[ldouble619]

Hello all,

I have set up tool life on one of our machine, however I do have some questions and concerns..

1. How do I change my program to setup it up in cycles not minutes?


2. Is there anyway to alert the operator when the tool changes? Right now they are loading from the back of the machine, so they have no idea when a tool is being changed out and to inspect that part.

It would be nice to have them hit cycle start or something to confirm a new tool.

Thank you for the time.

[stevo1]

Welcome to the group.

You are forgetting 1 thing…..you never told us what kind of machine and control you are using.

There are many different ways that you can do this. I would personally set up a macro for counting the pieces and notify the operator of the tool change.

Stevo

[ldouble619]

Thank you.

The machine is a Mitsui seiki HW55. Controler is 31i


Thanks for the help.

[stevo1]

1. Do you have a programming or operator manual for this control?? There should be a timer for cycles as well as minutes. The manual should explain it.

2. You can put a message in the tool change macro. If you do not have one on this machine we can set one up either using the M6 code or the T code. It is very simple to do. You can have the machine stop and display a message along with needing the cycle start button pushed in order to continue.

Stevo

[MysticMonkey]

Maybe this will help

[ldouble619]

1. Do you have a programming or operator manual for this control?? There should be a timer for cycles as well as minutes. The manual should explain it.

2. You can put a message in the tool change macro. If you do not have one on this machine we can set one up either using the M6 code or the T code. It is very simple to do. You can have the machine stop and display a message along with needing the cycle start button pushed in order to continue.

Stevo

I got number one taken care of, it was a param change 8430 I think..

Stevo, If you can help me with that, it would be awesome! What you describe is exactly what I need. However I have no idea how to do that.

Thanks for all the help.

[stevo1]

I have never worked on the 31i control so you should double check the syntax for this control.

First thing you have to do is see what programs are being called for your tool change macro if you have one set up. The best way to do this is by calling a tool and seeing if it jumps to a subprogram in the 9000 range. The other way to tell is looking at the parameters that need to be set in order to call a macro with an M-code. For your control the following parameters will call subprograms.
Parameters 6071-6079 calls programs 9001-9009
Parameters 6080-6089 calls programs 9020-9029

Check these parameters to see what they are set to. For example if parameter 6072 is set to 6 then program 9002 is going to be called when a M6 is programmed.

Once we establish which program is being called or if none are called then we will set one up to be called with every M6. For example sake lets set up program 9001 to be called with a M6. So set parameter 9001 to 6. Now make a 9001 program and you can write a stop inside of this program so that the operator has to push cycle start if a tool is changed.

Now IIRC #3006 is still the system variable to stop the control with a message in your control. You can set up the stop in a few different ways. You can use a M1 for optional stop, M0 for program stop, or #3006. If you ALWAYS want the program to stop then use M0 or #3006.

If you use M0 then the program will stop at that code and sit until cycle start is pushed. If you use #3006 then you have to program it like so.
#3006=1(tool change cycle start)
Now the program will stop and it will go to the message screen and display what you what written in the parenthesis on the screen. You can then push cycle start to continue.

If you have a program currently being called for the tool change then post that code so we can find the best place to insert the program stop.

Stevo

[sinha_nsit]

#3006=1(tool change cycle start)
Now the program will stop and it will go to the message screen and display what you what written in the parenthesis on the screen.
Stevo

As far as I remember, on my machine with 0i Mate TC, the message screen does not automatically come. The program does stop (and re-starts with CYCLE START button), but the message is displayed only after pressing the MESSAGE key. How can the message be automatically displayed?

[stevo1]

I have not worked enough on the Oi series control to notice the message is displayed after cycle start. So does that mean you have to push cycle start twice to continue the cycle? You say it stops with no message, then you push cycle start and it displays the message…..does it stop at that point as well or will it continue the cycle with the message displayed on the screen??

What does the screen display when it reads the #3006?? Does it stay in the main program and sit on the #3006 line like an M0??

On the 10,11,12,15,16,18,21 series and IIRC the O series when #3006 is set to 1 the screen will change to the message screen, display the message in parentheses and stop the cycle.

Stevo

[sinha_nsit]

CYCLE START is required to be pressed only once for restarting execution. Everything is same as in other control versions, except that the screen does not automatically change to message screen. If you want to see the message, you have to select message screen. If you wish, you can even restart execution without reading message. It is like M0. Possibly, it is parameter-related issue. If I come to know about it, I would post it here.

[stevo1]

CYCLE START is required to be pressed only once for restarting execution. Everything is same as in other control versions, except that the screen does not automatically change to message screen. If you want to see the message, you have to select message screen. If you wish, you can even restart execution without reading message. It is like M0. Possibly, it is parameter-related issue. If I come to know about it, I would post it here.

