Re: [CAD_CAM_EDM_DRO] Question Re: Work Offsets

Tom,

For a quick check, you may want to make sure your g-code post program
isn't by default assigning a coordinate system (G54 through 59.3) different
from the one you see in the MDI mode. Also beware of tool height offsets.

To see the coordinate system origin offsets for EMC from the GUI, select
'View'->'Offsets and Variables'. This pops up the variable table file.
Numbers 5221-5226 are G54, 5241-5246 = G55, 5261-5266 = G56, etc. The G92
offsets are from 5211-5216.
G54 is the default coordinate system, so you can change the variable
table in a persistent fashion by modifying the values in the file, then
saving the file. (it's called emc.var, or your_setup_name.var)
The variable table is loaded at startup.

I find it important to remember that in EMC, the G92 offsets apply
'globally' to all the coordinate systems, but are only valid relative to the
one coordinate system you were in when you entered the 'G92' command.
If you 'G92' an origin point in the first coordinate system, then do it
in another, you've just lost the first origin point setting. Or, if you G92
the origin in one system, when you go to the other, it's offsets are moved
by the arbitrary G92 offsets from the first system.

To make the changes directly to the coordinate system offsets (not G92)
from the MDI, use G10 L2 Pn. 'n' is the coordinate system number, 1-9.
(G54-G59.3)
A bit odd at first, but no offsets to get deleted. It's become second
nature to me, because there is no doubt about the values being what I want
them to be.

For example, coordinate system G54 you want to be x0 y0 z0. You're
looking at the actual position display, and 'relative' coords selected.

From MDI type: G10 L2 P1 x0 y0 z0 (or x0.100 y-0.100)

The numbers displayed are the offsets from machine absolute zero to x0 y0
z0. (or x0.100 y-0.100) For example's sake, I'll say the GUI axes display
now reads X=1.111 Y=2.222 Z=3.333

Re-type (or use arrow keys to move cursor): G10 L2 P1 x1.111 y2.222 z3.333

Voila! The origin is set, and the values are persistent axis offsets. Now
you can use G92 for temp values, and not lose your original origin.

Other EMC things that were strange to me at first:
Files must begin and end with a '%' sign, unless using M2/M30. M2 & M30
may be used, if you like the offsets deleted and everything reset to
defaults when your program finishes. Perhaps you've an errant M2 resetting
things.
Another quirk is to beware of DOS carriage return characters. To clean
an NC program of them from 'konsole' (terminal), type: tr -d \\r <
Your_Dos_format_prog.nc > Your_CR_removed_prog.nc
Once aware of it, you can find the post-processor settings that output
it correctly.
Beware when in F3/Manual mode! If you are holding down an arrow key, and
at the same time press another axis jog key, the first axis will go on by
itself when you release its' key. Hitting the key again will stop the
motion, but it is surprising.

Fred's point was a good one - normal machine Z absolute zero is the position
with the most distance between spindle and table. In which case a Z0
absolute is a fully retracted spindle, or fully lowered table.

Hope this helps,

Keith

> Ok, let me put this question another way:
>
> I am generating absolute coordinate G-code (i.e. if I do a "G0X1.0"
> followed by a "G0X0.0", I expect to be at x=0).
>
> I am using an edge finder to set my workpiece (0,0,0) point. In this
> coordinate frame, z=0 has the tool touching the top of the workpiece (so
> all negative Z coordinates are inside the material, and positive Z
> coordinates are above it.) In this coordinate frame, the centerline of
> the tool is lined up with the lower left corner of the material.
>
> What steps do I need to perform so that when I reach a line in my program
> that says "G0 X0.000 Y0.000 Z0.000", the tool moves to the workpiece
> (0,0,0) point?
>
> Tom
>
>