Re: [Emc-users] Tool Offsets
On Wed, 23 May 2012 06:45:22 -0500, you wrote: Good point, are there any two controls from different manufacturers that are completely portable between each other? Unfortunately not in my experience. I know from reading my CNC g code manuals from other machines that I have that even generation to generation of the same controller the g code is not portable. Fanuc G So the question is do you cobble up your software just to be portable when no one else seems to do this... Just open up the list of post processors on most cam software and you see hundreds of choices usually... There's hundreds in my copy of FeatureCam. It's a PITA. I do some Gcode optimisation for a few engineering companies that farm some of their work out and getting the right post processor that works is problematic and it's often the small things that catch you out. As Stuart says the integrator often changes things too, so you can't even rely on a stock post processor :( However, both LinuxCNC and Mach used the same base for their code and the radically different behaviour of not stipulating the H value on a G43 can be disastrous as I know from bitter experience. LinuxCNC - not using the H value loads the offset for the current tool. Mach3 - not using the H value sets the tool offset to zero ! The Fanuc style where the H value must be stipulated is much safer. Steve Blackmore -- -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
On 5/24/2012 2:50 AM, Steve Blackmore wrote: On Wed, 23 May 2012 06:45:22 -0500, you wrote: Good point, are there any two controls from different manufacturers that are completely portable between each other? Unfortunately not in my experience. I know from reading my CNC g code manuals from other machines that I have that even generation to generation of the same controller the g code is not portable. FanucG So the question is do you cobble up your software just to be portable when no one else seems to do this... Just open up the list of post processors on most cam software and you see hundreds of choices usually... There's hundreds in my copy of FeatureCam. It's a PITA. I do some Gcode optimisation for a few engineering companies that farm some of their work out and getting the right post processor that works is problematic and it's often the small things that catch you out. As Stuart says the integrator often changes things too, so you can't even rely on a stock post processor :( However, both LinuxCNC and Mach used the same base for their code and the radically different behaviour of not stipulating the H value on a G43 can be disastrous as I know from bitter experience. LinuxCNC - not using the H value loads the offset for the current tool. Mach3 - not using the H value sets the tool offset to zero ! The Fanuc style where the H value must be stipulated is much safer. Steve Blackmore -- Pure speculation on my part, but I wonder if there are enough rules of thumb known to justify writing a code checker that could alert a user to potential gotchas with a particular G-code file with LinuxCNC. Obviously, the more cross-system knowledge like yours, Steve, the better. Students armed with knowledge-based expert-system tools used to eat this kind of problem for breakfast in the 1980s when every engineering school added an intro course in expert systems. In this case simple decision logic trees would suffice. Regards, Kent -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
On 24 May 2012 07:50, Steve Blackmore st...@pilotltd.net wrote: LinuxCNC - not using the H value loads the offset for the current tool. Mach3 - not using the H value sets the tool offset to zero ! Eeek! Well, there is something lurking to catch me out in a big way if ever I try using Mach. M6T4G43 is something I just type automatically in MDI much of the time. -- atp If you can't fix it, you don't own it. http://www.ifixit.com/Manifesto -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
On Tue, 22 May 2012 05:38:16 -0500, you wrote: Why does it matter how other controls work? Portability of Gcode between different controls. Steve Blackmore -- -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
Good point, are there any two controls from different manufacturers that are completely portable between each other? I know from reading my CNC g code manuals from other machines that I have that even generation to generation of the same controller the g code is not portable. You would think that the simple G0 would be the same between controllers but that is not the case, some of my machines Z up before doing the XY move and if Z is down do the XY move before the Z move and some do a straight linear move... So the question is do you cobble up your software just to be portable when no one else seems to do this... Just open up the list of post processors on most cam software and you see hundreds of choices usually... John On 5/23/2012 2:48 AM, Steve Blackmore wrote: On Tue, 22 May 2012 05:38:16 -0500, you wrote: Why does it matter how other controls work? Portability of Gcode between different controls. Steve Blackmore -- -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
