Le 09/01/2014 11:22, Tomasz Wlostowski a écrit : > On 01/08/2014 04:39 PM, jp charras wrote: > >> Tracks do not store the net name but just the net code, because they are >> expected to be connected to pads which store this info. >> (this is the reason tracks and vias not connected to a pad lose their >> net after loading a board, or reading a netlist) >> Therefore, after loading a board, or reading a netlist, the track net >> code should be initialized, but you have to store this net name in pads. >> (Of course, one can use an other way to store net names, and an other >> way to calculate net codes) > > Hi Jean-Pierre, > > I see another point in modifying the net assignment mechanism. If we > allow tracks/vias to retain net names and propagate them from the pads > only when the schematic netlist has changed (not every time the board is > loaded), it would also fix the infamous zone stitching issue... > > Regards, > Tom > >
Stitching vias and generally speaking not connected (to a pad) items (stitching vias, usual vias and tracks) create an other problem than retaining the net name. Retaining the net name of items not connected to a pad (or a zone) items is easy to fix (I already received a patch to do that). But the major issue is: if the net names are retained in not connected (to a pad) items, all track ends and vias should be included in the ratsnest generation. Otherwise, we will have not connected vias and/or not connected copper zone areas (floating copper islands). This is the only one reason stitching vias do not exist in Pcbnew. Therefore fixing stitching vias issue is: 1 - finish and validate (this is the more important step toward stitching vias) the new ratsnest algorithm which takes in account pad+vias+track ends: mainly for very complex boards, see if it is fast enough. The current ratsnest algorithm is very fast for 6000 pads (50 ms on my computer). What happen for 10x to 20x more (roughly 6000 pads + 30000 tracks (2 point) and 3000 vias for instance) 2 - after this, Retaining the net name of items not connected. And be sure the calculation time to know if 2 items are connected by a zone area is fast. Currently, this is 90% of calculation time. Because stitching vias will create a *lot* of items connected by zones, the calculation time in a very important criteria. 3 - add tools to change items net names, when a net name has changed in schematic (for instance AGND changed to GND) (easy, obviously, but needed) I know the ratsnest need to be rebuild only for the modified net (this is also currently the case). But the full ratsnet need to be fully rebuild, for instance when existing copper zones are modified (when creating/moving a via, for instance). This is frequently the case, for complex boards. In Altium, you need to deactivate (shelve) copper polygons to be able to work on you boards when the calculation time is too long... -- Jean-Pierre CHARRAS _______________________________________________ Mailing list: https://launchpad.net/~kicad-developers Post to : kicad-developers@lists.launchpad.net Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp
