Re: [Emc-users] end of program
On Wednesday 17 December 2008, Ray Henry wrote: > (1) What you are describing was addressed when an attempt was made to > allow integrators the ability to set these behaviors by parameter > changes. I've argued for such things for years and a first stab at it > was made by Keith Rumley about three+ years ago on the BDI versions. > You could see his revisions in CVS. Minor correction - The changes were made on a branch of the original EMC code. The bug fixes were merged in to the BDI-4 branch of emc2, but possibly not in to the main trunk. > IMO the proper way to handle these things will require a major rework > and expansion of the EMC2 task planning code. Offsets are predominantly in the realm of the interpreter and have little to do with the task planner. > (2) A related ability, suspending a program using abort or some such > then switching to manual and moving to allow the replacement of a broken > or worn tool, has been discussed at some length. A similar issue is > raised with auto tool wear sensing. Now this does require changes at the task planner level, and also in the trajectory planner - Manual moves & unplanned tool changes opens up a number of problems associated with tool offsets. > IMO there is a solution to this and several other "issues" but it would > require a significant revision of the interpreter code. There is/was an extensible interpreter being worked on that allowed for custom G/M codes via a config file - The intent was to provide different "personalities" to emulate various controls (i.e. Fanuc or Heidenhain) along with closer coupling of PLC functions.. -- SF.Net email is Sponsored by MIX09, March 18-20, 2009 in Las Vegas, Nevada. The future of the web can't happen without you. Join us at MIX09 to help pave the way to the Next Web now. Learn more and register at http://ad.doubleclick.net/clk;208669438;13503038;i?http://2009.visitmix.com/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] end of program
On Tue, 2008-12-16 at 22:44 -0600, Len Shelton wrote: > With the method that Ray described with G92.2 and > G92.3, its still several un-necessary steps I think. I mean, what if it is > the first time you run the program? Would you have to set the offsets with > G92 in MDI and then save with G92.2 in MDI, then place G92.3 at the > beginning of every file? All of the offsets used by EMC are defined when it starts up. They are assigned the values that their variables hold in the var and tbl files. A call to restore g92 values will assign them zero values if the relevant g92 values are zero. For that reason you don't need to worry much about a first encounter with g92.3 in a program unless you change these offsets and they are saved when EMC2 shuts down. If you have set g92 values in manual or MDI mode before you start your program, and that program has a g92.3 near the start, you don't loose anything. It simply rereads them from the status structure which holds the current values you previously set. There are a couple of gotchas that are described in detail in the g92 doc I wrote a few years ago. http://www.linuxcnc.org/dropbox/g92test1.pdf (This doc was not intended for bedside reading.) (1) What you are describing was addressed when an attempt was made to allow integrators the ability to set these behaviors by parameter changes. I've argued for such things for years and a first stab at it was made by Keith Rumley about three+ years ago on the BDI versions. You could see his revisions in CVS. IMO the proper way to handle these things will require a major rework and expansion of the EMC2 task planning code. (2) A related ability, suspending a program using abort or some such then switching to manual and moving to allow the replacement of a broken or worn tool, has been discussed at some length. A similar issue is raised with auto tool wear sensing. IMO there is a solution to this and several other "issues" but it would require a significant revision of the interpreter code. HTH Rayh -- SF.Net email is Sponsored by MIX09, March 18-20, 2009 in Las Vegas, Nevada. The future of the web can't happen without you. Join us at MIX09 to help pave the way to the Next Web now. Learn more and register at http://ad.doubleclick.net/clk;208669438;13503038;i?http://2009.visitmix.com/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] end of program
Len, Take the time to learn G54,G55 etc offsets. Once you learn them you will NEVER want to use anything else. try this assuming your home position the center of your table in XY and the Z up position put this next line on the first line of your program G10 L2 P2 X-1.0 Y-1.0 Z-1.0 put G55 on the second line - it doesn't have to be on the second line - you can put it on the first motion line the G10 line doesn't have to be in the first line - it writes the XYZ values into the parameters for G55 your zero will be the coordinates X-1.0 Y-1.0 Z-1.0 (from home position) home your machine and start your program play with the numbers to see what effect they have on the zero position L3 is G56 L4 is G57 On Tue, Dec 16, 2008 at 10:44 PM, Len Shelton wrote: > Thanks, but no. I still want to just end the program where it sets the stop > button so to speak, without jacking with my offsets, and restoring manual > control. > > And