[tmiuser]

Hey Gurus!

I am trying to discover why a CNC Lathe (Nardini) with a Series 20T Fanuc control will not execute a G01 code.

You can program a G00 and the lathe will respond perfectly and you have full control over Rapid Feedrate via the operator knob on the Crossfeed control box.

However, If you try to execute a G01, the lathe does not move at all.
There are no errors, and the 'DIAG' screen shows "In Motion = 1"

The 'Start' button is also flashing green.....

Hmmmm....It is almost like the lathe THINKS it is moving, but.....nope.

Example :

G00 W 3.0;
(Results in perfect operation.....)

G01 W3.0 F1.0;
(Results in no movement........no errors.....)

This machine was functioning perfectly with existing programs...and recently stopped.

I was wondering if it is possible to program some type of code that would block a G01 from operation.....

Be great to hear some suggestions!

Thanks!

[dcoupar]

Is the spindle turning? If not, is G98 (IPM) active?

[beege]

Program Check screen / Active
G98 = Inches per Minute
G99 = Inches per revolution
If Spindle = stopped AND G## = 99, no movement.
Also, feedrate override doesn't affect rapids (G00) but does affect Linear Interpolation (G01). Check override knob.

[tmiuser]

I did not program either of those instuctions in my little 'test' code, but will do so today.

However, programs that 'were' operating properly have stopped operating.....
So...that makes me wonder if a 'G99' has been ?accidently? previously programmed, and is still active.........

but, if I remember properly, they started the spindle on their programs before any G01 moves.

Good Info, though guys!....I'll get back to you with the answer shortly!

[fanuservicetech]

Please try turning "dry run" ON and see if the machine operates in G01. If it does operate with dry run ON then you may have spindle feedback problem (spindle position coder belt loose or broken) etc.

[Dan Fritz]

If you're in "feed per revolution" mode (G99) and the spindle is running, but there is no motion, you may have broken the belt that drives the spindle encoder. If the encoder is not turning with the spindle, there will be no motion in G99

[tmiuser]

Well.......

The spindle is turning, and the feedback on the contoller shows it.
(you can turn the spindle by hand, and it shows the speed......)

so...that rules out the belt being broken.

I have called FANUC service, and worked with Bill Caldwell for about 4 hours!!....we went thru many items in the machine to try and discover what was occuring.

All of the interlocks appear to be fine, there is no 'hold' signal active.....

The machine just sits....START Lamp flashing...with no errors, or movement.

I can try the DRY CYCLE idea...appreciate the input!

Bill's Idea was exactly what all of you have indicated:
Feedback belt broken. That appears to tbe the problem 98.9% of the time!!

So, we really examined that...and we have determined it is OK.

I did read in the Manual that you can issue a G01 W6.0 F0

If you issues that command with a F0, the G01 should operate in 'Rapid' mode.
I plan on trying that the next time I get to the lathe.
That will at least tell me that the G01 command is executing, and there is a feedrate issue someplace. (the feedrate knob operates properly in all positions during a rapid move (G00), so I must assume it operates properly for a G01...)

Still open for ideas!
Can't wait to discover/share the root cause of this issue!!!

[Dan Fritz]

I don't have a 20T parameter manual, but in the older Fanuc controls, there was always a parameter to determine the maximum G01 feedrate. If you programmed a feedrate greater than this value, the maximum was used instead. This prevented stress on the servos.

What if your maximum feedrate parameter got zeroed out for some reason ....

Hmmm. I love a mystery.

[tauntdesigns]

I not familiar with the 20T,

I did find a list on the web for lathe G-code PER MIN (G98, G94), PER REV (G99,G95).... Just for kicks and giggles, try G95 or G94

I'm curious too,
Jack

[Ozemale6t9]

check the diagnostics for the feed override. perhaps you have a broken wire to the override control, and the machine is assuming the knob is in the 0% position.

[bobo17]

try using g601. i have the fanuc control in a nardini and the g codes are all g601, g600, etc...

[sinha_nsit]

I was wondering if it is possible to program some type of code that would block a G01 from operation.....

Yes, it is possible to redefine G01 (or any other G-code), to call a macro. To check this, look at your program screen while G01 is being "executed". If the cursor jumps to a program of 9000 series, then somebody has done exactly this, to have fun with you! If the G01 block remains highlighted, then there is some other problem. I also faced this problem some time back. I had not programmed G98.

[chich2]

Hello,
I have the exact problem as tmiuser. The program get's to a g01 block and hangs!!!! The spindle is spinning and I have the cover off the machine so I can see the spindle encoder belt is fine. It also displays the spindle speed on the screen. Yes I do have G99 active.
G01 G02 G03 wont go. G00 is fine. G32 is fine also and when I alter the G32 feed rate the machine responds accordingly.

My control is a FANUC OT-C

Has anyone come up with a solution to this problem?

Chich

[underthetire]

Sounds like your timing belt for the spindle encoder broke.

[Ozemale6t9]

Hello,
I have the exact problem as tmiuser. The program get's to a g01 block and hangs!!!! The spindle is spinning and I have the cover off the machine so I can see the spindle encoder belt is fine. It also displays the spindle speed on the screen. Yes I do have G99 active.
G01 G02 G03 wont go. G00 is fine. G32 is fine also and when I alter the G32 feed rate the machine responds accordingly.

My control is a FANUC OT-C

Has anyone come up with a solution to this problem?

Chich

I would be checking the operation of the feed override switch...G32 should ignore the switch and set feed to 100% of programmed speed. If the override is faulty, or disconnected, it could be telling the machine that it is at 0% which would explain why G32 works and other feeds don't.

regards, Oz

[chich2]

Thank you both for your replies
Turns out my machine was in G99 "Feed per revolution" and the feed rate in the block of code was too high for the given spindle speed. I changed the block to go to G01 X0.0 Y0.0 F0.5 ; with a spindle speed of 500RPM and away it went!!!! :banana:

Previously I had the feed at 20.0 which would have meant that every revolution of the spindle the turret would have had to travel 20mm. Now with a spindle speed of 500rpm the turret travel feed would be set to go above the max speed in the machine parameters.
So simple, but a lesson well learned!

Once again, Thank you for your replies,
Chich

[sinha_nsit]

I had read somewhere that if you specify a feedrate higher than that permitted, the machine would move as fast as it can without giving alarm. As we see in your case, the machine may not move at all. Possibly, it depends on how ladder is designed.

[chich2]

Yes I believe I have read that as well. Yes you are correct as my machine just freezes. No warning lights, alarms, nothing. It just hangs. But now I know, I wont be programming anything that goes over the Max feed.

Chich

[chrose1286]

Had the same problem.This will give you G01...not very elegant but works on my fast trace.
%
O0007
N1 (TEST Z 7 FPM)
N2 G00 G40 G20
N3 G28 U0.
N4 G28 W0.
N5 (BORE MIN .75 FINISH)
N6 T0101
N7 G98 G97 F10.0 S750
N8 M04
N9 G00 X2.0 Z7.0
N10 G90 G01 Z5.0 F10.0
then where ever you want to go......CR