Newbie- OSP-U10L tool offset confusion

[brokenrinker]

I've got an E series Lathe with OSP-U10L control. Here's the senario; There are two tools in the carousel. With tool #1 loaded and the tool data set showing 0.000 offset for tool #1 in both axis I touch off / take a cut, measure the diameter and use the "CAL" function to adjust the zero offset.

I load tool #2, touch off the same diameter and use the "CAL" function to set the offset value for tool #2 in the data table. I use the same routine for the Z axis.

So far so good. I can change back and forth between tools one and two and using MDI I can manuever to the same diameter and part face with either tool.

However - when I press the manual button to jog the axis with tool #2 loaded the readout changes. The value changes to the part diameter + the tool offset value entered in the data table. For instance if I'm touching off on a .906 diameter part I press the manual button and the readout changes to 1.6209 which is the part diameter plus the value in the data table for tool #2 (.7149)

I know this something stupid I'm doing. Any suggestions?

[Algirdas]

I press the manual button to jog the axis

manual mode for this control takes "zerro" tool offset always. You can use it for virtual zerro tool (good to set coordinate axis zerro offset).
if You want to use real tool offsets for this control; Okuma provides "mid auto manual" function for that. It's a special button in the same grey button row with framed "return" button

[brokenrinker]

Thanks for the tips. If I use the mid auto manual button as you suggested I can jog the machine without losing the #2 tool offset. But if I try to go back to MDI or Auto mode I have to push the Reset button which causes the machine to drop the tool offset and I can't get it back without doing another tool change. Is this the way it's suppose to work? It seems like I'm missing something.

[Algirdas]

I have to push the Reset button which causes the machine to drop the tool offset and I can't get it back without doing another tool change

1. You can always use tool change with positioning "nowhere". Suppose, you have situation T020000 then, after command:
G91 G00 X0 Z0 T020202
G90
You have changing of present coordinates concerning the commanded tools offset. G91 means relative coordinate - zerro is where we are now. Take care, hold rapid feederate override on minimum and look at distance remaining - in some conditions turret may move, distance depending on the tool offset. Generally, if settings ar correct, turret will not move- exactly as commanded.
2. You don't need to reset. You have dangerous function - MID auto manual return - specially framed button. Use it with care. turret moves to initial position in closest way.

[brokenrinker]

Thanks very much for helping out. I really appreciate it.

As soon as I can I'm going to try what you've suggested.

Another dumb question. Should the turret move (in X or Z) when I execute a T0202 or other tool change? Mine doesn't.

[Algirdas]

Should the turret move (in X or Z) when I execute a T0202 or other tool change?

command "T" must be prepared by moving to index position or by command M66 (indexing turret anywhere)
Normally it looks as:
G00 X700 Z700 T0200 [active tool is T02]
G00 (X Z approach point) T0303 [go to approach point with tool T03 with zerro offset #03]
turret moves to positive software limit. which is also possible to change via variables or by setting parameters, if You want turret to move shorter way saving time and wasting guideways.

[brokenrinker]

OK - I guess what I'm asking is - does the turret move in order to respond to cutter compensation. In other words if the difference in length between tools one and two is plus one inch (two being longer) does the turret move away one inch when I do a T0202?

[Algirdas]

neither turret (axis) moves, nor indication of coordinate of axis will change.
You need to command go by distance "X0 Z0" to see coordinate change after tool offset reading.
G90 G00 X0 Z0
G91
use for axis coordinate indication cahnge. Turret nor axis doesn't moves.
That means, You have wrong display of coordinates if You execute tool change comand without commanding axis movement.

[brokenrinker]

neither turret (axis) moves, nor indication of coordinate of axis will change. You need to command go by distance "X0 Z0" to see coordinate change after tool offset reading.

That is especially helpful. I know it must seem obvious to a veteran but when you're trying to learn your way around it seems counterintuitive that the position display doesn't change nor does the machine move when you do a tool change.
Many Thanks.

[Algirdas]

yes, japanese philosophy and way of thinking is quite different. You must always look at distance remaining when testing the part program. Chuck barrier is also simple and very helpful feature of Okuma.