[rjCousineau]

Hi, I can't for the life of me figure out the proper use of G29

using SL20 or TL2

From the manual, it says it references Work Offset 7 (that being G110 P1). But even if I run the block:
G29 U0. W0.

The machine does not respond.

How to use?

[dcoupar]

I believe you have to do a G28 first.

G28 X5. Z5. (RETURN X AND Z TO MACHINE 0 VIA X5. Z5.)
G29 X2.1 Z0.1 (MOVE TO X2.1 Z0.1 VIA X5. Z5.)

I've actually never known anyone to use G29, but I think that's how it works. My manual doesn't mention work offset 7 with G29, but I may have an outdated manual.

[rjCousineau]

Thats interesting but I'm still pretty clueless. I thought it was a secondary home. I'm using an open bed TL2 and the machine home is not safe because of the tail stock being in the way of the 4-tool turret. I was hoping G29 was an alternative home position that can be used instead of machine 0. Right now i'm having to modify every tool change.. also the machine home is pretty far away

[dcoupar]

As far as I know Haas doesn't have a 2nd (or 3rd & 4th) reference point as Fanuc does (G30 P2, P3 & P4). How are you generating programs? Maybe you could modify the post so you could have it output the code with the mods you are making manually?

[angelw]

Thats interesting but I'm still pretty clueless. I thought it was a secondary home. I'm using an open bed TL2 and the machine home is not safe because of the tail stock being in the way of the 4-tool turret. I was hoping G29 was an alternative home position that can be used instead of machine 0. Right now i'm having to modify every tool change.. also the machine home is pretty far away

Dave's explanation is correct, and you could possibly benefit by using G28 and G29 to avoid the interference with the tail stock. Mostly you will see examples of G28 being used with incremental moves of Zero, but the slides are still returning to the Reference Return position via the intermediate point Zero distance away from the slide position when the G28 command was executed. You will see the function of G28 U0 W0 (lathe application) more clearly if executed in Single Block mode. On first press of the Cycle Start button to execute the G28 block, the slides remain where they are and the Feed Hold indicator is illuminated. On second press of the Cycle Start button the slides move directly to the Reference Return position.

G29 is used to move the slides to a coordinate specified in the G29 block, via the intermediate position setup by the previous G28 command. G29 can be programmed Incrementally but I it would be easier to use in a situation such as yours where you want to skirt around an object of interference, if absolute mode is used for both G28 and G29.


Regards,

Bill

[haastec]

Hi, I can't for the life of me figure out the proper use of G29

using SL20 or TL2

From the manual, it says it references Work Offset 7 (that being G110 P1). But even if I run the block:
G29 U0. W0.

The machine does not respond.

How to use?

I don't have a lathe handy to test this, but I don't believe you need to use the G28 in conjunction with the G29.

G29 is basically another work coordinate, you define where G29 (G110) X0, Z0 is by setting it in the offset screen.
Instead of programming G29U0 W0, which is a non-move, use G29 X0 Z0 to tell the machine where you want it to go.

Hope this helps.

[angelw]

I don't have a lathe handy to test this, but I don't believe you need to use the G28 in conjunction with the G29.

G29 is basically another work coordinate, you define where G29 (G110) X0, Z0 is by setting it in the offset screen.
Instead of programming G29U0 W0, which is a non-move, use G29 X0 Z0 to tell the machine where you want it to go.

Hope this helps.

Following is a direct Cut and Paste from the Haas manual I have.

G29 Return from Reference Point (Group 00)
The G29 code is used to move the axes to a specific position. The axes selected
in this block are moved to the G29 reference point saved in G28, and
then moved to the location specified in the G29 command.

Regards,

Bill

[dcoupar]

I don't have a lathe handy to test this, but I don't believe you need to use the G28 in conjunction with the G29.

G29 is basically another work coordinate, you define where G29 (G110) X0, Z0 is by setting it in the offset screen.
Instead of programming G29U0 W0, which is a non-move, use G29 X0 Z0 to tell the machine where you want it to go.

Hope this helps.

I don't believe it said anything like that in the latest manual I downloaded from HaasCNC.com. But I could be wrong.

[haastec]

Following is a direct Cut and Paste from the Haas manual I have.

G29 Return from Reference Point (Group 00)
The G29 code is used to move the axes to a specific position. The axes selected
in this block are moved to the G29 reference point saved in G28, and
then moved to the location specified in the G29 command.

Regards,

Bill

I don't believe it said anything like that in the latest manual I downloaded from HaasCNC.com. But I could be wrong.

Yes, you both are correct. I think I must have been drinking, see Machineit's lube pump post, when I made my response.

I have never used G29, and to be honest, I don't quite follow it's definition in the book either. So basically my answer was/is crap, sorry guys!

I was mixing the G29 command up with how an actual Second Home Switch mounted on the pendant works.

[CPInc]

Not sure if this is relevant or not. On our VM-2 with 2nd home position We have to set location in G154 P20 for all axis locations. In the program "G154 P20 G90 X0. Y0."
sends the machine to second home position. Not sure why this cannot be simplified to a G30 like on our Doosan machines. Hope this helps

[Geof]

Copied from the Mill Operator's Manual online today:

G29 Return From Reference Point (Group 00)
The G29 code is used to move the axes to a specific position. The axes
selected in this block are moved to the G29 reference point saved in G28, and
then moved to the location specified in the G29 command.

I think this description is a bit foggy, to say the least, but what I think it means is that a G29 command for a particular axis will send that axis to the zero position in the current work offset. This is what G28 does if you do not use G91 and is the G28 reference point. Then the axis goes to the home position specified in G154 P20.

But I don't think it is available on lathes.

[dcoupar]

Copied from the Mill Operator's Manual online today:

G29 Return From Reference Point (Group 00)
The G29 code is used to move the axes to a specific position. The axes
selected in this block are moved to the G29 reference point saved in G28, and
then moved to the location specified in the G29 command.

I think this description is a bit foggy, to say the least, but what I think it means is that a G29 command for a particular axis will send that axis to the zero position in the current work offset. This is what G28 does if you do not use G91 and is the G28 reference point. Then the axis goes to the home position specified in G154 P20.

But I don't think it is available on lathes.

Yes, it's available for lathes. The exact same wording is in the Lathe Operator's Manual.

For example, the following code will rapid to X5.0 and Z4.0, then rapid both to machine zero. After the program stop, the G29 block will rapid to X5.0 Z4.0, then rapid to X3.0 Z0.1.

G28 X5. Z4.
M00 (REMOVE CHIPS FROM BORE)
G29 X3. Z0.1 will rapid to X5.0 and Z4.0, then rapid to X3.0 Z0.1.

[Geof]

Yes, it's available for lathes. The exact same wording is in the Lathe Operator's Manual....

Thank you!!! Now things are less foggy. G29 is not the second home position, it is as the manual says a return through reference point command. I went back to the Mill Manual file and on page 29 found this mention of second home Second Home - Press this button to rapid all axes to the coordinates specified in G154 P20 . I also found a similar mention on page 32 of the Lathe Operator's Manual. But as far as I know these refer to the second home that you can get as an option not to G29. Also I could not find anything mention of Second Home in the manual that came with my TL2 so even if G29 is available on a TL machine I doubt that Second Home is, particularly if it was not included as an option.