G76 quit working on OT-C control

[g-codeguy]

Getting 62 P/S Alarm. Loaded a threading operation that ran 2 months ago. Same alarm. No one has changed a parameter far as we know. Owner said he hasn't touched one in 10 years. I looked at parameter 10 when I first started there to make sure I could load a 9000 program, but don't see how I could have accidentally changed a parameter. I've changed a few on purpose before, but not at this place. We are the only 2 that have been around the machine the past couple months as far as I know. What else is there to look at?

I asked last night if he had downloaded the parameters. Yes. So he can reload the parameters if necessary. I'm hoping it is something even easier.

Thanks.

[fordav11]

Please post your G76 line and also what is parameter 0001 bit 1 (FCV). Is it 0 or 1?

062 ILLEGAL COMMAND IN G71–G76
(T series)
1. The depth of cut in G71 or G72 is zero or negative value.
2. The repetitive count in G73 is zero or negative value.
3. the negative value is specified to Δi or Δk is zero in G74 or G75.
4. A value other than zero is specified to address U or W though Δi or Δk is zero in G74 or G75.
5. A negative value is specified to Δd, though the relief direction in G74 or G75 is determined.
6. Zero or a negative value is specified to the height of thread or depth of cut of first time in G76.
7. The specified minimum depth of cut in G76 is greater than the height of thread.
8. An unusable angle of tool tip is specified in G76.

Solution: Modify the program.

[g-codeguy]

Thanks for the reply. I'll check that parameter out this evening first thing. No need to post G76 line. All programs get sent back after running. It ran 2 months ago, not now. Plus there are a couple other programs with threading still in the control that the jobs have been completed, but the programs weren't deleted out of the control. Same error on all.

EDIT: Got a response back from the owner. These are Parameter 1 values:

Para 0001=11001010
bit 7 blank
bit 6 RDRN
bit 5 DECI
bit 4 CRC
bit 3 TOC
bit 2 DCS
bit 1 PROD
bit 0 SCW

Are you sure it is parameter 1? Thanks.

[fordav11]

ah you have the shi*ty 0-series. The FCV setting isn't on the 0-series. So don't worry about it. I was trying to ascertain if you are using a one line or a two line G76. You will be using two lines.
Either way my alarm description still stands, you must modify the program.
Probably your first line is wrong (according to related alarm description)
Now if you post the G76 lines we can maybe help..... if you don't post it then no one can help.

Or, try checking your parameters 723-726. See attached

[g-codeguy]

Nope, one line G76. I've been programming 2-line G76 commands for 20 some years. Pretty sure I know the correct format for them. We still have a Mori and Hitachi that use the 1-line format. I know how to program them too. The owner where I work my 2nd job has been in machining at least as long as I have. Pretty sure he knows the correct format also.

Like I said, we've tried 2-3 programs that have already run. Now they won't. I realized after my original post that I couldn't have accidentally changed a parameter on this machine because I've never turned the PWE on. The lathe is at my 2nd job. I originally thought it was an OT-C, because I thought that is what I saw on one of the Fanuc manuals. However, he has several different controls, both for lathe and mill. This lathe has an OT, I'm just not sure which flavor.

Appreciate your efforts in trying to help. You're right. O-series kind of suck. Of the 15 Fanuc controlled lathes I program, only one has an OT control. Others are 16TT, 18T, 21T or 21i-T. I use macros in a lot of my programs...which often require modifying when switched to this lathe. I'd like to see them sell it and get another 18T or better yet a 21i-T.

EDIT: I'm at home, but this is the code as best as I can remember.

X.44Z.3
G76X.3643Z-.548K.0296D90I-.0264F.037

A straight thread we ran a couple months ago.

X1.16Z.3
G76X1.188Z-.245K.0295D100F.05A50.

This last one is a guess as to actual values, but format should be good.

We've tried with and without an A-value...both with and without the decimal point. Pretty sure Fanuc uses a decimal while the Seicos control doesn't. Even added a P-value. I hadn't programmed the 1-block call in quite awhile before getting this 2nd job. Only programmed 2 of his lathes so far, and both use the 1-block call. I had to double check the Fanuc manual to make sure i was doing it right. Plus we compared the format to programs on the computer that had already been run. One of us should have seen an error in the format if there was one.

