Fanuc 18i G72 cycle

Hi all,
New machine to me, and new to Fanuc as well. I'm trying to get a G72 facing cycle going and I'm having trouble figuring out the syntax. It is a Fanuc 18i-TB. The manual for the 18i-TB shows a 2 line syntax for the G71 and G72, but the machine won't take it. Programming as:

G0 X33. Z0.
G72 U.1 R.1;
G72 P10 Q20 U0. W0. F.015;
N10 G0 Z-1.0;
N20 G01 X26.5;

Gives me alarm 061: Address P/Q not found in G70-G73. I'm under the impression that means I should be using single line syntax so I tried that out, but it's not in the Fanuc book I have and there's a few different examples I'm finding on the internet.

G0 X33. Z0.
G72 P10 Q20 U0. W0. F.015;
N10 G00 Z-1.0;
N20 G01 X26.5;

This "works", except from start point it rapids to Z-1, feeds to X26.5, rapids back to start, rapids back to Z-1 again, feeds to X26.5, then back to start point and finished. I'm unclear why it would do two loops here, but presumably it's starting at Z-1 because depth of cut isn't set anywhere. But adding

G72 P10 Q20 U0. W0. D.1 F.015; or
G72 P10 Q20 D.1 U0. W0. F.015;

Gives me alarm 009: Illegal address input.

Anyone know what I'm doing wrong?

Try this

G0 X33. Z0.
G72 W.1 R.1;
G72 P10 Q20 U0. W0. F.015;
N10 G0 Z-1.0;
G01 X26.5;
N20 G0 Z.1

Brent

SRF said:

Hi all,
New machine to me, and new to Fanuc as well. I'm trying to get a G72 facing cycle going and I'm having trouble figuring out the syntax. It is a Fanuc 18i-TB. The manual for the 18i-TB shows a 2 line syntax for the G71 and G72, but the machine won't take it. Programming as:

G0 X33. Z0.
G72 U.1 R.1;
G72 P10 Q20 U0. W0. F.015;
N10 G0 Z-1.0;
N20 G01 X26.5;

Gives me alarm 061: Address P/Q not found in G70-G73. I'm under the impression that means I should be using single line syntax so I tried that out, but it's not in the Fanuc book I have and there's a few different examples I'm finding on the internet.

G0 X33. Z0.
G72 P10 Q20 U0. W0. F.015;
N10 G00 Z-1.0;
N20 G01 X26.5;

This "works", except from start point it rapids to Z-1, feeds to X26.5, rapids back to start, rapids back to Z-1 again, feeds to X26.5, then back to start point and finished. I'm unclear why it would do two loops here, but presumably it's starting at Z-1 because depth of cut isn't set anywhere. But adding

G72 P10 Q20 U0. W0. D.1 F.015; or
G72 P10 Q20 D.1 U0. W0. F.015;

Gives me alarm 009: Illegal address input.

Anyone know what I'm doing wrong?

Click to expand...

Hello SRF,
The p/s 009 alarm is caused by the period being used with the "D" address. D0.1 should be specified as D100.

With regards to the other issue, in the version of your program that actually cycles you haven't specified a DOC (D address). When a D address is successfully executed, the value is stored in parameters and doesn't changed until another "D" value is specified. The extent of the Z in your profile description is only 1.0 (mm I assume) and its quite reasonable for a greater DOC to have been specified previously. Accordingly, the cycle is taking the whole profile in one cut.

The second loop is because you have G72 Type I cycle invoked. This happens when only the Z axis is specified in the P referenced block. G72 Type I cycle takes a final pass after the roughing cuts have been completed. If you specify both an X and Z address it should just execute the roughing passes.

For a G72 (roughing along the X axes) you don't want any movement in X to be initiated in the P referenced block, therefore, if an X address is used, the coordinate should be the same as the X coordinate specified prior to the G72 Cycle being called as shown in the following example:

G0 X33. Z0.
G72 P10 Q20 U0. W0. D100 F.015;
N10 G00 X33.0 Z-1.0;
N20 G01 X26.5;

A more convenient method is to specify a Zero Incremental move in X in the P reference block with a "U" address as shown in the following example:

G0 X33. Z0.
G72 P10 Q20 U0. W0. D100 F.015;
N10 G00 U0.0 Z-1.0;
N20 G01 X26.5;

Both above examples will invoke G72 Type II cycle.

Regards,

Bill

yardbird said:

Try this

G0 X33. Z0.
G72 W.1 R.1;
G72 P10 Q20 U0. W0. F.015;
N10 G0 Z-1.0;
G01 X26.5;
N20 G0 Z.1

Brent

Click to expand...

Hello Brent,
I thinks the OP has FS15 format dialed in; the reason for his first program failure.

Regards,

Bill

Unrelated but is it safe to say it's uncommon for a Fanuc i series T control to use single line canned cycles? And to assume someone musta purposely changed the control to FS15? Weird how his 18i book doesn't include them.

Brent

Hello Bill,

We musta posted at the same time. I was thinking his U in the first G72 line might have been causing him fits?

Brent.

yardbird said:

Unrelated but is it safe to say it's uncommon for a Fanuc i series T control to use single line canned cycles? And to assume someone musta purposely changed the control to FS15? Weird how his 18i book doesn't include them.

Brent

Click to expand...

Hello Brent,
Its a used machine and its just a single bit parameter change. Its not that unusual, some prefer the FS15 Format, just to have the comparability with other machines. The G76 Cycle for multi start threads can use a Q address to index the Thread Start using FS15 Format. Change the system for that and you change it to FS15 Format for all the Multi-repetitive cycles.

The Fanuc Manuals mention that the the control can be set to FS15 Format via parameters. but the details for the various cycles affected aren't included. Their thinking may be that, if you want to change the control to FS15 Format, you must have the relevant manuals, or you're familiar with the cycle syntax used with FS15 Format.

Regards,

Bill

Thanks Bill & Brent for the guidance!

I did try out your suggestions to no avail, but I did manage to figure it out.

The machine is set up to use G code C (Param 3401.7(GSC)=1), which is apparently uncommon considering it's just a 2 axis lathe. Anyways G72 is actually G74 on this machine, and G72 is G70. It's interesting it let me put U and W values in a finishing cycle but only balked at the D value, but I guess that's the way it goes.



Cheers
Sam

angelw said:

Hello Brent,
Its a used machine and its just a single bit parameter change. Its not that unusual, some prefer the FS15 Format, just to have the comparability with other machines. The G76 Cycle for multi start threads can use a Q address to index the Thread Start using FS15 Format. Change the system for that and you change it to FS15 Format for all the Multi-repetitive cycles.

The Fanuc Manuals mention that the the control can be set to FS15 Format via parameters. but the details for the various cycles affected aren't included. Their thinking may be that, if you want to change the control to FS15 Format, you must have the relevant manuals, or you're familiar with the cycle syntax used with FS15 Format.

Regards,

Bill

Click to expand...

Bill, trying to pm you but your bin is full. Appreciate your help if you would.

DMSentra said:

Bill, trying to pm you but your bin is full. Appreciate your help if you would.

Click to expand...

Try now.

Regards,

Bill