G50 is your tool offset geometry and you need it for each tool.
Normaly X is to centerline of spindle and Z is usually to the end of
your completed part.
Zero Return the machine
Origin X and Z axis if not 0 in each counter
Index to tool
Face off your part or touch the front.
Z axis reading + or - whatever the raw material condition is and
this is your G50 Z input.
Turn the OD
X axis reading + the OD diameter and the answer is your G50 X input.
Now some machines the Z could be Z- or + so you need to work that out
and X is the same way.
In this example I am assuming Z zero is the finish face (length) and X
is Zero is Spindle Centerline.
Z axis at home counter is 0. Face off part and the counter reading is
Z9.850, you check the part and you have .025 material left to face off.
Z = 9.850+.025 = 9.875
X axis at home counter is 0. Turn the OD and the counter reading
X5.908 mic the OD and the part is 1.507. X= 5.908
+ 1.507= 7.415
In this example G50 X7.415 Z9.875
Once your tools are set and you don't change the tool you never need to
change the X value. For Z you only need check one tool then make the
same adjustment to all the others (this is equivalent to a work shift).
For drills indicate the center of tool holder and that is your X value
and that will never change unless something changes on the machine.
For my example it assumes you are programming X+ values and Z- values.
Post by email@example.com
My machine does not have the rs232 port to send out from machine to
punch or BTR but when I look manually at the content of the addresses
the program seems to be there correctly downloaded. I think I just
have to get more familiar with the conventions required.
I plan to do a one block at a time download to see where the problems
I am confused by the g50 command. When the machine is zeroed the x and
z coordinates are 0 and 0. Why do I need the g50.? Is is possible to
change the absolute coordinates of the zero position for x and z? How
does one know what values to enter?