without me having to save my offsets, and then restore them at the > beginning of the file. With the method that Ray described with G92.2 and > G92.3, its still several un-necessary steps I think. I mean, what if it is > the first time you run the program? Would you have to set the offsets with > G92 in MDI and then save with G92.2 in MDI, then place G92.3 at the > beginning of every file? > > It'd be less tedious if I could just end the program, leave my offsets as > they were, jog the head out of the way (without having to hit the stop > button first), swap the stock, then hit start again. > > I could write the routine into the postprocessor to do what I need (maybe), > but I use the same CAM software for different purposes where the retract > vector is different depending on which machine and which operation. > > Let me also point out I have been a long time user of EMC (love it!), but I > just recently started using home switches and I am searching for their > usefulness. Previously without home switches, I just zeroed off of a part, > and never had to jack with offsets. At this point, they make no sense and > are cumbersome to have. I am hoping that there's just some connection I am > not making and it will all of a sudden make sense once I get that clue that > connects the dots. > >>Len > > -Original Message- > From: Chris Radek [mailto:ch...@timeguy.com] > Sent: Tuesday, December 16, 2008 9:52 PM > To: Enhanced Machine Controller (EMC) > Subject: Re: [Emc-users] end of program > > On Tue, Dec 16, 2008 at 08:23:38PM -0600, Len Shelton wrote: >> I pulled M60 from this documentation: >> http://linuxcnc.org/docs/html/gcode_main.html#sub:M0,-M1,-M2, > > Oh! My mistake - I was trying G60 instead of M60. > > Have any of the answers given you a solution to the original > problem? > > Chris > > > -- > SF.Net email is Sponsored by MIX09, March 18-20, 2009 in Las Vegas, Nevada. > The future of the web can't happen without you. Join us at MIX09 to help > pave the way to the Next Web now. Learn more and register at > http://ad.doubleclick.net/clk;208669438;13503038;i?http://2009.visitmix.com/ > ___ > Emc-users mailing list > Emc-users@lists.sourceforge.net > https://lists.sourceforge.net/lists/listinfo/emc-users > > > -- > SF.Net email is Sponsored by MIX09, March 18-20, 2009 in Las Vegas, Nevada. > The future of the web can't happen without you. Join us at MIX09 to help > pave the way to the Next Web now. Learn more and register at > http://ad.doubleclick.net/clk;208669438;13503038;i?http://2009.visitmix.com/ > ___ > Emc-users mailing list > Emc-users@lists.sourceforge.net > https://lists.sourceforge.net/lists/listinfo/emc-users > > -- SF.Net email is Sponsored by MIX09, March 18-20, 2009 in Las Vegas, Nevada. The future of the web can't happen without you. Join us at MIX09 to help pave the way to the Next Web now. Learn more and register at http://ad.doubleclick.net/clk;208669438;13503038;i?http://2009.visitmix.com/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] end of program
Thanks, but no. I still want to just end the program where it sets the stop button so to speak, without jacking with my offsets, and restoring manual control. And without me having to save my offsets, and then restore them at the beginning of the file. With the method that Ray described with G92.2 and G92.3, its still several un-necessary steps I think. I mean, what if it is the first time you run the program? Would you have to set the offsets with G92 in MDI and then save with G92.2 in MDI, then place G92.3 at the beginning of every file? It'd be less tedious if I could just end the program, leave my offsets as they were, jog the head out of the way (without having to hit the stop button first), swap the stock, then hit start again. I could write the routine into the postprocessor to do what I need (maybe), but I use the same CAM software for different purposes where the retract vector is different depending on which machine and which operation. Let me also point out I have been a long time user of EMC (love it!), but I just recently started using home switches and I am searching for their usefulness. Previously without home switches, I just zeroed off of a part, and never had to jack with offsets. At this point, they make no sense and are cumbersome to have. I am hoping that there's just some connection I am not making and it will all of a sudden make sense once I get that clue that connects the dots. >Len -Original Message- From: Chris Radek [mailto:ch...@timeguy.com] Sent: Tuesday, December 16, 2008 9:52 PM To: Enhanced Machine Controller (EMC) Subject: Re: [Emc-users] end of program On Tue, Dec 16, 2008 at 08:23:38PM -0600, Len Shelton wrote: > I pulled M60 from this documentation: > http://linuxcnc.org/docs/html/gcode_main.html#sub:M0,-M1,-M2, Oh! My mistake - I was trying G60 instead of M60. Have any of the answers given you a solution to the original problem? Chris -- SF.Net email is Sponsored by MIX09, March 18-20, 2009 in Las Vegas, Nevada. The future of the web can't happen without you. Join us at MIX09 to help pave the way to the Next Web now. Learn more and register at http://ad.doubleclick.net/clk;208669438;13503038;i?http://2009.visitmix.com/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- SF.Net email is Sponsored by MIX09, March 18-20, 2009 in Las Vegas, Nevada. The future of the web can't happen without you. Join us at MIX09 to help pave the way to the Next Web now. Learn more and register at http://ad.doubleclick.net/clk;208669438;13503038;i?http://2009.visitmix.com/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] end of program
