Error 065 Illegal Command in G71-G73

[CNCALLthethings]

Working on a simple profile canned program.
O0072;
G20;
T0301;
G0 X.55 Z0.;
G20 S1000 M03;
G71 W.005 R.5;
G71 P101 Q102 U.02 W.005 F0.005; (Error)
N101 G01 Z-1.5;
X.48;
Z-1.0;
X.375;
Z-.5;
X.25;
N102 Z.25;
M30;
%


Im getting an error 065 "Illegal Command in G71-G73" at the line specified with (error)

Any ideas on what this is about? I'm fairly new to writing G-Code, but have experience working with CNC mills and lathes.

Our Machine is a Hardinge Cobra 42 with a Fanuc 21T Controller

[txcncman]

Try:

O0072;
G20;
T0301;
G0 X.55 Z0.;
G20 S1000 M03;
G71 W.005 R.5;
G71 P101 Q102 U.02 W.005 F0.005; (Error)
N101 G00 Z-1.5;
G01 X.48;
Z-1.0;
X.375;
Z-.5;
X.25;
N102 Z.25;
M30;
%

[angelw]

Originally Posted by CNCALLthethings O0072; G20; T0301; G0 X.55 Z0.; G20 S1000 M03; G71 W.005 R.5; G71 P101 Q102 U.02 W.005 F0.005; (Error) N101 G01 Z-1.5; X.48; Z-1.0; X.375; Z-.5; X.25; N102 Z.25; M30; %

The W address should be "U" in the first G71 block.
In the G71 two block format U is used in the X Z plane, W in the Y Z plane and V in the X Y plane.

Note also that the value you have specified in you example for W in the first G71 block is depth of cut and the R is the retract amount at the end of each roughing cut. Notwithstanding that the W address is wrong, the values you have specified for W and R would result in a 0.005 depth of cut and a 0.5 retract respectively.

Also N101 G01 Z-1.5 should have an X move, as G71 is roughing in the Z axis. You can have X and Z in the first block and this will use G71 Type II cycle. Programming X (U) only will use G71 Type I. Z alone in the block referenced by P in the 2nd G71 will cause an error. The actual meaning of alarm 65 is that in the first block of the shape program specified by P in the repetitive canned cycle G70 to G73, G00 or G01 was not specified. There are many occasions when Fanuc alarm can occur for other reasons that are connected in some way to their desired error trap. Given that in your example program you show G00 specified in the first block, this lends weight to the error being in the first block but in the form of the Z and no X move.

It appears that you are roughing away from the chuck in a Z+ direction, starting at an X diameter larger than the finish diameter. In this case I believe the shape you have programmed is illegal, even when using G71 Type II cycle (pocketing). In the G71 cycle, the tool will return to the start point defined by the Z coordinate prior to the G71 cycle being launched. Accordingly, the cycle would return the tool to Z0.0 between cuts if your example program were to work at all. Why do you not start at Z0.25 and rough towards the chuck?

Something like the following.

G0 X0.55 Z0.25;
G71 U0.10 R0.02;
G71 P101 Q102 U.02 W.005 F0.005; (Error)
N101 G00 X0.25;
G01 Z-0.50;
X0.375;
Z-1.00;
X0.48;
Z-1.50;
N102 X0.55;


Regards,

Bill

[drdos]

If what "Angelw" tells you to do doesn't work then chances are good that you need the "Fanuc" option bit turned on in order to use that function. Only Fanuc can turn options on anymore. You need to verify if you have that option turned on or not. The option is either J877 Multi-Repetitive Canned Cycle (T) Type 1 or J889 for type 2. If you call Fanuc at Customer Support 1-888-326-8287
Parts #1, Service/Tech Support #2, Repair #3, Training #4
and give them what is in your 9900 to 9990 parameters, they can tell you if it is on or not.

[drdos]

065 ILLEGAL COMMAND IN G71–G73
(T series)
1. G00 or G01 is not commanded at the block with the sequence
number which is specified by address P in G71, G72, or G73
command.
2. Address Z(W) or X(U) was commanded in the block with a
sequence number which is specified by address P in G71 or G72,
respectively.
Modify the program.

[fordav11]

I would think ALL Fanuc T's are able to do the multiple repetitive cycles. they are pretty much stock-standard across the board. without them the whole thing is useless. might as well use a file, it'd be faster
I agree the W should be a U

[angelw]

Originally Posted by fordav11 I would think ALL Fanuc T's are able to do the multiple repetitive cycles. they are pretty much stock-standard across the board. without them the whole thing is useless. might as well use a file, it'd be faster I agree the W should be a U

In all my time in this game I've seen one machine that didn't have any multiple repetitive cycles, but quite a few that only had Type I. Late machines mostly have both, but I've worked on a few new machines as late as 2002 that only had Type I. They were low end, cheaper brands.

CNCALLthethings has more than one issue with his program, as pointed out in post #3, but I believe the cause of the alarm is the Z move in the block referenced by P in the G71 block. This block needs to have an X value, and he still may get the alarm if the control is only equipped with Type I and the Z move is retained with the X.

Regards,

Bill

[fordav11]

yeah. multiple issues. two G20's as well. maybe he meant to use G72. The profile (P-Q) seems to be facing in which case the Z movement and the W is right. Very strange programming method.
I expect to see his next post.... "how to remove the tool post rammed inside the chuck at 1000 RPM?'
Hahaha

[txcncman]

Since CNCALLthethings has not posted back (in over 36 hours) I would bet his problem has been solved.

[CNCALLthethings]

Sorry to go silent for two days...

I'm actually part of the Formula SAE team at my college, and this lathe has been sitting unused for a long time because nobody can get it running. We still are having trouble getting it to run the code, but are still working on the suggestions posted. Again, we have some combined experience with GCode and CNC machining, but trying to debug a machine is a bit tricky.

Thank you all very much for helping us! I'll post again with some progress as I work more with it.

And no, I figured that holding the tool post in the chuck would be a bad idea, so as tempting as it was I decided not to do it