how to add G28 to the first line of mt lathe post

[Guy Smith]

I want to add a safety line to the top of mt programs on my lathe post.  Something along the lines of

G28 U0. W0. 

 

That way the program does not start in some random place.   I'm using a generic fanuc post

[BehindYou]

Greetings Smith,

Open you post and search for lsof$  postblock.

 

Inside add what you want.

Just to remind you if you write g28 u0 w0

this will be posted only once, at the beginning of you file.

 

if you cant understand what I am talking about, PM and i will explain you.

 

Kind regards

Ivan.

[Guy Smith]

Thanks Ivan!
 

I found that variable it show up a lot in the post.  I added but it only shows up if there are no tools selected.  As in T0000.  I still need to find the right block that is at the top of the program so it the first thing it does.   A safety line so to speak no necessarily on tool change. 

[BehindYou]

can you generate G-code and show me how it should look like?

What i mean is mark what you want to add and where.

Because i think there is some kind of misunderstanding 

[BehindYou]

ltlchg$          #Toolchange, lathe
      toolchng = one
      gcode$ = zero
      copy_x = vequ(x$)
      pcc_capture   #Capture LCC ends, stop output RLCC
      c_rcc_setup$  #Setup LCC on first 60000
      plcc_lead_begin  #Save original in sav_xa and shift copy_x for LCC comp.
      pcom_moveb    #Get machine position, set inc. from c1_xh
      c_mmlt$       #Position multi-tool sub, sets inc. current if G54...

      if prv_spaces$ > zero, " ", e$
      #ptoolcomment
      comment$
      pop_desc, e$
      if prv_spaces$ > zero, " ", e$

      spaces$ = prv_spaces$
      pbld, n$, "G0", *sg40, "G80", sm24, [if nc_system_type = 0, *sg99], [if nc_system_type >= 1, *sg99_b], e$
      if home_type < two, #Toolchange G50/home/reference position
        [
        sav_xh = vequ(copy_x)
        sav_absinc = absinc$
        absinc$ = zero
        pmap_home   #Get home position, xabs
        ps_inc_calc #Set start position, not incremental
        #Toolchange home position
        if home_type = one,
          pbld, n$, *sgcode, pfxout, pfyout, pfzout, e$
        else,
          [
          #Toolchange g50 position
          pbld, n$, *sg28ref, "U0." e$
          pbld, n$, *sg28ref, "W0." e$
          if tl_offset = 1,
            [
            if t$ <> tloffno$, tloffno$ = t$
            ]
          toolno = t$ * 100 + zero
          if home_type = m_one, pbld, n$, *sgcode, *toolno, e$
          else, pbld, n$, [if nc_system_type = 0, *sg50], [if nc_system_type > 1, *sg50_b], pfxout, pfyout, pfzout, e$
          ]
        pe_inc_calc #Update previous
        absinc$ = sav_absinc
        copy_x = vequ(sav_xh)
        ]
      if tl_offset = 1,
        [
        if t$ <> tloffno$, tloffno$ = t$
        ]        
      toolno = t$ * 100 + tloffno$
      if t$ <> tloffno$,  " ///// Tool No. and Offset No. aren't same ///// ", e$
ADD ONE OF THE BELOW LINES HERE
      pbld, n$, *sgcode, *toolno, e$  #G0 tool change----------------------------------------------------------> Here is your tool number Output

HERE MOVE YOUR G54

 

what will you do here just add new line
 n$, *sg28ref, "U0.", "W0.", e$

or 

n$, *sg28ref, "U0.", e$
n$, *sg28ref, "W0.", [if y_axis_mch = yes$, "V0."], e$

It depends which axis you want to move first

 

Structure of your post probably looks different so just search for those variables in your post and set them in order 
First reference position
Tool change
G54 output

If you have some more questions feel free to send me msg