[ddanutz]

Hi,

I've recently started with an 0i-MC Fanuc controll and an ARM type
toolchanger.
How is the correct way of calling for the tool, since an M6 starts the arm, without replacing the current tool number. It produces a lot of mess in the program. I tried T and M on different lines, still, a total mess.
Also if i call an M6 and the machine is not homed on Z, it outputs error message. Why do i need to manually command an G28 Z0?
On other Drum toolchanger machines, with Fanuc 18MC it just call TxM6, and everything is so simple, the machine goes and leave the current tool at the same location, etc.
Does anybody have experience with ARM type toolchanger that can give a little help here?

Thank you,
ddanutz

[CNC SERVICE]

What machine brand and model? I think the problem came from ATC interlock which MTB had wrote in ladder. Basically check at PMC parameter. If parameter okay, send me ladder diagram then I can help you at [email protected].

Thanks!

[ddanutz]

Hi,

thank you very much for your post.
Unfoturnately, i do not know where to send the LADER from or how
What is the normal operation mode for these ARM toolchangers?
If you have T1 in the spindle and T2 waiting in the turret, and put an M6, it
changes T2 in the spinde, but still the T1 is indicated as current tool ! That is strange.
Is it also normal if you change a tool, with the M6, the tool that has been in the spindle and now is in the turret does not retract to horizontal pozition, still it is vertical?

Thank you,
ddanutz

[CNC SERVICE]

Hi,
I will explain you for the sequence of ATC tool change,
After you give command M6 they will function as follow,

1. Pot down (Finished signal by Limit or prox. switch)
2. Arm rotate to 60' (Finished signal by Limit or prox. switch)
3. Tool unclamp (Finished signal by Limit or prox. switch)
4. Arm Down (Finished signal by Limit or prox. switch)
5. Arm rotate to 180' (Finished signal by Limit or prox. switch)
6. Arm up (Finished signal by Limit or prox. switch)
7. Tool clamp (Finished signal by Limit or prox. switch)
8. Arm retract to 0' (Finished signal by Limit or prox. switch)
9. Pot up (Finished signal by Limit or prox. switch)

As you explain, I think that after the machine running through No. 8 then stop, that mean Arm retract to 0' finished signal does not turn on then they are waiting, If the Japanese machine they will put PLC timer for a while then alarm happen. If Taiwanese machine they don't like to put this function that mean the machine is waiting and no alram and cycle start lamp always on if no reset. For Spindle tool No. and Pot Tool No. indicator is not change when the machine unfinished cycle. Find the fault then reset as I explained.
Thanks,

[bob@apc]

With an arm type tool changer I'm assuming there is a "floating" tool belt not a turret.
With a tool belt I would write the program for our mill as follows;
N1(Drill)
G91G30Z0.T1 (On our mill this is tool change position)
M6T2 (this line changes the called up tool ,T1, and calls up the next tool for the program T2. if that gives an issue, just drop T2 to the next line in your program or where ever you want as long as it's called somewhere close to the top of the program so it's waiting at the tool change position before the previous tool is done working, saves machine wait time.)
G90G0G54X0.Y0.
S2000M3
G43H1Z1.M8
G98G73X0.Y0.Z-1.Q.1R.1F10.
G80
G0Z1.M9
M5
G91G30Z0.
M1
and so on with the rest of your program.

If Z home is tool change position I would write it this way for a single hole;

N1 (Drill)
G28Z0.T1
M6T2
S2000M3
G90G0G54X0.Y0.
G43H1Z1.M8
Z.1
G98G73XO.YO.Z-1.R.1Q.1F10.
G80
G0Z1.M9
M5
G28ZO.
M1

The first and last thing we do for each number sequence is send the machine to tool change position. Our Fanuc O-M actually does it in the M6 tool change macro but we write it just the same for consistancy in the programs because our Okk with Neomatic Mitzubishi Control doesnt send the machine to tool change position during an M6
Bob