On Tue, Dec 16, 2008 at 08:23:38PM -0600, Len Shelton wrote: > I pulled M60 from this documentation: > http://linuxcnc.org/docs/html/gcode_main.html#sub:M0,-M1,-M2, Oh! My mistake - I was trying G60 instead of M60. Have any of the answers given you a solution to the original problem? Chris -- SF.Net email is Sponsored by MIX09, March 18-20, 2009 in Las Vegas, Nevada. The future of the web can't happen without you. Join us at MIX09 to help pave the way to the Next Web now. Learn more and register at http://ad.doubleclick.net/clk;208669438;13503038;i?http://2009.visitmix.com/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] end of program
I pulled M60 from this documentation: http://linuxcnc.org/docs/html/gcode_main.html#sub:M0,-M1,-M2, Where it says: To exchange pallet shuttles and then stop a running program temporarily (regardless of the setting of the optional stop switch), program M60. It indeed does only "stop the program temporarily" (read "pause"). After which I have to actually hit the stop button to regain manual control over the machine. >Len -Original Message- From: Chris Radek [mailto:ch...@timeguy.com] Sent: Tuesday, December 16, 2008 1:48 PM To: Enhanced Machine Controller (EMC) Subject: Re: [Emc-users] end of program On Tue, Dec 16, 2008 at 11:10:32AM -0600, Len Shelton wrote: > Okay - the errors went away, but M60 only stops the program temporarily. I > sill have to hit the stop button in Axis to be able to jog the machine. I > want a full stop, like M30, but without resetting my offsets. > > Any ideas? Now you've lost me. M60 (and guessing it was a typo, M6) are not even valid codes. Can you start again at the beginning and say what you're trying to do? What offsets are you talking about? Ray asked this too. We may be trying to answer the wrong question. -- SF.Net email is Sponsored by MIX09, March 18-20, 2009 in Las Vegas, Nevada. The future of the web can't happen without you. Join us at MIX09 to help pave the way to the Next Web now. Learn more and register at http://ad.doubleclick.net/clk;208669438;13503038;i?http://2009.visitmix.com/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- SF.Net email is Sponsored by MIX09, March 18-20, 2009 in Las Vegas, Nevada. The future of the web can't happen without you. Join us at MIX09 to help pave the way to the Next Web now. Learn more and register at http://ad.doubleclick.net/clk;208669438;13503038;i?http://2009.visitmix.com/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] end of program
On Tue, Dec 16, 2008 at 01:51:10PM -0600, Len Shelton wrote: > I've been using G92. I still haven't wrapped my head around the point of the > G54 type coordinate systems. If using a vise with a vise stop or a jig that > isn't guaranteed to be in the same place every time you mount it, what's the > point? > > I know I am probably missing something obvious... Three things: You can recover an unapplied G92 offset with G92.3 You can keep the G92 from getting unapplied by using % instead of M2/M30 You can use G54 offset just as easily, or more easily, than G92 by using "Touch off" in AXIS. This is by far the best solution in my opinion. -- SF.Net email is Sponsored by MIX09, March 18-20, 2009 in Las Vegas, Nevada. The future of the web can't happen without you. Join us at MIX09 to help pave the way to the Next Web now. Learn more and register at http://ad.doubleclick.net/clk;208669438;13503038;i?http://2009.visitmix.com/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] end of program
I've been using G92. I still haven't wrapped my head around the point of the G54 type coordinate systems. If using a vise with a vise stop or a jig that isn't guaranteed to be in the same place every time you mount it, what's the point? I know I am probably missing something obvious... >Len -Original Message- From: Ray Henry [mailto:rehe...@copper.net] Sent: Tuesday, December 16, 2008 11:24 AM To: Enhanced Machine Controller (EMC) Subject: Re: [Emc-users] end of program What kind of offsets are these that you are trying to save? G92 offsets have a procedure for saving and recalling. G54-59.3 are saved. On Tue, 2008-12-16 at 11:10 -0600, Len Shelton wrote: > Okay - the errors went away, but M60 only stops the program temporarily. I > sill have to hit the stop button in Axis to be able to jog the machine. I > want a full stop, like M30, but without resetting my offsets. > > Any ideas? > > >Len -- SF.Net email is Sponsored by MIX09, March 18-20, 2009 in Las Vegas, Nevada. The future of the web can't happen without you. Join us at MIX09 to help pave the way to the Next Web now. Learn more and register at http://ad.doubleclick.net/clk;208669438;13503038;i?http://2009.visitmix.com/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- SF.Net email is Sponsored by MIX09, March 18-20, 2009 in Las Vegas, Nevada. The future of the web can't happen without you. Join us at MIX09 to help pave the way to the Next Web now. Learn more and register at http://ad.doubleclick.net/clk;208669438;13503038;i?http://2009.visitmix.com/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] end of program
