Output G99 with every toolpath?

[2LiterCola]

Hello all,

 

We have 3 Mazak lathes here and for some reason, if the operator stops the program in the middle of an eia/iso program, it reverts back to g98 instead of g99. I was wondering if there is a way to have the post out put g99 for every tool path? I'm using a lightly altered copy of the generic 2 axis post.

 

Thanks.

[K2csq7]

Find the ltlchg$ postblock in your post, it should look something like this.

 

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...
     ptoolcomment
     comment$
     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$, *sgcode, pfxout, pfzout, e$
       else,
         [
         #Toolchange g50 position
         pbld, n$, *sg28ref, "U0.", "W0.", e$
         toolno = t$ * 100 + zero
         if home_type = m_one, pbld, n$, *sgcode, *toolno, e$
         else, pbld, n$, *sg50, pfxout, pfzout, e$                            
         ]

 

 

The lines that look like this..

pbld, n$, *sgcode, pfxout, pfzout, e$

or,

pbld, n$, *sg28ref, "U0.", "W0.", e$

or

else, pbld, n$, *sg50, pfxout, pfzout, e$

 

 

add >>>>> *sgfeed,

so they look like...

pbld, n$, *sgfeed, *sgcode, pfxout, pfzout, e$

or,

pbld, n$, *sgfeed, *sg28ref, "U0.", "W0.", e$

or

else, pbld, n$, *sgfeed, *sg50, pfxout, pfzout, e$

[Chris McIntosh]

At the end of the lsof, ltlchg$ post blocks you can add in the line:

 

result = force(ipr_actv$)

 

This will force out the G98/G99 at the start of every tool.

 

If you want it to be output at the first line of every operation (including when both operations use the same tool), you need to do a little more work. At the end of lsof$ and ltlchg$ you'll need to add:

 

!op_id$

 

Then at the end of ltlchg0$ you will need to add the following code:

 

if op_id$ <> prv_op_id$, result = force(ipr_actv$)
!op_id$

[Chris McIntosh]

Or follow Keith's....that works too...

[2LiterCola]

Excellent, I will try those! Thank you!!

[2LiterCola]

Is there a way also with this to output a sequence number that with every new operation?

[Chris McIntosh]

There is a built in switch in the mplmaster and mpmaster posts called tseqno. Set this variable to 1 or 2 (depending on whether you want the sequence number to indicate the tool change number or the tool number) and you should get what you're looking for.

 

If you aren't using an mplmaster/mpmaster based post, you can download the post and follow the logic in the post by searching for tseqno. Then just apply the logic to your post.

[Guest Guest]

There is a built in switch in the mplmaster and mpmaster posts called tseqno. Set this variable to 1 or 2 (depending on whether you want the sequence number to indicate the tool change number or the tool number) and you should get what you're looking for.

 

If you aren't using an mplmaster/mpmaster based post, you can download the post and follow the logic in the post by searching for tseqno. Then just apply the logic to your post.

 

 

So with that, if I check the "force tool change" box, it will output a sequence number even if the machine isn't actually going to change tools?