What's new
What's new

FANUC 21M Rigid Tapping Issue

VTM

Hot Rolled
Joined
Jun 8, 2018
So this is on a Chiron FZ08W with a Fanuc 21M. I've owned this machine for quite awhile and I'm no stranger to Rigid Tapping on a Fanuc. But somehow we never got a job on It that required tapping holes until now. First off we were pulling parts out of the vise so I started looking at parameters. #5200 Bit 0 was 0. Manual says should be a 1. Changed that and tried again just cutting air. Now It taps all the holes and freezes at the G80 line? Doesn't throw any alarms just sits there. Is there another Parameter change that needs to be made? Drilling with G83 and a G80 cancel cycles fine. I posted the Rigid Tap code below. Maybe I'm missing something.

N4G17G80G40G90G49G0
T4M06 ( #2-56 CUT TAP )
G90G54
S1500M03
G90G0X2.805Y-.0075
G43Z.1H4
M08
M29S1500
G84G98X2.805Y-.0075Z-.34R.1F26.78571
X2.055
X1.59
X.84
X.375
X-.375
X-.84
X-1.59
X-2.055
X-2.805
G0G80Z.1
M09
G91G28Z0.
G0G90G53X0.Y0.
M30
 
On my Leadwell with 21M I call G95 with the pitch one line before the M29. Be sure to go back to G94 before running another tool.

Dave
 
On my Leadwell with 21M I call G95 with the pitch one line before the M29. Be sure to go back to G94 before running another tool.

Dave
Thanks for the response Dave. We Rigid Tap all the time In G94. I fail to see how switching to G95 will prevent the machine from hanging at the end of the cycle.
 
Now that you've turned on 5200.0, will it work without m29?

Because the way i read the manual, you need m29 (or another m-code depending on parameter) with bit 0=0, but if you no longer need an mcode (bit 0=1) then the M29 might be causing you issue?

Just an idea.

My 21 control has 5200.0=0 and 0 in 5210(which means m29 is the rigid tap m-code)


You could also try to see if that control supports g84.2 (rigid tapping) instead of plain g84. On my machines that do, no m29 is required for rigid tapping.
 
I could be mis Interpreting the manual. On our other Fanuc's that code this way 5200.0 is set to 0 and 5210 is set to 29. Originally on this machine 5200.0 was 0 and 5210 is set to 84. Does that mean to you that I should be using M84 instead of M29?

Running It the way it was originally set with the code I posted pulls the part and the machine doesn't appear to perform the cycle correctly as far as accel, decel.

And If I change 5210 to 29 I get an alarm.
 
Well Dan,

You got me looking and thinking anyway. I believe that might be exactly the case. I'll switch 5200 back off and try M84 in the program instead of M29.

According to the Chiron Manual
 

Attachments

  • FZ08W MANUAL.pdf
    254.8 KB · Views: 9
So with 5200.0 off and using the code I posted the cycle will run and complete. But It doesn't appear to be syncing the spindle correctly and pulls the part If I actually attempt to tap holes.

Again with 5200.0 off and changing the M29 in the posted code to M84. It looks to be syncing the spindle correctly but still hangs at the G80 line? Any Ideas?
 
What is parameter 9931 bit 2 set to?

Another question. Because i've been there.... are you sure its a 2-56 tap and not a 2-64? gotta ask.
 
The G80 freezing the machine happens on our machines too. We found that the RPM was too low. Try upping the spindle speed to 150 RPM or greater if you hadn't done that. You did not state what RPM you were running at.
Its In the posted code 1500RPM
 
Ok, this will run. For whatever reason It requires the M5 on the G80 line. Non of our other Fanuc 21's require that. Now If It will actually tap correct we will be good to go.

