Fanuc OT ycm lathe spindle speed problem after running a program

[twr]

Hi after I finished running a program l can't change the spindle speed in MDI with M3S200 or what ever speed. I tried it with the spindle stopped in MDI, M3S200 and also tried changing the speed in MDI with the spindle running at the last speed that was in the program s2000 by manual turning it on. If i turn the control off and on again its works fine. Fanuc OT control on a 2000 YCM lathe. This lathe is new to me and only the 5th/6th program i have tested but they all act the same.

 

[Vancbiker]

What is M13 and M14 on that machine?

 

[twr]

Hi Kevin, its my window air blast so i can see. Its chuck air blast ON M14 and OFF M13 from ycm but i made it into a window air blast.

 

[wmpy]

Try commanding G97S200M03 in MDI. It could be that you are still in constant surface speed mode from the G96 in your program.

 

[twr]

Ok i will try that Mon. when i go back to my shop.

 

[alphonso]

I always program a G97 S whatever just before tool goes home/toolchange when G96 has been used:

G97 S500 M3
G0 Z____ X____
G96 S400
WORK
G97 S500
G28 U0 W0
/M01

 

[sinha]

Actually, G97 is the default, unless there is a parameter to change this behavior. Therefore, after M30, G97 should be active.

 

[twr]

Hi Sinha, i thought M30 was reset to top of program and should cancel G96 this is not happening. As you said maybe its a parameter that needs to be changed but i can't find anything in my manuals. My old mori 6t did not do this.

 

[sinha]

M30 is reset and rewind.
Control is always reset. Rewind is parameter-controlled.
Of course, things slightly vary across control versions/models.

 

[twr]

So then M30 should cancel the G96 and the control should go back to G97 then.

 

[sinha]

This might be relevant (copied from 0i manual):

 

[sinha]

So then M30 should cancel the G96 and the control should go back to G97 then.

Normally.
3402#6 should be 0, as explained above.

 

[twr]

I just downloaded the manual for a OT control so i will start looking for a parameter that may do the same as you posted.

 

[twr]

Hi it looks like its 2 parameters affects how its cleared #0045 selects clear conditions if set to 0 or 1 then #0391 below. I will be going to the shop later today and will see how these parameters are set. I will post back my findings!

NOCLR 1 : Special G-codes are not cleared by reset operation.
0 : All G-codes are cleared by reset operation.
(Note) This parameter has meaning only when parameter 045#6 (CLER) is set to 1”.

 

[sinha]

set to 7

7 looks odd.
Is it a typo (for 0 or 1)?

 

[twr]

Yes i seen that to, its a 1 in the manuals print. I just copied and pasted it here and when i did that my computer seen it as a 7, I will fix here so no one gets screwed up.

 

[sinha]

If it is a bit-type parameter, it can take only 0 or 1 values.

 

[twr]

I changed parameter #45 bit #6 to a 1 now it works like it should. Thanks everyone for the help!