Program tool numbers greater than machine's number of pockets - Fanuc

Dan from Oakland said:

"Setup Sheets could be layed out as T144 Pot 7". That won't work on a machine with a random access tool carousel after you load tools because the tool won't get put back in the same pocket after a tool change.

Click to expand...

Ox said:

If you hand load the tools over T40, all should be fine I would think?

Call M6 T041 and it should empty the spindle and call offset 41.

M6 T041
M0
(Manuelly change tool here)
M3 S2500
G0 bla

bla
M0
(Manuelly unload spindle)
M6 T202


Unless the "M" series doesn't (can't be made to?) use T codes like that?



I doo it like this on a Siemens, but I am not able to pull up other offsets, so I hafta just run with no offset at all and code it according to the tool length figgered in. Much bigger hassle when replacing tools.


------------------

Think Snow Eh!
Ox

Click to expand...

Vancbiker said:

What you can do will be determined by how the machine builder wrote the PMC logic of the machine. Some have a table where tool numbers are assigned to pockets that can be edited by the user. This is pretty common on machines that have "random" style magazines. Other machines will have a fixed tool number to pot correspondence table. Builders can also have logic that prevents calling tool numbers outside of range they choose to allow.

Click to expand...

dandrummerman21 said:

Vancbiker is right in what he said above. It may or may not be possible on your machine(s) to do what you want.


There is a sort of workaround, but it is also limited. See post #13 (by angelw) in this thread: Side Mounted Tool Changer and Fanuc 0iMD

You would be limited by that method in the fact that you couldn't use tool 1 and tool 41 in the same program; the method outlined there would have the machine see them as "the same tool".

I would no do that method personally; I feel like it has a higher likelyhood of screwing up in some unforseen way, even though I don't know how it would.


My recommendation is to get a machine with more tools! Have 2 machines with 100 and 132 tools available to me. And I still find myself swapping some tools out because that is not enough...





Edit: I just realized you were the person who bumped the thread I just linked you to, so I know you've already explored that option. lol.

Click to expand...

Narf said:

Hello,

I'm looking for a means to assign all of our tools their own, unique tool number...3 Fanuc VMC's have a range from 1-400 offsets in their controllers, but are limited to 40 pockets. Is there anyway to program, for example, T144 to a random pocket? Obviously, we'd be limited to 40 tools in the machine at a time, but this would alleviate a lot of confusion on programmers side of assigning tool numbers, and operators side of finding and loading them. How do you all handle this?

Click to expand...

MΛCK;3301971 said:

I would think it would be easier approach to leave the T numbers be and use the N numbers and parentheses to identify the tool in the spindle. N144 N1144 N2144... (T144 1/2 in. endmill....)

T144 for example


N144 T7 M6

G90 G0 G54...
G43 H144 Z.1...

Setup Sheets could be layed out as
T144 Pot 7

Then when you have a job that requires a T300 in pot 7 you don't have to worry about the T (pot) number matching and you can utilize all the 400 offsets, which comes in handy when reusing tooling.

Click to expand...

couch said:

T, H & D values don't all need to match. You can use 1-40 for your Tool numbers, and assign a specific H & D value for the tool you want. For example, Call up T14 with H114 and D114, etc.

That type of stuff is typically the setup guys responsibility to reorder numbers if he needs to squeeze a job in a machine that's already setup with something else. Renumbering tools to ones that are available, or sharing tools with the same tool number but assigning its own unique H and/or D, and so on.

Click to expand...

Qwan said:

The old Fanuc controls did not have the ability to match all the comps for the tool using the same offset number, every one used a unique offset number.

Click to expand...

angelw said:

Hello Qwan,
What does that even mean?

With a Fanuc control since day dot, any Offset Number could be programmed with any Tool Number and multiple Offsets could be programmed with the one Tool. Only one offset could be active at one time of course. Of course, it is logical to combine the same Offset Number as the Tool Number, but if you wanted to dance outside the box, you could do what you likes.

Your second example appears to be for a machine that didn't have infinitely variable spindle speeds, but an S value that represents a particular RPM. For example:
S1=200
S2=250
etc.

You would see this arrangement with 3000C controls and earlier, but even early controls such as 3000C, infinitely variable (infinitely variable integer values) Spindle Speeds was available. I've never seen other than infinitely variable Spindle Speeds on FS6 controls, although this was more up to the MTB than Fanuc. But certainly never on an FS11 control. The MTBs would be shooting themselves in the foot to be still offering machines without infinitely variable Spindle Speeds at that stage.

Regards,

Bill

Click to expand...

Narf said:

If I understand this correctly, we would still have the issue of programmed tool having duplicate T numbers? N144(tool 144)T7, N220(tool 220)T7, etc. we would have to condense all tools to T1-40 resulting in many programs being modified trying to find open pockets. or did I misinterpret this?

Click to expand...

Narf said:

I believe he is talking about older fanucs when there was no differentiation between length and diameter...so you had T2 with H2 but D42 for example, because there is only one input for each offset.

Click to expand...

angelw said:

.....Your second example appears to be for a machine that didn't have infinitely variable spindle speeds, but an S value that represents a particular RPM. For example:

Click to expand...

Vancbiker said:

Hi Bill,

Qwan is talking about a unique bit of PMC programming used by Makino back in the 6, 10, 11, 12, and 0 series controls. The M57 invoked logic in the PMC to read the subsequent S and T addresses and populate the tool to pot correspondence table. At the end of the assignment program I think I recall that one had to execute M58 before the M30 to disable the tool to pot data setting mode. It was a rarely used function in my experience. Some folks may have found it useful, but I really never did. The only times I recall using it was to create the tool to pot table after re-initialization of the control.

Click to expand...