Hi,

G28 x0 y0 z0 sends the machine to a known home position, e.g. the machine has already been homed before.

G28.1 x0 y0 z0 will send the machine to find the home position whether its been there before or not.

Graham.

Thats awesome!!!

Okay guys,
Setup for a program at X8.00 Y7.00 Z-1.35 zero all as you would for a work offset. Then crank on your drives to intentionally loose position drastically. Executing the above G28.1 X0Y0Z0 send the machine to zero it's axis but does not reset the offset but corrects it!!! How cool is that!!! Touches off all homes and finishes with X-8.00 Y-7.00 Z1.35, brilliant, it's going into the post processor.

Only issue is the order executed is not Z axis first, but I can easily work with that, maybe as simply as execute a G28.1 Z0 followed by g28.1 x0y0. I'll have more time to play tomorrow. Hey, maybe a G28.1 Z0 Y0 X0... Graham, thanks so much!

Chip and ger21, thank you both as well!!! I will start playing with macros soon as well.

Thanks again to all,
Sam

Only issue is the order executed is not Z axis first, but I can easily work with that, maybe as simply as execute a G28.1 Z0 followed by g28.1 x0y0.

I think that's the way to go.

Thats awesome!!!

Another little known gem out in the open 

Graham.

Hi All,

I found this little gem. I have tried adding G28.1 A0 after a cycle of a specific cut before moving on to the next as a way of picking up of lost steps by referencing the A axis. I have found that the program stalls/stops at the addition of this code.

Is there somthing I have missed?

yOU can use G28.1 X#.## . Y#.## Z#.##  to reference the axis to the home switches. BUT it follows the fanuc convention of going by way of a waypoint(can be the present point) BUT it then makes an interpolated 3 axis move to the approx home switch positions then references the switches. It is the fastest way to ref home, Just make sure the path is clear(;-)

IF you want it to do exactly like the Ref all home  where it refs Z then X then Y  then you will need to create a macro that calls the "Ref all home" button.

Let us know if you need help with it, (;-) TP

Thanks TP

I only wish to reference the A axis.

Yes it would be great to have a macro and use M codes throughout the code.

I have never written a macro so I would certainly like some help

C

G28.1 A0     will reference A axis to the home switch by way of A0.000 If that is not what you need email me and I will send you a macro to ref A axis.

OR now is a good time to build your own Mcode(;-)

From the main screen at the top select the pulldown menu"Operator" then VB script editor. IF a file is loaded on the screen then from the editor select file, close. This will leave a blank page to work on. Type in the phrase   DoButton(25)

Save the file as M1001( you can use any number 1000 and up safely). Make sure it saves to the c:\mach3\macros directory (;-)

Close the editor

Go to the MDI screen and type in M1001 and the A axis should reference HOME from its present location .

NOTE : You do have to have a home switch installed on A(;-) for this to work.

If all is well then you have created a Mcode that you can call from a gcode program at any time you need.

NOTE: Make sure that you program the Z to a clear safe position before calling the M1001 (;-)


Hope that helps, (;-) TP

Thanks TP,

I have sent you an email