If you created a schematic and the PCB in a single EasyEDA Project then you can use the Schematic and PCB Design Managers to check the connectivity of both and to check that they are the same. Since your board is made from Gerber files generated by EasyEDA from the EasyEDA PCB Editor then the physical PCB will be correct to the PCB file in the EasyEDA PCB Editor. In other words the real physical PCB will have the same connectivity as the PCB file in the PCB Editor. So if you find a connectivity mistake in the PCB in the EasyEDA PCB Editor then that fault will exist in the physical board and therefore you will have found the problem. If you did not create a schematic in EasyEDA then you can still check the connectivity but it is harder to be sure since you have no EasyEDA schematic to refer to. To confirm the fault in the physical PCB you can use an Ohmmeter or a Continuity Tester. This situation demonstrates the importance of following the Design Flow in the EasyEDA Tutorial and doing all the essential checks detailed in (4) and (6) in (2) in the Forum topic marked [Must read]: [https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a](https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a)

Hello andyfierman, Thank you for your fast reply. I did not mention it before so as not to make the message too long, but I designed the circuit following all the steps indicated in the tutorials. I also did the checks you mention, before ordering the PCB’s. Additionally, it is a circuit that I have been working with for a long time (assembled in a proto board) and I know that the connections work. It is the first time I work with a PCB. In the attached image it is shown an example of what is not working. It is a part of the PCB taken from the 3D View of the EasyEDA software. The "-" and "+" holes at the bottom are where I connect the power (5V). The upper three holes are where the IR sensor is located. If I connect 5V in the lower holes and then I measure the voltage in the holes “A” and “B”, the result in the multimeter display is 0 V, but, theoretically, I should read approx. 5 V. Am I right?  It seems like there is no current flowing through the tracks. Is it possible? Is there any way to check and confirm it? Thank you again!

Screenshots of a PCB from the 3d viewer with no supporting idea of the schematic is somewhat less that helpful to diagnose a problem. There are other tracks on your board which are not shown. You may have a short between the 5V supplies elsewhere on your board but it is impossible to know this from your screenshot. A simple check with an Ohmmeter as already advised will tell you if you have a short circuit across the supplies on the board. To find it in the PCB use the Design Managers. That's what they are there for. Can you simply make your project public so people can see the schematic and the PCB in the editor?

Hello again, Thank you for your answer. I thought that showing the screenshot with a simple check of voltage would be enough to get an insight on what would be happening, but if the whole project is preferred, I have just made it public in the following link: [https://easyeda\.com/javi\_sin/prueba\_pcb](https://easyeda.com/javi_sin/prueba_pcb) I hope it can help to check the error in the pcb. Thank you!

@javi_sin, "...I designed the circuit following all the steps indicated in the tutorials." I think not. There is no Schematic in your project.

The Schematic is now available too: [https://easyeda\.com/javi\_sin/prueba\_pcb](https://easyeda.com/javi_sin/prueba_pcb) I worked on the project offline and I could only import the PCB to online mode. Since I couldn't import the Schematic (I didn't find the way), I have created it again. Between the D11 pin of the arduino and the DF Player mini will be located a resistance of 1 kOhms (it is not drawn in the Schematic, but the holes are defined in the PCB). I hope now you can help me. Thanks

Sorry but this is what happens when you do not follow the recommended Design Flow and do not take sufficient care when carrying out the checks from our list:  You have a bunch of copper traces that are not connected to each other or to pads because the nets have different net names from the pads and other copper tracks that they are supposed to connect to. Having seen this in the EasyEDA PCB file, they are just about visible in your screenshot but only because I now know they are there. If you check using the design manager you will see that lots of tracks that are supposed to be connected together and therefore should have the same net names in fact all have different nemt names. Also if you click on a track that you intended to be joined to others and then press the H key, you will see that only parts of the whole net light up instead of all the tracks that are supposed to. You also have tracks where one part of it has one net name and the other part of the net has a different name:   You can salvage your boards by scraping some of the soldermask back from the gaps and carefilly soldering wire bridges across them.

The symbol you chose for the DFRobot\_Mp3\_Player is incorrect\. As advised in:various places in EasyEDA you **must** check **all** User Contributed symbols and footprints. I have reported the following error for it: **Pin orientation is reversed: connect dot end is inside symbol, not outside.**

You are right about the unconnected traces. And it's a pitty, because when I drew them from one pad center to another, the software put above a yellow cross and then it turned into the current configuration, so I misunderstood that the software itself corrected and adapted the PCB and there was no problem there. I should ask in that moment to avoid the mistake (and also take more care of your recommendations). Thank you for your feedback! Regarding the incorrect symbol for the DFRobot, I don't understand why it is incorrect. The part fits dimensionally well in the PCB, but it's ok if your report serves to improve it.

@javi_sin, Given some of the  questions you have asked and comments you have made, I  strongly recommend that you re-read, including all the documents that it points to: [https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a](https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a) and then as advised in there, create a simple dummy project (you could redo yours from scratch) following all the steps and checks that you will find in those documents. You will have a lot more fun and success that way. :)

@andyfierman For sure, I'll do that. Thank you for your fast reply to all my comments during the day.

Here's what's wrong with the DFRobot\_Mp3\_Player symbol\. The grey circle at the end of the pin is the connection point. It is where a connection to that pin snaps to. The connection node should be on the outside of the device not the inside.  Consequently, for this symbol, none of your wires actually snapped to the pins on this symbol which breaks the inheritance of net names onto the pads of the PCB Footprint when you converted the schematic to a PCB. This is explained in detail in the Tutorial: [https://docs.easyeda.com/en/SchematicLib/SchLib-Create/index.html](https://docs.easyeda.com/en/SchematicLib/SchLib-Create/index.html)