Craig, The D word is optional with G41/G42 and is equal to the tool number for which the path is to be compensated. If a D value is not given explicitly the value for the currently loaded tool it used. I can't think if an instance when you would want to compensate for a tool that was not in the spindle, and it seems like specifying the wrong D would be an easy way to trash a part! My guess would be that the D word is rarely used with G41/G42.
You might be thinking of G41.1/G42. for which a D value is required, though in this case the D value is the actual cutter diameter instead the tool number. I believe Todd is only using G41/G42, so the D value is indeed not needed. In the code Todd posted the compensation lead in was greater than the radius of the tool, so no problem there either. I don't think this is a bug, I think we may just not quite understand the way cutter comp combined with an abnormally high value of Q behaves. I am still mystified as to why blending seems to be disabled with G41/G42 though. I need to so some more experimenting but I took the mill apart again, so that will have to wait! Thanks, Kurt *Kurt Jacobson, CMfgT* Mechanical / Manufacturing Engineer Center for Nuclear Studies | Southern Polytechnic College of Engineering Kennesaw State University | Marietta Campus E-mail: kurtcjacob...@gmail.com On Fri, Feb 17, 2017 at 5:42 PM, Craig Hodne <hsm...@yahoo.com> wrote: > The G41 and G42 require the use of the D-word. The D word refers to the > line in the tool table where the diameter of the tool is to be read. It > is often the same line as the tool number, but it doesn't have to be. > The second qualifier is the travel of the tool from invoking the G41 or > G42 must be greater than the radius of the tool. > > Craig > > > On 02/17/2017 12:44 PM, emc-users-requ...@lists.sourceforge.net wrote: > > Subject: > > Re: [Emc-users] G41-42 and G64 Bug?q > > From: > > "Todd Zuercher" <zuerc...@embarqmail.com> > > Date: > > 02/17/2017 10:38 AM > > > > To: > > "Enhanced Machine Controller (EMC)" <emc-users@lists.sourceforge.net> > > > > > > Another odd bug like behavior I am seeing. > > Set up a tool in the tool table with an extremely small diameter, load > that tool, and run the g-code below with the optional block skip on and > then again with it off. > > > > G64 > > G43 > > G0 X1.5 Y.375 Z1 > > /G41 > > G1X1Y.5Z.5 > > G1X0.5 > > G2 X4.5 I2 J0 > > G1 X0.75 > > G0Z1 > > G40 > > > > Notice how having G41 turned on seems to shut off blending. Why is that? > > > > ----- Original Message ----- > > From: "Todd Zuercher"<zuerc...@embarqmail.com> > > To: "Enhanced Machine Controller (EMC)"<emc-users@lists.sourceforge.net> > > Sent: Friday, February 17, 2017 11:25:06 AM > > Subject: Re: [Emc-users] G41-42 and G64 Bug?q > > > > The small radius "is" the tool radius, and it was created by Linuxcnc > when it created the G41 tool offset. > > > > ----- Original Message ----- > > From: "Jim Craig"<jimcraig5...@windstream.net> > > To:emc-users@lists.sourceforge.net > > Sent: Friday, February 17, 2017 9:27:23 AM > > Subject: Re: [Emc-users] G41-42 and G64 Bug?q > > > > Todd, > > > > Is the cutter radius larger than the small radius transitioning from > > the straight line to the semicircle. would this cause the issue? > > Grasping at straws here as I don't use G41/G42. > > > > I guess I don't understand why the small arc radius is being shown at > > all in white if the below code is the programmed path. > > > > Jim > > > > On 2/16/2017 3:04 PM, Todd Zuercher wrote: > >> Maybe, it is or isn't a problem. > >> The g-code is only: > >> > >> G43 > >> G0 X1.5 Y.375 Z1 > >> G41 > >> G1X1Y.5Z.5 > >> G1X0.5 > >> G2 X4.5 I2 J0 > >> G1 X0.75 > >> G0Z1 > >> G40 > >> > >> It runs perfectly fine without the G41 reguardless of the G64 setting. > I guess the planner must see that arc in the transition from one line to > the next in G41 and the Q is acting it, even though it isn't actually > written in the g-code. > >> Something else to remember when using tool comp. > > ------------------------------------------------------------ > ------------------ > Check out the vibrant tech community on one of the world's most > engaging tech sites, SlashDot.org! http://sdm.link/slashdot > _______________________________________________ > Emc-users mailing list > Emc-users@lists.sourceforge.net > https://lists.sourceforge.net/lists/listinfo/emc-users > ------------------------------------------------------------------------------ Check out the vibrant tech community on one of the world's most engaging tech sites, SlashDot.org! http://sdm.link/slashdot _______________________________________________ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