Huh….that is pretty weird. I have never seen that before. What is the point in having a program stop with a message if you are not going to display it? I would not even bother then with the #3006 and would just use M0 then. I would have to ass u me that it is a parameter setting. So does the code just stop on the #3006 line and sit?

Stevo

[sinha_nsit]

Yes, it works like M00. Just sits over #3006 line, waiting for CYCLE START to be pressed again.
This may be a parameter issue. I have just seen the following in 0i parameter manual (though I have not tested it):
3111#7 (NPA): Action taken when an alarm is generated or when an operator message is entered
0 : The display shifts to the alarm or message screen.
1 : The display does not shift to the alarm or message screen.

[ldouble619]

I have never worked on the 31i control so you should double check the syntax for this control.

First thing you have to do is see what programs are being called for your tool change macro if you have one set up. The best way to do this is by calling a tool and seeing if it jumps to a subprogram in the 9000 range. The other way to tell is looking at the parameters that need to be set in order to call a macro with an M-code. For your control the following parameters will call subprograms.
Parameters 6071-6079 calls programs 9001-9009
Parameters 6080-6089 calls programs 9020-9029

Check these parameters to see what they are set to. For example if parameter 6072 is set to 6 then program 9002 is going to be called when a M6 is programmed.

Once we establish which program is being called or if none are called then we will set one up to be called with every M6. For example sake lets set up program 9001 to be called with a M6. So set parameter 9001 to 6. Now make a 9001 program and you can write a stop inside of this program so that the operator has to push cycle start if a tool is changed.

Now IIRC #3006 is still the system variable to stop the control with a message in your control. You can set up the stop in a few different ways. You can use a M1 for optional stop, M0 for program stop, or #3006. If you ALWAYS want the program to stop then use M0 or #3006.

If you use M0 then the program will stop at that code and sit until cycle start is pushed. If you use #3006 then you have to program it like so.
#3006=1(tool change cycle start)
Now the program will stop and it will go to the message screen and display what you what written in the parenthesis on the screen. You can then push cycle start to continue.

If you have a program currently being called for the tool change then post that code so we can find the best place to insert the program stop.

Stevo

THank you! I am still a little confused, as I have never done anything like this before.

Writing the 9001 program...I understand that the #3006 is a program stop, can you give me an example of what the program will like? I don't want it to stop at every tool change, I use 15 different tools for the part....
I want it to stop if it grabs a tool life pocket tool.

For example, T 1001 uses T1 (or I should say pocket 1), once the life expires it grabs T45, T46, T47..etc.

I want the M0 to happen when T1 expires and moves to T45 to notify the operator.

Thank you for all your time.

[stevo1]

Sorry for the late reply.

Example would be probably about after your M6 call you would have a line #3006=1(cycle start to continue). Now when it reads that line it will display the message you have writtne in () parenthesis.

Ok now you are getting into areas I am not familiar with. I don’t use tool life or tool types on any of my machines. I don’t know exactly what the machine is doing to select the next tool after the life has expired. According to the 31i manual you specify specific tool types. You have 2 exact same tools these would be set to a specific type and when the life runs out on the first one then it searches for the same tool type, checks the life and if all is good it will use that tool.

I have attached the system variables that are used in your control for tool life. I am trying to figure a way that they can be used to throw a stop in the tool change program if you go to the next tool in the tool type with life left on it.

Hmmm, it’s a very good question and I wish now I had more experience with tool types and life. I am going to have to think on this one a bit. Stopping the control at every tool change is easy but after switching based on tool life is a different story. Anyone that can give some details on tool life syntax please oblige.

Stevo

[chucker]

Huh….that is pretty weird. I have never seen that before. What is the point in having a program stop with a message if you are not going to display it? I would not even bother then with the #3006 and would just use M0 then. I would have to ass u me that it is a parameter setting. So does the code just stop on the #3006 line and sit?

Stevo

On the 16i 18i 160i 180i parameter 3111.7 NPA says
When an alarm is generated the display shifts to the massage screen (0) does not shift (1)
I would think there should be one on other fanuc controls

[gurayunsal]

Dear Friends...

Do you know There is any opportunaty to totall cutting lenght on FANUC Oi to manage tool life. (G01 + G02 + G03 ...)

[email protected]

[gbowne1]

On the 10,11,12,15,16,18,21 series and IIRC the O series when #3006 is set to 1 the screen will change to the message screen, display the message in parentheses and stop the cycle.

I am just now getting to set up the TLM data in the 15M Model A, and the 16M Model B (now that it's basically all set up). I've just been following along in the manual(s). I'm just now starting to quantify data on where my tools are wearing, although I've been getting pretty good life out of them.

I would like to do this for the 18iM Model A too. Don't need the operator message.

I've never seen TLM set up on a 10T so I'm not sure how it would work on the lathe, and my lathe works pretty much like any early Mori Seiki SL type lathe.

If it works out ok, I'll integrate it into the 0M.