OKUMA MAX TOOL LENGTH

[SKIR68]

We have an Okuma LB300 EX Space Turn with OSP-2000l control. I know the max tool length for live tooling in the vertical position is 4.5" (don't ask HOW I know).

My question is this, Is there a parameter or variable to set so i can have the machine alarm out if i touch the tool off and the offset is >4.5" ??

 

 

Thanks in advance!

 

 

[Greg Williams]

LOL Let me guess how you know this.

 

Do you want the check code to come out of the post or use the machine G/M codes?

 

This will work for Tool 1. But you really need to check this when the tool is measured. Do you have an auto touch setter

 

G00 X800 Z300 T010101

IF [VETFX GT 4.5]NER01

GOTO N100

 

NER01

VUACM[1]='TOOL TOO LONG'

VDOUT[992]=1001

 

N100

M02

 

 

[SKIR68]

Thanks Greg! Yes!, I want to check this EVERY TIME a tool is measured! I have a request in for Okuma to add Macro programming to this control. I have it on our Multus but now our LB3000.

 

 

[Greg Williams]

Do you mean user task 2?

[SKIR68]

nope, we have a software upgrade comming that will allow us to use Macro programming on the lathe side. It seems Mill has had this option for some time, its just making its way over to the Lathe side at Okuma!

[chris m]

?? we have user task macros in [20] year old OSP lathe controls ??

[YoDoug®]

They are getting G/M code macro functionality for their lathe.

[SKIR68]

Thanks Doug!

 

BTW....NICE YO-YO's !!!

 

 

[chris m]

How is a G or M code macro going to have any effect; do you have automatic touch setter gaging?

[Greg Williams]

I agree with Chris.

 

Custom G and M code will work if you have an auto touch setter, If you want to add this to a manual touch setter you will need to rewrite the MSB file. and also change the machine software to use the custom G/M code.

[SKIR68]

We do indeed have a touch setter in the machine, its brand new! Don't you guys see the advantages of being able to write your own custom macro's???

 

 

[chris m]

I have never needed a G or M code macro in the lathe, to be honest; we have many user task operations running in our programs and some of them could probably be incorporated into a G or M code macro, but I never really thought about it. We have manual touch-setters, so this wouldn't help us combat the issue you face, but with an auto touch setter it's nice to have the added functionality of "IF VTOFX[01]GT 4.50 NALM1" written into the program. That being said, you must call a sub or something for the machine to touch the tool off; why not just write the IF statement into the sub?

[SKIR68]

We use ALOT of custom Macro programs in our lathes and Millturns. Everything from sending the machine to "home" position to custom drilling and milling cycles, probing cycles and even boring jaws and collets!

im also trying to keep everything the same across many machines. I need the same operator to run several different machines. I need "G205" (machine Home and clears out tool changer) to be the same on all machines.

 

 

 

 

[Greg Williams]

I believe that yiou will need an AUTO touch setter, That is one that comes in and out at the touch of the button on the panel to use the custom G/M code. I do not think that this will work on standard machine software with the manual touch setter

[chris m]

Totally agree with you, Greg; this is the point I have been trying to get across. If you have the manual touch setter you could possibly buy custom software from Okuma that would interrogate the TOFS register after the machine touches the tool off to generate an alarm, but I don't see how G/M code macros are going to help here.

 

C

[SKIR68]

yep, thats why we have those little buttons on the screen called "ARM ADVANCE" and "ARM RETRACT"

 

They work very nice thank you!

 

 

[chris m]

I have never actually seen a machine with that option; how does it work? Do you use it during program operation for tool breakage detection? Do you have a "touch off tools" program? If so, how does the machine know where the tool is to touch it off? Do your guys not touch off manually? Even if they don't, when they're loading tools in the machine they could still clean the sheetmetal out with an overly long tool before the machine "knows" how long the tool is. Could you preset instead? The tool crib guy would then know if the tool was too long before it ever got to the machine, but you'd need quick-change live tools for that.

 

C

[Charlie Pierson]

Not so sure how to do it on an OSP, but on Fanucs and Yasnaks we interrogate our tool length offsets at the beginning of each program be it Mill or Lathe.

 

seems to me that you want to detect a long tool before you index the turret.

 

in a nutshell:

 

begin loop.

 

Start w/ the system variable to tool 1's offset

compare it to the max length

if less or equal, continue

if more, trip alarm

update loop counter variable +1

back to top of loop, this time it will look at tool 2's offset..

 

etc.

 

We do this to look for decimal place typo's. (operators key in the values from the presetters.)

 

Same idea can be used to determing a safe index position for a lathe/millturn.

This time use the loop to determine the longest tool, add a half inch (or so) to that,

convert to machine coordinates, store that value in a common variable, then G00Z(variable) for safe index.

 

Applications for macro programming are endless IMHO

 

cp