[fordav11]

well something has changed otherwise it would still be working
I'm pretty sure 0-T needs 2 lines. Just try it for fun and see what happens (using the required 2-line formatting of course)

[angelw]

fordav11 is partially correct. 0T controls usually use the two block format, and I'm not aware that there is a parameter to select Series 15 format; at least I haven't been able to find it in all my reference manuals. However, I've recently seen three OT-C controls that will use the Series 15 format for all multiple repetitive cycles, G71 to G76.

With a control that is set to use the 2 block format, the first block can be omitted if the values for the arguments in that block are stored in parameters 0109, 0723, 0724, 0725, and 0726. Before you try the two block cycle check the value contained in parameter 0724, this is the parameter for Angle of Tool Tip; specifying an unusable angle will result in the 62 P/S alarm. In Series 15 format this angle can be between 0 and 120deg, in increments of 1deg. Series 16 standard format can only have angels of 0, 29, 30, 55, 60, and 80degs.

If your control was originally set to Series 15 and now, for what ever reason, is set to Series 16 standard format, the angle value may be causing the problem, depending on what value is stored in #0724, or the lack of a Q value in the G76 block. Only having one G76 block that equates to the 2nd block in the Series 16 format will not necessarily upset the control for the reason explained above.

Once you've checked the parameters listed above, do as fordav11 suggested and try using the Series 16 standard format. Proceed in single block and monitor the parameters listed above to see if they are altered to the values of the arguments programmed in the first G76 block. If yes, and particularly if you get no alarms related to missing K and D values expected in the Series 15 format, then it would just about be confirmed that the control is set to Series 16 standard format.

Regards,

Bill

[g-codeguy]

I think I did try the 2-block call earlier...just for giggles. However, I'll try again in case my memory is as bad as I think it is. This time I know what parameters to check. Thanks Bill.

fordav: I got to agree...something has changed, but what? That's the $64,000 question.

[angelw]

I think I did try the 2-block call earlier...just for giggles. However, I'll try again in case my memory is as bad as I think it is. This time I know what parameters to check. Thanks Bill.

fordav: I got to agree...something has changed, but what? That's the $64,000 question.

Some word processors or Editor packages can compare two files and highlight any differences. If you have a copy of the parameters prior to this issue, when the G76 cycle as is worked, download a copy of the current parameters and compare the two. I wrote software for just this purpose some time ago to speed up tracking any changed parameters. If you don't have any Editor with this function, I'll be glad to scan the two files if you care to send me copies.

Regards,

Bill

[HuFlungDung]

Any chance it could be something else altogether? Some times the error messages just don't reflect where the problem actually is. Maybe a bad spindle encoder (run a trial G3x)? Maybe a change in the machine home position versus soft limits?

[g-codeguy]

Went in Monday, and the lathe was running a part with 2 different threads. One being done with G92, the other with G76. The G76 obviously was working. Tonight I set up another lathe with the same control. Used G76 for the M10 x 1 thread. Wouldn't run. Copied G76 thread from other lathe. Wouldn't run. Looked in control and found a program that used the G76. Wouldn't run. Shut off control and restarted. G76 ran in both the one that had been in the control plus the new one we had just loaded.

Owner thought maybe I had used MDI to put something in the control because he couldn't find anything wrong in my program. I hadn't. Program used M8, M9, M3, M1, G0, G1, G97, G2, G4, G50 and G96. Nothing in these codes that should affect the G76 cycle far as I know.

I would seem that all we have to do is shut off the power and restart in order for the G76 to work. But why? Is there a code I should be entering at the beginning of my programs? I don't include a G40, G80, G99 or G20 as these should all be the default when the controls are turned on. It is bugging both of us.

[fordav11]

when it wasn't working did you check parameters 0109, 0723, 0724, 0725, and 0726.
And then after when it was powered off/on did you check the same parameters again?
If not then you need to do that first and you might find something is different......