All of the controls allow the integrator to determine the exact treatment of all of the symbolic commands. Some of the integrators allow the end user to adjust many (but not usually all) of the parameters to customize the interpretation of the symbolic commands for a particular preference. You may be able to change a parameter to match the G00 Zup/Zdown motion to your expected action. On Wed, May 23, 2012 at 6:45 AM, John Thornton bjt...@gmail.com wrote: Good point, are there any two controls from different manufacturers that are completely portable between each other? I know from reading my CNC g code manuals from other machines that I have that even generation to generation of the same controller the g code is not portable. You would think that the simple G0 would be the same between controllers but that is not the case, some of my machines Z up before doing the XY move and if Z is down do the XY move before the Z move and some do a straight linear move... So the question is do you cobble up your software just to be portable when no one else seems to do this... Just open up the list of post processors on most cam software and you see hundreds of choices usually... John On 5/23/2012 2:48 AM, Steve Blackmore wrote: On Tue, 22 May 2012 05:38:16 -0500, you wrote: Why does it matter how other controls work? Portability of Gcode between different controls. Steve Blackmore -- -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- dos centavos -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
So then the portability or not of say my Anilam 1100m depends on the integrator? No wonder there are hundreds of post processors in cam programs... John On 5/23/2012 7:29 AM, Stuart Stevenson wrote: All of the controls allow the integrator to determine the exact treatment of all of the symbolic commands. Some of the integrators allow the end user to adjust many (but not usually all) of the parameters to customize the interpretation of the symbolic commands for a particular preference. You may be able to change a parameter to match the G00 Zup/Zdown motion to your expected action. On Wed, May 23, 2012 at 6:45 AM, John Thorntonbjt...@gmail.com wrote: Good point, are there any two controls from different manufacturers that are completely portable between each other? I know from reading my CNC g code manuals from other machines that I have that even generation to generation of the same controller the g code is not portable. You would think that the simple G0 would be the same between controllers but that is not the case, some of my machines Z up before doing the XY move and if Z is down do the XY move before the Z move and some do a straight linear move... So the question is do you cobble up your software just to be portable when no one else seems to do this... Just open up the list of post processors on most cam software and you see hundreds of choices usually... John On 5/23/2012 2:48 AM, Steve Blackmore wrote: On Tue, 22 May 2012 05:38:16 -0500, you wrote: Why does it matter how other controls work? Portability of Gcode between different controls. Steve Blackmore -- -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
exactly On Wed, May 23, 2012 at 7:46 AM, John Thornton bjt...@gmail.com wrote: So then the portability or not of say my Anilam 1100m depends on the integrator? No wonder there are hundreds of post processors in cam programs... John On 5/23/2012 7:29 AM, Stuart Stevenson wrote: All of the controls allow the integrator to determine the exact treatment of all of the symbolic commands. Some of the integrators allow the end user to adjust many (but not usually all) of the parameters to customize the interpretation of the symbolic commands for a particular preference. You may be able to change a parameter to match the G00 Zup/Zdown motion to your expected action. On Wed, May 23, 2012 at 6:45 AM, John Thorntonbjt...@gmail.com wrote: Good point, are there any two controls from different manufacturers that are completely portable between each other? I know from reading my CNC g code manuals from other machines that I have that even generation to generation of the same controller the g code is not portable. You would think that the simple G0 would be the same between controllers but that is not the case, some of my machines Z up before doing the XY move and if Z is down do the XY move before the Z move and some do a straight linear move... So the question is do you cobble up your software just to be portable when no one else seems to do this... Just open up the list of post processors on most cam software and you see hundreds of choices usually... John On 5/23/2012 2:48 AM, Steve Blackmore wrote: On Tue, 22 May 2012 05:38:16 -0500, you wrote: Why does it matter how other controls work? Portability of Gcode between different controls. Steve Blackmore -- -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- dos centavos -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
