Fanuc OMC Control Quirks (freezes on pre-loading tools)

My VMC (Makino FNC-60, Fanuc OMC) has some strange control quirks, and I was wondering if anyone has run across these, or might know how to fix them.

For starters, if I stop the spindle mid-cycle, I am unable to re-start it. Is there a special button I need to press in combination with "Spindle Forward" in order to re-start it mid-cycle?

Secondly, pre-loading tools does not work on this machine. The machine has a side-mount toolchanger, but it freezes up when you call a tool which is already in the ready position. It does not throw an alarm or error or do anything at all. It just indefinitely stops executing the program. I have been working around this since I got the machine, but it's getting old, to say the least. The following code is an example of what freezes it:

N05 T1M6
N10 T2
N15 (T1 program)
N20 T2M6
N25 (T2 Program)
N30 M30

On the first execution, this program would freeze at line 20, before executing the toolchange. On subsequent program runs, the program would freeze at line 5, because T1 would already be in the ready pot from the toolchange at line 20. This makes running 2-tool programs annoying, since I have to add an extra tool-call at the end of every program.

Thanks in advance for any help. These problems are minor and stupid, but they are getting old.

I have an Omb
I have the next call in at least 1 line before the M6, usually right after the previuos tool change, that way your cutting while the next tool is moving into the change position on the carosel

re mid prog start/restart
once you stop a program, you need to manual restart the spindle, and coolant
If you don't you will push a non rotating cutter thru a part if you don't hit the cycle stop button
(did it once, hope not to do it again)
Mike

Could you do something similar to this?

N30 T08 (3" OTM FACE MILL) M6
N40 G54
N50 G0 G90 X-6.25 Y3.75 S500 M3
N60 G43 Z.1 H08 T20

(lots of) work

N450 T20 (13/16) M6
N460 G54
N470 G0 G90 X-3.5 Y3.5 S500 M3
N480 G43 Z.1 H20 T08

work

N580 G0 G28 G40 G91 Z.0
N590 G28 X.0 Y.0
N600 G90
N610 M30

We used to have a fanuc machine that had difficulties in pre-staging tools.

Until we tried this code

T1
M6
T2
<do T1's stuff>
M6
<do T2's stuff
M30

yes as Boris noted

the T call at least 1 line before and not in the same line as the M6
a few years ago buried within a 10m Fanuc manual I found the reason
I think the reason is all commands need to be able to be performed at once regardless of the order in the line.
Since you need to index the tool before you change, the separate lines are required
Mike

I agree with the toolchange format suggested. Almost all of our sidemount toolchangers need the T and m6 commands on separate lines. One of them (Kitamura Mycenter 3, mid 90s 0mc) can do either with seemingly no issue, but we program it as separate lines, just in case.

You should have no problem if it is like Boris' program. I suggest putting an additional T command before the m6, even if you had called it in the program, in case you wish to skip ahead, like:

T1
M6
T2(pretool)
<do T1's stuff>
T2 (again)
M6
<do T2's stuff>
M30

I doubt the machine would freeze if the pretool was called twice.

Is the tool change written into the ladder, or is it a 9000s program? If a program, you may look into what might be causing the control to freak out. I would bet that it is written into the ladder, though.


As for the spindle being able to be turned off while in cycle, that sucks. Our Kitamura does the same thing; the spindle off button actually turns the spindle off during automatic operation, but you are unable to turn it back on, short of stopping the machine, putting it into MPG, turn the spindle on, then throw it back in auto. (our machine also turns the spindle off at M00/M01, and doesn't turn it on after pushing cycle start, which I also find annoying). That may be a MTB set diagnostic bit (possibly) that deals with that. Look at the manual, or call Makino, maybe they can be of assistance on that.

Thanks for the responses guys.

Re: Alphonso, that is the sort of code that causes the control to freeze. Calling the tool already in the tool ready position freezes the control, at least when there is an M6 in the second line.

For production programs I do manually edit them to call the next tool as while the current tool is rapiding to the cut, but I thought all controls with side-mount toolchangers could handle code of the form Alphonso posted. It sounds like this is just a quirk I may have to live with though.

Tomorrow I will try separating the tool call and the M6 command, but I don't think that will change it. I seem to rembemer it always freezes when the tool called is already in the ready position, whether there is an M6 in the line or not. I have also noticed the control freezes when M6 is called in isolation, unless the tool in the "tool ready" pot has changed since the previous M6 was called. Is there a way to change this behavior?

I think the toolchange program is in the ladder. The toolchange macro itself is pretty basic:
:9001
M9
G0G28G91Z0.M5
G40G49
M19
M6
M99

As for the spindle, thanks. I was afraid that was the answer. I know that I can crash the machine by stopping the spindle and then letting the program resume execution; thankfully this hasn't happened (yet). Is there a way to get into MPG mode during drip feed to re-start the spindle, and then return to executing the drip fed program? I may try this tomorrow.

Halcohead said:

Secondly, pre-loading tools does not work on this machine. The machine has a side-mount toolchanger, but it freezes up when you call a tool which is already in the ready position. It does not throw an alarm or error or do anything at all. It just indefinitely stops executing the program. I have been working around this since I got the machine, but it's getting old, to say the least. The following code is an example of what freezes it:

N05 T1M6
N10 T2
N15 (T1 program)
N20 T2M6
N25 (T2 Program)
N30 M30

On the first execution, this program would freeze at line 20, before executing the toolchange. On subsequent program runs, the program would freeze at line 5, because T1 would already be in the ready pot from the toolchange at line 20. This makes running 2-tool programs annoying, since I have to add an extra tool-call at the end of every program.

Thanks in advance for any help. These problems are minor and stupid, but they are getting old.

Click to expand...

Many MTB use a Tool Change Macro program to facilitate the tool change, others use the PLC (PMC in Fanuc talk) excusably. If a Macro program is being used, there may be a problem there, or a work around may be possible in a Macro program.

Set parameter bit 0010.4 to "0". This will allow programs 9000 to 9999 to be viewed. If programs are registered under any of the following numbers, check the settings of the parameters shown in brackets:

O9000 (TMCR bit of parameter 0040)
O9001 to O9003 (parameters 0240 to 0242)
and
O9020 to O9029 (parameters 0230 to 0239)

If 1 is set for the TMCR bit of parameter 0040, program number O9000 will be used as a Tool Change program. If this parameter bit is set post a copy of program number O9000 for the forum to view

If the numeral 6 is set in any of the parameter numbers 0230 to 0242, post the program that is associated with the parameter that has the 6 registered therein. Refer to the program and parameter range above to find the associated program.

Regards,

Bill