[bowmaster]

I would like to jog my table backe to x -20.00 y .00 after in machine my part to unload it, here is the last lines of my program

N210 G1 Z-.05
N220 G0 Z.5
N230 M5
N240 G91 G28 Z0.
N250 G28 X0. Y0.
N260 M30
%

and I am using a G55 work offset.

please advise I am a newbie to Haas
thx

[dcoupar]

Try this?

N210 G1 Z-.05
N220 G0 Z.5
N230 M5
N240 G91 G28 Z0.
N250 G90 G53 X-20. Y0.
N260 M30
%

[bowmaster]

Still goes back to machine x0,y0
what now?

[mactec54]

bowmaster


Just on line
N249 G0Z4. Put what number that you want the Z to clear your work
N250 G0X-20. Y0. This will Rapid to this point
N260 M30

Remove The G91G28 stuff

If you want it to jog back do it as G1X-20.Y0.F20.

[JWK42]

N210 G1 Z-.05
N220 G0 Z.5
N230 M5
N240 G91 G28 Z0.
N250 G28 X0. Y0.
N260 M30


This is the way we do it.


N210 G1 Z-.05
N220 G0 Z.5
N230 M5
N240 G53 G00 Z0.
N250 G53 G00 X-20.0 Y0.0
N260 M30

We have never used G28 at the end. The G53 is the distance and direction from the machine zero. So X-20.0 puts the table in the center of a 40 inch travel, the Y0.0 puts the table at the outside edge and the Z0.0 puts the head all the way to the top. Be sure there is a decimal point after whole numbers. This is a Haas requirement and can be a PIA to find if you have a problem that was written by hand.

[Pondo]

G91 G28 Z0. is basic home movement in Fanuc controls. It does work fine in Haas controls, but a better option is G53 Z0. The G53 is non modal and is only active in the block it is in. The G91 is modal and needs to have a G90 after it to go back to absolute. The G53 offset is always the machine 0 point, so G53 X-20. Y0. will get you to where you want to be.

The N249 G0Z4. N250 G0X-20. Y0. example above will put you over your G55 Y0. and 20" to the left of your G55 X0. - I don't think that's what you were looking for.

[JWK42]

On the Haas G53 is not tied to any other coordinate system. It is distance and direction from machine zero. The X numbers are in the range of zero to minus 40.0 on a 40 inch "X" machine and zero to -20.0 on a 20 inch "Y" machine.

[Donkey Hotey]

The G53 offset is always the machine 0 point, so G53 X-20. Y0. will get you to where you want to be.

Nope, evidently not. I had this misunderstanding a couple of months ago. G90/G91 still affects G53 moves. Yeah, that's really stupid but, that's the way the control treats them.

More here:
http://cnczone.com/forums/showthread.php?t=100601

[djr76]

Where is your G55 X0. in relation to center of table?

G28 G91 G00 Z0. Y0.
G55 G90 G00 X(whatever the distance is from G55 X0. to center of table)
M30

[Pondo]

Nope, evidently not. I had this misunderstanding a couple of months ago. G90/G91 still affects G53 moves. Yeah, that's really stupid but, that's the way the control treats them.

More here:
http://cnczone.com/forums/showthread.php?t=100601

I see - that's a new one to me. G91 disregards the WPC called out, so I guess it would not matter if it was G54, G55, G53, or whatever. I don't think I've ever run a post that mixed G91 G28 homing with G53's. It's always one or the other.

This is what I do when posting from MasterCam like Djr76 does, since it posts the G91 G28 home positions in Z and Y after each tool. I just handwheel it to where I want it for part changeover and add the X move.
G91 G28 G00 Z0.
G91 G28 Y0.
G90 G00 G54 X(whatever the distance is from G54 X0. to center of table)
M30

For the Gibbs posted programs, I reference the G53 for the X move since the Z and Y home moves are in G53.

[offsetxyz]

N250 G28 X0. Y0

Most of the time simply removing the X0. from that line of yuor progarm will leave your table about where you need it.

If I program it I put
G28 G91 Z0.
G53 G90 X-20.(X-26.0 in my case)
G28 G91 y0.
M30

To me G90 translates as "go there, right there and nowhere else".