Amada Vipros 358 King II Return to Origin without using G50

Hello,

I'm trying to make a CNC program for an Amada Vipros 358 King II with a Fanuc controller. The program will have 3 pauses in it for the operator to rotate or flip the part as needed.

The operator will start the program, the program will punch a notch, a radius, and a hole, then return to home and pause with M00.
The operator will then rotate the part 180 degrees and resume the program. Program will punch some then return home and pause with M00.
The operator will flip the part keeping the gripper edge the same. Program will punch some then return home and pause with M00.
The operator will then rotate the part 180 degrees one last time. Program will punch some and then end with G50.

The problem I'm running into with this program is that I'm getting a 4702 OT+ in the Y-axis when I try to return the axes to the origin using G70 X78.74 Y50.75 (X78.74 Y50.75 is the same as our G92).

Anyone know what am I doing wrong?

Thanks in advance for any help you can give.

Hi
Your machine turret is Triple track, it means there are three tool set in a row with the same index pin. 1xx tools are inner, 2xx are center and 3xx are outer track. So they have a Y axis offset with each other.
You can use
G70“machine home position” T 2xx

Or simply don’t use machine home position at G70 line. Subtract Y axis offset from Y value.
Ex:
G70 X1830. Y1200.
M00

But in this case the X gauge block may not raise.

Mail me if the problem was not solved.
[email protected]
Good luck

Quote:

---

Originally Posted by norin1373

Hi
Your machine turret is Triple track, it means there are three tool set in a row with the same index pin. 1xx tools are inner, 2xx are center and 3xx are outer track. So they have a Y axis offset with each other.
You can use
G70“machine home position” T 2xx

Or simply don’t use machine home position at G70 line. Subtract Y axis offset from Y value.
Ex:
G70 X1830. Y1200.
M00

But in this case the X gauge block may not raise.

Mail me if the problem was not solved.
[email protected]
Good luck

---

Thank you!

This makes perfect sense and it solved my issue.

I changed

Code:

---

G70 X78.74 Y50.75
M00

---

to

Code:

---

G70 X78.74 Y50.75 T229
M00

---

T229 was the next tool in the sequence, so it seemed a logical choice. The carriage returned to the home position and the operator was able to raise the x gauge block and reposition the sheet before resuming. We did a dry run first with punching off and then again with punching off just for the first stage, since we already had one part that had finished the first stage before triggering the OT+ error. We turned punching back on for the remainder of the program and it executed flawlessly.

Thanks again!