okuma tool registry bug

[mastercamguru]

okuma control doesn't know what tool is in spindle - if tool 1 is in spindle and "T1M6" is called machine alarms -- macro is needed to check tool registry for tool in spindle before tool change then jump past tool change line if sp T# equalls called T# WHY CAN'T OKUMA AVOID THIS BY HARDCODING THIS FUNCTOIN INTO THE MACHINE'S FIRMWARE ? If anyone has a beeter alernative to coding macro before each toolchange PLEASE LET ME KNOW!




THANX MASTERCAMGURU@COMCAST.NET

[theokumaguy]

A macro is the best way to do this really, and you can use the same unmodified macro for all your programs regardless of your starting tool. In your macro, use T=VC** (Use any common variable you'd like to dedicate to this), then before the macro call in your program, set that variable to the first tool (VC**=1). That's the most simple way to explain it. Unfortunately, I think it's gone so long without being fixed is there is a well-known, easy workaround for it. The good news is their lathe programmers have always had the code right, and it has made it's way into the Macturn/Multus platforms, so perhaps it will migrate into the mills soon too

[cadman]

Put this at each tool change. You'll need to number your sequences accordingly.


.
.
.
.
IF[VATOL EQ 2]N2
T2
M6
N2
M1
T3
(TOOL 2)
(.97" CARBIDE ENDMILL)
(OPERATION 3)
G0 G90 G15 H1 Xx.xxxx Yx.xxxx Sxxx M3
.
.
.
.

[theokumaguy]

Program branching is only allowed in A method. If you are in B method (large volume method), DNC-B (RS232 trickle feed), or DNC-DT (trickle feed from a hard drive in the machine) you have to use the macro method.

[cadman]

The IF statement above works in both A & B methods and does not violate any of the restrictions for either method. I use this in all of my Okuma posts on every tool change sequence.

[littlerob]

I agree with the mastercam guy, I have the utmost respect for okuma, I have run them all, Mori, Daewoo, Haas, Mazak, I am not bias to a mill or a lathe, and I think Okuma builds the best machines out there, that being said I think that the whole tool change situation on that mill is a little frustrating, too many steps to accomplish a simple task. just my opinion.

[broby]

Seems to me that this is user problem, NOT an Okuma "bug".
The mills do know what tool is in the spindle, otherwise why the alarm?
If YOU the programmer selects the incorrect tool then YOU are the one at fault, not the machine, or the software.
On the other hand, if the operator selects the wrong tool without knowing what it is that they are doing, then the machine is really only guilty of protecting itself.
If you are getting tool selection alarms during a program run I would be more concerned, but I really fail to see what your problem is. Maybe I have got the wrong end of the stick, but mayb not also.
Anyway, just my 2c worth.
Brian.

[skullworks]

okuma control doesn't know what tool is in spindle - if tool 1 is in spindle and "T1M6" is called machine alarms -- macro is needed to check tool registry for tool in spindle before tool change then jump past tool change line if sp T# equalls called T# WHY CAN'T OKUMA AVOID THIS BY HARDCODING THIS FUNCTOIN INTO THE MACHINE'S FIRMWARE ? If anyone has a beeter alernative to coding macro before each toolchange PLEASE LET ME KNOW!

THANX MASTERCAMGURU@COMCAST.NET

The alarm is perfectly valid. The Okuma KNOWS exactly which tool is in the spindle, you didn't ask that.

You have told the machine "T1 M6" and the machine checked the tool magazine and there is no T1 in the magazine. You gave it a tool CHANGE command.

I use a macro check like above but a bit more detailed.

DIREC V
ORIGIN Hxx
CYLNDR 2P,[0,0],[100,100],0,10
END
DRAW


...
N04 IF [ VATOL EQ 1 ] N10 (TESTS ACTIVE TOOL)
N05 IF [ VNTOL EQ 1 ] N09 (TESTS TOOL IN READY POT)
N06 IF [ VNTOL EQ 0 ] N08 (TEST FOR NO READY TOOL)
N07 M65 (RESET READY TOOL)
N08 T1
N09 M6
N10 G00 G15 Hxx M8
...

The macro does the job and acts as a safety net if the operator hits reset (such as a machine going into power save during lunch.) It makes sure the machine has the right tool at the program start.

( Oops, I didn't need to include the graphics plot header...)

(As M$ might say, "Its not a bug, It's a Feature.")

Now on the other hand, the Mazak lathes I use will do almost anything you tell them, like index the turret while in a bore if the programmer isn't smart enough to put the Txxxx in a safe location.

[littlerob]

Broby and Skullworks, you really dont think that this is maybe a little more complicated a tool change (mechanically and code wise) than it needs to be? I have had Hartwig tell me that nobody really complains about the tool change, but to me it seems over complicated, but I do alot of hand editing. Just wanted your opinions.

[skullworks]

Every Machine builder has choices to make on how they choose to implement a tool change cycle.

On the Okuma an M6 takes the spindle home to the tool change position (Vertical Mill). Same for Haas. Try that on many FANUC's without doing a G28 G91 Z0 first and you will get an alarm... Some might say THAT behavour is a bug/error. Its not - its just the way the tool builder chose to do it.

[littlerob]

I agree with that, but "tool change cycle" getting back to my first point why does it have to be a cycle? (yes I understand that all things need to accomplish specific steps before the goal is achieved) The Haas does not use a "cycle", it is just a tool change, let me say again I am less unimpressed by any machine tool manufacturer than Okuma but I think that tool changer sucks. I work with a lot of operators that make it more diffficult than it has to be (surprised?) but on a Haas when something goes wrong with the tool change, you push the button that says toolchange restore and it walks you through it, easy? Not so much with the toolchanger on those mills. I think. Every manufacturer does have decisions to make, and most of the reason i have stuck with Okuma is that they are so freindly, just this one gripe from me.

[broby]

If the machine has stopped mid tool change, use the ATC manual Advance/Reverse buttons on the operator panel to recover. Either that or use the ATC "Return to Cycle start" button. Works wonders here when things go potty.

Why, as a programmer, do you feel the need to check what tool is in the spindle?
YOU should already know what tool is there. You programmed it didn't you?
Surely you start off with no tool in the spindle, call up the first tool, Tool change, call up the second tool, and start machining. i.e.
T1
M6
T2
M3 S...
M8
G0 x.. y.. z..
etc...
Machine somthing... with Tool 1
M9
M5
G0 Z800
M6 (Get tool 2 into the spindle)
T3 (Pre-stage TOOL 3)
M3 S...
M8
G0 x.. y.. z..
etc...
Machine somthing... with tool 2
M9
M5
G0 Z800
M6 (Get tool 3 into the spindle)
M63 (tell the machine that there is no next tool)
M3 S...
M8
G0 x.. y.. z..
etc...
Machine somthing... with tool 3
M9
M5
G0 Z800
M6 (Return tool 3 to the magazine)
M2 (end of program)

See, no need to check what tool is in the spindle, you know what is there!

My programming method and 2 cents worth.
Cheers
Brian.