okuma next tool cal cancel

[one shot]

Hello everyone.

Does anyone know how to cancel the next tool call on an okuma w/5000 control? Right now I must go to manual and hit the reset button to clear the next tool called up. I was wondering if anyone has found a way to do this with code.

[elbro]

Change this in your post to a 0

 

stagetool : 1 #0 = Do not pre-stage tools, 1 = Stage tools

[jeff]

one shot,

I don't think there is a way to do it.

It's a problem with Okumas,the tool staging should be able to be reset by hitting the reset button.

[one shot]

I've been trying to find a way around that for years. It's no big problem. Just looking to see if anyone has found a way around it. Been hitting that reset button for over 20 years now and am tired of it.

Thanks for the input.

[jeff]

Does that control have a return cycle start button?

That will "unstage" the tool.

As much as I love the Okuma controls, this is something so simple that really gets me mad and I wish they would fix it!!!!

[one shot]

Yes it has a return cycle start, but you can't activate via code. I use a sub to do all my tool chg and want to cancel next tool call at end of prog to leave mach open for mdi input on next setup.

[jeff]

Just out of curiousity,why do you use a sub for tool changes?

And what does it look like?

[Fig sign]

do not use staging .

Also if your controller not supports the tool change skipping like Okuma i used ,

you can add to the program (and postproccessor ) condition check like I did :

Something like

If[VATOL]Not equal ....(do not remember proper format for Okuma parametric ,it was 7 years ago )

[one shot]

I use a sub to save code lines and do all my error checking ( if vatool...)also it set my rpm and call my next tool. It saves me about 7 lines of code per tool. I'll send it to ya if ya want.

[chris m]

If you want to have it '0' all of the time you can try this: VNTOL = 0 in the program [or in MDI] and see if that gives you the result you want. I think you could also try M63 but I believe you'll get 'Wrong T Command' at the next tool change with that

 

C

[jeff]

Good point Iskander.

Yes you may be able to write a variable to help you.

I forgot about those.

OR you could just use a tool change like this:

T2M6

Like Iskander said, do not stage tools.

The only downfall to that is waiting for the magazine to find the tool and that can take up valuable cycle time.

Maybe try calling Okuma themselves and ask them if you can set a variable.

If they say yes, I would love to know how it is written!

[jeff]

oneshot,

yes please send it.

Thx.

[one shot]

I'm trying variable set now. Can't wait for magazine to find tool. Have called Okuma rep in past with no results. There must ba a way.

M63 resulted in error.

[Fig sign]

All this stuff like 5 seconds gaining on every tool change have no sense when you making molds like I do mostly ,so I never use staging .

also if you use staging for T2 and call after the Vatol checking

T2M6 nothing wrong can happen ,this will add you safety ,if someone changes T2 for other tool .

I prefer to use subroutine for change only for positioning ,this I used a lot working with Very big Tsudikoma 4-th axis ,where a straight toolchange would sure crash it

Make a sub only for positioning point and leave

T2m6 call in main program ,you will always be able to see what happens

And it is safe

HTH

[jeff]

Iskander, I have changed all my Fanucs to do this every time they read an M06.

When M06 is called, it goes to a certain position.

No sub needed.

But I'm sure you already know how to do that lol.

 

Iskander teh smart.

[Fig sign]

Actually my M6 is a parametric subroutine

in Sinumeric ,as in any other controller .

So I know how to do it .

But I do not use it .

I have a special subroutine CHANGE ,HOME ,END,

AND MANY OTHERS FOR SPECIFIC THINGS .

I make some parametric subs too when I start to use any new machine

I always call a sub for anything it can save me typing and my work with MDI is like foreign language like this

 

Ho55

kv24

kv5

home

start

[jeff]

oneshot,

Got you email,thanks.

So, by writing this as a .SSB, can ANY .MIN program call this up?

That's a pretty neat way of doing it.

[one shot]

Yes, and I leave it in loaded in memory and every prog uses it. All code generated via MC also use it. I had the post altered to make the sub call

[jeff]

I knew there had to be a way to do that!

Up until just now, I have been putting all subs at the end of my main program.

This helps me out tremendously!

Thanks for sharing!!!

[jeff]

Oneshot,

I did a little experiment on our Okuma,try an M64.

That clears the Next tool staging.

If you put it on the same line as the T call,it will wait until the magazine has rotated to that tool,maybe there is a spot after the T call you can insert it.

HTH

[one shot]

It did what I wanted. I will now include this at the end of all my progs.

Thanks

[jeff]

No problem,

I'm just glad that I could finally lend some advice for a change.

[chris m]

That's a good one, Jeff, thanks for the digging; I'll add that to my bag of tricks

 

C

[one shot]

One downfall. Must have one empty pod in the magazine, of error occurs

[jimspac]

I was only running into that on 2D programs,not3D.I was editing the tool stage call out for awhile then edited the post processor to not prestage tools, now no more editing. This is on a 5000M control.