G28 question

[yoshi900]

I got a question about G28, homing the Z axis on a Fanuc OM-D.

currently, all my program at the end of each tool, there is a line:
G91 G28 Z0.

and it homes the Z axis to the machine zero. which is working fine.
the machine has the umbrella type tool changer, and the Z axis has to come down Z-4.8566 to do tool change. so right now, the z axis would go all the way up to Z0, then come down again to Z-4.8566 when it does tool change for the next tool.

Is there anyway to send it directly to Z-4.8566 instead of Z0? I have tried putting in:
G91 G28 Z-4.8566

but it actually wanted to go down -4.8566 from the last cutting position, and then still go to home Z0. so definitely that didn't work.

If anyone has any solution or suggestion to try, I would appreciated it.

[Geof]

You should be able to use G53 (G90) G00 Z-4.8566

G53 tells the machine to use machine coordinates.

The G90 may not be needed, I just wanted to emphasize this is an absolute move.

[yoshi900]

Originally Posted by Geof You should be able to use G53 (G90) G00 Z-4.8566 G53 tells the machine to use machine coordinates. The G90 may not be needed, I just wanted to emphasize this is an absolute move.

Thank you Geof. That worked perfect!

[tnik]

you could also try to not send z home.. eg.

.......
G00 Z1. M09 (last movement away from part, kill coolant)
T3 M06 (do a tool change)

Not all controllers/machines require you to send things home before a tool change. I know on our haas I can call up a tool change and it will stop the spindle and send the spindle up for a toolchange.

[HuFlungDung]

That sounds like kind of a nuisance sort of problem, almost like the setup parameters are not quite correct. I would think the machine should find its Z index on startup, call that point Z+4.8566 (via an internal parameter setting which would define the position), and then move to G53Z0 as the last step of the homing routine.

[stevo1]

Tnik, That will usually depend on the MTB if the tool change was written into the ladder using the M6 or if there is a tool change macro. I am not firmilar with Hass but I would assume that if your machine does all of that automatically that you have a macro unless the Haas comes standard like that. I know on the Fanucs most of the time when the tool change is built into the ladder it is very basic and need to be in the right position when programming the M6.

I agree with you it is much easier when you add a macro for the tool change. Then you don't have to worry about anything. All you have to do is program T#M6 from any point in the machine.

On All of our machines I have the machine go to Z position tool change then Y postion. Cancel coolant and spindle off. Change tools cancel offset, reinstate current tool offset with no tool movement, get speed and feed for the tool, and skip the tool change if the tool your calling is already in the spindle.

Stevo

[tnik]

Stevo,

Yea, It is probably a macro that it comes with, I have other fanuc machines here that are picky about what axis is home or not for a tool change..

yea, normally each block ends like:

G00 Z(safe rapid height) M09
G28 G91 Z0. M05
G28 Y0.
M01

Just because thats how I have my post processor setup..

Unless I have a production job.. Then any movements I can take out I do..

[stevo1]

Tnik thats the way I have most of my macros set up for the tool change. Depends on how I have my reference postions set up for home postion in the machine.

Sorry Huflungdung I over typed you in my last post and didn't see your post.

He is spot on with how it should be set up. On some of my machines with a rotary table I have the machine postion for the first point postion set to the center of the table for Z so G53Z0 does not get me to my tool change postion. However if appears for what Yoshi900 is trying to accomplish if the floating reference point or first through fourth coordinate value are set to the tool position of 4.8566 then programming a G53Z0, or G30, or G30.1 will take you to the tool change position.

Stevo