no line numbers

[weirdharold]

Good Day. I would like to be able to post code with no line numbers , but I don't know where to change it. Using NX5. Attached is sample code. Also using modified default 3 axis mill pui. post. Thank's in advance. Harold C.

[trandolph]

If you are using a NX post created using the post builder, open the post in the post builder. Go to the Program and Toolpath tab and select the Program Start Sequence in the left side window. Go to the right side window and see the Start of Program event that contains some block entries. Select the Mom_set_seq on and delete or remove it. Save the post and try it now. This should eliminate the sequence numbers.
If you do not have a NX Post, then go to the first operation and add an Start of Path command in the maching control tab. Sequence numbers needs to be set inactive.

Remember that the sequence numbers are used at the floor for restarting the program at a specific block and with this you will not longer have that option.

Hope this helps.
Tim

[weirdharold]

Thank's Tim. Going to the first operation and adding a Start of Path command in the maching control tab worked great for now. The box I'm on now does not have Post Builder on it, but when I get a little time I'll try the post modification on the one that does have it. Have a good Day ! Harold





After submitting this comment , realized Post Builder is on this box & modified post per your instruction's & it work's also. Again , thank's !



Harold C.

[SnakeD0ct0r]

I myself do not like sequence numbers throught my programs, however I do like one at the start of an operation. I use the tool offset number for the N#, not the tool number. I do this because the first time I use a tool it would be T01 H01, but the second time I use it it I would change the offset number, T01 H31. I find it easier to search the program by offset number. The following is a command you can cut and paste into your post that will give you N offset # and tool description at the beginning of an operation.

#=============================================================
proc PB_CMD_announce_tool { } {
#=============================================================
# -------------------------------------------------------
# PB_CMD_announce_tool
#
# Issues operator display message for tool change
# - uses TOOL CATALOG NUMBER field if present, else
# tool parent object name
#
# Bind somewhere in the AUTO TOOL CHANGE event
# -------------------------------------------------------

global mom_tool_adjust_register
global mom_sys_control_out mom_sys_control_in
global mom_tool_number mom_tool_catalog_number mom_tool_name

# set up some variables so that control OUT and IN can be
# used as needed in output blocks:
# - CONTROL OUT = ${co}
# - CONTROL IN = ${ci}
set co $mom_sys_control_out; set ci $mom_sys_control_in

if { $mom_tool_catalog_number!="" } {
set tnam [string toupper $mom_tool_catalog_number]
} else {
set tnam [string toupper $mom_tool_name]
}

MOM_output_text "N$mom_tool_adjust_register ${co}TOOL NO. $mom_tool_number - $tnam${ci}"
}

[weirdharold]

I like this modification, SnakeD0ct0r. Sometimes I have to use one tool with 2 or more H offset's. I have seen it cause some problem's in my work-place, but usually due to lack of communication. I leave note's to day-shift to alert them of this mod , but they never let me know, if say they broke Tool 1, with H1 & H11 assigned to it. But I've learned to never assume anything & first thing I do is spend a few moment's reviewing controller at start of shift, ( we use Haas ) & see what's going on . Enough rambling . The only place I found any text like your's was in the .tcl file & was here :


#------------------
# Tool list footer
#------------------
shop_doc_output_literal "$co=============================$ci"


#-------------------------------------------------------------------------------
# Restore info for the currently active tool in the program being post-prcessed.
#-------------------------------------------------------------------------------
if [llength [info commands PB_CMD_restore_active_oper_tool_data] ] {
PB_CMD_restore_active_oper_tool_data
}
}


#=============================================================
proc PB_CMD_custom_command { } {
#=============================================================
}


#=============================================================
proc PB_CMD_custom_command_1 { } {
#=============================================================
MOM_output_literal "
"
}


#=============================================================
proc PB_CMD_end_of_alignment_character { } {
#=============================================================
# Return sequnece number back to orignal
# This command may be used with the command "PM_CMD_start_of_alignment_character"

global mom_sys_leader saved_seq_num
set mom_sys_leader(N) $saved_seq_num
}






Am I even close ? Don't really know where to insert your text or replace & where .

Thank's for your help !

Harold C.

[SnakeD0ct0r]

Download attached zip file, it contains a sample post, open it up in post builder. Go to Operation Start Sequence section, I added the custom command just before the tool change. This is a hand written custom command and is not part of the out of the box data. Try this post against a sample file.

[weirdharold]

Got a little free time at work to try this out & work's good . Could not open up your post with our PostBuilder as your's is a newer version , but with the other info you gave me , I realized custom text goes in PostBuilder & I went from there & got the end result .


Thank's
Harold C.