To not be different, means that you need to be like one other controller. If you do that, who do you follow? Fanuc? Fanuc has incompatibilities between their various models. I know that Mach3 strives to be somewhat compatible with Fanuc, but the truth is that Fanuc has capabilities well beyond what Mach3 can do, so the code is not portable.It is Fanuc like and that is about it. This is only gong to get worse as new controller features are added by the big CNC makers. Dave On 5/23/2012 7:45 AM, John Thornton wrote: Good point, are there any two controls from different manufacturers that are completely portable between each other? I know from reading my CNC g code manuals from other machines that I have that even generation to generation of the same controller the g code is not portable. You would think that the simple G0 would be the same between controllers but that is not the case, some of my machines Z up before doing the XY move and if Z is down do the XY move before the Z move and some do a straight linear move... So the question is do you cobble up your software just to be portable when no one else seems to do this... Just open up the list of post processors on most cam software and you see hundreds of choices usually... John On 5/23/2012 2:48 AM, Steve Blackmore wrote: On Tue, 22 May 2012 05:38:16 -0500, you wrote: Why does it matter how other controls work? Portability of Gcode between different controls. Steve Blackmore -- -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
Andy, I am not writing to the tool table with gcode, and I can post some code, but I have a question first. I modified the Sim Axis-9 configuration to simulate what I am doing on the real machine. When I run a program using external named subroutines I get one of two errors if I stop the program in the middle, do a motion like G53 G0 X0 Y0 And then run again without reloading. My question is, do named external subroutine files need to end with '%'. If I include a '%' at the end of the file, on rerunning I get an error: Bad character '%' used. If I delete the '%' from the end of the file, I get: File ended with no percent sign or program end. If I do a reload, I do not get this error. Thanks, Eric Can you show us the G-code? Are you writing to the tool table in G-code? I wonder if the software only writes to the tool file on exit? -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
On 23 May 2012 16:52, Eric H. Johnson ejohn...@camalytics.com wrote: Andy, I am not sure I am the one to best answer this. My question is, do named external subroutine files need to end with '%'. If I include a '%' at the end of the file, on rerunning I get an error: Bad character '%' used. I have a feeling that I have heard that there are quirks with subroutines, but I am not sure what they are. I think Michael Haberler probably has the best handle on this, but I am not sure he is around at the moment. -- atp If you can't fix it, you don't own it. http://www.ifixit.com/Manifesto -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
On Wednesday, May 23, 2012 12:40:50 PM andy pugh did opine: On 23 May 2012 16:52, Eric H. Johnson ejohn...@camalytics.com wrote: Andy, I am not sure I am the one to best answer this. My question is, do named external subroutine files need to end with '%'. If I include a '%' at the end of the file, on rerunning I get an error: Bad character '%' used. I have a feeling that I have heard that there are quirks with subroutines, but I am not sure what they are. I think Michael Haberler probably has the best handle on this, but I am not sure he is around at the moment. I found that if you took the instructions for named subroutine file literally, I had no problems of that sort when machine etching my encoder boards. The only problem that bothered me was that the subroutine files did not echo into the code flow being displayed in the lower code window of axis, so the machine was effectively flying blind while the subroutine was executing. These 'canned' subroutines were called and ran as many as 7 times while the main code to do one side of the board was executing. Named for the subroutine call with an appended .ngc, they started with: cat bedautoz.ngc obedautoz sub [...gcode to establish this tools auto z reference and apply it, and ended] obedautoz endsub No M2, or % sign was ever asked for or given. They Just Worked(TM) :) Cheers, Gene -- There are four boxes to be used in defense of liberty: soap, ballot, jury, and ammo. Please use in that order. -Ed Howdershelt (Author) My web page: http://coyoteden.dyndns-free.com:85/gene Duct tape is like the force. It has a light side, and a dark side, and it holds the universe together ... -- Carl Zwanzig -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
On Mon, 21 May 2012 18:04:53 -0700 (PDT), you wrote: I never use the H-number, it is only useful for applying the offset of It may be not useful in LinuxCNC but I guarentee you 90% + of the mill programs in the world use it (Fanuc has to have it) also the Dxx If you omit the D on Fanuc no offset will be applied to G41,G42 Agreed - it should really error if you fail to tell it which offset to apply. Steve Blackmore -- -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
On 22 May 2012 02:04, Terry Christophersen tcninj...@yahoo.com wrote: I never use the H-number, it is only useful for applying the offset of It may be not useful in LinuxCNC but I guarentee you 90% + of the mill programs in the world use it Well, yes, but we are using LinuxCNC. -- atp If you can't fix it, you don't own it. http://www.ifixit.com/Manifesto -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
