Hi,
I used to just open Mach 3, zero the machine coordinate system at the work zero and cut away (all work offsets being zero).
What was happening was that when you jogged to the start location and 'zeroed your machine coordinates' what you actually
did was 'home in place'. It is an option (Mach3 AND Mach4) that when you <RefAllHome> or <RefAxis> to have the machines
current location be the new home position. It is a poor practice.
Now that you have proper home switches when you <RefAllHome> the machine will home and zero its machine coordinates.
I believe the machine starts in G53 and is located at 0,0,0
No, G53 is a non-modal Gcode that causes Mach to interpret the axis coordinate destinations on the line on which it occurs
as machine coordinates.
So you start a Mach4 session by starting the machine and hitting <RefAllHome>. Then jog to the start location, commonly
the corner of the material, and then 'zero the axes' per attached. Note that this zeros the work coordinates NOT the machine
coordinates. Mach does this by setting numbers in the current work offset (G54 by default) such that the current
machine coordinates MINUS the G54 offsets cause the DRO to be zero.
In the pic I have posted I homed the machine and then jogged 28mm in the X axis, 26mm in the Y axis and 22mm down
in the Z axis and then zeroed all three axes. The DROs all now read 0.0000 This means the work offsets (G54) are set to
28, 26 and -22. Thus the work offset is set without you having to do anything and you can now start machining.
Lets say you wish to run the same program again on the same piece of material (still in the vice) you can use the button
<GoTOWorkZero> and the machine will traverse to the corner of the material. You might consider then that the G54 offsets
are the machine coordinate location of the corner of the material. The DROs should all read 0.0000 and you can now run
your Gcode again.
Lets say you want to finish the Mach session without completing the part. When you shut Mach down the work offsets
are flushed to the registers which are stored in the .ini file. Lets say you come back the next day. Start Mach and the work
offsets will be restored to what they were at the end of your last session.Home (<RefAllHome>) as normal and then
<GoToWorkZero> and the machine will traverse to the corner of the material which is still in the vice. You don't
have to touch off again.
Note that Mach3 and Mach4 behave the same in this regard. I fact ALL CNC machines operate this way. It is for this reason
that I argue that good home switches are ESSENTIAL to operating Mach. In your case you have added index homing to the
mix but the essential idea remains the same. The work offsets (G54, G55, G56...etc) are in effect the machine coordinate
locations of various points of interest, the corner of the material in the vice for instance.
Sometimes it seems like the first line runs and throws some weird number into the Z axis DRO,
When m6 runs the DRO will change to the current work coordinate location of the Z axis. The number represents the difference
between the actual and current machine coordinate and the current work offset but with NO tool offset. When the second
line runs the tool offset is set per the attached and the DRO recalculated to include the G54 offsets AND the tool offsets.
Craig