LATHE G28 Help Understanding!!!!

[1ctoolfool]

I have used G28 on mills for years with very predictable results. The G28 X0. always sends the machine straight to machine (G53) X0.

BUT, when I try this on a lathe it send the turret to SPINDLE CENTER!! which is PART Zero!!, then it goes to machine X home.

I really wasn't expecting this and almost had a crash. Replaced all G28's with G53 G00 X0.

The manual says G28 return home "thru reference point" If I just enter x and push the G28 button then it does what you would expect, but G28 X0. at the end of a program will send the turret to the lathe centerline.

Please help me understand what the hell G28 means on a lathe (or mill for that matter)

thanks
joev

[PBMW]

I've seen the same thing on my SL10. I use G53's for that very reason.
I find it interesting that my Daewoo with a Fanuc 0iTc control does notmake wonky moves like that. The first time I saw it do that, I was into the post changing that around....
My Haas does not have a tailstock, so I always send Z home first, but I have to send the Daewoo home differently to clear the tailstock.

[pit202]

I have used G28 on mills for years with very predictable results. The G28 X0. always sends the machine straight to machine (G53) X0.

I don`t think you rigth , G28 with any Axis XYZ moves to machine zero but thru zero point if you want to move only to machine zero you need to add G91 code, this is how my TM works and this is how it is explained in manual.

http://www.cnczone.com/forums/archiv...p/t-43172.html

[jorgehrr]

G28 U0 Return machine home Incremental move to machine home (home is ZERO)
G28X0 In here you are returning to part zero in X (middle of the spindle).
The catch is in the diference of Incremental (UW)and absolute(XZ) lathes, machine centers use G code to make this change. G90 Absolute G91 incremental.

Jorge

[1ctoolfool]

I disagree, my mini mill will go to machine X home when G28 X0. is commanded regardless of coordinate system offsets or absolute or incremental.

The lathe will not behave this way. Our SL30 has the tool probing option and I think that this has something to do with the way the lathe behaves. The TL2 does not have this option and I am going to do some experiments on Monday to see if they execute G28 differently.

For instance if I am in the offets page G54 and do a Z face measure on the SL 30, it will input the distance from the part face to the TOUCH PROBE, not the absolute machine ref. coordinate difference which is what the TL2 will do.

I think this is a significant difference between these two machines that someone forgot to mention and this may be part of my problem. Confusing to operators to say the least.

Joe V.

[dcoupar]

1ctoolfool,

Yes, your mini mill will go to machine X home no matter if you're in absolute or incremental. However, it will take a different route to get there depending on G90/G91.

G90 G28 X0 tells your mini mill to go home (machine zero) via absolute (part) zero. That is, it should move to absolute X0 then continue on to machine X0.

G91 G28 X0 tells your mini mill to move X an incremental distance of 0" then go home. If you program G91 G28 X4., the X should rapid 4" in a + direction, then go home.

The lathe SHOULD work the same way, only use X/Z for absolute intermediate points, U/W for incremental intermediate points.

[1ctoolfool]

yes you are absolutely right, I have misunderstood G28 for a long time, lucky I never had a crash.
thanks,
joev

[dcoupar]

Glad to be of help. That's why we're all here, isn't it?

[BlueChip]

Take a look here for a little more info :
http://www.kentechinc.com/tip6.html

[Geof]

Originally Posted by 1ctoolfool ....For instance if I am in the offets page G54 and do a Z face measure on the SL 30, it will input the distance from the part face to the TOUCH PROBE, not the absolute machine ref. coordinate difference which is what the TL2 will do....Joe V.

I saw this and thought I would comment there is a Setting #64 T. OFS MEAS USES WORK that can be ON or OFF. See if this is set the same on the two machines. When it is ON the automatic tool offset entry key enters the difference between the machine position and any work offset that is active; when it is OFF the entry is the machine coordinate position.

[SeymourDumore]

I dunno about you guys, but I have an SL10, Minilathe, MiniMill and a VF4, ranging from '01 through '06.
On each and every one G28 by itself sends the turret or the spindle ( respectively ) to absolute 0 position, that is G53 X0 Y0 Z0.
I NEVER use any U or X values on the G28 line, nor have I ever used G91 in any of my programs. The clearance plane move is taken care of within the program by G01-s, so there is seldom an issue of crashing. If there is, G00 G53 Xxx Yyy Zzz is used exclusively.
This is true on my machines regardless of setting 64. On the lathes I have it ON, mills have it Off. G28 on Haas seem to work differently than Fanuc in the sense that it does not NEED ANY specifiers within the block. On the Fanuc the equivalent code would be G28 U0 W0

Now, why is your turret goes to spindle center? That is a really good question!!!

[1ctoolfool]

I understand why now, because G28 with an absolute reference will go to machine home THRU the specified point, which is why you use the relative U0 W0 reference and not the absolute X0 Z0.. This thread has been very informative.
The only problem using a straight G28 with no reference is that I typically want to clear Z first when drilling/boring and clear X first when turning. Straight G28 will move XZ equally in a diagonal to X max then Z the rest of the way.
joev