How to handle nc pins of ICs

Schematic
1

This is actually about schematic, schematic symbols and layout.

I am using some semiconductors with many pins marked as not connected (nc) in the data sheet.
Of course, I could add all those pins to the symbol and mark them with the no connect cross in the schematic. This clutters the schematic, though. So, I have just omitted the nc pins in the symbol definition.

But then, upon importing the schematic + footprints into the layout, I get warnings for all those unconnected pins like:
“Warning: No Net found for Symbol XY Pin Z”

Now, can those pins be handled in the schematic or schematic symbol in a way invisible in the schematic such that the warning upon import into the layout does not occur?

Background:
I get many of those warnings and I just found that one was severe as I had assigned a wrong footprint with too many pins. DRC did not show this and the other irrelevant import warnings hid it in plain sight.

2

You can mark pins as Visible . . . untick makes them not Visible . . .

image

3

Will invisible pins implicitly be handled as not connected?
Else, ERC will report connect errors…

4

You can set them in the symbol editor as Type not connected . . . I don’t use ERC so you will have to give it a try and see what works.

5

Set them to the non connected type, mark them as not visible and place them somewhere it’s unlikely to connect to a wire (e.g. the boundary box of the symbol). If you haven’t changed the default ERC rules for non connected pins no error or warning should appear.

image
image1375×551 9.12 KB

6

Excellent, will do. Many thanks!

7

I have updated my symbol. Is there a simple way to update all components in the schematic with the updated symbol other than delete and place again?

8

e at any symbol,
Update Symbol from Library…
Update all symbols in schematic.

Opps. I supposed that you modified it in your library.
May be “Update symbols matching value:” is what you need.

9

I hope he did. Otherwise this issue will pop up again and again.

10

I think that would be a terrible idea, one accidental click on invisible and an important pin could be disconnected.
ERC is to make you stop and check.
Personally I would not hide NCs, someone coming along years later might want to check the pin

11

I have not seen your symbol, but I would probably be tempted to put those NC pins in a separate unit and then tug it away somewhere in a corner. I find the A4 paper quite small for a complete schematic, and often I divide a schematic over two sheets. The main sheet gets all the “important” stuff, and the other sheet collects things like voltage regulators, decoupling caps, mounting holes, and possibly this unit with the NC pins.

Also, remember there are different interpretations of “NC”. Sometimes it means you can not connect anything to it. (It may have internal connections for test purposes), and at other times, it means it has no internal connect (I.e no bond wire from the frame to the chip) and you can connect anything you want to it. This may be handy because you can use it to route other signals under an SMT chip. KiCad has the Fee pin pin type for this.

1 Like