Bar Feed on Mazak Problems

[chucker]

I have a Mazak quick turn Nexus 250 II with a LNS Quick Load 80 bar feeder works great lathe runs great but when the lathe sees the end of bar at the M69 it jumps to the sub program 9999 it will run the sub just fine open the chuck bring the stop down push to the stop close the chuck but here is where it gets funny it will get to the M99 and jump back to the top of the sub star all over again not go back to the main program I have even tried to use a M98 to get back to the main program and get an alarm that says it can’t find that program number put a M30 at the end it will go back to the top of the sub and stop I can write test programs and jump back to the main from the sub run in a loop jumping back and forth it all work just fine this only happens when the M69 calls the sub. LNS says its Mazaks problem Mazak has no ideas at this point anyone ever run into this?

Thanks for your help in advance

O3030 (main program)
Do
All the
Work
N30 (BAR PUSH FOR NEXT PART)
M5
T1010
G0Z1.
X0
Z.03
M69 (END OF BAR CHECK) jump to sub 9999 if EOB
M206 (OPEN CHUCK)
M68 (BAR PUSH)
M207 (CHUCK CLOSE)
G0Z3.
X10.
M1

O9999(BAR SUB PROGRAM)
(*)
(*)
(*)
M5
M9
G28U0
G28W0
M0(REMOVE DROP)
T1010
G0Z1.
X0
Z.03
M206
M68
M207
G4P2500
G0Z1.
G28U0M5
G28W0
M1
(*)
(*)
(*)
M99
%
I forgot to say I have another set of machines just like this and it works fine on it

 

[calcul8r]

We had this same problem with a QTN 200 and a FMB barloader.
We ended up putting the part program # after the M99
We have a top cut program running after EOB btw.
IE. M99S1 (S1 for program 1)
Might be worth a try.

Mike

 

[chucker]

Tried the M99S and program number and M99P and program number and M98 and program number still goes back to the top of the sub and starts over

 

[calcul8r]

I just relooked at the program and its M998 sorry about that. Trying to do too many things at once.
We tried many things and went through the same kinda thing that you did with Mazak, and finally had an app guy give us the M998 as a last resort but the whole order is a little different than normal.
Having trouble uploading the program pictures, if you would like I can email them to you
Mike

 

[angelw]

I have a Mazak quick turn Nexus 250 II with a LNS Quick Load 80 bar feeder works great lathe runs great but when the lathe sees the end of bar at the M69 it jumps to the sub program 9999 it will run the sub just fine open the chuck bring the stop down push to the stop close the chuck but here is where it gets funny it will get to the M99 and jump back to the top of the sub star all over again not go back to the main program I have even tried to use a M98 to get back to the main program and get an alarm that says it can’t find that program number put a M30 at the end it will go back to the top of the sub and stop I can write test programs and jump back to the main from the sub run in a loop jumping back and forth it all work just fine this only happens when the M69 calls the sub. LNS says its Mazaks problem Mazak has no ideas at this point anyone ever run into this?

Thanks for your help in advance

O3030 (main program)
Do
All the
Work
N30 (BAR PUSH FOR NEXT PART)
M5
T1010
G0Z1.
X0
Z.03
M69 (END OF BAR CHECK) jump to sub 9999 if EOB
M206 (OPEN CHUCK)
M68 (BAR PUSH)
M207 (CHUCK CLOSE)
G0Z3.
X10.
M1

O9999(BAR SUB PROGRAM)
(*)
(*)
(*)
M5
M9
G28U0
G28W0
M0(REMOVE DROP)
T1010
G0Z1.
X0
Z.03
M206
M68
M207
G4P2500
G0Z1.
G28U0M5
G28W0
M1
(*)
(*)
(*)
M99
%
I forgot to say I have another set of machines just like this and it works fine on it

Hi Chucker,
There are parameters to specify a Custom "M" code to call a Macro, or Sub Program. The setting range is 0-9999. Also, there are parameters to specify the calling type of the "M" code. The setting range for this is 0-3, and relates to M98, G65, G66 and G66.1 respectively. I believe your issue is with the calling type setting. To confirm this, replace M69 in your program with M98 P9999 and test. If the program O9999 is called and returns to the Main Program after one execution, then I'd say that its the Calling Type Setting specified for M69 that is causing your problem.

If the Calling Type is set to M98 or G65 (setting 0 and 1 respectively), then program control should return to the Calling Program from the Called Program after execution has been completed. If its set to G66 or G66.1 (setting 2 and 3 respectively), then I'd expect the Called program to repeat when the Z and X moves are read back in the Main Program. You may not be aware that control is actually returning to the Main Program, as unless you're operating the machine in Single Block, the Modal action of G66, G66.1 will not be obvious.

I don't have a manual in front of me at the moment to direct you to the required parameter area, but you will be able to find reference to what I'm saying in the manuals for your machine.

Regards,

Bill