Hi André, I understand what you mean, that's a very reasonable use case. It is a known issue that the design rules framework is not flexible enough for all use cases, it is already on the roadmap to overhaul that system and make it more flexible.
-Jon On Fri, Jun 8, 2018 at 1:02 AM, André S. <[email protected]> wrote: > Hi Jon, > > just for clarification: > I can attach a NC to a signal thats connected to only one component pin in > eeschema. ERC then recognizes that the signal is terminated and does not > throw an error. I can also give that net a label that is then exported to > the netlist (with a leading "/", maybe to signal it's a single pad net?). > > > What I did not check until today (with 4.0.7): > I can put that net into a net group. When reading the netlist into Pcbnew > I have to check "keep single pad nets". Then the design rule is observed > during routing. Very fine! > > Why would I do something like this? > Lets say I have a transformer in my design that has two mains windings > with a common middle pin. That pin is not used in my design but still > carries mains voltage. I would give that pin a net with a name and then in > pcbnew in the design rules I can put that net (easily, due to its name) in > a net group with a high distance from other nets. > > On a sidenote: > > I work for a company where we do this all the time (in Zuken) to be able > to handle (very) complex designs where high voltages and low voltage > control circuits are on the same board. > > Checking this today in Pcbnew also showed me, that net groups can only > have one distance. I wonder if no one until now had the requirement where > nets in different voltage domains need to be kept away from another but can > have a close distance within the net group. Can Pcbnew/Kicad do this? Or is > this too exotic of an requirement? I know that this can get _very_ complex > when you have up to over 100 net groups due to isolation requirements… > > Regards, > André > > Zitat von Jon Evans <[email protected]>: > > > For your PS, do you mean NCs attached to the end of wires rather than the >> end of pins? I don't think that's how it's designed to work today (NC >> symbols are only for pins) We could add that though. >> >> On Tue, Jun 5, 2018 at 12:50 PM, André S. <[email protected]> >> wrote: >> >> One reason one wants (labeled) NC nets can be isolation of nets via net >>> classes to ensure proper distances between not connected pins and other >>> signals. >>> >>> Regards, >>> André >>> >>> PS: This reminds me that eeschema correctly recognizes NC symbols as >>> termination for nets (via ERC) but still shows a “not terminated" marking >>> on that NC terminated net ending. Is there a bug filed for this >>> somewhere? >>> >>> >>> >>> On June 5, 2018 2:38:24 AM UTC, Jon Evans <[email protected]> wrote: >>> >>>> >>>> Hi all, >>>> >>>> In the current netlisting algorithm, pins with no-connects sometimes >>>> appear in the netlist, with auto-generated names like Net-(U1-Pad1). >>>> >>>> This seems to not always happen, but I haven't investigated why yet, >>>> since I'm approaching netlisting from a different direction with my new >>>> connectivity algorithm. In my algorithm, a pin with a no-connect >>>> attached >>>> will never generate an entry in the netlist. >>>> >>>> Is there some reason we should be including these pins on the netlist? >>>> It seems like if they are marked as no-connects and don't actually >>>> connect >>>> to anything, we shouldn't be forwarding them to the layout. >>>> >>>> -Jon >>>> >>>> >>> > > >
_______________________________________________ Mailing list: https://launchpad.net/~kicad-developers Post to : [email protected] Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp
