[rotec]

For years I've wanted to set a safe distance for the LS30 lathe to perform its tool changes on both front and rear turrets. The LB15 we have is great in that the tool turret wont index unless its against a limit on either Z or X.

Can I get the LS30-N to do this also? We have had one too many tool crashes and one edit mistake and the tool will index even when inside a job, ouch!

If any one knows how to set this parameter please let me know.

Thanks.

[DSIF]

Your LB-15 will do a tool change wherever you want it to,unless Okuma has changed their software since I last ran one. Are your programs in Z-,or Z+? Just curious. In my opinion,Z0.0 is always the face of the part.

[littlerob]

Your LB-15 will do a tool change wherever you want it to,unless Okuma has changed their software since I last ran one. Are your programs in Z-,or Z+? Just curious. In my opinion,Z0.0 is always the face of the part.

WHAT??? No it will not, if it is running it will NOT do a toolchange unless the turret is up against one of the stops. You can change the parameters to move the limits, but it will not index unless it is against the soft switches. Not from 2200 to P200.

[rotec]

The LB15 we have definatley will not change tools unless its against a soft limit in either X or Z. I'm not saying this cant be removed. But thats how our is. I personally like this feature and so this thread is actualy about me trying to find out how to get the LS30-N we have to do the same.

At the moment our Okuma LS30-N with tool change any where which I dont like, especialy on a twin turret machine with long drills hanging out every where!

Im hoping there is a parameter somwhere to set this?

[cncserveng]

As a former service tech for Okuma in CA, I find this question strange because I thought the OSP5020 control setting pages allow you to set the turret tool change X-Z positions.

Please check if this page exists and set the change position to suit the longest tool to prevent collisions.

[underthetire]

5000L and newer must be at a soft limit on slant bed lathes, and small lathes (LC10, LB9 ETC) x or z or both.

The flatbed lathes were different, because they were slower and usually way too long of beds.
Limit was adjustable (user limit) to help shorten cycle time if you wanted. Variables can also be used for each tool to change the user limit if you really wanted to. The old 2000, 2200, and 3000 may not do that. It's been too long since i touched the older controls, so IDK.

[DSIF]

It's in the "user parameter" page. Z axis and X axis stroke limits. Move a safe distance away with your longest tool and put that value in. Enter that value or greater in your program-(it wont over travel),and do your tool change. The OSP 5000 and 5020 will both do it. In contrast,you can also set your turning tool to where it will not hit the chuck(a chuck barrier if you will).The Okuma controls have many "bells and whistles" like this.

[rotec]

I know about stroke limits and chuck barriers etc, but this is not what I'm after. What I need to is set a Z and X value that will see neither turret index near the chuck. In not concerned about crashing tools but to hear the machine index 3mm from the chuck is gut wrenching!
Just last week a worker missed a tool change edit and the he stuck a 2" drill into the chuck. It bent the H turret spindle and I’ve worked half the week to fix it.
So thus I'm looking for a way to set a safe tool index position say X300 Z250 for both turrets.
I don’t wont to set any tool barriers.

Attached is the control its mono tone OSP 5000 year 1982-08

[broby]

Sorry Rotec, I am not sure which parameters to alter to get what you want...
But...

Have NONE of you used or heard of cycle time reduction coding?

I can get the turret to index away from it's set home position very easily.
Using M65 and M66
With out the manual to hand, I may have the code explanations flipped but basically one is Turret Free Indexing (M65 I think) and Ignore Turret tool in-Position command (M66)

Basically what you can do is tell the machine to index whilst on the move using these codes. Can be a bit interesting if you fail to take into account longer tools and the amount of time it takes the machine to index between stations!
The way I use these codes is:

Machining Program... with tool T010101
N100 G0 Z800 (move at rapid to z Home position)
N102 X(next diameter require) Z800 T020202 M65 M66 (Machine will now index the tool to Tool 2 while moving to the Next X axis position stated while keeping up against the Z axis home posn).
N104 X(same value as on line N102) Z(reference position) T020202 (NOTE! REPEAT the tool number here!)
Machining program for tool 2.
...

