1
\$\begingroup\$

I'm using a RASPBERRYPI-40-PIN-GPIO_PTH_NO_SHROUD_NO_SILK component in Eagle as part of a Hat for a Raspberry Pi. The Raspberry Pi pinout has a number of duplicate pins for GND, 5v and 3.3v. The board layout is requiring that airwires be created between these duplicate pins (e.g. all 3.3v pins must connect to each other). This is a bit redundant and it's making routing of the other airwires difficult.

Is it possible to stop Eagle requiring that pins on the header be connected to eachother?

\$\endgroup\$
2
  • \$\begingroup\$ I assume you've connected wire stubs to all of the pins on the schematic and named all of the wires? Just change the net names to be unique (e.g., 3.3V_1, 3.3V_2) \$\endgroup\$
    – Justin
    Jan 19, 2021 at 21:58
  • \$\begingroup\$ The component does that itself - it doesn't actually have multiple pins for each function so you can't choose which pin something connects to. I could replace it with a standard 40 pin header and do as you suggested but it feels a bit hacky \$\endgroup\$
    – phil-lavin
    Jan 19, 2021 at 22:00

1 Answer 1

3
\$\begingroup\$

You have two options:

  1. Ignore the airwires, perhaps with a note saying that it's intentional - this is not a good design practice.
  2. Use a different part/device.

Going with the second option. There are a number of approaches you can choose from:

  1. Use an existing 40-pin pin header from any library. This will work fine in the layout, and allow you to choose the pinout you want. It's perhaps less clear than having a dedicated symbol which names each of the pins.
  2. Modify the existing library device to add a new package variant. Here you can use the same footprint and symbol you're already using, but simply change the pin mapping to not link the pins you don't want to use.
  3. Create a new symbol (could copy the old one as a starting point), and add seperate pins in the symbol for each of the power supply pins (e.g. GND_1, GND_2, GND_3, etc). Then create a new device with the existing package and new symbol.

The last option is probably the best. All pins in the footprint now map to a pin in the schematic, so this one gives you full flexibility as to which you connect up. When doing this, I tend to be quite precise in how I name the multiple supply pins. Instead of arbitrarily naming them GND_1,GND_2, etc., I tend to name it based on the pin number, so if pin 12 of the header was GND, I'd name that one GND_12 so you can quickly verify which pins you've left unconnected.

\$\endgroup\$
2
  • \$\begingroup\$ Thanks for writing this up :) I see a lot of advantages to the current approach as you don't need to know where on the board a component will reside to get the most efficient airwire routing. That said, it's not a huge issue to change the schematic to facilitate easier routing \$\endgroup\$
    – phil-lavin
    Jan 20, 2021 at 9:45
  • \$\begingroup\$ Whilst I think about it, creating a 3.3v plane on one side of the board would make this easier also. I've seen a lot of mixed feelings about flooding copper for non-GND purposes. What is the general thought about this approach? \$\endgroup\$
    – phil-lavin
    Jan 20, 2021 at 9:46

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.