Tool change Macro 9020?

[Tricky1]

I've been reading a lot about this macro, and I am really confused, was hoping someone can shed some light on this topic.... What exactly is the purpose of using a macro for a tool change? In all my yrs of cnc machining, I have never run across this. A simple T command with an M06 is all I ever needed to change tools. The ATC on this Funuc O-M will not work. There is a 9020 macro program in the memory. Do I need to call it up as a subprogram in order to change tools? That just doesn't make sense to me to use a separate program for a tool change... Can someone post an example of how the progrom should look to change tools? Any help is appreciated.

[christinandavid]

All controls use a 'background' program to perform a tool change, invoked by the M6 command, using the T value as an argument. The program should be full of obscure M-codes to check relays and work the ATC hydraulics/mechanisms. As machines vary, you will need to get in touch with the relevant machine tool builder to assist you with setting up a tool call macro.

If 9020 is indeed the correct program to use, and is in the correct directory (system folder, for example), it should be a simple task to set up the controls system parameters to invoke this program at every M6 command.

DP

[r.kynaston]

i found myself in the same position about a year ago. we picked up a horizontal
which needed to go to a set point in the x,y axii and up to that point i had been
only dealing with vertical mills that only required to be sent home in the z axis
---G0 G91 G28 Z0;G90T1;M6;
nice and simple
in the case of the new(to me) horizontal i entered --T1;M6;--turned on the
single block switch,put the rapid over-ride on "slow" and began pushing the cycle start button,after two pushes the screen was showing a 9000-series program which sent the spindle to the required G53 X,Y position and the z axis home, gives the control a couple m codes including M6 and the tool changed.
the control on that machine is set up to run the 9000-series program to change the tool every time an M6 is read along with handling the M6 as a tool change
in the 9000-series program---in the same way that a haas control can be asked
to check for H+T code every time a G43 is read,this can also be done with the fanuc using a 9000 series program. so take a look in the 9020 program you mentioned and see what it's doing,i picked he one apart from the horizontal and used it in one of our verticals to avoid interference between
tool and fixture during changes of long tools while tall fixtures are mounted on the table. hope this helped, and have a nice day

[dcoupar]

It's done in a macro to eliminate you having to program the individual commands for each tool change.

On your 0-M, parameter #0230 should be a 6. This parameter specifies the M-code that calls macro O9020. If #0230 isn't a 6 then when you program an M6 it won't call the macro.

[sinha_nsit]

Another reason for using a tool-change macro is safety. Tool change has to be done is a safe position, say, at home position, to avoid a possible interference between moving parts (of ATC) and fixtures. A macro can be designed to automatically send the tool (spindle) to a safe position before changing the tool. If you need, you can also include spindle orientation in the macro, among other things.

[stevo1]

The macros in the 8000 and 9000 range can also be set so you do not see them running on the screen. So it could have been that some of the machines you were running did actually use a macro but you never noticed it because it was not visible. I would have to say that 98% of the machines that I have dealt with, setup, or installed have had macro programs for tool changes. If they didn't I would write one.

To add to what Sinha has mentioned. I use the macro not just to move to a safe position but to skip the tool change if you are calling a tool that is already in the spindle. I also set my G43H() so that I do not have to program it after every tool change in the main program. I also set the S&F to the tools. The list can go on for the reasons to have a macro tool change.

As you said all you needed was a T() command and an M6. Macros can be setup so that it is called every time a T() or a M6 are programmed just by setting the proper parameters as Dave specified. This is not the same thing as a subprogram call with M98 which I believe you are referring to. If 9020 was indeed your tool change program you do not need to call it. By setting #230 to 6 this will call program 9020 every time a M6 is programmed.

Stevo

[Swemill]

Anybody that have info on which parameter these Macro - as Stevo describes would call on the 3M control?
I cant find the right parameter but i also dont know if its even possible on my old control....

Thanks.

[gbowne1]

I need a much more defined M6. It's pretty good, but I don't know if there could be improvements. It's a sort of homebrew ATC w/20 station carousel, but the M6 macro runs so that it moves to X, Y and Z safe locations, and then snap, out comes the arm and flips around the tool meanhile replacing the tool in the carousel and the spindle at the same time. I do not remember which 8000 or 9000 program it is. I believe when Brent came over to build the ladder and the 9000 series programs for my 15-MA, he set the M6 they way it is standard on most machine tools.

I remember that he and I talked at legth about how my other FANUC controls and machines were built and set up when he built the ladder and programs for this 15-MA like my 11M and 0M are.

Greg

[stevo1]

Greg,
Did he set it up via ladder or parameters? What is it that you would like to change or add? Can you post the code?

Stevo

[gbowne1]

I think it is Parameters I need to call Brent anyhow so I will ask him.

[stevo1]

Originally Posted by gbowne1 I think it is Parameters I need to call Brent anyhow so I will ask him.

This is a list of the parameters that will set the custom codes on the 15series.

7050-7059 parameters calls programs 9010-9019 with a custom G-code
7060-7069 parameters calls programs 9040-9049 with a custom G-code
7071-7079 parameters calls programs 9001-9009 with a custom M-code
7080-7089 parameters calls programs 9020-9029 with a custom M-code

So as an example if you want to call program 9020 as your tool change macro with M6 then you have to set parameter 7080=6

Stevo

[gwarble]

in my experience, you never know...

we have some machines with a macro tool change... from the factory (and ard copied in the manuals) which use m codes for each action of the toolchange (umbrella changer)

some machines that needed a toolchange macro added to home the axis to the change position, but otherwise the m6 directly actuates the toolchange action sequence internally, without any NC code besides the m6


some more modern fanuc's have other ways to "embedd" certain macros in the f-rom and you can't see them, but they are still NC driven, or at least home and orient with NC code and then internal drive the toolchange action by the ladder or macro executor via the m6

also be aware o9001-09 toolchange macros handle the t# differently than o9020-29... o9020 toolchange will treat the t# passed in the same line as internal variable #20, while an o9001 macro (subprogram style) will allow the t# to be system-applied to variable #4120 before the macro is called, so you will have to handle this internally like:

T#20

to apply the system tool # before the machine's tool change action in most cases...


- gwarble