Edit Tool Change Macro Oi-MC

[dtmtim]

The current tool change macro does not check to see if the called tool is already in the spindle. As a result the spindle will do a G91 G28(or G30) Z0 several times before starting the machining cycle. I would like to edit the macro to skip everything if the called tool is already in the spindle. Does anyone know the variable numbers that store the called tool number when the M6 is executed? There are no variable definitions in the tool change macro but it has to get the input fromn somewhere. Also does anyone know the variable number that stores the number of the current tool in the spindle?

Thanks to all !!!

Tim

[f-bu]

#4120=last T code
For the tool in the spindle, if it is not stored in some variable #500..#999, then the PLC stores that info. But you can add a line just before M99 in TC macro like:
#999=#4120 (CURRENT TOOL)

best regards,

[dtmtim]

Great - thanks f-bu. I thought it was 4120 but when I checked it the first time it was empty. It looks like you have to grab that variable right away because it doesn't stay. I think my code is going to look something like this ...(pseudocode)

beginning...
#998 = #4120
If #998 = #999 then (skip all the spindle moves)

end...
#999 = #4120
M99

Does this make sense?

[f-bu]

Yes, that is. Well, you can add come checks for correct values, because switching off during tool change will not update #999.
Another thing, if the tool change is made only by T##, without M06, then inside o9000 #149 holds the T-code.

[dtmtim]

Thanks for all your help f-bu!!!