On Tuesday, May 22, 2012 05:38:32 AM andy pugh did opine: On 22 May 2012 02:04, Terry Christophersen tcninj...@yahoo.com wrote: I never use the H-number, it is only useful for applying the offset of It may be not useful in LinuxCNC but I guarentee you 90% + of the mill programs in the world use it Well, yes, but we are using LinuxCNC. Yep. I was watching a big machine, a 5 axis, doing a 427 ford block from a nearly 400 lb block of alu forging, and was amazed to see it doing the sailors hornpipe jig as it bored the liner holes. We all know that LinuxCNC can do that in one spiral motion, probably 2x faster than that HAAS control was doing it. Blew me away. Cheers, Gene -- There are four boxes to be used in defense of liberty: soap, ballot, jury, and ammo. Please use in that order. -Ed Howdershelt (Author) My web page: http://coyoteden.dyndns-free.com:85/gene I'd love to go out with you, but the man on television told me to stay tuned. -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
Why does it matter how other controls work? John On 5/21/2012 8:04 PM, Terry Christophersen wrote: I never use the H-number, it is only useful for applying the offset of It may be not useful in LinuxCNC but I guarentee you 90% + of the mill programs in the world use it (Fanuc has to have it) also the Dxx If you omit the D on Fanuc no offset will be applied to G41,G42 Terry - Original Message - From: andy pughbodge...@gmail.com To: Enhanced Machine Controller (EMC)emc-users@lists.sourceforge.net Cc: Sent: Monday, May 21, 2012 5:57 PM Subject: Re: [Emc-users] Tool Offsets On 21 May 2012 20:51, Eric H. Johnsonejohn...@camalytics.com wrote: T3 M6 G43 H3 I never use the H-number, it is only useful for applying the offset of a non-loaded tool to the loaded tool. Though I doubt that is your problem. -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
the h number is also useful for code that is explicit. implicit and default treatments are the typical haunts of misbehavior and error. application of ambiguity to machine control command articles may be some kind of requirement for thinking machines. automating a defined, standardized process is not really a good place for custom tribal practices. --- On Mon, 5/21/12, andy pugh bodge...@gmail.com wrote: From: andy pugh bodge...@gmail.com Subject: Re: [Emc-users] Tool Offsets To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net Date: Monday, May 21, 2012, 3:57 PM On 21 May 2012 20:51, Eric H. Johnson ejohn...@camalytics.com wrote: T3 M6 G43 H3 I never use the H-number, it is only useful for applying the offset of a non-loaded tool to the loaded tool. Though I doubt that is your problem. -- atp If you can't fix it, you don't own it. http://www.ifixit.com/Manifesto -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
On Tuesday, May 22, 2012 07:39:37 AM John Thornton did opine: Why does it matter how other controls work? John So you don't have to totally retrain a new hire? Cheers, Gene -- There are four boxes to be used in defense of liberty: soap, ballot, jury, and ammo. Please use in that order. -Ed Howdershelt (Author) My web page: http://coyoteden.dyndns-free.com:85/gene If Microsoft built cars, you would have to press the Start button to turn them off. -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
2012/5/22 John Thornton bjt...@gmail.com: Why does it matter how other controls work? Not to reinvent the wheel and learn from existing examples of good solutions to some problems. -- Viesturs If you can't fix it, you don't own it. http://www.ifixit.com/Manifesto -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
reducing the rtfm overhead would be a nice break also. --- On Tue, 5/22/12, gene heskett ghesk...@wdtv.com wrote: From: gene heskett ghesk...@wdtv.com Subject: Re: [Emc-users] Tool Offsets To: emc-users@lists.sourceforge.net Date: Tuesday, May 22, 2012, 4:40 AM On Tuesday, May 22, 2012 07:39:37 AM John Thornton did opine: Why does it matter how other controls work? John So you don't have to totally retrain a new hire? Cheers, Gene -- There are four boxes to be used in defense of liberty: soap, ballot, jury, and ammo. Please use in that order. -Ed Howdershelt (Author) My web page: http://coyoteden.dyndns-free.com:85/gene If Microsoft built cars, you would have to press the Start button to turn them off. -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
Terry, I am strongly suspecting that it has something to do with named external subroutines. I have used coordinate systems (G54-59, G10 L2, etc.) extensively in the past without any problems. This is the first time I have used the tool table for X, Y, etc. offsets, but the problems I am encountering are similar enough to what I was seeing with coordinate systems that it seems it must be related. The main difference with this application is the extensive use of name subroutines. However there are no motion commands in any of these subroutines, they are mainly for asserting digital outputs, checking inputs, applying dwells, etc. This is on a production machine, so I have limited ability to run tests on it, but I have just put a box together for simulation purposes. I should be able to do some better problem isolation on it over the next couple days. I am open to ideas as to what to look for. Thanks, Eric G49 cancels G43 Se just nd the machine home at the end of the prog using: G28G91Z0.0 Y0.0 X0.0 You should not need to use G49 You must be doing something else wrong Start of every one of my progs look like this: T1M6 G54G90G0XxxYxxS500M3 G43H1Z.1M8 moves the tool down to .1 above the workpiece blah blah ends look like this: G28G91 Z0.0 send the Z home G28G91Y0.0 send the y home to put in a new part M30 -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
