I'm using G83 to drill a deep hole and having issues. I'm drilling 1 hole per part so the program is really short. The following is the entire program:

T6
G00 G90 S2000 M03 X0 Y0 Z1.
H6 M7 Z.1
G83 G99 R0+.1 Z-3. F8 Q.25 P.02
G00 G49 G90 Z3. M9
XO Y5.3
M30

I keep getting the following error message:

Bad Z or R0 in canned cycle, N=5.0000

I've changed just about everything with no luch. What am I missing?

Try deleting the + after R0

Hmm, perhaps someone else can confirm or not, but doesn't G and M commands need to be on different lines otherwise only the last will be performed? Not 100% on this though... Been a while since I did stuff like that and my controller was old even then :)

No G and M codes can be on the same line with all of the machines I have delt with. You can only do 1 M code unless you change the parameters on a Fanuc. Kind of dangerous move unless you are really good with M codes. Usually done on special machines. My guess is like the guy above I would take out the +.

T6
G00 G90 S2000 M03 X0 Y0 Z1.
H6 M7 Z.1
G83 G99 R0+.1 Z-3. F8 Q.25 P.02
G0 G80 Z.1
G49 G90 Z3. M9
XO Y5.3
M30

I believe the problem is the g83 is never canceled. try the g80 as above.

I agree with the others... take out the "+" sign from your R value. Also, you won't need the "P" (unless you're forcing a dwell. but at ".02", that's next to nothing... not even sure thats a valid value), and your feed has no decimal (which would make this very, very slow). And you never cancel the drill cycle with a G80.

but doesn't G and M commands need to be on different lines otherwise only the last will be performed

As Jetski stated, you can have G and M codes on the same line. Most machines can handle 1-3 M codes per line (depending on parameters and some machines are capable of more). And, most machines can do many G-codes per line as long as they are of a different 'Group'. For G codes though, that's where generally, only the last one of a particular Group type will take effect.


[edit]: Not sure on Fadal controls though...

Ah! that's what I meant, you can only have one M Code on each line otherwise only the last one gets performed. Not relevant in this situation since it doesn't occur though (my bad).

I notice he's in G90 (absolute) mode... perhaps his co- ordinate system
is trying to drive the tool somewhere illegal (I note that he's G92'd it as well canceling CAR presets).

I agree that the + sign should be dropped, would a G91 R0.1 G90 phrase work better?

Thanks for the help guys. The + in the R value is how Fadal shows it in all of their programming examples for all canned cycles. It worked fine on the operation before this which was a L99 pocket clean out. The code I've used to prep the G83 is virtually identical to the L99 so I thought I was good above the G83 line. I'll try the G80 in the following line when I get into the office.
One of my concerns was that it might just be the machine. This one is an 87' and has been rode hard and put away wet. We no longer use it for production because it has so many quirks. I'm only using it for this because the spindle on the bridgport is out having bearing pressed on.
I'll post an update in an hour or so.

Thanks,

Bob

A +/- is not optional for the R value (in format 1, and I believe in format 2 as well) the control will put in a + if you don't put it in yourself.

You were missing the G80. Fadal's will execute multiple M-codes per line assuming that you are using the Fadal side of the control(I think this one is format 2)

You definitly need the G80 to cancel any canned cycles. Depending on the age of the control you may need the G43 to set the cutter height offset. You should also have a G80 after the cycle to cancel the canned cycle.

To run in format 2 it simply needs a G80 to cancel the G83. I tried it on our 1990 4020 exactly as you programed it and it worked fine after adding the G80. Be sure to add a decimal after the Feed or it will be super slow.

It turns out you either need an x or y move in the G83 line or a G45 in the line following it. It also turned out that the manual I was using is 15 years newer that the machine I am working on. It seems that Fadal actualy made some changes in that time! Who would have guessed. Thanks again for all of your input.

Bob

The need for x y location on the G83 line can be set in the parameters. 'immediate execute fixed cycle' set to on does not require the xy word in that line. Otherwise requiring the xy.
The G80 should be included to cancel the cycle, not canceling a canned cycle can give you some issues.

Looks like he figured it out. It is interesting that with a machine that old that he did not have problems until now?