retract the boring bar

[MARK DEL TORNO]

hi, i need help anybody knows what the code to control retract move on boring bar canned cycle ussually move 0.100" but i want it to move .020"
please any help is apprecciated.

[John Bennett]

G89 is boring cycle. The steps would be 1) position of x and y 2) feed down (-z) 3) operation at bottom of hole 4)retract to intial z position.

It might help if you said what control and machine you are wanting boring help on and supply present code you are using, as each machine has different canned cycle input.

[MARK DEL TORNO]

THANKS JOHN,
we have diferent machine controls but i want to try in a turning center to open the bore (mori seiki sl 400) it run one line canned cycle ,i was reading on a diferet post that i can use "R" in the canned cycle ,sometime if i'm using a big boring bar is no much room to retract.
thanks.

[dcoupar]

Originally Posted by MARK DEL TORNO THANKS JOHN, we have diferent machine controls but i want to try in a turning center to open the bore (mori seiki sl 400) it run one line canned cycle ,i was reading on a diferet post that i can use "R" in the canned cycle ,sometime if i'm using a big boring bar is no much room to retract. thanks.

What model Fanuc do you have?

[MARK DEL TORNO]

Originally Posted by dcoupar What model Fanuc do you have?

fanuc 18T

[angelw]

Originally Posted by MARK DEL TORNO THANKS JOHN, we have diferent machine controls but i want to try in a turning center to open the bore (mori seiki sl 400) it run one line canned cycle ,i was reading on a diferet post that i can use "R" in the canned cycle ,sometime if i'm using a big boring bar is no much room to retract. thanks.

Mark,
The R command for escape amount is used in the two line G71 cycle. The U and R values in the first G71 block are passed to parameters 5132 and 5133 respectively and are model and will remain unchanged until other values are specified by the U and R in this first G71 block.

The R command is not available in the one line G71 cycle (series 15 format) and the escape amount can be and is set via parameter. However, Programmable Parameter Entry via G10 is available. According, you could write a simple Macro program that includes the G10 Programmable Parameter Entry format and change the escape value held in the parameter by passing your desired value when the Macro is called. From a CNC programming perspective the G71 cycle definition would look the same with the addition of an R command to pass the escape value to the Macro program. In essence, you would have created your own G71 cycle definition and the Macro program will be called with G71.

Regards,

Bill