Return through reference point?

[RBrandes]

Self taught on CNC so I was wondering what the purpose of
the return to zero through reference point command is used for.
Thanks in advance.
-Ray

[gar]

051202-0933 EST USA

RBrandes:

I believe you are referring to G28 and G29. I have never used these. I suggest that you experiment with no tool in the spindle, 25% rapid, and safe points.

It is often times very hard to read the HAAS description of a function and understand what is supposed to happen. And there are times when the HAAS description is wrong.

It appears that G28 can do several things. G28 alone takes you to machine home, maybe. HAAS manual says that G28 cancels tool length offsets. What does that mean? What does machine zero point mean? I would think it means absolute zero, but maybe not since in other ways the current coordinate system is being used.

Do some experiments in a safe way and report back. Maybe use feed hold and the position screen to see what is happening.

.

[JPMach]

I use G28 all the time at the end of my programs:
...
G01 X.5 Y.375
G0 Z1.
G91 G28 Z0. M9
G28 Y0. M5
G90
M30

This brings the head up, turns the coolant off, and then brings the table out and turns the spindle off.

JP

[HuFlungDung]

I think that G28 is used in a general sense to return the tool to home. The confusing part is including a set of coordinates with the G28 specifies an intermediate point through which the tool should pass on its way to home.

I don't know if this has much purpose on a milling machine. However, on a lathe, it makes more sense. If you have a boring bar deep inside a hole, and it has finished its profile, then call a G28, the machine could attempt to move the tool through the part on its way to home.

So, if you add an absolute coordinate, G28 X1. Z1., the lathe would first withdraw the tool to the X1.Z1. then, move to the home position.

I think intelligent use of this command requires programming by hand, with thought directed to where a safe position would actually be.

From what I have seen, most of us disregard the intended purpose of the G28 intermediate coordinate by switching to incremental mode for that command.

On many lathes, some kind of coordinate is required with the G28, or it does nothing. So, lathes often use G28 U0 W0, with it being understood that U and W are incremental movements, whereas X and Z would be absolute. Anyways, adding an incremental axis movement of zero with the G28 specifies that the intermediate point is 'zero' away from the current position, so the machine 'moves there' and then to home.

G29 is supposed to do the inverse movement of the G28 to get you back to a position that was occupied before the G28 was called.

I could be wrong on some of these points, but that is what I understand at present.