Need Help!- Fanuc OM acting up

[Machinist3]

Back again.
Fanuc OM on a Makino Mill.
Will load a program from DNC.
Won't change a tool. By program or MDI. MDI won't do anything. It comes up and you can type in the info but it won't accept it. Getting an 078 alarm when it tries to change a tool from a program.
Book says "A program or sequence # which was specified by address P in the block which includes an M98,M99, or G66 was not found" which has nothing to do with the program. Also can't edit a program. Maybe the input or insert button is bad on that part.
Any ideas fellas?
Thanks in advance!
John

[dcoupar]

Did these problems just suddenly appear, or did something happen?

Your toolchange problem sounds like maybe the ATC macro got deleted from the memory.

Check parameters 230 to 239. These set the M-code that call macro programs O9020 to O9029. One of them should have a 6 in it. So if parameter 230 has a 6 in it, M06 calls macro O9020. That program must be in memory or you'll get alarm 078 when you try to execute an M06.

[Machinist3]

I think it had been sitting for about 2 weeks and started when we fired it up.
I'll try your suggestions in the morning. Thanks for being so helpful and for your quick reply.
John.

[Bruce Griffing]

I had a similar problem on my machine. I couldn't get anything to make sense. After much thought I realized that there was a parameter, FLKY, 38 bit three, that tells the control what keyboard you have. Somehow it was hosed and the control thought I had a different keyboard. Once fixed - everything went well.

[Machinist3]

Hey Guys.
Thanks for the input.
I talked to fanuc today.
They were very helpful, must be the economy.
Turns out it was parameter 240.
There was suppossed to be a "6" in it.
Got that straight, still no toolchange.
My toolchange program had been deleted.
I then remembered that one of my former employees had
accidentally deleted all the programs.
There has to be a O9020 program in there for toolchange.
The parameter that lets it accept 9000# programs was wrong to.
I had taken the key out to open up the cabinet to check for a tripped fuse on the toolchanger . This left it in program protect and that was why i couldn't input anything.
Feel pretty stupid about that.
I'm assuming the TC program would be something as follows.
G90 G28 Z0
G28 X0Y0
M06
M30.
Any advice is greatly appreciated.
BTW, It's a Leblond Makino VMC.

[glovebox20]

Hello

You might want to add these lines in your tool change code

O9020 (TOOL CHANGE MACRO)
#3001= 1 (turn off single block?)
M9 (coolant off)
G91 G80 G40 G28 G0 Z0 M5 (home Z axis, cancel Canned Cycle, Cutter comp. cancel, spindle off)
M1 (Option Stop)
G91 G28 G0 Z0 M19 (ReHome Z axis in case machine was moved after Option Stop, orientate spindle)
G28 X0Y0 (This line may not be needed)
M06
G90 (back to Absolute coordinate system)
#3001=0 (single block on)
M99 (sub program end, back to main)

Note: your machine may require a G30 (2nd Ref position for tool changer) instead of a G28 (Machine Home position)

The possibilities are almost endless, just make sure what ever you decide, the mill will not alarm out or crash under ANY!! circumstance.

[sinha_nsit]

If M06 calls O9020, check O9020 also.

[Machinist3]

Thanks Glovebox.
I found something similar to this last night,
but it didnt have the single block ignore.
I'll try it out today hopefully.
John

[glovebox20]

Correction!!

System variable #3003 controls the single block mode not #3001 on a fanuc OM control.

You may also want to check out System Variable #3004, this controls the feed hold, and maybe some may to control the rapid override so it's always 100% regardless of the Rapid override knob. You should be able to find more information in the Fanuc OM Operators manual under the Custom Marco section.

Sorry If I miss lead you.

[Machinist3]

It's Alive!
Thanks for the help guys.
Been sitting long enough for the spindle drive belt to make racket.
I'll tackle that monday, time permitting.
Probably change the backup battery too.
There is no trick to that, right?
Just do it while the power is on?
Thanks a million!
John

[glovebox20]

Yes!! Change the batters when the power is on or you will loose your parameters, programs, and offsets, just like you would loose the time on your alarm clock if your change the battery if it was not plunged in. Always refer to the Fanuc manual or Machine Tool Builders book for more instructions.

This bring up another important point. When your finally get the mill up and ruining like how you want it, take the time to download/write all the parameters and programs needed to run the mill and save them in a safe place. It may take a while, but you will save your self a lot of trouble if you ever find your self needing this info again.

[gbowne1]

I guess I should do that too. I've got several FANUC machines with 11M, 15M, 0M controls. When I had my 6M-B machine I had its parameters backed up and written down.

The nice guy who did the ladder programming ended up doing my 11M and the 0M made hard copies of his work and put them in a folder for me. I may invite him back to do my 15M when it gets finished being built. He also sat down and wrote out specific documentation for my machine, nearly the same as what the MTB made when they built my machine.

Greg Bowne