G72.1 G72.2 Figure Copying - PS010 Improper G Code

Hi fellas. Long time lurker.
Google'd and Forum-searched for the following tags:
G72.1
G72.2
Figure Copying
Fanuc
Inactive G-Codes
Activating G-Codes

Couldn't find my answer, or people with my issue.

What I'm trying to do is practice a simple G72.1 Rotational Figure Copying command.
Based on the following code, I get Alarm PS010 Improper GCode.
I've followed the Fanuc book examples, and online examples. I only omit tool compensation.

What I'm trying to do: Rotate a simple X-motion to the Y axis.

The following program is my version of the Fanuc rotational copying example provide on pg 306 of Ch. 14 Function to Simplify Programming, Fanuc Series 30i-Model B, 31i, 32i Operator's Manual

<FigCopy> (Main Program)
G92 X1 Y1
G0 G90 X1 Y0
G01 G17 X0 Y0 F10
G72.1 P0909 L1 X0 Y0 R90 (<<Alarm PS010 Activated Here)
G01 X1 Y0
G0 X1 Y1
G92 X#5021 Y#5022
M02

O0909 G01 X-1 (Subprogram)
G04X1
X1
G04X1
X0
M99

Follow up questions:
If I am writing this code correctly, is there a way to activate/deactivate certain G-codes? Perhaps Figure Copying (G72.1/G72.2) is not "activated" on my machine?

Let me know if I'm missing some critical information I forgot to mention.
Thanks for the help!

Follow-up.

Tried G68 instead, and it resulted in what I was trying to achieve. However, I would still like to figure out why G72.1/G72.2 appear to be inactive G-Codes on my machine.

The following solution is with respect to page 320 of the Fanuc operator's manual regarding a simple G68 example.

Solution:
<FigCopy> (Main Program)
G92 X1 Y1
G0 G90 X1 Y0
G01 G17 X0 Y0 F10
G68 X0 Y0 I0 J1 R90 (<<rotates XY coordinate system to 90 degrees)
M98 P0909 L1
G69
G01 X1 Y0
G0 X1 Y1
G92 X#5021 Y#5022
M02

O0909 G01 X-1 (Subprogram)
G04X1
X1
G04X1
X0
M99

G71.1/G71.2 is an option. Which control do you have? For 16/18 controls parameter 9945.2 turns it on. Have no idea which parameter for other series of controls.

Your G71.1 format is correct except for L value. The L value should be the total number of times you want sequence to occur, i.e. the first instance plus all the repeats. L8 = operation done eight times(first plus seven repeats).

Positive R value repeats in counter-clockwise pattern, negative value, clockwise pattern. Decimal point required( Don't ask how I know.).

Forgive me for not knowing exactly what "control" is refering to. According to the software on the PC, under "About...", it is CNC Type 32i, Software Series G501, version 68.0.

I looked for parameter 9945 or 9945.2, but there's nothing referencing it.

Going to look into how to change modal list.

That is because it's supposed to be a secret. It's a option you pay extra for. I'd use caution before just changing this parameter. If the machine isn't setup for this option? It could be a real bad day for you.

Brent

Oh I see. So by option, you mean an add-on that I may not have. That makes sense in receiving the PS010 alarm, then.

Thanks for the help guys. G68 it is then.

xpertsnowcarver said:

Forgive me for not knowing exactly what "control" is refering to. According to the software on the PC, under "About...", it is CNC Type 32i, Software Series G501, version 68.0.

I looked for parameter 9945 or 9945.2, but there's nothing referencing it.

Going to look into how to change modal list.

Click to expand...

I should have asked what model or series of Fanuc control. And, yes, G71.1/G71.2 is an extra cost option. The cycle is in the control, but until you pay Fanuc for it or find out what the parameter is, it won't be turned on.

Was this machine bought new? Dealer might be persuaded to give you the parameter. Mine did when I asked.

BTW, G68 is an extra cost option too.

alphonso said:

.....The cycle is in the control, but until you pay Fanuc for it or find out what the parameter is, it won't be turned on.

Click to expand...

This may be a dangerous statement to make. Not all firmware versions support all software options. Turning on a software option that is not supported by the firmware leads to one having to initialize the control and re-loading all the parameters and associated data. IME, the "common" options are supported in all firmware versions. When you start talking about less common or less popular options that's where the firmware version starts being a concern.

Vancbiker said:

This may be a dangerous statement to make. Not all firmware versions support all software options. Turning on a software option that is not supported by the firmware leads to one having to initialize the control and re-loading all the parameters and associated data. IME, the "common" options are supported in all firmware versions. When you start talking about less common or less popular options that's where the firmware version starts being a concern.

Click to expand...

You are correct for the most part. In my instance though (18mc), if G68 can be turned on, then G71 can be turned on. At least, that's what my dealer said. I presume that would follow on newer model controls. Yeah, I know, never presume what the fuck Fanuc might do.

I'll just say that I've had the joy of reloading control parameters a time or two or so playing "what option works Russian Roulette". Newer controls with the ability to do a SRAM backup to a PCMCIA card make this pretty painless, but older than those it's a lot of fiddling around with hand loading some and RS232 loading some.

alphonso,

I hope you didn't take it as I had any problems with you posting option parameters because I don't. You and I have on a couple of occasions helped guys get stuff turned on. Maybe some would think I'm a bit unethical or its wrong and maybe it is but I've been in that situation myself.

I posted the polar coordinates parameter for a guy once and thought I fucked up his machine. I was just giving the OP a little warning that things could go wrong then after that it's on him.

Brent

yardbird said:

alphonso,

I hope you didn't take it as I had any problems with you posting option parameters because I don't. You and I have on a couple of occasions helped guys get stuff turned on. Maybe some would think I'm a bit unethical or its wrong and maybe it is but I've been in that situation myself.

I posted the polar coordinates parameter for a guy once and thought I fucked up his machine. I was just giving the OP a little warning that things could go wrong then after that it's on him.

Brent

Click to expand...

Fanuc G72.1 Rotational Copy program for milling
August 10, 2018 - Fanuc G72.1 Rotational Copy [M]


Fanuc G72.1 Rotational Copy program for milling - CNC PROGRAMMING TUTORIAL
Main Program
O1423
N10 G90 G00 X100 Y100 ; [P1]
N20 G17 G42 G01 X100 Y0 D01 F100 ; [P2]
N30 G72.1 P1422 L4 X0 Y0 R90 ;
N40 G90 G40 G00 X100 Y100 ; [P1]
N50 M30 ;

Sub Program
O1422 G91 G03 X5 Y5 R5 ; [P3]
N100 G01 X-68 Y2 ; [P4]
N200 G03 X-20 Y20 R30 ; [P5]
N300 G01 X-2 Y68 ; [P6]
N400 G03 X0 Y100 R5 ; [P7]
N500 M99 ;