That was helpful... I can't see what is causing the problem directly, however there is something very odd going on regarding the uP part.
Look at the top of U201. Connected to pin 56 there is a cap, C206 and a power port. The bottom of C206 and the power port is connected with a wire. However do a DRC and the wire gets flagged up as a problem. BUT - try to edit the wire and it does not get picked up as a wire. the system thinks it is part of U201, the microprocessor. So I shifted the cap and the power port out of the way, drew a block select around the "wire" and sure enough the entire U201 was selected. Where did you get the uP part from? I would think that somehow it has got a few extra bits in it that should not be there, which might explain a few things. I then created a blank sch, and just added the uP, no wires ports on NC, then generated a netlist Looking at the netlist nets were generate on pins above 14 - that should not happen. So that led to a bit of editing of the component. Big clue, I did a duplicate pins check and there were loads. This explains why a net has been generated, take pin 16 the duplicate pin check shows that it is connected to a pin at exactly the same position. So the system apparently tries to create a net between them Now check the lib cache and... X PGEC1/AN1/VREF-/CVREF-/CN3/RB1 15 -2100 -700 300 R 50 50 1 1 I X PGEC1/AN1/VREF-/CVREF-/CN3/RB1 15 -2100 -700 300 R 50 50 1 1 I X C2IN-/AN2/CN4/RB2 14 -2100 -600 300 R 50 50 1 1 I X C2IN+/AN3/CN5/RB3 13 -2100 -500 300 R 50 50 1 1 I X C1IN-/AN4/CN6/RB4 12 -2100 -400 300 R 50 50 1 1 I X PGEC2/AN6/OCFA/RB6 17 -2100 -300 300 R 50 50 1 1 I X PGEC2/AN6/OCFA/RB6 17 -2100 -300 300 R 50 50 1 1 I The above is a small extract from the lib cache file, After the name there is the pin number. So the first line shows pin 15, which is the first pin that generates a net, and sure enough there is a duplicate line. pins 14, 13, and 12 are OK they only have single lines, but pin 17 is duplicated again that generates a net. The problem is that the editor does not show the duplicate pins graphically, I assume that this is because the part was generated by some form of import rather than drawing the part from scratch. I think that explains your problems. Time to go back the the source of that component and see if you can get a clean version. Interesting problem... Andy On Mon, 19 Oct 2009 22:32:56 -0700 (PDT) Berceanu Cristian <[email protected]> wrote: > Hi, just for reference, I have archived the project and added it to the Files > of this group. The archive is "test.zip". Just check pins 64 and 2 of the > micro. They are identical, they are marked as NC, but pin 64 is assigned a > N-000047 net name (unique, so it is not connected to any other pins) while > Pin 2 is assigned the "?" net name. I fail to see any reason for this. > > Regards, > Cristian > > --- On Tue, 10/20/09, Berceanu Cristian <[email protected]> wrote: > > > From: Berceanu Cristian <[email protected]> > Subject: Re: [kicad-users] NC pins appear differently in PCBnew > To: [email protected] > Date: Tuesday, October 20, 2009, 7:55 AM > > > > > > > > > > > > > > > > > > Hi Andy, > I had alread checked for these aspects, these were also my initial > suspicions. The component is drawn exactly on the grid and the pins are > completely identical except their number, of course. Any other ideas? > > Thanks! > Cristian > > --- On Tue, 10/20/09, Andy Eskelson <[email protected]> wrote: > > > From: Andy Eskelson <[email protected]> > Subject: Re: [kicad-users] NC pins appear differently in PCBnew > To: [email protected] > Date: Tuesday, October 20, 2009, 1:06 AM > > > Check that: > > 1. you have hit the pin with the X (no connection) marker > (if you change grid sizes sometimes things do not align up correctly) > > 2. Check that the pins are really defined as normal pins in the lib > editor. If they are anything special such as power out, power in and so > on, the system may try to assign nets to them. > > Andy > > > On Mon, 19 Oct 2009 13:46:26 -0700 (PDT) > Berceanu Cristian <[email protected]> wrote: > > > Hi guys, > > I have a microcontroller with several pins being NC (and I have explicitly > > placed NC markings in the schematic. However, when I generate the netlist, > > some of the pins to get the "?" mark but others get a numeric net name. > > These last ones, which do get a net name, do not get connected to any other > > pins, but I am concerned as to why some NC pins are treated differently > > from others in the netlist. > > > > I have uploaded the file test.net, representing the netlist. Pins > > 2,3,8,12,13,14 and pins 21, 22, 23, 24 are all marked as NC in the > > schematic. However the first ones appear in the netlist as "?", while the > > latter do get unique net names. What could be the caouse of this? > > > > Regards, > > Cristian > > > > > > > > > > > ------------------------------------ > > Please read the Kicad FAQ in the group files section before posting your > question. > Please post your bug reports here. They will be picked up by the creator of > Kicad. > Please visit http://www.kicadlib.org for details of how to contribute your > symbols/modules to the kicad library. > For building Kicad from source and other development questions visit the > kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups > Links > > > > > > > > > > >
