[Rockettrans]

Just acquired 1981 Mori Seiki TL5A with Fanuc 6T control. No manual. Trying to figure out how to set "part zero"? Any help would be appreciated. Thanks

[hitachibos]

the 6T used G50's to set geometry offsets.
use a sfety start up program section at the begining of your program.

EX:
G0 G90 G40
G28 U0 W0
G0 X7.0 Z7.0
M01

run this program section. What it will do is return the machine to home then move it to a point somewhere on the machine it thinks is X7. Z7.

Then you need to get the distance from the tip of your tool to your part zero.


you would then use this distance in your program as a G50

EX:
T0100
G50 Xnumber Znumber

G0 X=above the dia Z=infront of part T0101

[angelw]

EX:
G0 G90 G40
G28 U0 W0
G0 X7.0 Z7.0
M01

In your above example G0 X7.0 Z7.0 could be absolutely any where depending on what the Absolute Position Display happened to be at the time.

If G50 is being used to set the Work Coordinate System, G Code System A must be being used. Accordingly, G90 in G Code System A is a Cutting Cycle and does not belong in a block with G0 and G40.

Rockettrans
G50 should always be executed with the slides at a fixed repeatable position. If the Work Coordinate System by G50 is not being set at the Zero Return Position, the following is often used:

Metric Example
N1 G00 G21 G40 G99
/G28 U0.0 W0.0 (REFERENCE RETURN - FIX POSITION)
/G00 U-150.0 W-200.0 (INCREMENTAL MOVE AWAY FORM ZERO RETURN POSITION)
G50 X222.000 Z222.000 (SET THE ABSOLUTE POSITION OF THE CURRENT TOOL)
G50 T0100 S3000
G96 S250 M03
G00 X100.000 Z10.000 T0101 M08
-----------
-----------
-----------
-----------
G00 X222.000 Z222.000 T0100 M09
M01

In the above example, the slides are set to a known repeatable fix position by executing a Zero Return for both axes. The slides are then moved an Incremental distance closer to the workpiece if the Zero Return Position is deemed to far away for a Tool Change Position. A Block Delete has been included in the Reference Return and the Incremental Shift blocks. You only need execute these blocks at the initial start of the program, or when you may have to re-establish the physical Tool Change Position after an unexpected stop of the program (broken insert etc)

There are a number of methods of determining the G50 for each tool. Following is one:
1. At the Tool Change Position, be it the Reference Return Position, or the incremental distance away from it, set the U W, relative position display to Zero.
2. Index to the tool to be set. Do so via manual mode, or if MDI is used, do not call the Tool's Offset.
3. With a workpiece mounted in the chuck and the spindle started, move the tool to the workpiece and cut a diameter for length sufficient to be able to take a measurement.
4. As the Relative Display was set to Zero at the Tool Change position, the Display should now be showing a negative distance the tool tip is away from the Tool Change Position.
5. Without moving the tool in X, move it clear of the work, stop the spindle and measure the freshly cut diameter.
6. Add this diameter as a negative value to the Relative U Display. This number as a Positive value will be the X G50 for this tool. Note it down.
7. Start the spindle and take light cut on the end of the workpiece. Move the tool clear of the workpiece in X only.
8. Stop the spindle and measure how much more material needs to be removed until the tool would be at Z0.0
9. The measured amount is added as a negative value to the Relative W Display. This number as a Positive value will be the Z G50 for this tool. Note it down.

Repeat the above from point 2 for all other tools used in the program.

The values you obtain will rarely be whole numbers; there will almost always be a decimal component. If the machine is set to metric mode, G21, I use the Integer component of the number as the G50 number, and the decimal component as the Tool Offset. The reason being is that the decimal component in a metric system will be less than 1mm or less than 0.040". Accordingly, the result is a clean, whole number in the program as the G50 value, and a relatively small value in the Tool Offset.

When the Tool is returned to the Tool Change position, its important that the Tool Offset is cancelled. Failing to do so will result is a gradual shift of the Tool Change Position.

Regards,

Bill

[Rockettrans]

Thanks, gonna try this, this morning. WHEW.