Need Help!- macro

[msantaji1]

anyone can say the macro variable no for current tool in spindle?

[luky]

I think it is #148,please check macro variable list as ATC.

[dcoupar]

#148 is a local variable, not necessarily the tool # in the spindle.

On a 21iM, #4120 is the active T# (last T read), not necessarily the tool # in the spindle.

I'm not sure there IS a variable for the tool # in the spindle. You may have to store the T# in a 500 series variable, i.e.: #520=#4120 after the M06.

[stevo1]

Sometimes the MTB will assign a variable for the current tool in the spindle. Check your parameter book from the MTB it should specify if they used one. If they did then it will probably be assigned to one of the input/output variables #1000-#1035 or #1100-#1135. If they did not use one Dcoupar is correct the best way to track the tool in the spindle is to write it to a variable in your tool change macro.

Stevo

[luky]

Dear dcoupar,as your say,#148 is a local variable.on our Mori MC is #148=#4120 everytime as ATC.if your need system variable,please check my attached file.

[msantaji1]

hi

this is the best way to trace current tool in spindle but
if #500 changed after m06 may not possible to trace the tool. ie restriction to change #500,

thanks

msantaji1

Originally Posted by dcoupar #148 is a local variable, not necessarily the tool # in the spindle. On a 21iM, #4120 is the active T# (last T read), not necessarily the tool # in the spindle. I'm not sure there IS a variable for the tool # in the spindle. You may have to store the T# in a 500 series variable, i.e.: #520=#4120 after the M06.

[stevo1]

Lucky,
What Dcoupar means is that #148 is not "Fanucs" variable for the current tool in the spindle as you stated. #4120 is also not the current tool in the spindle. You have this in your program because either the MTB wrote it to the tool change macro or a programmer did. #148 is specific for "your" machine but there is a bunch of ways this can be done. With using #148 this variable is cleared at power down. How do you know what tool is in the spindle at first power up?

Msantaji1,
What do you mean you can't change #500? You should be able to read and write to these variables. What kind of control are you using? You should be able to program right to these variables by #500=#4120. I would use #500 and above as these do not clear at power down.

#1-#33 are local variable assignments. They clear at reset and power down.
#100-#199 are common variables. They clear at power down.
#500-#599 are permanent common variables. They stay until programmed to change.

Stevo

[ALEXCOMO]

Put #500=#4120 in tool change program for mill(9001)

is the best way!!!

Attention!!! dont use #500 in any other way!!!
#500-#530 keep value when you turn off!!!

I used this metod on my mill!!!