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?
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.
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.
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.
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.
Do not forget inside the device is a tiny, tiny chip bonded to external pins.
If multiple pins are connected internally, the reason is probably to reduce the load on each bond to the chip.
Leaving an internally connected pin unconnected also makes it a small antenna.
And while connecting remember large loops is where magnetic fields, tv programs, cosmic flares from the sun and nuclear blasts can induce current and disintegrate the project sometime in the future.