Re: [CAD_CAM_EDM_DRO] Question Re: Work Offsets

Ok, between this and Fred's reply I've got some stuff to try tonight when
I get home.

I'm using Vector for generating g-code. Right now it's using the stock
3-axis ISO model. Nothing at the head, nothing at the tail unless I put
it there. So I'm pretty sure I don't have an errant G54-G59.3 in there
anywhere (but you can betcha I'm going to check tonight when I get home!)

I *was* ending my programs with M2, which may be what's clearing things.

What's odd is it isn't acting like the offsets are being cleared. If I
right-click and set each axis to zero, the Work Offsets line picks them
up. Running a program seems to put it in absolute machine coordinates
rather than relative work coordinates. The offsets are still there. I
can see them on the Work Offsets line. It's just not using them.

Right now I'm after consistant results, whatever those may be. If it's
going to behave in a predictable way, that'll at least keep me from
breaking any more tools and wrecking any more material.

Thanks for all the help. I'll play with it tonight, given Fred and
Kieth's ideas, and see what I come up with.

Tom

On Thu, 12 Jun 2003, Keith Rumley wrote:

> 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
> >
> >
>
>
> Addresses:
> FAQ: http://www.ktmarketing.com/faq.html
> FILES: http://groups.yahoo.com/group/CAD_CAM_EDM_DRO/files/
> Post Messages: CAD_CAM_EDM_DRO@yahoogroups.com
>
> Subscribe: CAD_CAM_EDM_DRO-subscribe@yahoogroups.com
> Unsubscribe: CAD_CAM_EDM_DRO-unsubscribe@yahoogroups.com
> List owner: CAD_CAM_EDM_DRO-owner@yahoogroups.com, wanliker@..., timg@...
> Moderator: pentam@... indigo_red@... [Moderators]
> URL to this group: http://groups.yahoo.com/group/CAD_CAM_EDM_DRO
>
> OFF Topic POSTS: General Machining
> If you wish to post on unlimited OT subjects goto: aol://5863:126/rec.crafts.metalworking or go thru Google.com to reach it if you have trouble.
> http://www.metalworking.com/news_servers.html
>
> http://groups.yahoo.com/group/jobshophomeshop I consider this to be a sister site to the CCED group, as many of the same members are there, for OT subjects, that are not allowed on the CCED list.
>
> NOTICE: ALL POSTINGS TO THIS GROUP BECOME PUBLIC DOMAIN BY POSTING THEM. DON'T POST IF YOU CAN NOT ACCEPT THIS.....NO EXCEPTIONS........
> bill
> List Mom
> List Owner
>
>
>
> Your use of Yahoo! Groups is subject to http://docs.yahoo.com/info/terms/
>
>