Okuma tool setter program

[scottincolo]

We have a new MF-46VAE with the P200M-H control. We're very familiar with the control but this is our first Okuma with a tool setter. We'd like to have a program that will allow us to load up the magazine and set all the tools automatically. We're currently doing this with our Brothers so we know what needs to happen, but the Brother control is very Fanuc-ish and the program doesn't easily translate to Okuma . Anybody doing this?
Thanks.

[Algirdas]

the program could be supplied with a new machine. Just check MD0: contains

[budgieW]

Save this as a custom G code (G111)


OTOOL (PROGRAM NAME)
(************TO CALL**********)
(G111 MEASURES THE TOOL IN THE SPINDLE)
(G111 T1 [SELECTS THE TOOL AND MEASURES IT])
(NOTE: THE TIP OF THE CUTTER MUST BE IN LINE WITH THE KEY)
(AND THE CUTTER RADIUS MUST BE SET)
(SET CUTTER RADIUS FOR BORING BAR TOOLS ALSO)
(TIPPED TOOLS CAN BE MESURED WITH G111 PA=??)
(G15 H20)
IF [PA NE EMPTY] N1
PA=0
N1
IF [PT EQ EMPTY] N4 (IF T IS NOT SET GOTO LINE 4)
IF [VTLCN EQ PT] N4 (IF T=TOOL IN THE SPINDLE GOTO LINE 4)
IF [VNTOL EQ PT] N3 (IF T=NEXT TOOL GOTO LINE 3)
IF [VNTOL EQ 0 ] N2 (IF NEXT TOOL IS VACANT GOTO LINE 2)
M64 (CANCEL PRE-SELECT TOOL)
N2
T=PT (PRE-SELECT COMMANDED TOOL)
N3
M06 (TOOL-CHANGE)
N4
CALL OO30 PX=[VTOFD[VTLCN]] VFST=#81H PRS=PA
(TOOL GAUGE CYCLE)
RTS (END)

Then the Min file will be
G111 T1
G111 T2
etc
etc
M02

[broby]

Save this as a custom G code (G111)


OTOOL (PROGRAM NAME)
(************TO CALL**********)
(G111 MEASURES THE TOOL IN THE SPINDLE)
(G111 T1 [SELECTS THE TOOL AND MEASURES IT])
(NOTE: THE TIP OF THE CUTTER MUST BE IN LINE WITH THE KEY)
(AND THE CUTTER RADIUS MUST BE SET)
(SET CUTTER RADIUS FOR BORING BAR TOOLS ALSO)
(TIPPED TOOLS CAN BE MESURED WITH G111 PA=??)
(G15 H20)
IF [PA NE EMPTY] N1
PA=0
N1
IF [PT EQ EMPTY] N4 (IF T IS NOT SET GOTO LINE 4)
IF [VTLCN EQ PT] N4 (IF T=TOOL IN THE SPINDLE GOTO LINE 4)
IF [VNTOL EQ PT] N3 (IF T=NEXT TOOL GOTO LINE 3)
IF [VNTOL EQ 0 ] N2 (IF NEXT TOOL IS VACANT GOTO LINE 2)
M64 (CANCEL PRE-SELECT TOOL)
N2
T=PT (PRE-SELECT COMMANDED TOOL)
N3
M06 (TOOL-CHANGE)
N4
CALL OO30 PX=[VTOFD[VTLCN]] VFST=#81H PRS=PA
(TOOL GAUGE CYCLE)
RTS (END)

Then the Min file will be
G111 T1
G111 T2
etc
etc
M02

On the call to the G code line G111 PA=?? you actually only need to program G111 A45
The A45 command is passed into the subprogram and referenced via PA in the subprogram.
The "P" in front of the Letter "A" tells the subprogram to reference the stated parameter letter on the call line.

So using G111 A45 the subprogram would have PA equaling 45.
Cheers
Brian.

[littlerob]

Wow good info in post #3 and 4, thanks guys.

Robert

[broby]

This is the program we use on our OSP-E100M MA600HB machine.

$TOOL.LIB%
OTOOL
M00
HSET=0 (PRESET VARIABLE)
IF [VACOD NE 0] N1
G15 H50 HSET=1
N1 CALL OO30 VFST=1 PY=VTOFD[VTLCN]
IF [HSET NE 1] NEND
G15 H0
NEND
G0 Z800
RTS
%

Very similar to Budgie's code but less clear in what it does...
We have this one set up as a M-Code macro rather than a G-Code, but either way will work.
Both codes use the tool radius to put the tip inline with the tool setter point.

To calibrate the tool setter I use the following instructions:

Setting the Touch Sensor ZERO Point (Z Axis)

1. From MDI: execute Sensor Advance M144
2. Position Setting Bar in front of touch sensor.
3. MDI: CALL OO30 PAXI=7 PLI=0

After this, use the tool setting code to check the length of the setting tool, should be spot on.

Setting the Touch Sensor ZERO Point (X+Y)
1. From MDI: execute Sensor Advance M144
2. Mount a small diameter drill into the spindle (size not important)
3. Bring drill point up to sensor head and position centrally on sensor.
4. From MDI: CALL OO30 PAXI=3
a. X and Y axis zero offset is executed so that the present (actual) position of the drill becomes X0 Y0. Z axis will not move.
b. After the execution of the X and Y zero set, Z axis will move, at rapid, to the positive end of the axis and the sensor will retract.

Hope this helps.
Brian.

[scottincolo]

Thanks to all.