Hi Ryan, This is a workaround I have been using so far.
Let's use an example of a diode designated D1 (ie. Reference D1) in a board open in PCBNEW . You can try the following: 1) Always save your board .brd file first before trying out new stuff! KICAD is pretty stable but it does crash sometimes. 2) In PCBNew , point the mouse cursor over your component and right click. In the popup menu select>Footprint D1 (Component)>Edit>Properties tab>Edit Module. 3) This will open Module Editor in a MINIMIZED mode on your Windows Start toolbar. It doesn't pop in the same way it does when we invoke it from the PCBNEW's menu button. 4) Clicking on this minimized Module Editor, should open its window. You will see your component there. Edit your silkcreen, or any other changes that you want, eg. pad sizes. If you need finer resolution for your silkcsreen editing, you can do a Right Click>Grid Select and choose a smaller grid setting. Be careful not to accidentally move the component pads, otherwise they will be misaligned on a different grid when you update the component into your board(see next step). So I normally reset the grid back when I am done with the changes for safety reasons. 5) After your are done editing, click "Update module on current board" button in the Module Editor menu bar. DON'T save it unless you want to update it for your library. 6) Return to PCBNew. Your component has already been updated. But all the other instances of this component (D2, D3, etc.) will remain unchanged. 7) If you wish to move any designator (ie. reference), make sure to first select "Mode track and autorouting" button in PCBNEW menu bar. 8) Point the mouse cursor over your designator; change to a smaller grid size if the mouse cursor can't detect it. Right click>Reference D1 item. In the next popup, select Reference D1>Move. Then you can start moving it around. Left click to place it at the new location. Rgds, Andy --- In kicad-users@yahoogroups.com, "rcrowell23" <[EMAIL PROTECTED]> wrote: > > Hi all, > > I have a component module that has a pin 1 designator, a small square > on the silkscreen layer near pin 1 of the footprint. In general the > location of the designator is fine, but for one instance in my design > I need to move it so that it doesn't partially cover an adjacent > copper pad. I don't want to change the designator location for all of > the other instances of this module, so I can't change the module > footprint in my library. > > So what I want to do is simply move the module silkscreen markings > around, but I can't select any silkscreen features that are defined in > the module footprint other than text (reference designators, etc.) Is > there some way to do this that I haven't stumbled upon? > > I would greatly appreciate any help you can give! > Thanks, > > Ryan >
