| ID: | 5648 |
| From: | Gabriel Paubert <pa...@iram.es> |
| Date: | Mon, 16 May 2022 12:52:34 +0200 |
| Subject: | Re: [pcb-rnd] RFC: multi-sheet netlist |
| in-reply-to: | 5647 from pc...@cuvoodoo.info |
| replies: | 5655 from pc...@cuvoodoo.info |
--5cd54PRfmeQw3Wq6 Content-Type: text/plain; charset=us-ascii Content-Disposition: inline Hi, I just put the appended file in my designe directory. This eliminates all the prefixes in the netlist generation. It is not perfect but works reasonably well for moderate size designs (~10 schematic pages). Gabriel On Mon, May 16, 2022 at 12:25:41PM +0200, pcb-rnd@cuvoodoo.info wrote: > gEDA/gschem and lepton-eda/schematic support hierarchical design (with multiple/sub-sheets). > this is explained in http://wiki.geda-project.org/geda:faq-gschem?s[]=gtag&s[]=sch#can_gschem_do_hierarchical_designs_with_sub_sheets and an example is shipped with these software in gTAG.sch. > > I tried for the first time this feature because may schematic became too large, unreadable (on one sheet), and parts are just repeated (e.g. multiple ports). > but I have an issue with how netlist are handled with subsheets. > I attached a basic example. > In the tEDAx netlist, components have a unique refdes, using the "_sheet-refdes_/" prefix/path. > pcb-rnd treats the name as a string, and does not have the concept of hierarchical design/name. > thus when I reuse a component (with the same refdes) on multiple sheets (because the connection of one of the pins only makes sense in this sheet), then pcb-rnd imports multiple times the footprint (one for each name, which includes the path). > this component re-use also applies to multi-part symbols (e.g. dual-opamp). > > the same prefixing is applied to netnames. > thus the GND symbols (using the GND netname) are not interconnected across sheets (this also applies to the provided gTAG.sch example). > > a kind of solution is to use pins on the symbol for the subsheet, and use and INPUT/OUTPUT symbols in the subsheet. > but doing it for all nets (e.g. VCC/GND) just clutters the sheet symbol, and kind of goes against the concept of defining/using netnames. > plus, this does not solve the refdes reuse issue. > > for now my solution is to use a netlist intermediate (pcb-rnd will not import the schematic directly), and have a script that removes all prefix/path. > but maybe I just did not understand correctly how to do proper hierarchical design (I really did not find a lot of documentation). > maybe tEDAx can be extended to integrate the concept, or interpret the '/' in the name. > any comments/suggestion is welcome. --5cd54PRfmeQw3Wq6 Content-Type: text/plain; charset=us-ascii Content-Disposition: attachment; filename=gnetlistrc ; hierarchy-uref-mangle string ; ; Controls if uref names are mangled to make them uniq when traversing ; down into the hierarchy. If this is disabled then urefs are not changed ; and it is the user's responsibility to make sure they are unique. ; If you disable this, you really are taking your netlist's life into your ; own hands. You *MUST* have unique urefs throughout the entire hierarchy ; or bad things might happen. Also you cannot reuse underlying schematics. ; ;(hierarchy-uref-mangle "enabled") (hierarchy-uref-mangle "disabled") ; hierarchy-netname-mangle string ; ; Controls if net names are mangled to make them uniq when traversing ; down into the hierarchy. If this is disabled then the net names are not ; changed and it is the user's responsibility to make sure they are unique. ; If you disable this, you really are taking your netlist's life into your ; own hands. This basically has the effect of making all same named nets ; in the entire hierarchy be electrically connected. Hope you know what you ; are doing. ; ;(hierarchy-netname-mangle "enabled") (hierarchy-netname-mangle "disabled") ; hierarchy-netattrib-mangle string ; ; Controls if net created by using the net= attribute are renamed to make ; them uniq when traversing down into the hierarchy. If this is disabled ; then the net= created nets are not changed. This feature is handy to have ; global nets which spawn the entire hierarchy (like power or ground nets). ; Please make sure you know what you are doing. ; ;(hierarchy-netattrib-mangle "enabled") (hierarchy-netattrib-mangle "disabled") ; ; End of mode related keywords ; --5cd54PRfmeQw3Wq6--
Reply subtree:
5648 Re: [pcb-rnd] RFC: multi-sheet netlist from Gabriel Paubert <pa...@iram.es>
5655 Re: [pcb-rnd] RFC: multi-sheet netlist from pc...@cuvoodoo.info
5656 Re: [pcb-rnd] RFC: multi-sheet netlist from Nicklas SB Karlsson <nk...@nksb.eu>
5657 Re: [pcb-rnd] RFC: multi-sheet netlist from Roland Lutz <rl...@hedmen.org>
5671 Re: [pcb-rnd] RFC: multi-sheet netlist from ka...@aspodata.se