioneer
Pioneer

YES I'M USING BOTH OF THIS

Re: Suggestion for Cam Improvement

Solution Partner Creator Solution Partner Creator
Solution Partner Creator

Pleasw refer this thread. I hope this is what you are searching for.

 

https://community.plm.automation.siemens.com/t5/Discussion-Forum-NX-Manufacturing/Post-processor/td-...

 

Re: Suggestion for Cam Improvement

Pioneer
Pioneer

YES @Ritesh Its work , but it not work properly ..., i need proper solution.

Re: Suggestion for Cam Improvement

Pioneer
Pioneer

@Paul_Hartrick 

yes it was work for me but its not a proper solution im needed,

 

example , i have a 3 nc file

this command work not proper for me ,,.,

(1) first nc file you shows this line "N1 G40 G17 G90 G642 G54",and also end off program not shown "m30" code.

 

(2) second nc file does not shown this line in program start "N1 G40 G17 G90 G642 G54",and also end off program not shown "m30" code.

 

(3) last nc file does not shown this line in program start "N1 G40 G17 G90 G642 G54",and end off program shown "m30" code.

 

so this is not a proper work,,, im need evrytime manually add this code for all nc file.. so this is not work for me.

 

1.png2.png3.png

Re: Suggestion for Cam Improvement

Siemens Phenom Siemens Phenom
Siemens Phenom
Hi @Patel
Please make those missing commands to be force output for each operation inside postbuilder. That’s will solve the problem.
Regards
Paul

Re: Suggestion for Cam Improvement

Pioneer
Pioneer
OK , I'LL SHOW IT FOR YOUR SUGGESTION..

THANKS

Learn online





Solution Information