Terry, open your NE555 schematic symbol in the library editor, click on the "Edit component properties" icon on the toolbar, and de-select the checkbox marked "Power symbol". The popup tooltip you get if you hover the mouse over this option explains what it does. For a real component, you don't want this selected!
I also noticed that you defined all the pins to be "passive". This isn't a brilliant idea. If you define them to be what they really are, then the electrical rules check will tell you if you've done something silly in the schematic like connect 2 outputs together, or have an input that isn't driven from an output etc. The only thing to watch out for is that when you've defined the Vcc pin to be a "power" pin, it needs to be driven from a power source. On this simple design, the power is coming in from the connector, which of course should have all pins as "passive". You therefore need to add a "pwr_flag" from the power ports list to tell Kicad that it's ok. Nick. --- In [email protected], "TERRY" <terryll...@...> wrote: > > Ok - I've added w_analog.lib, w_analog.dcm to the zip file and re-uploaded > into files section as _KiCadLearn.zip > > These two files where copied into the zip but where stored on my hard drive > only under ..\kicad\share\share\library\contrib\ > > Thank you for your help to understand. Perhaps the library is added > incorrectly? > > Terry > > --- In [email protected], "nickoatley" <nickoatley@> wrote: > > > > I see what you mean. Can you put a new version of your zip file in the > > files section, this time including your w_analog library? Might be > > something wrong with that maybe. > > > > --- In [email protected], "TERRY" <terryllong@> wrote: > > > > > > I'm working on a simple schematic for an SDR Sound card tester. To build > > > the schematic, I added into my lib the component NE555. However, netlist > > > generation does not show NE555 as a component. Can someone tell me why? > > > > > > Thanks > > > Terry > > > > > > I've upload a zip file of my work to this group/files as _KiCadLearn.zip > > > > > >
