calvingrier a écrit : > > --- In kicad-users@ yahoogroups. com > <mailto:kicad-users%40yahoogroups.com>, Pedro Martin <[EMAIL PROTECTED]> > wrote: > > > > Hi, > > > > I think you are not doing anything wrong. > > > > But there are only 2 choices: > > 1. Edit eeschema R an C and change pin numbers to 1 an 2. > > 2. Edit the modules and change pin numbers to A and B. > > > > Maybe there is another choice: copy and paste your old R and C from > an older > > project to a new library and use them. > > So I tried copy/save from a project with a netlist that works > (generates netlist connections for pins 1 and 2) and pasting the > block into a project that's "broken". > > EEschema removed the old annotations, and I had it update for the new > schematic. Then I generated the netlist. Once again the netlist had > pins numbered A and B. PCBnew just can't understand that numbering > for the default modules in KiCAD. > When copying (duplicates) a block eeschema reset references because 2 components cannot have the same reference (or the same time stamp). > > I looked at the library and the pin numbers on all the standard 2 pin > passive elements were "~". I could go through and force them to 1 and > 2, but that's a lot of work, and I'd have to do it to each element I > want to use... > I believe you are confusing pin names and pin numbers. For passive components like R and C, pin names are void (~ in lib) but the pin numbers are 1 and 2 pin numbers are the link between schematic and boards. (pin number can be in fact a word using up to 4 ascii code : 1 , 2 or inp or anod o AA11)
Please ckeck you library ans see the pin *number* (pin name is not used by netlists) they must be 1 and 2 (and not A or B, unless you are also using A or B as pad names in footprints). Generally speaking pin *numbers and pad names must be the same word (or number) > I could also modify all the modules I need, so they all use A and B > for pin numbers... but again, I'd have a custom set of footprints and > I'd need to do it every time. > > HELP! Jean-Pierre! > Here is some things to verify: 1 - Verify in your schematic (not in libedit) the pin number (click on a pin) A common mistake is a duplicate component in 2 different libs. Eeschema takes the first (this is a feature: lib order is significant) Be absolutely sure eeschema (not libedit) see 1 and 2 (and not A and B) as pin *numbers* 2 *DO NOT* use spaces in labels, values, references, component names ... This is not a problem in eeschema, but a *lot* of netlist formats do not accept spaces in names. I do not know the kicad version you are using. The last version replaces spaces in labels in pcbnew netlist, but it is better to avoid spaces in names. See (with a text editor) the .net file to verify what is exactly created. -- Jean-Pierre CHARRAS Maître de conférences Directeur d'études 2ieme année. Génie Electrique et Informatique Industrielle 2 Institut Universitaire de Technologie 1 de Grenoble BP 67, 38402 St Martin d'Heres Cedex Recherche : Grenoble Image Parole Signal Automatique (GIPSA - INPG) 46, Avenue Félix Viallet 38031 Grenoble Cedex
