--- In [email protected], Greg Dyess <gregory.dy...@...> 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. Use freerouter, and do not autoroute, but manual route with it: 1) Place your components while in pcbnew. 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. 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. 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. 7) Run DRC check in pcbnew. 8) Export to gerber. Always do the fill in pcbnew near the end. 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
