[solved] Import component in multiple unit component

Schematic
1

Hi,

I’m new to KiCad and used Eagle before.
I’d like to create a new component for a matched transistor pair in a single package and thought about creating a component with 2 units e.g. Qa and Qb.
But how can I import a transistor symbol for each unit, after I created a component with 2 units? Obviously I can reuse symbols only for non-multiple unit components, isn’t it?

TIA
Olli

2

If you got the multi unit set up you should check the properties and have "All units are not interchangeable’ ticked:

Once that’s done you can chose if elements (options) will appear in only one or all of them, example (‘Common to all units in component’):

3

I see - thanks!
But can I import a component drawing like a for a NPN so that my transistor drawings look exactly like the other ones?

4

I give you an easy and quick example how to create dual transistor as multi-unit.

  1. Open Library editor (via Eeschema or direct from KiCad Manager).
  2. Be sure you have transistors.lib in your project library list. If not, add this library.
  3. Set working library in editor to transistors.lib.
  4. Select any existing transistor symbol which you want to clone. For example BC237B if you need NPN.
  5. Select Create new component from current one and enter new name.
  6. Now you have new single unit component with pins and drawing, but you need multi-unit component.
  7. Go to the Properties and increase number of units to your needs.
  8. If you need dual NPN or PNP transistor just increase only Number of units to 2. If you need complementary pair NPN+PNP select also All units are not interchangeable.
  9. You can edit remaining options from Descrition, Alias, Footprint filter tabs now, or edit it later. Click OK.
  10. Now you have two units but the pin numbers are identical in both units. Don’t worry, we will fix them.
  11. Edit pin numbers in Unit A to match your package.
  12. Select Unit B and edit pin numbers again to match your package.
  13. Now, if your package have two NPN or two PNP transistors no action is required. Skip next step.
  14. If you need NPN+PNP pair, back to the Unit A and double click on the arrow drawing (poly line[s]) over emitter and deselect Common to all units in component. This way this arrow disappear on Unit B (and any other units except unit A). Select Unit B, and redraw arrow to indicate opposite polarity.
  15. Complete other options in Properties if you didn’t do that in step 9.
  16. Select destination library as working library. Update component and finally save library.

To copy whole drawing (Caution! Pins are included too!) use Export current drawings and Import existing drawings from right toolbar.

2 Likes
5

I followed your description and it worked very well.
Thank you so much! I already love KiCad :slight_smile: