Tool Life Management

[rogkick]

Hi Guys,

 

I want to make a machining process on a HMC use tool measurement between certain operations, and swap to a new tool if it is broken.

It is on a FANUC 15M control, and was thinking that I could put something in Mastercam manual entry etc.

Does anyone have any background on this, and could start me off in the right direction? Would be great.

[Guest]

You'll need do a few things on the Mastercam side; add in the tool breakage cycle to the end of the tool, all the tools you intend on using TLM on have to have H and D be 99 (ex. H99, D99), then your tool numbers will need to be changed as well.

 

You'll need to start thinking of tools in terms of groups rather than single tools. Granted, you may not always have multiple tools in the group, but you could and really, it makes more sense to do it this way. So, you have say 3 tools in your job. A .500" Flat EM, a .375" Flat EM, and a .250 Flat EM. Old method would be T1, T2, T3 respectively. NOw, you'll have T1001, T1002, and T1003 respectively. T1001 is Group 1 and it contains T1, T11, and T22 (all 3 are .500" Flat EM's with similar stick out values), T1002 is Group 2 and it contains T2 and T12 (both tools are .375" Flat EM's), T1003 is Group 3 and it contains T3, T13, T23, T33 and T43). Now that we've laid out our tools and their groups, you have to set their life. You set this up with either counts or time. WHen each tool expires it will automatically expire the old one and move to the new one. WHn you are setting your tools, T1 will use offset 1, T2, Offset 2, T3 uses offset 3, etc.... When you call T1001 and H99 and D99, it will automatically use the proper offset for the tol in the spindle.

 

HTH

[rogkick]

James,

Cheers for the reply.

The machine has the Management option in the control, and is available on the second LCD monitor. I can assign groups etc, but the problem is that it cycles through the tool group based on parts made or minutes in cut.

Is there a method/macro to allow code to check the tool, if it is broken, then cycle to the next tool?

[Oscar R.]

James,

Cheers for the reply.

The machine has the Management option in the control, and is available on the second LCD monitor. I can assign groups etc, but the problem is that it cycles through the tool group based on parts made or minutes in cut.

Is there a method/macro to allow code to check the tool, if it is broken, then cycle to the next tool?

 

I think you're OP title might have better been put as Broken Tool Detection, or or something of that sort, It seems like that's what you're looking for. What James explained is true tool life management, where you know to what extent you want to use your cutters before swapping them out.

What it looks like you want is a broken tool detection system( you may already have one, not sure) and a tool change out macro.

This is usually a macro that works between your control and your broken tool detection system, like a Renishaw laser or touch probe. You'll have to use what ever macro is specific to you system.

[Guest]

Apologies for mis-reading the question. Like Oscar said, when a tool swaps out due to a broke condition, that is a result of the breakage cycle flagging the tool. In most machines what happens is in the TBD cycle, if a broken condition is sensed (usually #148=1), then within the software either a Data bit, or parameter is changed whiel that tool is in the spindle. Once it is removed from the spindle, the condition is reset for the next tool and operation continues as normal. NOw, I've set up things like when a broken tool is enountered, not only will the tool flag and then next available tool in the group is selected, but I'll eject the tpallet abnormally then maachining continues normally on the outboard waiting pallet.

 

Basically it's going ot come down to how your Renishaw SOftware is setup to flag the tool as broken to TLM. You may have to do some digging in there. That code does not go into Mastercam just the TBD cycle.

 

Hope That Helps.

[rogkick]

No worries, I was probably trying to explain two things at once, hence the vagueness. Yeah, well, I think we will look at BLUM and see what they have to offer, until then we will use groups and amount of time in cut to swap out.

Thanks again.

James, I might connect with you on LinkedIn...if you notice a strange connection appearing...it is me.

oh I cant...need your email

[Rotary Ninja]

The way my old boss handled this was with custom macros. The Haas also has a tool load monitor which he tied into the macro to automatically change out the tool if it reached a certain load. But it did have a touch-off after every roughing tool to check for breakage also. I could ask him if he still has this macro and see if he will share it if you want. It's way over my head but maybe you could make sense of it.