an example program using values might look like the following (simplified lots):
N100 G0 X400 Z800
N102 G97 S500 M3 M8
N104 X100 Z102 T010101
N106 G1 Z100 F0.2
N108 X0 (FACE PART)
N110 G0 Z800
N112 X102 Z800 T020202 M65 M66
N114 X102 Z102 T020202
N116 G85 N118 D5 F0.3 U0.5 W0.1
N118 G81
N120 G0 X20
N122 G1 Z100
N124 X100 Z50 (MACHINE A TAPER FOR EXAMPLE)
N200 G80
N202 G0 Z800
N204 X20 Z800 T030303 M65 M66
N206 X20 Z102 T030303
N208 G87 N118
N210 G0 X400 Z800 M5 M9
N212 M2

In the above example, the machine will index the turret to the next tool whilst moving along X axis and keeping the turret at Z home.
The reason for putting the same Tool number on the next line is so that the machine will confirm the required tool is actually in position BEFORE moving to the nominated posn.
If you do not do this and the turret is still indexing when the next X axis position is reached, the machine will then start moving towards the part... now THAT could be very exciting if a long tool was between tool positions programmed!

Another 2cents worth
Cheers
Brian.

[littlerob]

Can I get the LS30-N to do this also? We have had one too many tool crashes and one edit mistake and the tool will index even when inside a job, ouch!

If any one knows how to set this parameter please let me know.

Sorry, has the question for this machine been answered? I cannot speak from experience. I can only be a smart ass when it is called for. Oh I guess sometimes when it isn't called for also.

Robert

[underthetire]

Again, the flatbed lathes didn't have to be at limit. They were just too big and slow, so Okuma didn't put the limit in the software.

[rotec]

Tool changes while the turret is in transit is the exact oppersite of what I'm after! hahaha.
Those codes in the hand of my dyslexic programers would lead to disaster

Looks like the flat bed machines cant have this feature. ie where a tool changes only occure at a set distance from the chuck.

I'm surprised that this cant be done.

Oh well. Thanks for listening.

[broby]

Tool changes while the turret is in transit is the exact oppersite of what I'm after! hahaha.
Those codes in the hand of my dyslexic programers would lead to disaster

Looks like the flat bed machines cant have this feature. ie where a tool changes only occure at a set distance from the chuck.

I'm surprised that this cant be done.

Oh well. Thanks for listening.

Yes well... I did realise that this was the case... But I was mainly trying to make a point that you can index a machine away from the limits using the appropriate codes!
I also agree with you that these codes, used in the wrong way could be a disaster in the making.
Good luck.
Brian.

[OkumaWiz]

Does your machine have User Task 2? If it does, there may be another way to make it happen using System variables.

You could check the VAPAZ to see IF it is > or = to Z123.4567 or whatever.
If yes, index, if not, Alarm. Zero offset could be taken into account as well.

Let us know.

Best regards,

[broby]

Does your machine have User Task 2? If it does, there may be another way to make it happen using System variables.

You could check the VAPAZ to see IF it is > or = to Z123.4567 or whatever.
If yes, index, if not, Alarm. Zero offset could be taken into account as well.

Let us know.

Best regards,

The problem with that would be that you need to call the macro before each and every tool change! Once again, operator error can creep in and really mess up your day!
The only solution that would work would involve a change in software on the machine that would command the machine to only perform a tool change when on a limit.

[OkumaWiz]

Yes, you will need a tool change "SUB". Everyone know that your chances of getting Okuma to get you new software for that control are as likely as taking a deep breath with your helmet off on the moon...

Even though it's not ideal, I think you could throw a parameter with the sub call to get the correct tool and always pull back away from the spindle by a fixed distance based on your Zero set and a distance of your choice.

Still better than indexing 3mm from the chuck. Yikes!

If you don't have User Task 2, A spec change from Okuma would be possible...

Best regards and happy "safer" indexing,