Ultra Librarian Part has Symbol&Footprint - Missing Pins

I am a KiCAD newbie, but have made PCBs before with Multisim/Ultiboard. I have an unusual very high density 2x20 pin female edge card connector, 1mm pitch by Sullins. The component has 4 rows of 10pins each, each row staggered by 0.5mm. Luckily I found the part in Ultra LIbrarian and the footprint is perfect. It also had the symbol and everything imported into KiCAD 5.1. When I place the symbol, it only shows the first pin (unit A), it seems I have to manually add every pin and line them up. My PCB project needs lots of these. If I look at the symbol with Edit, it shows all 4- ‘units’ and I unchecked hide unused pins. Is there any short cut to lay down all 40 pins in one step? My fall back was to take a generic 2x20 connector and assign it the Sullin footprint. Does KiCAD automatically assign Symbol pin 1 to Foortprint pin 1, etc, etc?

Thanks for the help!!

Correction: "f I look at the symbol with Edit, it shows all 40 ‘units’ and I unchecked hide unused pins. "

tl;dr: Yes

Long answer:

Thank you, I understand that. How do I access the table or list where the symbol pin and footprint pin match can be displayed or edited?


There is no table as the mapping is very simplistic. All pins numbered 1 will be connected to all pads numbered 1. All pins “numbered” SCLK will be connected to all pads “numbered” SCLK. Note the plurals. In KiCad the program doesn’t prevent you from having multiple pins in the schematic and multiple pads in the layout with the same number. In the schematic I consider multiple pins with the same number as bad practice because it is too easy to then accidentally cross-connect two nets. But in the layout multiple pads with the same number is often useful for building up a complex pad shape from smaller pieces (though this practice is now depreciated with the custom pad shape capabilities), and to connect multiple shield pads to a single schematic pin.

The potentially confusing bit is the term “numbered” here. For simpler designs with discrete components and chips with connections around the perimeter (DIP, QFP, SOIC, PLCC, etc) it is easy to have pins numbers fully numeric (ignoring for now those who choose to “number” their diode pins A and K) so the term “pin number” is used to differentiate from “pin name”. (Here “pin name” is just a way on the schematic to give a functional name to a pin that only matters to the human reading the schematic, the net/connection algorithm doesn’t pay attention to what is in the “pin name” field.) But grid array style package (PGA, BGA, etc) solderable contacts (pins, balls, pads, etc) are identified with a row letter and column number (or maybe I have those backwards, I haven’t used one in a while…). This forces considering alphabetic characters in the pin number and now the term “pin number” becomes less accurate, and “pin alphanumeric” is too cumbersome… :wink: I’ve also seen edge connectors that are numbered A1-An for the top side fingers and B1-Bn for the bottom side fingers, again needing more than just numbers for the connectors pin numbers.

1 Like

Don’t forget SOT-23 :sob: :sob: :sob: :sob:

Due to some historical *&^%$#@!~ nobody is sure where pin number “1” is on that package, and different pinouts are used. A long time ago (In the DOS age) I used a PCB program which used pin numbers “C”, “B”, “E” for transistors, and you had to choose between the variants of SOT-23 available.

1 Like

Thank you all for the clear explanations. Could you help with my first question: The component footprint I downloaded from Ultra LIbrarian is perfect. The symbol imported only shows the first pin (unit A), however if I do a Symbol edit I can see all 40 pins (units labelled alphabetically). Is there a shortcut to place a symbol showing all 40 pins or do I have to manually add every pin and line them up? Isnt there a shortcut or is there something I am missing in the Symbol editor?

In your first post you wrote you used one of the generic connector symbols and combined that with the footprint of your downloaded connector.
This is a perfectly normal thing to do. I would not even consider it a hack or workaround.

When placing schematic symbols you can open the symbol as a tree, and then select one of the units directly:

You can also use the Insert key to repeat the last action (such as add a symbol). Handicap with this method is that all inserted schematic symbols are of the same “unit”, and you have to change that afterward.

I think it would have been nice if the unit was added to the spreadsheet in:
Eeschema / Tools / Edit Symbol Fields
This would speed up changing them.

Or even better probably:
While placing labels with Insert there is an auto increment. I think it wouldd be ideal if this auto increment is also used for the Unit.

These last two ideas are current not in KiCad, but may be items for the wishlist on Gitlab…

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.