G28 Z0

[Tinyfxds]

I wanted to move the machine away from the part in order for our indexer to rotate.  We now have 2 extra holes in the part because it seems that after the G28, it plunges thru the part a bit and then retracts back up to the correct height and continues machining.  Does G28 cancel tool height offsets?  I'm running a Hurco if that makes a difference.

[Rstewart]

G28 Z0. sends the Z axis to the Home position (tool change).

 

Sounds like you have some linking parameters jacked up!

 

Reference points are your friend!!!

[GIZMO 21]

g28 does cancel height offsets

[The Cathedral]

Did you put it in incremental first? If you didn't, there's your problem!

[Tinyfxds]

g28 does cancel height offsets

 

So if I slap a g28 z0 into the middle of a program I have to enter in my height offset again?

[Rstewart]

**** G91 G28 Z0. *****

[chris m]

Or just move the machine up X inches to clear it and skip the G28

 

G00 G91 Z4.

G90 A45.

Z.100

[GIZMO 21]

So if I slap a g28 z0 into the middle of a program I have to enter in my height offset again?

yes sir. I used to do that for horizontals. retract to home position ,rotate tombstone and recall a g43.

[Guest]

Yes, G28 will cancel your height offset.....it will need to be recalled

[Tinyfxds]

I ended up taking out the G28 and just moving the tool up 7 inches. 

[Newbeeee™]

G28 Z0. sends the Z axis to the Home position (tool change).

 

Sounds like you have some linking parameters jacked up!

 

Reference points are your friend!!!

+1 to ref points.

Z up to safe point, move X, rotate, and away you go.

[tim_h]

I haven't tried ref points but on a 4th axis this could be very beneficial, if it isn't too much of a hassle to set it up...

I have it outputting a G91 G28 Z0, Then index and G43 again. This way I don't rotate with the tools too close to the part.

[Guest]

I use G53Z0 everywhere now (Machine Coordinates).

 

JM2CFWIW YMMV

[kunfuzed]

I use G53Z0 everywhere now (Machine Coordinates).

 

JM2CFWIW YMMV

+100000