[Bill Johns]

Years ago I spent 2 days on an okuma control, and had asked one simple question and got some bs for it. On Fanuc's, Haas, Mazak, Yasnak etc.
If you desire to manually run it or just simple indicating and dialing off a dimension, you can ZERO or ORIGIN the read out to say 000.0000
for all axis's.
I asked the guy showing me how do you zero the read out, and he said you don't need to know that now. Why couldn't he just answer my question?
I could not see a way to zero it. Is there? This is my only gripe with an Okuma control well I guess there would be others since I hear they don't use the good old G54 on up for work offsets??????????????
They should its very stupid not to follow the norm in the CNC control world.

[Superman]

Very, very simple

The Okuma's can have multiple co-ordinate systems
Caution, if using G54 or G92 and the co-ord system is not returned back to H0 ------PROBLEMS----- this is why the instructor held back

They are accessed and set thru the Work Zero page, basic machines can have up to 20, options allow even more (300+)

"Machine Zero" co-ordinate is non adjustable ( for VMC it is usually the table centre )

To set machine zero active, MDI--> [G15 H0], <Write>(this puts it into the buffer), <Cycle Start>(this executes that block of code in the buffer)

G15 is the code to change co-ord systems
Hxx , the xx is the co-ord you want to change to. These codes must be in the same block
It allows you to adjust the work zero without having to edit the program, the Hxx is a point that is defined on the work zero page.

An indicator (-->) on the Work Zero page shows which co-ord is active and is also shown on the prog.run pages ( Auto, etc pages )

if you want #3 co-ord active
MDI--> G15 H3 <Write> <Cycle Start>


To set the current X and Y as zero ( Calc and Set are F-keys )
Work Zero page, bring cursor to the X position of #3 line and Calc 0(zero), do the same to Y, you position is now 0,0 .Now put your cursor on #3X and type Set -10 <write> , that value is placed where the cursor is, and your current position is X10, try using Calc 10 <write>, this makes the current position as X10.
Always be aware what you are changing--double check the cursor position and value before <write> and check again that it is approx what you expected ..... ( there is no undo, get into a habit of recording numbers )

Caution.....Calculate Zzero is not the way to set it to run a part program, but can be used for checking height differences when using a dial indicator ( it does not utilise the length of the tool in the spindle )

REMEMBER To return back to the original co-ord system

link to a sample

More in-depth info is in the Programming and Operation manuals----look up co-ord system or G15 setting

[broby]

OR... as per usual on an Okuma there is many ways of skinning the cat as they say...
From any of the Manual, MDI or Auto modes, display the position screen (the one where the position readout is in large numbers).
One of the function keys will (or should, use the Next button to change options) will allow you to Set/Pre-Set the Relative position of any or all of the Axis's to any value you want.
This position is TEMPORARY and does not interfere with the Zero Set position of the current selected co-ordinate system.
Great for use when setting up, and checking sizes with a dial gauge like you stated.
As for G54 etc... Okuma uses G15 Hxxx where xxx is a number between 1 and what ever limit is set on your machine (50 on one of my machines and 200 on the other).
This system works very well once you are used to it.
Does that clarify something for you?

[Bill Johns]

Well thats cool if it has a zero set button. Similar to Fanucs origin button????
I guess it has its deals to learn kinda like Mazak. Is it similar to Fanuc when reset, ie doesn't rewind the program to beginning? Is that a parameter deal? How about a restart would be nice if all machines did the Haas restart.

[broby]

Well thats cool if it has a zero set button. Similar to Fanucs origin button????
I guess it has its deals to learn kinda like Mazak. Is it similar to Fanuc when reset, ie doesn't rewind the program to beginning? Is that a parameter deal? How about a restart would be nice if all machines did the Haas restart.

Hmm, considering I have never used a HAAS machine, let alone restart on a Haas machine, I can not offer an opinion on doing that restart. I do know that the restart on the Okuma's is pretty darn straight forward tho!
Pressing "Reset" on an Okuma will reset the program to the start every time.
Bit of a bugger if you are at a program stop and you forget etc...

[Bill Johns]

Hmm, considering I have never used a HAAS machine, let alone restart on a Haas machine, I can not offer an opinion on doing that restart. I do know that the restart on the Okuma's is pretty darn straight forward tho!
Pressing "Reset" on an Okuma will reset the program to the start every time.
Bit of a bugger if you are at a program stop and you forget etc...

All CNC's will reset.
Haas restart will start at anyplace in the program. Really cool deal. If you have a problem you can number the lines and watch the graphics, and figure out where you want to jump in at. Most preferably at a Z retract point, but doesn't have to be. Then you restart to that point, the control reads the program real fast just like it had done previous, it does that to load any prep codes etc. then it may make a few spooky moves and into the cut where you wanted to start. So does Okuma do that?
Also on Haas when you reset you can set weather you want the program to go to the begining or just stay at are you reset, kinda like a Fanuc. What does Okuma do?

[broby]

All CNC's will reset.
Haas restart will start at anyplace in the program. Really cool deal. If you have a problem you can number the lines and watch the graphics, and figure out where you want to jump in at. Most preferably at a Z retract point, but doesn't have to be. Then you restart to that point, the control reads the program real fast just like it had done previous, it does that to load any prep codes etc. then it may make a few spooky moves and into the cut where you wanted to start. So does Okuma do that?
Also on Haas when you reset you can set weather you want the program to go to the begining or just stay at are you reset, kinda like a Fanuc. What does Okuma do?

Okuma resest is a hard reset. Press the button and the machine stops, much like an emergency stop but more gentle. Program will reset to the start.
You can use the cursor to scroll down through the program and then press restart and the machine will restart from that point, BUT, it will not re-establish any pre-existing conditions or variables etc... the Sequence Restart function is pretty quick, but does depend on the complexity of the program. Using full sequence Restart will establish all pre-existing conditions and any variables in use.
I use a statement like the following to help reduce restart problems:
IF [VRSTT EQ 128] Nxxxx
The system variable VRSTT is assigned the value 128 when the Restart Mode is selected. When the RESTART button is pressed it changes value back to 0 (Zero).