Go Down

Topic: Eagle - Many package connections to one device pin? (Read 8623 times) previous topic - next topic


Another Eagle component library question - if you have a package that has several pins all connected internally together (multiple grounds for example) is it possible to connect these all to the same pin in the device / symbol?

The pins to pads connection process seems to be a one to one relationship. I tried renaming the pads to the same name but it won't allow that... is there any other trick?



I think it's the Append button in the Connect dialog.


For things like multiple GNDs, I name them GND1, GND2, GND2, etc, and then make sure they are all connected on the schematic.
Designing & building electrical circuits for over 25 years.  Screw Shield for Mega/Due/Uno,  Bobuino with ATMega1284P, & other '328P & '1284P creations & offerings at  my website.

Tom Carpenter

Yup. Make one connection as normal, then select each additional pin in turn, pressing append after selecting.


There's a trick for that; IIRC it involves @ in the name.  e.g. pins GND@1 GND@2 GND@3 are all GND.

Do some googling and you'll find details.



Ah yes - append what I needed - screamingly obvious when you know!


Spoke too soon - the Append isn't quite what I needed since Eagle will still run a ghost wire between the two pads and expect them to be connected with a trace, whereas they are electrically connected on the physical device, so the trace is unnecessary.

I looked at the @ option too but that seems to require a symbol pin for each connected pad. The example I have is a battery holder, so obviously I want a standard 2 pin battery symbol for the circuit...


I looked at the @ option too but that seems to require a symbol pin for each connected pad. The example I have is a battery holder, so obviously I want a standard 2 pin battery symbol for the circuit...

I think you call the one on the symbol GND, but it will want all of the GND@X pins connected on the PCB.

You don't have to connect all of the pins to the device, so you can have GND, GND2, and + pins on the package, but only have GND and + on the device.  This would leave you with a permanently isolated pad on the board (so you have mechanical mounting) but no electrical connection.

For example, here's a coin cell battery holder from the Sparkfun eagle library that has a large SMT pad for one side of the battery and two through-holes which are electrically connected on the battery holder, but only one of them is connected in the library device and the results is the electrically isolated through-hole.

Is that what you're after?



Not quite - I want to be able to connect to either of the hole pads on a layout by layout basis, and want it to know that they are electrically connected/equivalent without having to connect them myself via PCB traces.

From looking at what Sparkfun have done, I think it's safe to assume I can't.


This is a common Eagle question, and no, it can't be done. Crossroads' advice is the way to go.


Yes it can be done.

Just click the append icon that shows when you append a pin. It changes to an diferent pic. That makes eagle assume the signal is routed internally in the component.


Blimey! talk about hiding functionality!!


I agree it can be done and doing it as separate gnd1 gnd2 I think is not really a good way to do it.

besides making it internally connected, there is yet another (hidden) functionality to make the router still route a pcb trace or not.

when you view the connection dialog and after you append pads with the same connection together, you will see there is an icon with 2 pads and a trace. you can click on the icon to connect or disconnect the trace.

if trace is connected, the router will connect all pads with traces. this is usually not desired in my case.

I usually leave it disconnected, and this allows the router to connect trace to one pad, and use another internally connected pad to route a trace to other devices if that is more optimzed way.

Go Up