Need Help!- TOOL CHANGE NOT WORKING

[rajesh_1355]

Dear Friends

(MACHINE: MORI SEIKI-VMC-FANUC OMD)
In my machine alarm 901 appeared few days back, found its memory card defective same got repaired & reloaded the data. Everything is running ok except tool cycle.
I Redownloaded MACRO PROG. 9020 prog but I dont know how it got corrupted. Here it is...
&HE:%
:9020(CAMBIO UTENSILE)
WHILE[#11GT0]DO1
G90YY[#25+#18*SIN[#1]]
#3=#4003
G28G91Z0M5
T#4120
M6
G#3
M99

I am sure above prog need some little correction. Pl suggest me how to correct it.
Any help will be a great help .
Thanks

[suman]

Why dont u try by just Txx M6 code.

[dcoupar]

Originally Posted by suman Why dont u try by just Txx M6 code.

M6 on his machine probably calls macro O9020, which appears to be incomplete.

[dcoupar]

Originally Posted by rajesh_1355 Dear Friends (MACHINE: MORI SEIKI-VMC-FANUC OMD) In my machine alarm 901 appeared few days back, found its memory card defective same got repaired & reloaded the data. Everything is running ok except tool cycle. I Redownloaded MACRO PROG. 9020 prog but I dont know how it got corrupted. Here it is... &HE:% :9020(CAMBIO UTENSILE) WHILE[#11GT0]DO1 <------------- No matching END1 block G90YY[#25+#18*SIN[#1]] <------ Double address YY #3=#4003 G28G91Z0M5 T#4120 M6 G#3 M99 I am sure above prog need some little correction. Pl suggest me how to correct it. Any help will be a great help . Thanks

Where did you download this macro from? It appears to be missing some blocks and has errors (see comments <---)

[underthetire]

If it is a mori with a 0m, you don't need a macro for atc. Someone has probably installed a macro assigned to m6. That was a common thing for people to do way back, if you called the tool that was in the spindle for a tool change, the machine would alarm out. There was a keep relay to do the same thing.

[rajesh_1355]

Originally Posted by dcoupar Where did you download this macro from? It appears to be missing some blocks and has errors (see comments <---)

Dear I downloaded it from machine when in good condition. I don't know how it got corrupted. Pl suggest some remedy to run the cycle. Its Mori Seiki Fanuc OMC machine.

Do u have detail of Micros.
Pl send.

Thanks

[dcoupar]

Can you post your program here? Especially the tool change section.

[rajesh_1355]

Dear Sir,
I tried many combination suggested in this forum for tool change prog 9020 but could not success-ed. Actually this machine is MORI SEIKI - MV 40 S WITH FANUC OMC. I tried to understand the ladder but it is too complicated. In the ladder for tool calling D 3265 bit is used which normally does not shown in ladder unless u make bit 64. 3 / 4 high. As soon as Txx command executed. Machine shows alarm EX 201 Tool data error ( like ).

Any suggestion will be very helpful.

Regards.

[stevo1]

We are going to use program 9020 since this is what you have. First thing you are going to have to do is make sure that parameter 230 is set to 6 as this will call program 9020 when you program an M6.

Now since your program was corrupted I am only going to use what I think you will need and how I would write it.

:9020(CAMBIO UTENSILE)
#3=#4003
G28G91Z0M5
T#4120
M6
G#3
M99

This is just a basic tool change. You are setting your modal G90/G91 to #3 then sending the machine to Z0, calling your modal T() then the M6 to change the tool, finally setting your G90/G91 back to its original state.

I always like to skip the tool call if you are calling the tool that is already in the spindle. You would need to see if the MTB set up a system variable that tracks the tool in the spindle or you have to set a common variable up to do this. Let me know if you want this and we can add it.

Stevo

[underthetire]

Or just set parameter 230 to 0 and use the factory embedded macro...
All mori's use an M6 that is embeded. Someone added that macro, not the factory. As long as z is at home, M6 will do a tool change when M6 is commanded. The ONLY time i've seen factory macros in the 9000 series, was for APC( pallet change) spec, and a couple for probing.

[stevo1]

That is another solution. Someone wrote the macro for that machine for a reason I would think. I had many machines that had the embedded macros but would not work unless Z0 was positioned before the tool change which was a PITA for some guys to remember. I also had machines that would alarm out if you were calling the current tool in the spindle. The custom macros came in handy to avoid any of these issues.

Stevo

[underthetire]

I agree. Mori did use a keep relay just for the tool in spindle. It would just ignore and move on. The Z0 was no easy solution other than a macro.