Home Position

I have an older Nakamura lathe with an 11T control on it.
when i sent my machine home my home lights are on and all positions read zero

Although I still have about 5" that i can still travel back in my X
How can i reset my home position for X axis

The home position does not mean that is the end of the travel. If the soft limits are set correctly, you can program the machine to use the whole travel.

What does the position screen indicate for the X axis?
Are all value 0 or a value about 5"
What are your work coordinates set at ?

DAVID ROMERO said:

I have an older Nakamura lathe with an 11T control on it.
when i sent my machine home my home lights are on and all positions read zero

Although I still have about 5" that i can still travel back in my X
How can i reset my home position for X axis

Click to expand...

Errr, doesn't the 11t use G50 for "home position"?

R

That's an offset. An offset from home.

What I was trying to say is the machine can go past 0. The home position is arbitrary.

isn't home a short distance after the soft limits?

It's entirely up to the machine builder. I've seen machines where the home switch is several inches from the limit switch. On modern machines with absolute encoders, the home position is even more arbitrary.

ewlsey said:

That's an offset. An offset from home.

What I was trying to say is the machine can go past 0. The home position is arbitrary.

Click to expand...

I don't know if the 11T uses G50 as a function, but the OP is asking how to make his "Home position" where he wants it to be, not whether or not it is useful. So yes He can program it beyond the zero return position/home whatever, but He wants to change it so that that is the "Home position".

R

Huh? It's a lathe. There's no G50 for X.

He specifically said "home position" and "home lights" on the panel.

ewlsey said:

Huh? It's a lathe. There's no G50 for X.

He specifically said "home position" and "home lights" on the panel.

Click to expand...

The older Fanuc's use G50 as a reference return position, so

o1111
G50 S1000 X$#^% Z@#$@

Go program
program
program
G28 U0 W0 (return to G50 reference return)

All the 11T's I have run use G54.

Parameter 1850 should be grid offset.

Where is the home position at relative to the homing dog?

Usually, it's grid shifted a tiny amount after coming off of the homing dog and before the over travel limit dog.

ewlsey said:

Huh? It's a lathe. There's no G50 for X.

He specifically said "home position" and "home lights" on the panel.

Click to expand...

Hello ewlsey,
I agree, the OP is referring to the Reference Return Position when he mentions the "home lights on the panel".

Fanuc Lathe Controls can be set to use one of three different G Code Systems, A,B and C. There are two different G Codes used to set the Coordinate Systems for a lathe, depending on the G Code System being used (G50 and G92). Overwhelmingly, Fanuc controls use G Code System A and therefore, will typically use G50 to set the Coordinate System. Machining Centre Controls use G92 to set the Coordinate System.

litlerob1 said:

The older Fanuc's use G50 as a reference return position, so

o1111
G50 S1000 X$#^% Z@#$@

Go program
program
program
G28 U0 W0 (return to G50 reference return)

Click to expand...

Hello Rob,
That is not how it works. G50 is used to set a Coordinate System and it can be executed at any axes slide position. However, when G50 is used to set a Coordinate System, it must be executed with the axes slides in the same position for every execution of the program. For this reason, its often the case that G50 is executed with the axis slides at the Reference Return Position; but G50 doesn't set the Reference Return position.

To make your program example correct, it would be written as follows with a G28 U0.0 W0.0 preceding the G50 Block.

o1111
G28 U0 W0
G50 S1000 X$#^% Z@#$@

Go program
program
program
G28 U0 W0 (return to the reference return - which happens to also be the G50 Coordinate System Set position)

If your original example were to be run with the X and Z axes, say 100.0mm away from the Machine Reference Return position, the slides would return to the Reference Return position when the G28 U0 W0 at the end of your program is executed. The next execution of the program would result in the axes slides (and therefore the tool) being 100.0mm out of position for each axis.

A Fanuc 11T control will generally be supplied with the G54 to G59 Work-shift Offset option and would be used in preference to setting the Coordinate System using G50.

Regards,

Bill