Turning multiple parts from Bar in one program.

I have a job that requires me to thread and part off 3" x 1/4" Rings out of 6061 aluminum. Our spindle only has a 2.5" Bore so we chuck a piece hanging out long and slice them off one at a time. I would like to write something that will repeat this cycle 20 times without having to make a long program. This machine has a Fanuc OT controller and does not support G54 style work offsets, only a single work shift set in the controller. Currently, I have the program set to stop the parting tool above the stock so I can press measure after each cycle.

This can be done, I use a "Main Program" (it controls the offset) and a "Sub Program" (it controls the tool path)

O2120 (MAIN PROGRAM)
G10 P0 X0.0 Z0.0 [SETS WORK OFFSET TO ZERO]
G65 P2121 L1 [RUNS SUB PROGRAM]
G10 P0 X0.0 Z0.450 [SETS WORK OFFSET IN TO 0.450] {THIS MAY BE NEGATIVE ON YOUR CONTROLLER}
G65 P2121 L1 [RUNS SUB PROGRAM]
G10 P0 X0.0 Z0.900 [SETS WORK OFFSET IN TO 0.900]
G65 P2121 L1 [RUNS SUB PROGRAM]
REPEAT AS MANY TIMES AS YOU LIKE
G10 P0 X0.0 Z0.0 [SET WORK OFFSET BACK TO ZERO] {I DO THIS AT THE END FOR SAFETY}
G28 U0.0
M30
%

O2121 (SUB PROGRAM)
(1" MATERIAL)
(1.7" ON PULL STICK)
(20.125" SAW CUT)
G20 G40

(0.087 WIDE PART OFF)
T1111
G99
G50 S2000
G96 S8000 M03
M08
G00 X1.05
G00 Z-0.430
G01 X-0.05 F0.008
G50 S25
M09
T0000
G28 U0.0
M18
M99
%

Hope this helps.
Tony

Looks exactly what I was looking for. Never used G10 to program. I am guessing the L is the work offset number and will always be 1 because there cannot be other values?

Quote:

---

Originally Posted by destroyer125

Looks exactly what I was looking for. Never used G10 to program. I am guessing the L is the work offset number and will always be 1 because there cannot be other values?

---

No L is how many times to loop thru the subprogram. That would be used when using a bar puller/feeder and you want to loop intil you get to the end of the bar.

The P0 is telling it which coordinate system to use, I only use zero.

As far as possible, system variables should be used instead of G10. If available, system variables offer more flexibility.

Quote:

---

Originally Posted by sinha_nsit

As far as possible, system variables should be used instead of G10. If available, system variables offer more flexibility.

---

8
I assume by system variables you mean
G65 P1111 L1 A0.500 B1.5
Then in Sub program "X#1" and "Z#2"

I find it easy to dial in a program just like any other part.. And then use G10 to move in the workoffset for each subsequent part. No messing around with making sure variables are set.

I can see using variables for families of parts. But to make same part over and over off the same bar G10 seems like the way to go.

But am certainly open to learning how to use system variables to accomplish what the OP wants.

Please explain.

I was talking about system variables for offset values, such as #5221 for G54 X, on Fanuc.

You could also setup the machine tooling to cut multiple parts at the same time, I've done that turning inner bearing races.

Quote:

---

Originally Posted by sinha_nsit

I was talking about system variables for offset values, such as #5221 for G54 X, on Fanuc.

---

I see that in the book, so would it look like this?
#5222=0.000
#5242=1.000
#5262=2.000
G54
G65 P1111 L1
G55
G65 P1111 L1
G56
G65 P1111 L1
M30

I have been trying to get the G10 to work and I keep getting a PS 010 Alarm on that line. My machine does not use G54 style work offsets and will error out if you try entering G54. It only has 1 "Work Shift"
:

Quote:

---

Originally Posted by kart17wins

I see that in the book, so would it look like this?
#5222=0.000
#5242=1.000
#5262=2.000
G54
G65 P1111 L1.
G55
G65 P1111 L1
G56
G65 P1111 L1
M30

---

Set G54 Z to suit the first job.
Save the offset value for restoring it later (#100 = #5222)
Machine the first job.
Shift G54 Z for the second job (#5222 = #5222 - 1)
Machine the second job.
Repeat the process as per requirement.
For starting the process all over again, restore the original offset (#5222 = #100)

No need to use G55 etc.
Use M98 instead of G65.

Oh this is brilliant! Ive been searching for a way to bring my G54 back to the start of my bar .#5222 does the job perfectly I use a sub program with a Z increment and an L count for the no of parts but I manually return to the original G54 at the end of my program. Thank you sinha_nsit

You are welcome, Henners.

And, it cannot be done through G10.