[442jet]

I am looking for the system variable that is used to store the "initial point" for canned cycles.
I use several different Fanuc and Mazak controls but this system variable should be the same for all of them.

Thanks in advance.

John

[sinha_nsit]

There is no such system variable on Fanuc.

[442jet]

Then where is the value for the initial point stored? It has to be stored some where as you can go back and forth from G98 to G99 and the control know what point to return to.

[sinha_nsit]

When we call a canned cycle, control remembers the specified data. Storing data in some system variable is a different thing.

[442jet]

Ok. Let me rephrase what I am looking for. Maybe we can expand the answers by expanding the question.

I am writing a custom drilling cycle using a modal call, "G66", and would like to return to the initial point or the R-plane depending on G98 or G99. In order to do that I need be able to recall both values.

Does anyone know where the values are stored and how they can be recalled?

Thank you,
John

[sinha_nsit]

#4010
If G98 is active, it stores 98
If G99 is active, it stores 99.
After reading its value, appropriate action can be taken.
IF [#4010 EQ 98] GOTO ...

[442jet]

#4010
If G98 is active, it stores 98
If G99 is active, it stores 99.
After reading its value, appropriate action can be taken.
IF [#4010 EQ 98] GOTO ...

I understand all of that. I am hung up trying to take the appropriate action.

IF [#4010 EQ 99] GOTO100
G00 Z "Initial Point"
GOTO150
N100 G00 Z "R-plane"
N150 M99

[sinha_nsit]

If you are defining your own drilling cycle, you would define your R-point and initial point, which you would use.
Several drilling macros are available on the net. Some of these might exactly suit your requirement. At least, the logic can be studied.

[norbert.barnard]

Hi John,
the below example is in the fanuc manual:
O9110;
#1=#4001; .......................Stores G00/G01.
#3=#4003;.........................Stores G90/G91.
#4=#4109;.........................Stores the cutting feedrate.
#5=#5003;.........................Stores the Z coordinate at the start of drilling.
G00 G90 Z#18;.................Positioning at position R
G01 Z#26 F#9;..................Cutting feed to position Z
IF[#4010 EQ 98]GOTO 1; Return to position I
G00 Z#18;.........................Positioning at position R
GOTO 2;
N1 G00 Z#5;........................Positioning at position I

hope this help

norbert