Troubleshooting MO3/M04 operation

I have a 1983 Kitamura mycenter 3 with Fanuc 6m controller. I can issue a spindle speed and m03 or m04 command in MDI and machine responds. RPM gage reads whatever S**** I entered. However when I right a test code with a few moves etc it comes to the S500 M03 line, spindle turns on and program stops like it's not receiving speed obtained signal. I can hit reset, spindle stops and rest of program continues on thru. Anyone have ideas on fixing this...or even a parameter to change to eliminate the speed verify?

put up you bit of test code that is not working
.... it may not be that line that is at fault

Superman's suggestion is a good one. In full auto the control reads in several lines ... so the issues may well be further down the code.
Another suggestion ... did you try single block instead of full auto? ... does it go any further in single block?

Hope this helps ...
Check out our Real World Machine Shop Software at Kipware® Software - Real World Machine Shop and CNC Software

Good morning gentlemen and thanks for the response. I'm sure you'll get a chuckle out of my feeble attemp at g-code programming but here is what I did

G90 G17 G28 X0 Y0 Z0
G54
G01 X2.00 Y2.00 Z-1.00 F50.00
G01 X4.00 Y2.00 F50.00
G02 X6.00 Y6.00 F50.00
G01 Z-2.500 F40.00
M8
S500 M03
G01 Z-2.625 F20.00
G02 X2.00 Y3.00 F50.00
G02 X2.00 Y2.00 F50.00
M9
G01 Z.00 F60.00
M30
%

I tried different spindle speeds as well as M04 instead of M03 Always same results. Machine moves to Z-2.500, spindle turns on and program stops and machine stops. I can press reset, spindle turns off. Press cycle start and program and machine continues to end of cycle

single block still will not continue past Mo3 unless I press reset first.

Hi,

Remove the G02 in all the lines or add a R-value ( I / J) in these G02 lines.
Is there no alarm ?

Regards,
Heavy_Metal.

Heavy Metal thank you so much. That simple to you correction fixed it right up Program cycles all the way to end. Now all I should have left is troubleshooting the tool changer carousel and I should have chips flying

Another suggestion:
G28 X0 Y0 Z0 must be commanded in G91 mode. Change to G90 thereafter.
For safety reasons, it is better to home Z first, followed by XY home::
G91 G28 Z0;
G28 X0 Y0;;
G90;

Quote:

---

Originally Posted by Hopcycle1

... I'm sure you'll get a chuckle out of my feeble attemp at g-code programming but here is what I did

G90 G17 G28 X0 Y0 Z0
G54
G01 X2.00 Y2.00 Z-1.00 F50.00
G01 X4.00 Y2.00 F50.00
G02 X6.00 Y6.00 F50.00
G01 Z-2.500 F40.00
M8
S500 M03
G01 Z-2.625 F20.00
G02 X2.00 Y3.00 F50.00
G02 X2.00 Y2.00 F50.00
M9
G01 Z.00 F60.00
M30
%

---

a little chuckle....????????
you 1st need to form some sort of programming structure...
everyone had to have a start sometime...
ie.
top of prog...
O1234 (job info)
(header info... setup etc)
G0 G17 G40 G80 G99 (safety codes)
M5 M9
G91 G28 Z0 (Z home)
G90
M1 ( optional stop)
()
(toolchange)
Ttt M6 ( tool info)
()
(set tool data)
G90 G54 ( set co-ord system.... you could use more in one program)
G0 Xx Yy
Ssss M3
G43 Htt Zz ( add toollenght to spindle while moving to z)
.... your prog
( retract procedure )
M5 M9
G91 G28 Z0.
G90
M1
()
...repeat for next tool from (toolchange) for each tool
...
(final retract)
G91 G28 Y0. (move table to front for part unloading)
M30
%

This is only a guide... but a point to remember....
if you turn a code ON..... turn it OFF ..... & build a good set of safety codes that restate the machine's startup condition.
... I've seen drilling done at near rapid rate because feed per rev. was not corrected after a tapping cycle....

Thank you Superman! I'm going to use your example to help me troubleshoot the ATC. At least I'll know it's not another one of my program failures :)