On 9 October 2013 06:40, Richard Thornton <richie.thorn...@gmail.com> wrote:
> X 0-550 home 275
> Y 0-400 home 200
> Z 0-60 home 5
> Program exceeds machine minimum on axis x
> Program exceeds machine minimum on axis y
> Program exceeds machine minimum on axis z
> Linear move on line 7 would exceed joint 0's negative limit
The problem is that the machine thinks that the G-code lies outside
its limits. If you look in the graphical preview you will see a red
box, this is where the machine thinks that its limits are.
You need to ensure that its view of the situation is accurate.
There are two stages to go through here. One of them is normally
automatic, and happens during the homing sequence, the second is part
of setting up for the current job.
The first thing you need to do is home the machine. As you don't have
home switches you need to jog the machine to the specified home
position (275,200,5) and then home each axis via the GUI. This tells
the controller where the machine is on each physical axis. ("Homing"
basically means telling the machine that the current axis physical
location matches the "HOME" location in the INI file. You can use
labels on the axes, or pointers. scribed marks or a datum block or
anything for this part.
LinuxCNC now knows where the ends of travel of the physical axes are,
and can avoid running in to them.
There is an alternative to this. You can set the NO_FORCE_HOMING
option in the INI file. If you do this then the machine will assume
that wherever it is can be called machine-coordinate home. In this
case you probably want to make the axis limits at least twice as large
as the physical limits. (to account for the machine being powered up
anywhere in the work envelope, and still being able to reach anywhere
else.
If there is any danger at all of your machine hurting itself against
the end stops I would discourage the NO_FORCE_HOMING option.
Once the machine is homed you then need to tell it where the workpiece
is. This is the "touch off" stage. If you are using the Axis GUI then
you will see an XYZ triad on the display, this shows the (0,0,0)
location that the G-code is referenced to. This is almost never the
same as the machine (0,0,0) You should jog the (possibly imaginary)
cutter to a point on the (possibly imaginary) workpiece that matches
the origin of the G-code and use the "Touch off" button to set the
axis positions,
For more accuracy you can follow this process. Jog the cutter close to
the work in the axis being set. Hold a dowel (I use a broken 6mm
milling cutter) against the side of the tool, then slowly jog away
until the dowel slides underneath. Then touch-off and type the dowel
diameter in the box.
--
atp
If you can't fix it, you don't own it.
http://www.ifixit.com/Manifesto
------------------------------------------------------------------------------
October Webinars: Code for Performance
Free Intel webinars can help you accelerate application performance.
Explore tips for MPI, OpenMP, advanced profiling, and more. Get the most from
the latest Intel processors and coprocessors. See abstracts and register >
http://pubads.g.doubleclick.net/gampad/clk?id=60134071&iu=/4140/ostg.clktrk
_______________________________________________
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users
