HOW-TO: Create Eagle parts with pins that have the same name

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 and name multiple part pins the same thing.

Keep reading below, see our other Eagle tutorials here.

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.

Join the Conversation


  1. It can be helpful to include the @PIN# suffix on every pin, not just the repeated ones.

    This makes mapping the schematic pins to package pins during device creation faster and less prone to error.

  2. I just discovered another way around this, I would like to share: I have a component with 9 heatdistributing groundpads in the middle (its a 20QFN package) and I don’t wan’t them to show up in the schematic as that would be pretty messy. So I have a symbol that has the 20 pin connections and a package with 29 pads. When making the final component and connecting the symbol pins to the package pads there is an option called “Append” as opposed to “Connect”. It seems like it is possible to connect the VSS pin to the right pad and after that append all the 9 ground pads to that same pin. This is another way to solve it if you wan’t to hide some of the groundpins in the schematic, like in this situation!

  3. There is another, dirty way of doing this, if you do not want your part in the schematic show so many pins with the same name.

    When you create the symbol, create eg the GND PINs with the name with GND@1 , GND@2 , GND@3 etc as described.
    However, now put all these pins on on top of each other. In the schematic they will show as one pin with the name in front of the @ character, so in the case pin GND .
    But be carefull,
    To make sure you connect to all stacked pins, in the schematic, not only draw a connection to this pin, but also put a junction dot on top of it, so you are sure to connect to all three.

  4. The Proper way to connect multiple Pads to one Pin is however to just create both the Symbol and the Package as they should be, the Package with more Pads then the Symbol has Pins.
    When building the Device, connect the the appropriate Pin to the first of its Pads, then select the second Pad in the list and hit Append.
    Now the second Pad is connected to this Pin, regardless name.

Leave a comment

Your email address will not be published. Required fields are marked *

Notify me of followup comments via e-mail. You can also subscribe without commenting.