Need Help!- Rigid Tapping G-Gode for Fanuc Pro 3

[need-a-day-off]

Hey everyone - new recruit here.

Recently jumped into the world of Fanuc controls after years of being a Haas only shop. I have a Makino S33 with a Fanuc Pro 3 control. So far it has been a reasonably smooth transition...until yesterday. Rigid tapping. The code that I am using is as follows:

T21 M6
G55 G90 G0 X-0.25 Y0.25 S500 M3
H21 D21
M56
G43 Z10.
M26
M135
G84 X-0.25 Y0.25 Z8.185 R9.035 F27.8
Y2.75
G80
M9

When it gets to the M135 line, I get an error message that states:

5110 Improper G Code (G05.1 Q1 Mode)

I have searched the manuals and cannot determine what is wrong with this code. Any help is greatly appreciated!!

[psychomill]

This part of the code looks OK but given the error for High speed mode (G5.1) it must still be active from a previous tool. Try cancelling G5 at the end of whatever tool is running it or put the cancel into a block before M135 and it should run. You can't run canned cycles in G5 or G5.1

[cnc-king]

Originally Posted by need-a-day-off Hey everyone - new recruit here. Recently jumped into the world of Fanuc controls after years of being a Haas only shop. I have a Makino S33 with a Fanuc Pro 3 control. So far it has been a reasonably smooth transition...until yesterday. Rigid tapping. The code that I am using is as follows: T21 M6 G55 G90 G0 X-0.25 Y0.25 S500 M3 H21 D21 M56 G43 Z10. M26 M135 G84 X-0.25 Y0.25 Z8.185 R9.035 F27.8 Y2.75 G80 M9 When it gets to the M135 line, I get an error message that states: 5110 Improper G Code (G05.1 Q1 Mode) I have searched the manuals and cannot determine what is wrong with this code. Any help is greatly appreciated!!

Try this out
the G8P0 & G8P1 turns of and on the high speed machining
This is the format for the Pro3 on the A55 & A61

T29M6
( 10-32 HELICOIL FORMTAP )
G54.1P2G0G90G17X.325Y-.4M3S1280
B0.M11
G43Z1.H29M8
Z.1
G8P0
S1280
M135
G98G84X.325Y-.4Z-.4413R.05F40.
G80
G8P1
M9
G0Z6.
G0G91G30X0Y0Z0M319
M99

[Zuma]

We had some problems with rigid tapping on makinos and this is what we found works. The book isn't quite correct but what you must do is have the feed rate as a whole number. (this is directly from makino)
Following is what my code would look like for a 3/8-18 using 50sfm. (Of course positions and coolant and all that is up to you.)

MAKINO SYNTAX FOR RIGID TAPPING:
G0 G54 X*** Y***
M3 S504
G43 Z*** H** M8
M135 S504
G84 G98 Z*** R*** P300 F28
X*** Y***
X*** Y***
X*** Y***
G80
G4 P300

We have found that if we didn't turn the spindle on before going into M135 we would get errors. Normally I would just use G0 to cancel tapping but makino wants the G80 then the dwell line.

[need-a-day-off]

Thanks, Guys. I've tried all of your methods and I still am getting the same error (5110 Improper G Code (G05.1 Q1 Mode)). When I tried the G8P0/G8P1 insertion, I get an error that reads "G08 cannot be commanded". Any other thoughts?

[psychomill]

Try cancelling G5.1 by commanding this on its own line...

G5.1 Q0

Another thing, if you RESET the machine and just started the program from the tap tool, do you still get the alarm? Skip the tool change command (make sure you at least tool change into the spindle) and start from the work offset line.

Something else I noticed too, why do yo bother commanding a M56 after you've already established "H" and "D" on the previous line?

[need-a-day-off]

G5.1 Q0 is the ticket. Works like a champ. Thanks for the help...I feel like I'm amongst friends...

[mjsmith]

Originally Posted by need-a-day-off Hey everyone - new recruit here. Recently jumped into the world of Fanuc controls after years of being a Haas only shop. I have a Makino S33 with a Fanuc Pro 3 control. So far it has been a reasonably smooth transition...until yesterday. Rigid tapping. The code that I am using is as follows: T21 M6 G55 G90 G0 X-0.25 Y0.25 S500 M3 H21 D21 M56 G43 Z10. M26 M135 G84 X-0.25 Y0.25 Z8.185 R9.035 F27.8 Y2.75 G80 M9 When it gets to the M135 line, I get an error message that states: 5110 Improper G Code (G05.1 Q1 Mode) I have searched the manuals and cannot determine what is wrong with this code. Any help is greatly appreciated!!

Try this out!

N10 T21 M6;
N15 G00 G90 G40 G80 G49 G17;
N20 G00 G55 X-.25 Y0.25 S500 M3;
N25 G43 H21 D21 Z10. M8;
N30 M29;
N35 G84 X-.25 Y0.25 8.185 R9.035 F27.8;
N40 Y2.75;
N45 G80;
N50 M9;
N55 M1;

Make sure there is no spaces between digits.