looks like there are some numbered params listed in the master doc also: #<_x> - Return absolute machine X coordinate. Same as #5420. #<_y> - Return absolute machine Y coordinate. Same as #5421. #<_z> - Return absolute machine Z coordinate. Same as #5422. #<_a> - Return absolute machine A coordinate. Same as #5423. #<_b> - Return absolute machine B coordinate. Same as #5424. #<_c> - Return absolute machine C coordinate. Same as #5425. #<_u> - Return absolute machine U coordinate. Same as #5426. #<_v> - Return absolute machine V coordinate. Same as #5427. #<_w> - Return absolute machine W coordinate. Same as #5428. #<_current_tool> - Return number of the current tool in spindle. Same as #5400.
i wonder if these are also effected in the released versions? this is more like what i was imagining might be the access to various states of machine and loaded table values like tool offset values. on many milling machine controllers, G43 Hxxx requires a movement of the z axis to'take up' the tool length offset, like G0 G43 Z-3.0 H5. at the end of the move (which differs from the commanded -3.0 units by the length offset value in offset table position number 5) the end of the tool is aligned with the currnt coordinate system. if you know the parameter locations of the current tool and its length offset, the code for taking up the current tool offset becomes G0 G43 Z-#[<current tool number> + <tool length table parameter offset>] H#[<current tool number> + <tool length table parameter offset>]. so there is no axis movement, and that coding step in a tool introduction is uniform for all tools, regardless of length. (the tool change is often near the travel limit of the z axis, so a large tool offset might result in an overtravel if the axis movement is not large enough. so in the first example, G0 G43 Z-3.0 H5, if H5=10.00 and there is only another +1.0 to go in the z axis beyond the tool change position, the limit will be reached 6.0 short of completing this step.) at the place i have been working, all the mill controllers have been set up with a macro override of the T word that encapsulates all the discreet coding steps required for MDI tool changing, as well as part programming. the result is improved setup time on the machine, and faster part operation coding which is portable between the various different machines. another handy macro (call it G192 for example) finds the center of two touch off locations along an axis. the procedure goes like, touch the -x edge of the part with edge finder G92 X0 touch the +x edge of part G192 X0 (<- "X0" is just convenient, the X-word value is not used in the calculation.) where the G192 macro uses the machine coorinate parameter values of the selected axis name (X in this example) to set the origin at the center of the part edges. it would be nice to adapt such tactics in linuxcnc, using the custom M codes perhaps? will the custom codes work from MDI? they would at least be valuable for modularization of part programming, like for the tool change routine. command M106 Txx Sxx: (M106 TOOL CHANGE MACRO) M9 G91 G30 Z0 M5 T#5400 M6 S#???? M3 G0 G43 Z-[H#5400] H#5400 G17 G90 M8 M99 ..or something like that. --- On Fri, 3/23/12, Sebastian Kuzminsky <[email protected]> wrote: > From: Sebastian Kuzminsky <[email protected]> > Subject: Re: [Emc-users] Tool change question > To: [email protected] > Date: Friday, March 23, 2012, 9:29 PM > On 03/23/2012 11:42 AM, charles green > wrote: > > nicer, but still only a handful of documented > params. i was looking at a document dated a little > over a year ago (11jan2011). > > > > do you know if the params #31 to #5000 contain useful > info? like g90/g91 state, for example, or any > registration of the other groups apart from group 12? > > > > "you started this. show me everything." - ellen > ripley > > Oh... I don't think you want to mess with > that... - Hicks > > Parameters 31-5000 are deliberately unused by linuxcnc, and > thus > available for the g-code programmer to use. > > Ah yes, that's even what the docs say (somewhat cryptically, > focus on > the "user parameters" part): > > > * > > > > /1-5000/ - G-Code user > parameters. These parameters are global > > in the G Code file. > > > > The (slightly) improved docs in the master branch > (http://linuxcnc.org/docs/devel/html/gcode/overview.html#sec:parameters) > > say this: > > > 31-5000 > > > > G-Code user parameters. These > parameters are global in the G Code > > file, and available for general > use. Volatile. > > > > > Oh hey look! In master (aka devel), there are some > predefined named > parameters that carry the g90/g91 state: > > http://linuxcnc.org/docs/devel/html/gcode/overview.html#_predefined_named_parameters_a_id_sec_predefined_named_parameters_a > > I think those variables are new in the master branch, and > not available > in the 2.5 branch. > > > -- > Sebastian Kuzminsky > > > ------------------------------------------------------------------------------ > This SF email is sponsosred by: > Try Windows Azure free for 90 days Click Here > http://p.sf.net/sfu/sfd2d-msazure > _______________________________________________ > Emc-users mailing list > [email protected] > https://lists.sourceforge.net/lists/listinfo/emc-users > ------------------------------------------------------------------------------ This SF email is sponsosred by: Try Windows Azure free for 90 days Click Here http://p.sf.net/sfu/sfd2d-msazure _______________________________________________ Emc-users mailing list [email protected] https://lists.sourceforge.net/lists/listinfo/emc-users
