This is the official schematic of ESP32-CAM:
Here is the area of interest:
Why does this schematic imply that the 3.3V and 5V power lines are shorted through 0 ohm resistors? The masured voltage at P1 pin 4 is 3.3V.
I took a closer look at the PCB and noticed that there are unpopulated resistor pads. Is this a normal way to indicate 0 ohm permanent (factory configuration) jumpers on the diagram? If so, is there a clearer way to indicate that only one of these resistors is present?
The schematic as shown is adequate to create the PCB but does not indicate how it should be populated.
Typically we’d place a DNP (do not populate) designation on one of the parts, or place a note on the schematic to populate only one of the two.
But even professionally designed schematics lack this sometimes- you may have to consult the BOM, or even look at a physical board.
That board was designed in Altium, by the looks of it, which has features to support assembly variants. I’m not sure how many actually use those features. The variants are shown as tabs on a ‘live’ schematic, which doesn’t translate directly to a static printed page.
This is an easy way to provide selection for the desired voltage. The Bill of Materials (BOM) will indicate if a part is to be installed or not by using a do-not-install (DNI) or do-not-populate (DNP) indication. Sometimes you will see this on the schematic diagram as well.
Special pad-only parts called solder-bridge jumpers can be used as well. They are normally open and a solder bridge is installed at production or in te field. THe same pad shape can be used with a copper trace in between (normally closed) that can be cut with a knife toreconfigure, It can later be closed with a solder bridge.
So, no, the 0 ohm resistors would not be installed at the same time.
The resistors are easily placed by a pick-and-place machine. The solder bridge parts must be configured manually.
Only one zero ohm resistor should be installed. This allows you to select the power supply voltage, either 5.0 V or 3.3 V. If you have it wired for 3.3V, perhaps U2 should be removed unless the regulator can handle 3.3V on its output without anything connected to the input.
A more informative schematic would have a comment beside this conundrum.
They are in the schematic but they wouldn't be on the board.
This is used to allow a single design to have two uses. One could be 5v and one can be 3.3v based on which resistor is populated. Or a user selectable feature.
In agreement with many of the other answers in that only one of those zero ohm resistors would be installed for any given usage of the circuit.
One thing that was asked is if there is a better way to indicate the "not used" installation of a component. Here are examples of two different designs I have done where this indication can be shown on the schematic. In this first example the circuit board design had provisions for two different types of LEDs at the edge of the circuit board for two different options of the LED size and mounting.
Another example uses a special graphic on the design to show "not installed" resistors as follows:
