Okuma OSP-P300 question

[The Cathedral]

G20 HP=4

 

Does anybody know where to set the home positions that are used in the above line? We're working on a new post for our twin-saddle twin-spindle machines. We use the G20 HP=4 code on the MacTurns/ Multus to send the live spindle to the toolchange position. They were set by the manufacturer so I don't know where they are at. I would like to try using the G20 on our turret lathes, although I'm thinking it might only be usable for machines with an ATC.

 

Thanks for the help.

[The Cathedral]

Nevermind, found the answer: it only works with ATC machines. Thanks, Cathedral!

 

I'm welcome!

[Mr. M]

Glad you could help

[chris m]

Not sure what you are trying to do, but you can write to Positive and Negative Variable Limits in your programs. We do this all day, every day, to make sure the machines are in a safe index position before toolchanging.

 

If you wanted the machine to index in the same place all of the time, you could put the encoder values in common variables and then read those values into the Positive and Negative limits in the program.

 

For instance, we use V181 for X and V182 for Z to establish index position; in the Common Variables for [1] machine, V181=961.4179, V182=639.5625

In the program, we set VPVLX=V181 and VPVLZ=V182, so when you send the machine home (G00 X100. Z100. or whatever you use) it always goes to the same spot; if the operator changes it for some reason, the program writes over it and goes there anyway.

 

Not sure if this is what you are trying to do, but OSP controls can do damned near anything you want.

 

C

[The Cathedral]

It's more for the hopes of a common structure, so shifting programs around from one machine to another can be relatively painless. For our machines with ATC (Macturn/Multus) we use the G20 because that's the tool change position, for the turret lathes (LT's, LB's, LU's) we just send them to their "limits."

 

Calling G00 X20. Z32. is good enough for our LT's, but the LB's have a lot more travel than that!

 

Your idea is a good one, though, so I'm going to look into that further. Thanks!

[chris m]

You could write a .SSB or a G-code macro for each machine to go "home," then call that before toolchanges, so programs for all machines would be the same / similar