Re: g18

[Ray <rehenry-at-up.net>]

Dave

I think that there may be something to the suggestion by Dale.  The new
interpreter document says concerning program end;

-----snipped from linuxcnc.org/handbook/RS274NGC_3/RS274NGC_3TOC.html-----
To end a program, program M2. To exchange pallet shuttles and then end a program, program M30. Both of these commands have the following effects.

 1. Axis offsets are set to zero (like G92.2) and origin offsets are set to the default (like G54). 
 2. Selected plane is set to CANON_PLANE_XY (like G17). 
 3. Distance mode is set to MODE_ABSOLUTE (like G90). 
 4. Feed rate mode is set to UNITS_PER_MINUTE (like G94). 
 5. Feed and speed overrides are set to ON (like M48). 
 6. Cutter compensation is turned off (like G40). 
 7. The spindle is stopped (like M5). 
 8. The current motion mode is set to G_1 (like G1). 
 9. Coolant is turned off (like M9).
-----end of snippet-----

What you might try is setting the xz plane in the ini file right alongside
the inch setting and then restarting the machine. (if you use inch)  See
below.

; Startup codes for RS-274-NGC interpreter
RS274NGC_STARTUP_CODE =	G20 G18

Some of these default actions at the end of a program run have bothered
others as well.  I was kinda wondering if it might be possible to read these
behaviors from ini settings but alas my C reading ability is meager to none.

HTH

Ray


On Tue, 21 Aug 2001, you wrote:
> Hi Dave,
> Since I don't have a working machine yet I tried your code in sim mode.  What
> you may be seeing is that an M2 at the end of the program resets the control
> back to G17. The code snippit you posted doesn't have a G18 at the beginning.
> With G18 active G3 is a counterclockwise arc as viewed from the positive side,
> viewed from the negative side it is clockwise. A program end appears to reset to
> G17 and your snippit entered as posted will cut a counterclockwise arc in the xy
> plane. If you enter G18 in MDI it should work same as the program does in AUTO.
> Dale
> 
> Dave Engvall wrote:
> 
> > List,
> >
> > I am working in xz plane with g18.
> >
> > Snippet:
> >     g01 z .1 f 15
> >     x 0
> >     z -.184
> >     y .1908
> >     g03 x 2.249 z - 1.3584  r 2.55 f5
> >     g01 z .1 f 15
> > ...........
> >     m2
> > This snippet occurs several times with various y offsets to create a
> > surface.
> >
> > If one thinks about a disk lying in the xz plane then this creates a surface
> > from the top center of the disk and going to the right and down (top surface
> > or radii of the disk, i.e. CW ).
> >
> > Now at the end of the program...either do m0 and shift to mdi or m2 and go
> > to mdi.
> > Enter the same snippet line by line. The g03 now does a COUNTERCLOCKWISE
> > cut. Surprise!!!
> >
> > Certainly glad I was testing this in pink foam not steel.
> >
> > BTW- this is repeatable at least on my machine...600 MHz P3, 2.0.36, 09J.
> > Mar 2000 emc.
> >
> > I would appreciate someone else trying this.
> >
> > Thanks,
> >
> > Dave Engvall