Creating parts with the same pin names
Most chips have multiple power pins that need to be connected to the same power supply, but Eagle doesn't allow you to give 2 different pins the same name. This short tutorial shows how to get around this limitation and connect multiple part pins to the same trace.
Create a symbol
We start by creating a symbol for the part. A good example for this exercise is the LTC4053 IC which has a large exposed pad on the bottom that connects to ground.
This IC has two GND pins, one on pin 5, and the other connected to the exposed pad (pin11).
Eagle will allow you to use the same name provided that you differentiate them by using ‘@’ character after the name, followed by a number. The suffix ‘@x’ will be omitted in the schematic, only the name will be shown.
The pins with the same name still act as individual pins, and are not connected to each other. You still have to wire them to the same trace in the schematic.
Create a footprint
Create a package. This IC has an MSOP-10 footprint, notice the exposed pad right at the bottom of the chip.
Create a device
Create a new device. Add the symbol we made and the “MSOP-10” footprint.
Connect the symbol pins to the correct footprint pins. GND@1 is connected to pin 5 and GND@2 to pin 11 (the exposed pad), or vice versa.
Check your work
Create a new schematic, and add the part (LTC4053 in our example) you've made. Both pin 5 and pin 11 should have the same pin name as shown here.