N4G17G80G40G90G49G0
T4M06 ( #2-56 CUT TAP )
G90G54
S1500M03
G90G0X2.805Y-.0075
G43Z.1H4
M08
M84S1500
G84G98X2.805Y-.0075Z-.34R.1F26.78571
X2.055
X1.59
X.84
X.375
X-.375
X-.84
X-1.59
X-2.055
X-2.805
G80M5
G0Z.1
M09
G91G28Z0.
G0G90G53X0.Y0.
M30
 
Now that you've turned on 5200.0, will it work without m29?

Because the way i read the manual, you need m29 (or another m-code depending on parameter) with bit 0=0, but if you no longer need an mcode (bit 0=1) then the M29 might be causing you issue?

Just an idea.

My 21 control has 5200.0=0 and 0 in 5210(which means m29 is the rigid tap m-code)


You could also try to see if that control supports g84.2 (rigid tapping) instead of plain g84. On my machines that do, no m29 is required for rigid tapping.
What you have said is all correct.
There are three methods for rigid tapping:
1. Set 5200#0 = 1 and use G84 without M29 for rigid tapping. Conventional tapping is never done.
2. Set 5200#0 = 0 and use G84 with M29 for rigid tapping, and without M29 for conventional tapping.
3. Use G84.2 for rigid tapping and G84 for conventional tapping.
 
Ok, this will run. For whatever reason It requires the M5 on the G80 line. Non of our other Fanuc 21's require that. Now If It will actually tap correct we will be good to go.

N4G17G80G40G90G49G0
T4M06 ( #2-56 CUT TAP )
G90G54
S1500M03
G90G0X2.805Y-.0075
G43Z.1H4
M08
M84S1500
G84G98X2.805Y-.0075Z-.34R.1F26.78571
X2.055
X1.59
X.84
X.375
X-.375
X-.84
X-1.59
X-2.055
X-2.805
G80M5
G0Z.1
M09
G91G28Z0.
G0G90G53X0.Y0.
M30
Long time back, I read somewhere that the control sometimes hangs at G80 in rigid tapping because of look-ahead feature when it reads the block next to G80 and tries to interpret it in the rigid mode.
The suggested remedy was to insert a buffering-preventing block after G80 or simply command G80 twice in two consecutive blocks.
 
Well that's a weird solution, I guess. so long as the threads gage good, make chips!

according to your parameter you do have rigid tapping, btw. I thought it was a long shot that maybe your machine didn't have the option. But the machine would probably throw an alarm with M29 if you didn't have the option installed.

If you figure out a parameter solution, rather than M5 hack, let us know.


Edit: according to your manual, after G80 they had a M95. What's M95 in your machine? While it's my opinion that it should get past G80, maybe M95 is actually required. they had it on the G80 line in your book.
 
Ok so this code does actually run and make very nice threads, but remove the M5 and no go. And If I substitute M95 for the M5 I'm sure it would work as well but I haven't tried it. Thanks everyone for trying to help, much appreciated!!

And to answer your question Dan. M95 on this machine is Spindle Stop and Coolant Off.

N4G17G80G40G90G49G0
T4M06 ( #2-56 CUT TAP )
G90G54
G90G0X2.805Y-.0075
G43Z.1H4
M08
M84S1500
G84G98X2.805Y-.0075Z-.34R.1F26.78571
X2.055
X1.59
X.84
X.375
X-.375
X-.84
X-1.59
X-2.055
X-2.805
G80M5
G0Z.1
M09
G91G28Z0.
G0G90G53X0.Y0.
M30
 
Our machines have been known to do this. It was found that there was a minimum tapping speed and if lower than that speed, the program would hang on the G80. If the tapping speed was increased to be over 150RPM, then no problem.
Since you are tapping at 1500 RPM, I wonder if the reverse might be true and you are tapping too fast.
 
Its In the posted code 1500RPM
I thought I had deleted that post after seeing what you were tapping at. I added another stating that the reverse may be true and you might be tapping too fast.

Edit: Just checked and Par#5241 sets the max spindle speed in rigid tapping.
 
Last edited:








 
Back
Top