[rogkick]

Rotary Ninja, that would be great, I would love a look at it, if possible

[RayD]

Talk to your reseller about Productivity+, its a software that runs inside of Mastercam where you can add Probe cycles inside of Mastercam, and manage them with your operations manager.

 

You can of course do this manually in your NC editor or with Manual Entry, but P+ streamlines the functions

 

http://mastercam.com/Products/Productivity/Default.aspx

[?Mark]

Hi James,

Can we turn this option on and off in parameters as needed? According to our AE person only fanuc can do that. Would like that confirmed if possible.

 

Thanks!

[Guest]

"This Option" is a hair vague.

 

Do you mean turning Tool Life Management on and off? If so, you can use it or not, T1xx H99/D99 is what effectively turns it on or off. If you call a tool normally T1 H1/D1, then the time/count does not get added to the tool's life.

 

Or do you mean Tool Breakage Option? If so, you can not call a broken tool cycle and essentially you have turned it off.

 

Please clarify so I can give you the correct answer.

[?Mark]

I'd like to be able to turn "Tool Breakage Option" OFF so I can use matching tool and offset numbers. It's still a new machine for us and I got "burned" last night when trying to use T99 with H99 and D99. Got around it by using different D and H numbers.

Ideally, I'd like to be able to turn it on and off as needed.

Thanks!

[Guest MTB Technical Services]

Take a good look at the Fanuc data sheet included with the machine. It should be included the main electrical panel.

That shows every option included with the machine.

Anything that is an extra cost option that requires a service tech to enable in the field will also require a service tech to disable.

 

You don't want to turn off the option.

That approach indicates a fundamental misunderstanding of how the functions actually work.

 

It is the program itself that determines if you are actually using the option or not.

If you don't want to use it, modify the program so it uses standard tool number and offset calls and you're not using tool life management.

Don't call a tool breakage detection cycle in your code and there's no issue.

 

You are making it harder than it has to be.

[Guest]

@ Mark, if you press the Offset/Setting button, scroll right using the Right Arrow Softkey (membrane buttons below the CNC Screen). If you don't see TOOL LF (or something similar), then you don't have the option and this discussion is relatively pointless.

 

Like Tim said, your program dictates if you are using Tool Life Management or not. If you don't understand TLM then you're not alone. 90% of people that have it don't use it. Some by choice, others bacause they have not had it explained to them properly.

[?Mark]

@James

We do have this option and it's on.

I get S0154 alarm (Not using tool in life group). Apparently the Tool Management on this Okuma is turned on by using H99 and D99. I happened to use tool T99 and with that H99 and D99.

It's a new machine and apparently they failed to tell us details like that.

According to our ME:

"The 99 designation is what commands the tool group selection

I do not believe it can be used as long as the tool life option is installed on the machine "

 

Kind of awkward...use matching tool and offset #'s except for #99.

 

How do I adjust a program to avoid this? Right now I have a tool T99 using H199 and D199 offsets. Is it the only way?

 

And no, I don't want to uninstall this option. I thought there might be a simple parameter switch to disable/enable it as needed.

 

Thanks!

[Elmer Fudd]

My method is "don't use T99".

[Guest]

#13265 and #13266 are the parameters that dictate what offset is used for Tool Life Management (on the 30i series controls).

 

I think that alarm you are getting is because you are not using TLM correctly. In my experience, you get that alarm one of two ways; 1) You've gone and used H99/D99 (Cardinal sin on FANUC machines) or 2) You've called a Tool Group without using H99/D99.

 

HTH

[?Mark]

Thanks James!

One would hope for Fanuc to have an option to be able to specify any offset number, lol. Like a number that is higher than a number of pots

We have 125 tools in there and all pots are already filled.

 

Thanks again.

<cheers>

[Guest]

You can (on certain controls) set that number as high as the number of offsets your options allow. I'm working on a MAM72-63V this week and I set it to 999 so they can use T99.

 

[djstedman]

From the Fanuc 0i-model D manual

 

This is on the newer Fanuc's but its worth taking a look in your manuals..

 

(works better when I attach the image lol)