Re: gEDA-user: No-Net Copper
On 01/01/2011 12:20 PM, Rick Collins wrote: If copper is left behind because of manufacturing, it doesn't really impact the layout process or connectivity checking. Sure does if it is DRC rule close -- it could be short in etching process results. On 01/01/2011 01:58 PM, Christian Riggenbach wrote: press 'f' (to mark it as found) - start the line from the not marked copper. Both should now be marked as found and should be connectable. This is possible, because Auto enforce DRC clearance only relies on the found flag. Also it only resets the found status on entering the line mode. I suppose toggling enforce makes sense if that's the way it is. I wish we were attaching netnames to pcb trace segments as we create them and using that to do auto enforce without having to toggle of add f flags first. Guess I need to try out that Auto enforce DRC feature -- I've never purposely used it yet, but have seen it somewhere...showing up by accident. :-) John Griessen -- Ecosensory Austin TX ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: No-Net Copper
John Griessen j...@ecosensory.com writes: I wish we were attaching netnames to pcb trace segments as we create them and using that to do auto enforce Please don't! Guess I need to try out that Auto enforce DRC feature -- I've never purposely used it yet Same here. If you do not use it, why do you care about associating netnames to traces? -- Stephan ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: No-Net Copper
Christian Riggenbach wrote: There is a trick to connect to some other copper not in the same net: - enter the line mode - hover over the copper to connect - press 'f' (to mark it as found) - start the line from the not marked copper. Both should now be marked as found and should be connectable. This is a nice one! :-) I added it to the pcb-tips in the wiki (and remembered that I promised to merge pcb-tips and FAQ-pcb) http://geda.seul.org/wiki/geda:pcb_tips?#pcb_won_t_let_me_connect_to_copper_that_is_not_connected_to_anything mit freundlichem Gruss Christian Riggenbach Allmählich sollten wir über eine deutsche User-Gruppe nachdenken ;-) Sozusagen als Gegenstück zu den Free-Dogs in Boston. ---)kaimartin(--- -- Kai-Martin Knaak Öffentlicher PGP-Schlüssel: http://pgp.mit.edu:11371/pks/lookup?op=getsearch=0x6C0B9F53 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: No-Net Copper
On Sat, 2011-01-01 at 10:33 -0500, Rick Collins wrote: Why is no-net copper useful? Rick -- use copper like silk, i.e for text, marks... -- some like to have copper below screws, for mechanical reasons -- use copper where it does not hurt, i.e if milling your boards or to save chemicals ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: No-Net Copper
Rick Collins wrote: Maybe someone could explain to me why there would be copper on a PCB that is not part of a net? Possible reasons: * the pcb will be done by milling. (as opposed to etching) * a logo in copper contains portions not connected to anything * text in copper contains lots of isolated snippets * to save chemicals, large areas may deliberately stay as copper ---)kaimartin(--- -- Kai-Martin Knaak Öffentlicher PGP-Schlüssel: http://pgp.mit.edu:11371/pks/lookup?op=getsearch=0x6C0B9F53 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: No-Net Copper
At 11:54 AM 1/1/2011, you wrote: On Sat, 2011-01-01 at 10:33 -0500, Rick Collins wrote: Why is no-net copper useful? Rick -- use copper like silk, i.e for text, marks... -- some like to have copper below screws, for mechanical reasons -- use copper where it does not hurt, i.e if milling your boards or to save chemicals If you are milling a board, do you layout the material not removed??? I expect that would just be a by product of the milling and not a part of the layout. In this case, I would consider any net connection to the unmilled copper to be an error that should be flagged. If you want to use it for ground plane, then this is part of a net. For copper under screws, I always spec that in the schematic by adding a component for the hole and pads. I guess if you are happy spec'ing things outside of the schematic you don't need a net for that, but I don't see a need to support a separate class of copper for it. As to text, etc, I suppose that is not typically considered part of a net unless it is done as openings in a copper layer. But when do you connect a trace to text? If anything, I would want that flagged as an error even if it only connects to one net, or at least a warning. I can see where no-net copper might be ok in a design, but I don't see a need for it. Does this add any complexity to the tools beyond not being handled correctly in connectivity test/DRC (according to some no matter how you do it). Does using no-net copper simplify anything? Rick ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: No-Net Copper
On Sat, 2011-01-01 at 12:57 -0500, Rick Collins wrote: At 11:54 AM 1/1/2011, you wrote: On Sat, 2011-01-01 at 10:33 -0500, Rick Collins wrote: Why is no-net copper useful? Rick -- use copper like silk, i.e for text, marks... -- some like to have copper below screws, for mechanical reasons -- use copper where it does not hurt, i.e if milling your boards or to save chemicals If you are milling a board, do you layout the material not removed??? Kai-Martin and I only answered your simple question: Why is no-net copper useful? Have you ever tried to use gEDA's PCB now? ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: No-Net Copper
At 01:05 PM 1/1/2011, you wrote: On Sat, 2011-01-01 at 12:57 -0500, Rick Collins wrote: At 11:54 AM 1/1/2011, you wrote: On Sat, 2011-01-01 at 10:33 -0500, Rick Collins wrote: Why is no-net copper useful? Rick -- use copper like silk, i.e for text, marks... -- some like to have copper below screws, for mechanical reasons -- use copper where it does not hurt, i.e if milling your boards or to save chemicals If you are milling a board, do you layout the material not removed??? Kai-Martin and I only answered your simple question: Why is no-net copper useful? The context was supporting it in a layout tool and specifically how it impacts DRC and connectivity checking. I'm just trying to understand the thought here. If copper is left behind because of manufacturing, it doesn't really impact the layout process or connectivity checking. It just struck me as odd that there would be support in a layout tool for no-net copper that might be connected to nets. Rick ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: No-Net Copper
On Saturday 01 January 2011 19.26:35 kai-martin knaak wrote: If no-net copper is connected to a net, it automatically becomes some-net copper. The current issue with pcb: You need to toggle enforce_DRC to do the connection. This is a hassle that should be removed from the GUI. There is a trick to connect to some other copper not in the same net: - enter the line mode - hover over the copper to connect - press 'f' (to mark it as found) - start the line from the not marked copper. Both should now be marked as found and should be connectable. This is possible, because Auto enfore DRC clearance only relies on the found flag. Also it only resets the found status on entering the line mode. I don't know about the Lesstif GUI, but in GTK it works. This is perhaps something for the wiki, as it is a FAQ (IMHO). -- mit freundlichem Gruss Christian Riggenbach signature.asc Description: This is a digitally signed message part. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
