fq1ip- Invisible Pins (General)

create counter

Invisible Pins- What do they need?

Some components have invisible pins. They are often for connections to power rails, e.g. Vcc or GND. When you use a component with an invisible pin, you often need to know the pin's **name**. (The pin's number isn't- directly- terribly important to you. It is essential to the mechanism by which KiCad will associate the pin of the schematic with one of the pads on the footprint which will go on the PCB. But that "mapping" is one of the things KiCad does for you, about which you don't need to think very hard.)

Apologies! This page was a mess until late (UK time) on Nov 11, 2011. It should be much better now.

It has been thoroughly checked to see that confusion in my brain (before 9 November, 2011) about the roles of pin names and pin and pad numbers hasn't led to errors here. I have a page with more on this if you are really curious.

How do you learn what the invisible pin's name is, so, for instance, you can include a suitable power port in the schematic?

If you are not familiar with power ports, do read the page about them, which is brief, but gives you a link to a full tutorial if you want that. It won't answer your every invisible pin question, but it will introduce you to some important concepts and tools.

Discovering invisible pin names:

First option… use DRC while running PCBnew

Neither the pin nor its name show with the component while you are working on the schematic. However, assuming that you PCB passes the DRC tests, the footprint you assigned to the component will have pads for all of the pins, including any invisible pins.

You can just make a first pass through the design cycle without worrying about the invisible pins. When you have started PCBnew, and "dumped" the footprints on the page, zoom in on the footprint for the component with invisible pins. You should see some pads with no rat's nest lines going to them. Zoom in quite close, and a name will often (always?) be shown on the pad, in addition to the pad's number. This will be the invisible pin's name. You can then go back to the schematic, attach a power port to a suitable line, re-save the netlist, go back to PCBnew, re-read the netlist, and all should be well.

This only works if, in CVpcb, you assigned a suitable footprint to the component with the invisible pin.

Discovering invisible pin names:

Second option… use ERC while running eeSchema

The ERC tool of eeSchema can help you a bit. If you have errors associated with an invisible pin, there will be a little arrow pointing to a part of the symbol on the schematic, a part not associated with one of the visible pins….

If you just make a first pass through the design cycle without worrying about the invisible pins, after you have the PCB sketched out you can run the design rule checking tool, the DRC. In the "unconnected" list… although it will be long, if you take my advice and don't lay down tracks before you have made most of your footprint placement decisions, you may be able to pick out the reports of "unconnected" concerning the invisible pins. They will tell you what the name of the invisible pin is.

Discovering invisible pin names:

Third option… examine component

While you are in eeSchema, you can use the component editor to open the component's design, and there you will see the invisible pins… and their names.

If you look at the 7400 with the component editor….

… you will see "GND" and "Vcc", identified as being on pins 7 and 14 You don't see those on the schematic. They are "invisible pins". (All of this is in the excellent PDF which comes with eeSchama, in fact. But it can be hard for a novice to know where to find things, isn't it?) (You open the PDF by clicking eeSchema's menu item "Help | Contents". There are separate PDFs for each of the modules of KiCad, and another for the KiCad central project manager.)

Unless otherwise stated, the content of this page is licensed under Creative Commons Attribution-ShareAlike 3.0 License