--- In [email protected], "Dick H." <d...@...> wrote: > > --- In [email protected], Greg Dyess <gregory.dyess@> wrote: > > >I will try autorouting and tell it the layer pair is my component >layer and > >the VSS layer and do an autoroute. > > You are wasting your time with "the autorouter". The term "the autorouter", > is ambiguous since Kicad can work either with its internal autorouter or with > freerouting.net's autorouter. My statement assumes the former. I think the > internal autorouter has fallen into largely disuse, and there is no way it > will ever catch up with the power and capability of the freerouter found at > freerouting.net. But a simple search of this list would have told you that. > Use the search feature of this mailing list please. > User/developer Notes: (schematic to layout ARM SOC, flash, SDRAM, power) My primary confusion was updating modules and module libraries. It was never clear which library was being used for the module I was editing. Even cvpcb would show a part name multiple times without a library name[path].
This info should be added to the user FAQ/autoroute section and the pcbnew help document, which didn't install for me. (I also need to add some doc for EEschema footprint backanno) > Use freerouter, and do not autoroute, but manual route with it: > > 1) Place your components while in pcbnew. I noticed that any change in schematic parts needs to be run through cvpcb to update the cmp file even if the footprint information is included in the schematic or the cmp file is deleted. > > 2) In pcbnew, put in the zone perimeters and make sure their netcodes are > correct, i.e. that they are tied to the correct net. You do not have to fill > yet. Manual route and set Net trace width seem to work fine for me. Also the selection filter is working much better with the newer releases. I decided to manually route short power tracks and human easy routes such as buses then let freerouter/autorouter crank away over night on the harder ones. If you use multiple track widths or via sizes remember to save your configuration. Manual route seemed more intutive, easier to use and snapper for me in pcbnew. The pcbnew menu layout is great given I didn't read documentation from either pcbnew or freeroute! > > 3) Export to DSN, and load the *.DSN file into freerouter. Learn it, it may > take you a day. Feel free to search this list about it, and get support from > their forum. I needed to install Java6 mentioned at http://www.freerouting.net/ for Linux > > 4) Manually route your board in freerouter. This is the only way you will > have net specific control over the width of traces. > > 5) In freerouter, save a "session" file, as *.ses. "Back import" the session > file into PCBNEW. > > Repeat steps 2 through 5 until you are happy. > > 6) Export to DSN one last time. Load design into freerouter. > > 7) check clearance "violations" and fix them. The clearance tolerances that > freerouter uses come from your *.brd file and are established in pcbnew under > the Dimensions menu choice. > > 8) back import one last time into PCBNEW. > > 6) Fill or re-fill your zones in pcbnew. pcbnew DRC check does this but inorder to view the ratsnest the zones need to be filled and "do not show filled zones" left hand menu button needs to be pushed. This feature should probably be in preference/colors and visablity menu. > > 7) Run DRC check in pcbnew. > > 8) Export to gerber. > > Always do the fill in pcbnew near the end. unless you want to use pcbnew manual route, edit and ratsnest. I never saved the pcb file with zones filled. > > You can view the DSN file and understand the nets, and copper areas. It can > be a way to trouble shoot the kicad *.brd file in essence, in a more human > readable form, one that is well documented. > > > HTH, > > Dick >
