Re: [Emc-users] gcode and coordinate system explanation needed.

[Andre' B. <an...@us...>]

At 11:02 AM 6/23/2008, you wrote:

>On 22 jun 2008, at 22:06, John Thornton wrote:
>
> > G28 goes to a predefined position (home as defined in parameters
> > 5156-5166).
> >
> > To make G28 go to 0,0,100 you must home the machine there which will
> > become
> > 0,0,0. Then a G28Z0 with no space will home the Z axis only. The
> > space between
> > the G28 and the axis must call up an undocumented feature...
> >
>
>I'lltry what happens if I remove the space.
>
>I'll play around with the G28 a bit but I think I'll remove from the
>postprocessor. I don't see the need for going to 0,0,0 before starting.
>
>Dirk

Most of the controls I write programs for are Fanuc and Mitsubishi and of 
the bunch only one needs to be at home at the start of a program, and that 
is because of some bug in the integration of the machine and control, if it 
is not at home at the start of the program it tries to send the first tool 
down thru the floor.
Normally as long as there is a clear path from the current location to the 
position of the first move in the program, homeing at the start is not needed.

So most of my programs just start with a safty line to make sure all the 
correct modes are active.
At the end of each tool I send the spindle home with the line.
G91G28Z0M5

Note that the G91 is important other if the machine is in G90 the G28 will 
first go to the Z0 of the current work offset and then to the machine home, 
in many setups that will produce undesirable results.

And at the end of the program I add a second line to send the Y home after 
the Z is up out of the way, making it easier for the operator to change parts.
G91G28Z0M5
G91G28Y0
M30

Machines with pallet changers need to put the Z in some safe location 
(home) and then move the X and Y to some specific location at the start of 
the program to bring in the new pallet, but that should be handled by the 
pallet changing code.
__________
Andre' B.  Clear Lake, Wi.