On 21 May 2012 20:51, Eric H. Johnson ejohn...@camalytics.com wrote: Per the Setting Coordinate Systems thread, I converted from using coordinate systems (G54-G59.3) and setting the offsets with G10 L2, to using the offsets specified in the tool table. Mostly it worked without a problem. The exception is when re-running a program without reloading it. Can you show us the G-code? Are you writing to the tool table in G-code? I wonder if the software only writes to the tool file on exit? -- atp If you can't fix it, you don't own it. http://www.ifixit.com/Manifesto -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
I agree it is good to learn from other control systems but the wheel is reinvented every day with a better wheel. If not we would still be driving Model A's in any color you like as long as it is black. I did a brake job on my van yesterday and the rear calipers were strange and different than any other disk brake caliper that I had seen before and I had to search the internet to figure out how to retract the piston... same principle but reinvented to be better. snip white noise that added nothing to the thread snip John On 5/22/2012 6:50 AM, Viesturs Lācis wrote: 2012/5/22 John Thorntonbjt...@gmail.com: Why does it matter how other controls work? Not to reinvent the wheel and learn from existing examples of good solutions to some problems. -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
[Emc-users] Tool Offsets
Hi all, Per the Setting Coordinate Systems thread, I converted from using coordinate systems (G54-G59.3) and setting the offsets with G10 L2, to using the offsets specified in the tool table. Mostly it worked without a problem. The exception is when re-running a program without reloading it. The beginning of the program will have two lines similar to the following: T3 M6 G43 H3 If I just rerun, the tool offsets seem to be ignored, but if I do a reload of the same program it runs fine. Do I need to add a G43 H0 to the end of the program, is there another explanation for why the offsets are ignored when rerunning? Thanks, Eric -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
G49 cancels G43 Send the machine home at the end of the prog using: G28G91Z0.0 Y0.0 X0.0 You should not need to use G49 You must be doing something else wrong Start of every one of my progs look like this: T1M6 G54G90G0XxxYxxS500M3 G43H1Z.1M8 moves the tool down to .1 above the workpiece blah blah ends look like this: G28G91 Z0.0 send the Z home G28G91Y0.0 send the y home to put in a new part M30 - Original Message - From: Eric H. Johnson ejohn...@camalytics.com To: 'Enhanced Machine Controller (EMC)' emc-users@lists.sourceforge.net Cc: Sent: Monday, May 21, 2012 2:51 PM Subject: [Emc-users] Tool Offsets Hi all, Per the Setting Coordinate Systems thread, I converted from using coordinate systems (G54-G59.3) and setting the offsets with G10 L2, to using the offsets specified in the tool table. Mostly it worked without a problem. The exception is when re-running a program without reloading it. The beginning of the program will have two lines similar to the following: T3 M6 G43 H3 If I just rerun, the tool offsets seem to be ignored, but if I do a reload of the same program it runs fine. Do I need to add a G43 H0 to the end of the program, is there another explanation for why the offsets are ignored when rerunning? Thanks, Eric -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
On 21 May 2012 20:51, Eric H. Johnson ejohn...@camalytics.com wrote: T3 M6 G43 H3 I never use the H-number, it is only useful for applying the offset of a non-loaded tool to the loaded tool. Though I doubt that is your problem. -- atp If you can't fix it, you don't own it. http://www.ifixit.com/Manifesto -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool Offsets
I never use the H-number, it is only useful for applying the offset of It may be not useful in LinuxCNC but I guarentee you 90% + of the mill programs in the world use it (Fanuc has to have it) also the Dxx If you omit the D on Fanuc no offset will be applied to G41,G42 Terry - Original Message - From: andy pugh bodge...@gmail.com To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net Cc: Sent: Monday, May 21, 2012 5:57 PM Subject: Re: [Emc-users] Tool Offsets On 21 May 2012 20:51, Eric H. Johnson ejohn...@camalytics.com wrote: T3 M6 G43 H3 I never use the H-number, it is only useful for applying the offset of a non-loaded tool to the loaded tool. Though I doubt that is your problem. -- atp If you can't fix it, you don't own it. http://www.ifixit.com/Manifesto -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
