EAGLE Implicit Pins – Addlevel Explanation
EAGLE Addlevel Parameter
Implicit Pins
Sometimes in EAGLE, you’ll see errors and warning based on implicit pins. I touched on this before, but it’s something that deserves a little more attention. For many ICs, the device in EAGLE includes the I/O pins in the symbol you place on the diagram, and the power and ground pins as a separate symbol that can only be accessed through the Invoke tool. By default, these pins are connected to particular power and ground nets, such as VCC and DGND, or VDD and VSS. If you don’t have these same power and ground names in your schematic, then these pins will be unconnected in your schematic.
There are different ways to remedy this situation. One, is to rename your power and ground nets to the same name as the implicit pins. This is fine if you have one pair of implicit pins, but what if you have multiple ICs with implicit pins, all using different name sets? You could add and connect multiple supply symbols, each with a name corresponding to the names you need for your implicit pins, but this can cause problems later on during editing. My preferred method is to simply use the Invoke tool, add these pins to the schematic, then connect whatever supplies you have on your schematic to these recently added implicit pins.
Creating Implicit Pins
This, and other available options, can be very useful in the devices you create in EAGLE. To do this, you need to have more than one symbol in your device, and then set the addlevel parameter to the appropriate value for each symbol. EAGLE refers to multiple symbols in one device as gates, and I will keep with this naming convention for consistency. The addlevel values and outlined below.
Next – Any gate whose addlevel is set to next (the default value) will be added to the schematic one at a time in the order they were placed when you created the device. These gates can be deleted from the schematic without deleting the entire device. For a dual op-amp IC, you can set each to next so that you can add only one if you only plan on using one of the op-amps, but still allows you to add both gates if you’re going to use both op-amps.
Must – These gates will be added along with the first gate. They cannot be deleted until all other gates are deleted, and all will be deleted at once. Use Must for parts of an IC that, if unused, would prevent proper operation.
Always – Gates with addlevel set to Always, will always be added to the schematic when you use the device. The difference between Always and Must, is that these gates can be deleted after the device is added. Use always for parts of an IC that rarely go unused, but that aren’t required for proper operation.
Request – This is the setting for implicit pins. They will not be an option like the gates marked as request, but can be added by using the Invoke tool and clicking on one of the gates you’ve already placed.
Can – Similar to request. The only difference comes when all gates are set to Request or Can, in which case it seems that all gates are added simultaneously. I had to create a test device for this, as I’ve never seen this addlevel used.
Usefulness
For ICs with high pin counts, using multiple gates within the device can help keep your schematic clean and easy to read by allowing you to place each gate in an area of your schematic that makes sense, rather than placing one big block of pins in one place. It also helps keep it uncluttered by allowing you not to place a bunch of pins that you won’t use. The video shows an example using multiple dip switches.
I hope this and my other EAGLE tutorials have helped. I’ll continue posting things that I think are interesting, that helped me, or that took me some time to learn, but if you have any questions, shoot me an email at chris@ece101.com.