2
\$\begingroup\$

I am designing a circuit board or hat for a raspberry pi 3 with the pinout below:
Raspberry pi pinout
I have a schematic symbol that is defined just as the raspberry pi header is (pin locations/numbers/names). It has multiple ground pins, which are all connected to their respective pins on the footprint.

When I am routing the PCB:
I want to tell altium that the GND pins are all interconnected on the raspberry pi, and so they don't need to be connected on my PCB. How can I do this?

Another way to put this:
How can I tell altium that parts connected to net [GND] on my PCB need to be connected to pin 6 [GND] OR pin 9 [GND] OR pin 14 [GND], but not all of the [GND] pins?
I dont want to run traces between all of the separate ground pins on the raspberry pi header while routing, but at the moment that is the only work around I can think of.

EDIT:
I say not all grounds need to be connected together because not all of them are actually used. I wanted to do this because I wanted to be able to decide which pins were actually going to be used in the PCB design stage, and not have to swap between PCB and schematic to decide which pins to be connected.

An example: screensot of my PCB the ground conected to pin 30 above is not normally connected to anything when this board is in use. It is broken out for debugging purposes. Being on the edge of the board, there is no reason to try to connect it to another ground, since it is only used when the raspberry pi is in use.

Thanks to desqa, I know the name of the characteristic I was looking for- Jumper IDs - and I was able to get it working in my design.

\$\endgroup\$
4
  • 3
    \$\begingroup\$ Generally you want as many redundant ground connections as possible. I suggest using a copper ground pour to connect all of your ground pins together. That's generally the most effective way to connect grounds on PCBs \$\endgroup\$
    – DerStrom8
    Dec 12, 2016 at 20:11
  • \$\begingroup\$ DRC will complain if the ground pins are not connected together, but the DRC errors will not prevent you from creating the PCB manufacturing files. Altium just considers DRC errors as warnings to the user, so you can ignore the "errors" that you find acceptable. \$\endgroup\$
    – Peter Bennett
    Dec 12, 2016 at 20:27
  • \$\begingroup\$ @DerStrom8 That is a solution I may go for, but it means that all of the raspberry pis ground pins need connected to the ground pour. I only want to connect to the pins I need to. I am not concerned about the redundant ground connections, because this board will be carefully inspected and tested every time it is used. \$\endgroup\$
    – ambitiose_sed_ineptum
    Dec 12, 2016 at 20:29
  • 2
    \$\begingroup\$ You "need" to connect all the GND pins to the ground pour on your board if you want the best signal integrity and power integrity for the other lines. The only reason you would not do this is if you are trying to save money by using a very low layer count board and you are willing to compromise on performance. \$\endgroup\$
    – The Photon
    Dec 12, 2016 at 20:31

2 Answers 2

Reset to default
2
\$\begingroup\$

I think you can do this, by using "jumper ID's".

Go to the footprint editor, open your "Rapsberry Pi" footprint, double click on one of the GND pins and in the next window set "Jumper ID" to "1" (or any other number). Do the same thing for remaining GND pads using the same number. Now you should see thin grey arcs between those pads - they are connected and you can route ground track to only one of them.

\$\endgroup\$
3
\$\begingroup\$

As the commments say, generally you should not do this. It's better to just connect all the GND pins together on your board.

If you must do this, for example because you're making a 1 layer board and signal integrity is not critical or not all GPIO pins are used, you will just have to do it manually. Start working on your schematic and figure out which GND pins are convenient to connect and which aren't. Then go back to the schematic and disconnect the ones that you don't want to have connected in the layout.

\$\endgroup\$
2
  • 2
    \$\begingroup\$ And give each one (i.e., each ground net) a unique name. Then, as you do the layout, you can update the schematic to connect each component pin that needs ground to the most appropriate ground net. \$\endgroup\$
    – Dave Tweed
    Dec 12, 2016 at 20:48
  • 1
    \$\begingroup\$ Although the OP is talking about multiple GND pins, I have a situation where a dozen I/O lines are duplicated on 4 B2B connectors. It's a nightmare to connect them all, and also not pleasant to go back and forth between layout and schematic to disconnect most of them. \$\endgroup\$
    – TimH - Codidact
    Feb 21, 2019 at 1:06

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge that you have read and understand our privacy policy and code of conduct.

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