Fanuc tool change homing issue

[openforbiz]

I have a Ooya 2185 with a fanuc 15M controller.

The problem is every time I want to do a tool change I have to make sure it is allways homed in the Z axes. It attemts to do a tool change even when the spindle is 2 inches of the table.

All the cnc machines I have ever ran you can do a tool change command anywhere and the machine will automaticly move the spindle to the appropriate position and do the tool change.

Why doesn't T1;M6; work the way I want it too.

Please help

Thanks

[psychomill]

I'd start at the tool change macro. Should be one of the 9000 programs. Probably doesn't have a move in there to back the Z axis out.......

Although additionaly, I would think that the machine would have some switches in place to check and make sure Z is at the right position before trying to toolchange...

[tobyaxis]

Why not just write a Tool Change Sub-Program to address the issue for now. Then do more research as to why the machine is doing this.

O9800
(ATC)
G0G40G80M5
G0G98M9
G91G28Z0M19
G0G49G90
M99

[codyst]

Originally Posted by psychomill I'd start at the tool change macro. Should be one of the 9000 programs. Probably doesn't have a move in there to back the Z axis out....... Although additionaly, I would think that the machine would have some switches in place to check and make sure Z is at the right position before trying to toolchange...

I would start with the tool change macro also sending it to Z0 before the tool change.

Not all machines have switches to ensure that it is in position for a tool change. An old Okuma I used to run didn't have any switches. You had to tell it to go to Z0 before changing the tool or it would drop tools.

[openforbiz]

There is nothing in parameter in the 9000's dealing with the tool changer.

So how do you make a sub program recognize T1;M6;

[PBMW]

9000 is the program number not a parameter number. It's a protected program.
On my 0iMc if I MDI a T1 M6, the contents of the 9000 program go by on the screen as it's tool changing

[psychomill]

As I said (and PBMW restated), a 9000 PROGRAM, not parameter...

What Toby suggested works too... but it only takes seconds to look at your existing toolchange macro and correct it....

[Bluesman]

Originally Posted by openforbiz I have a Ooya 2185 with a fanuc 15M controller. The problem is every time I want to do a tool change I have to make sure it is allways homed in the Z axes. It attemts to do a tool change even when the spindle is 2 inches of the table. All the cnc machines I have ever ran you can do a tool change command anywhere and the machine will automaticly move the spindle to the appropriate position and do the tool change. Why doesn't T1;M6; work the way I want it too. Please help Thanks

You may want to call the MB and find out what they are not doing. The 9000 programs are generally created by the Machine Builder. But you can make a user M code program your self if you want to.

Go to Parremeter 7080 and put in a value of 616 (M616)

This will call up program O9020

O9020(TOOL CHANGE MACRO)
G0G91G28Z0
M19
M6
M99

Then anywhere you would use an M6 use M616 this should keep you from crashing untill you can figure out where the 9000 program is for tool change. Some Machine builders have them set up internally and you can not edit them.

Bluesman

[Al_The_Man]

Originally Posted by Bluesman Some Machine builders have them set up internally and you can not edit them. Bluesman

Also to stop erasing them accidentally, on the 15M it is P2201 bit #0 = 0 allows editing, set back to a 1 afterwards to prevent accidental erasure.
Display during execution P2201 Bit1 = 0
Al.