apluscw wrote: > I see that the intermediate layers are labeled L1, L2, etc. > > For a 6 layer board, are the boards laid out as follows: > > ---component--- > ------L1------- > ------L2------- > ------L3------- > ------L4------- > ----copper----- > > Or is it: > > ---component--- > ------L4------- > ------L3------- > ------L2------- > ------L1------- > ----copper----- > > I would think it would be the former, but the order in the pull down > menu suggests it is the latter. I want to be certain I know which > plane to use as my ground plane. > > Regards, > > a+
To be absolutely sure what to get when ordering your board you have to draw a board layer cross section outside of your board edge in an engineering layer (and print this as a separate file). The cross section should for a 6 layer FR4 include the following information: Layer name Filename Type Thick Material ========================================================== Component comp.gbr electric 45 um Cu-17 um + plating IsoC iso 200 um FR4-200um L2 l2.gbr electric 45 um Cu-35 um Iso2 iso 400 um FR4 L3 l3.gbr electric 45 um Cu-35 um Iso3 iso 200 um FR4 L4 l4.gbr electric 45 um Cu-35 um Iso4 iso 400 um FR4 L5 l5.gbr electric 45 um Cu-35 um Iso5 iso 200 um FR4 Solder sold.gbr electric 45 um Cu-17 um + plating The order or the naming of the layers inside pcbnew is not that important. The board manufacturer only gets the output gerber files. Maybe there is a way to generate this information from pcbnew but I don't think so. Remember that the thickness of the iso layers are important when designing 50 ohm traces, and that the layer design must be specified somewhere when ordering the boards, unless you want the manufacturer to decide the layers thickness and material... I'm sure there are an number of ways to do this but this is the way we do it. You also have to add information weather you want the component print on your board... // Magnus
