[fomaz]

This should be a simple question.
I need to move the machine (lathe) in machine coordinates so that I can change the tool safely.
I would prefer to move the machine away from the work piece in both X++ Z++ direction and then change the tool (in fact I can only change tool if the turret is in top most position on X axis).
How this is managed in a Okuma lathe? The controller is U100L
Thank you

[Algirdas]

no mess with machine coordinates in Okuma at all.
just a command G00 X1000 Z1000 and the turret will stop at X positive and Z positive (operator defined) software limt. It is the location for safe turret indexing.
One limit could be enough for tool change - depends on machine specificatin and parameter choice

[fomaz]

So you suggest to send the machine in such a way that it will hit the soft limits, so would be indifferent to call G00 X9999 Z9999 and so on...
I started to do that, but it does not seem a correct/elegant way to do it.
Thank you very much.

[iMillJoe]

So you suggest to send the machine in such a way that it will hit the soft limits, so would be indifferent to call G00 X9999 Z9999 and so on...
I started to do that, but it does not seem a correct/elegant way to do it.
Thank you very much.

I know it's not very elegant, but just issuing a G00 to a number more than large enough to hit the soft-stop is the way its done on an Okuma lathe. I don't use such a large number, G00 X50 Z50, works in all our machines, not sure if your's requires a decimal in the X and Z addresses though.

[broby]

Yep, to get an Okuma Lathe to execute a tool change it needs to be up against the soft limit (user defined).
It is up to the operator to set where this limit is in the machine. Obviously, if you set it too close to the part/chuck where a tool may hit on the way past, then you are a fool.
I have seen operators set their limits 20mm away from the end of the job (only using 2 tools) and the cycle is very quick) but then are shocked when the turret failed to pickup the tool position correctly (it was a known problem at the time on this machine) and indexed past the required tool and smashed a boring bar into the chuck, not pretty.
On an Okuma, you can specify a rapid move to any point, inside or outside the available working area without problems, if the position is outside, then the machine will move towards the specified point and stop at the defined limits for any axis being moved.
If you try and FEED, either G1, G2 or G3 past a limit you will get an alarm.
You CAN specify M66 (Turrent Indexing Position Free) so that the machine will index without being up against the soft limit, but unless you know what you are doing, can be rather dangerous.
You do not need to use decimal points when using G00 X400 Z800 (Metric)
Cheers
Brian.

[neilw20]

In an earlier model I remember I always moved to the soft limits.
I had to be careful because I had an overlength boring bar. Soft limits was the way I did it.

[broby]

In an earlier model I remember I always moved to the soft limits.
I had to be careful because I had an overlength boring bar. Soft limits was the way I did it.

I must admit that I NEVER moved my Hard Limits, Only ever controlled the tool change position by way of the Soft Limits.
Boring bars can ruin your day if you forget about them when indexing!

[neilw20]

Turret index codes are very useful when there is a big boring bar in the turret. The codes are since erased from my carbon based memory.

[fomaz]

You CAN specify M66 (Turrent Indexing Position Free) so that the machine will index without being up against the soft limit, but unless you know what you are doing, can be rather dangerous.
You do not need to use decimal points when using G00 X400 Z800 (Metric)
Cheers
Brian.

I must try that one (M66). In my case all tools have the same length in respect to the turret, so no collisions will occur and the cycle will be much faster.
Thank you

[fordav11]

bear in mind M66 is an option of Cycle Time Reduction Function. If it doesn't work you don't have the option.
The M66 goes on the same line as the T

[broby]

Also, if you do you M66 to remove the "Tool Change at Home only" requirement, make sure you follow up with M65 and a repeat of the same tool number on the next line.
The M65 and Tool number repeat will force the machine to confirm the required tool is clamped and in place BEFORE trying to use it.
If your machine moves faster than your tool change, you could end up moving on in the program before your tool is in position, just image the mess you could end up it you have the machine still indexing whilst trying to machine!
As fordav11 states, this all dependent on having the optional cycle time reduction feature on your machine.

[neilw20]

Go by what the manual says. It will have been well written and tested.
Using internal commands can have expensive consequences because of side effects.

[fordav11]

eh? Okuma manuals well written and tested? You must be from another planet.
But it's good to know there are beings from other planets out there reading these forums and interested in CNC programming ;-)

If you check Okuma manuals from series to series most of it is duplicated and identical. some of it is just plain wrong.
For example in User Task II checking signals on OSP5000 was done with VIRD. On OSP-7000 they changed it to VORD. A really stupid change that should have remained the same (VIRD or VORD who gives a f**k) but in real life it doesn't work if you use the wrong one. The OSP-7000 manual states VIRD with several examples. I found out later it is a straight copy from the OSP-5000 manual. I had to contact an Okuma Applications Engineer to get the info and even then he had to research it to find out the right format and usage.

[neilw20]

Sorry. I Was from earlier times when there was just enough in the manual. OSP300 was it?
So short on examples, you had to READ it all to even make sense of it. Many of those engineers are pushing daisies now.

[Algirdas]

and the cycle will be much faster

You can set software LS closer to chuck if all tools are almost the same <- that makes point. Sure it is a lot of adjustment to change tool faster when turret is moving G00 and indexing simultaneously. Suppose, M66 will not give any advantage.

[fordav11]

The software limits can also be set at the top of a program via Okuma System Variables. i.e. VNVLZ = 123.456
So in this case you can set the limits specifically to suit each program and tool set-up you are using and it will never be wrong :-)