On Tue, Dec 16, 2008 at 11:10:32AM -0600, Len Shelton wrote: > Okay - the errors went away, but M60 only stops the program temporarily. I > sill have to hit the stop button in Axis to be able to jog the machine. I > want a full stop, like M30, but without resetting my offsets. > > Any ideas? Now you've lost me. M60 (and guessing it was a typo, M6) are not even valid codes. Can you start again at the beginning and say what you're trying to do? What offsets are you talking about? Ray asked this too. We may be trying to answer the wrong question. -- SF.Net email is Sponsored by MIX09, March 18-20, 2009 in Las Vegas, Nevada. The future of the web can't happen without you. Join us at MIX09 to help pave the way to the Next Web now. Learn more and register at http://ad.doubleclick.net/clk;208669438;13503038;i?http://2009.visitmix.com/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] end of program
What kind of offsets are these that you are trying to save? G92 offsets have a procedure for saving and recalling. G54-59.3 are saved. On Tue, 2008-12-16 at 11:10 -0600, Len Shelton wrote: > Okay - the errors went away, but M60 only stops the program temporarily. I > sill have to hit the stop button in Axis to be able to jog the machine. I > want a full stop, like M30, but without resetting my offsets. > > Any ideas? > > >Len -- SF.Net email is Sponsored by MIX09, March 18-20, 2009 in Las Vegas, Nevada. The future of the web can't happen without you. Join us at MIX09 to help pave the way to the Next Web now. Learn more and register at http://ad.doubleclick.net/clk;208669438;13503038;i?http://2009.visitmix.com/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] end of program
Okay - the errors went away, but M60 only stops the program temporarily. I sill have to hit the stop button in Axis to be able to jog the machine. I want a full stop, like M30, but without resetting my offsets. Any ideas? >Len -Original Message- From: Chris Radek [mailto:ch...@timeguy.com] Sent: Monday, December 15, 2008 10:40 AM To: Enhanced Machine Controller (EMC) Subject: Re: [Emc-users] end of program On Mon, Dec 15, 2008 at 09:34:53AM -0600, Len Shelton wrote: > Is there a code to just simply end a program? I have a scenario where I > don't want to reset my offsets (M2 or M30) and I don't have a cycle start > button (which makes sense with M60), but I want to jog the machine manually > between runs. Axis keeps warning me that my program doesn't have a percent > sign or end of program, so I thought maybe a percent sign would work, but it > does not. This warning is really annoying. You have to start AND end with the % as stated here: http://www.linuxcnc.org/docs/html/gcode_main.html#cha:Language-Overview -- SF.Net email is Sponsored by MIX09, March 18-20, 2009 in Las Vegas, Nevada. The future of the web can't happen without you. Join us at MIX09 to help pave the way to the Next Web now. Learn more and register at http://ad.doubleclick.net/clk;208669438;13503038;i?http://2009.visitmix.com/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- SF.Net email is Sponsored by MIX09, March 18-20, 2009 in Las Vegas, Nevada. The future of the web can't happen without you. Join us at MIX09 to help pave the way to the Next Web now. Learn more and register at http://ad.doubleclick.net/clk;208669438;13503038;i?http://2009.visitmix.com/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] end of program
On Mon, Dec 15, 2008 at 09:34:53AM -0600, Len Shelton wrote: > Is there a code to just simply end a program? I have a scenario where I > don't want to reset my offsets (M2 or M30) and I don't have a cycle start > button (which makes sense with M60), but I want to jog the machine manually > between runs. Axis keeps warning me that my program doesn't have a percent > sign or end of program, so I thought maybe a percent sign would work, but it > does not. This warning is really annoying. You have to start AND end with the % as stated here: http://www.linuxcnc.org/docs/html/gcode_main.html#cha:Language-Overview -- SF.Net email is Sponsored by MIX09, March 18-20, 2009 in Las Vegas, Nevada. The future of the web can't happen without you. Join us at MIX09 to help pave the way to the Next Web now. Learn more and register at http://ad.doubleclick.net/clk;208669438;13503038;i?http://2009.visitmix.com/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
[Emc-users] end of program
Is there a code to just simply end a program? I have a scenario where I don't want to reset my offsets (M2 or M30) and I don't have a cycle start button (which makes sense with M60), but I want to jog the machine manually between runs. Axis keeps warning me that my program doesn't have a percent sign or end of program, so I thought maybe a percent sign would work, but it does not. This warning is really annoying. >Len -- SF.Net email is Sponsored by MIX09, March 18-20, 2009 in Las Vegas, Nevada. The future of the web can't happen without you. Join us at MIX09 to help pave the way to the Next Web now. Learn more and register at http://ad.doubleclick.net/clk;208669438;13503038;i?http://2009.visitmix.com/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
