buffereaglepcb-designschematics
I am using a 4050, the schematic uses the triangle representation.
I have added VCC and GND connectors to a power supply of 3.3V in the schematic, hoping Eagle recognizes the connections. However the physical pins on the PCB aren't connected to any net. Also I have tried completing all the buffers on one chip, but no results on finding the connections.
Maybe it should be done manually?
Thanks for the help.
Try running the invoke command: 
It is possible that the power/ground has been made a separate gate from the main switch block. Usually this is done when you have multiple functional blocks within a chip sharing a single power supply (e.g., a dual/quad switch), but perhaps it is the case here also.
The Electrical Rule Check executes, depending on the pin direction (specified by the author of the schematic symbol), various checks. It expects for the direction of type Pwr a Sup pin set for this net. Sup is a pin type for power supply outputs for ground and supply symbols.
From the Eagle manual:
"[...] For every Pwr-pin there must be at least one pin with the same name but the direction Sup(a supply pin). There must be one on every sheet. These Sup pins are fetched into the schematic in the form of power supply symbols, and are defined as Devices in a library (see supply*.lbr). These Devices do not have a Package, since they do not represent components. [...]"
Further...
"If there is no supply pin in the supply libraries that fits to your voltage in the schematic, you have to define a new supply pin! Renaming an already existing supply pin is the wrong way and can lead to unexpected results!"
Best Answer
In Eagle, single physical parts can be broken into logical "gates". This is meant for exactly this situation, where you have a collection of independent logic gates in a single package that share certain pins, like power and ground.
In this case, there will be one gate for each inverter, and a separate one for the power and ground pins. This allows the power and ground to be connected once and not clutter the schematic of every gate or make one gate look different.
The way to get another gate of a multi-gate device onto the schematic is with the INVOKE command. Do HELP INV to see all the details, but briefly, INV IC4 should bring up a dialog window that shows you all the gates, which ones are already on the schematic, which ones are left, and allow you to add one of the unused ones to the schematic.
By the way, it is good practice to bring all the gates onto the schematic, whether used in the circuit or not. In the case of unused logic gates, tie inputs low or otherwise ensure they can't switch or oscillate from capacitively coupled noise.