geometry

[Htech]

Hi!
Can anyone help me with a Fanuc T6, this T6 does not have a geometry page, so the operator is using G50 for offset and tool comp. I was asked the question? How do you teach the tool with this specific control? I work on CNC’s, I do not run them, and so I do not know! I just thought I could get an answer here to help them out.


Thank you.

[dcoupar]

From what I remember (it was 24 years ago or so), you don't "teach" the 6-T. It's an old dog, and it doesn't learn new tricks!

1. Zero out the machine.
2. Set the position displays to 0,0
3. Index the turret to the tool you want to set.
4. Touch off the tool to the face of the part.
5. Write down the Z Machine Position, i.e.: -10.756
6. Add the amount of to remove from the face, i.e.: 0.03 + 10.756 = 10.786
7. Touch off the tool to the OD of the stock.
8. Write down the X Machine Position, i.e.: -12.594
9. Add the diameter of the stock, i.e.: 2.99 + 12.594 = 15.484

In the program:

%
O1234 (FACE AND TURN 2.937 X 3.00 LG)
G00 G40 (SAFETY FIRST)
G28 U0 W0 (GO HOME)
T0100 (SELECT TOOL)
G50 X15.484 Z10.786 S2000 M08
G97 S400 M03 (PRE-SET RPM)
G00 X3.1 Z0.1 T0101 (RAPID TO CLEARANCE)
G96 S450 (ACTIVATE CSS)
G92 X-0.06 Z0 F0.012 (FACE END)
G90 X2.937 Z-3.00 (TURN 2.937)
G00 G28 U0 W0 (GO HOME)
M01 (OP STOP)
(REPEAT ABOVE FOR REMAINING TOOLS)
%