Okuma Change M06 to G116

[timwilliames]

Im running an Okuma M560-V-e and to complete a tool change we use a macro called G116. We do this because to do a tool change using M06 it also requires M62 - M64 which is annoying to always do. Im wondering if anyone knows how to edit the post processer so instead of using M06 it can be changed to G116?
I have looked in the generic Okuma mill post but cant find anywhere to edit or change it

A typical start to a program looks as follows. Note the N4 line

N1 G40 G80 G90 G94 G17
N2 G21
N3 G00 Z999.
N4 G116 T106
N5 S11716 M03
N6 G15 H01
N7 M08
N9 G00 X-54.004 Y27.021
N10 G56 Z60. HA

Thanks to anyone who can help

[sam.byrnesKB9TR · Accepted solution]

There should be a line in your post processor that looks like this:

writeBlock("T" + toolFormat.format(tool.number), mFormat.format(6));

if you change it to 

writeBlock("T" + toolFormat.format(tool.number), gFormat.format(116));

This should fix it.

[Anonymous]

Hi, in the OnSection() fuction you ha to change the code:

 if (properties.preloadTool && !isFirstSection()) {
     // writeComment("T" + toolFormat.format(tool.number));
     // writeBlock(mFormat.format(6));
     writeBlock("G116 T" + toolFormat.format(tool.number)); // senza M6
    } else {
      //writeBlock("G116 T" + toolFormat.format(tool.number), mFormat.format(6)); // con M6
      writeBlock("G116 T" + toolFormat.format(tool.number)); // senza M6
    }

[Tomek.G · Accepted solution]

Hi @timwilliames,

Could you please check the newest Okuma post with property Enable safe tool change logic set to Yes instead?

Thanks!

[tntmachineco]

I'm unable to locate this specific >>> OnSection() <<< line item in my 2023 Okuma.cps version. What line item should I be looking for?
Thanks
John