There are a bunch of different things that affect the relationship
between machine coordinates and gcode coordinates.
"G5x coordinate systems":
At any time, one G5x coordinate system is in effect. Normally the
G54 coordinate is in effect at emc startup and after readahead
reaches M2.
You can set the offsets of the nine program coordinate systems
using G10 L2 Pn (n is the number of the coordinate system) with
values for the axes in terms of the absolute coordinate system.
G54 corresponds to P1, G55 to P2, and so on.
Generally, G5x offsets are saved even when exiting emc.
"G92 coordinate offset"
The G92 coordinate offset is programmed by G92, and also affected by
M2, G92.1, G92.2 and G92.3 as documented in the gcode manual.
http://linuxcnc.org/docs/html/gcode/main/#sub:G92_-G92.1_-G92.2_
Particularly due to the way the G92 coordinate offset is disabled if
the interpreter readahead reaches M2, many users find that the
behavior of G92 is confusing.
"G43 Tool offset"
When G43 is in effect, the Z coordinate is modified by the tool
length. On lathes, G43 can offset both X and Z
All three of these (G5x coordinate system (one is always in effect), G92
coordinate offset (unless disabled by G92.1 or G92.2), and G43 tool
offset (when enabled)) are combined to get the coordinate value
shown on the AXIS DRO when "Relative" coordinates are selected. When
the "Relative" coordinates are different than the Machine coordinates,
AXIS draws a cyan icon at the machine origin and the tricolor coordinate
system marker at the origin of the relative coordinate system.
"Home" (GUI button):
In a machine with home switches, use these home switches to move the
axis to its home location.
In a machine without home switches, notify emc that the current axis
position has been manually jogged to the home position.
Even in a machine without home switches, you should establish and
use a home position. After homing, the inifile "soft limits" are
applied, so you can be confident that the machine will not walk the
table right off the end of the leadscrew.
After invoking Home, the value shown could be nonzero for several
reasons:
* A coordinate system or offset is being added to the axis value
* The inifile HOME is not 0
"Touch Off" (GUI button):
Touch Off is a way of setting the G54 coordinate system based on the
current location of the axis and the entered value. Touch Off
ignores G93 coordinate offsets even if they are currently in effect.
So if you're lost, what should you do?
* Move to the machine origin. MDI: G53 G0 X0Y0Z0 (A0B0C0)
* Clear the G92 coordinate offset. MDI: G92.1
* Use the G54 coordinate system. MDI: G54
* Set the G54 coordinate system to be identical to the machine
coordinate system. MDI: G10 L2 P1 X0Y0Z0 (A0B0C0)
* Turn off tool offsets. MDI: G49
* Turn on Relative coordinate display from the menu
now, you should be at machine origin (0,0,0), and the relative
coordinate system should be the same as the machine coordinate system.
What should you do to set your origin on material? For each axis,
* Jog to a known or measurable location with respect to the material
* Invoke "Touch Off", and enter the current position with respect to
the material
For example, when I mill circuit boards, (0,0) is almost always the
lower right-hand corner of the board. I jog X and Y to this corner of
the circuit board blank, and Touch Off each one of these and enter a
value of 0. This measurement is almost never critical, as I'm cutting
small boards (typically under 3x4") from a 4x6 blank.
With tool inserted, I move to the approximate middle of the area being
milled. Then using a feeler gauge I jog Z down towards the material,
switching to small incremental moves as I get close. When the feeler
gauge just passes between the board and the tool, I Touch Off and enter
the thickness of the feeler gauge (e.g., 0.0020). I don't have
repeatable tool length, so I don't use G43 while cutting; if I did, I'd
also enable G43 while doing the Z Touch Off.
This got long winded, so if you got this far give yourself a pat on the
back.
Jeff
-------------------------------------------------------------------------
This SF.net email is sponsored by: Microsoft
Defy all challenges. Microsoft(R) Visual Studio 2005.
http://clk.atdmt.com/MRT/go/vse0120000070mrt/direct/01/
_______________________________________________
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users
