Please post a link to a datasheet for the NRF24L01 wifi module. You probably need to move it so the antenna is clear of the edge of the board and need extra supply decoupling and maybe input filtering/pullup/downs on the other devices to avoid the wifi signal interfering with them.

[https://components101.com/sites/default/files/component_datasheet/nRF24L01%20Datasheet.pdf](https://components101.com/sites/default/files/component_datasheet/nRF24L01%20Datasheet.pdf) Yeah, I was wondering whether I should put it on the edge whether there is no need to do that.

My 2c: wifi is probably not the best solution here in terms of range and power. Have you considered low-power sub-1GHz modules? You will use less than a tenth the power for more than 10x the range, since you probably don't need that much bandwidth.

@martin I haven't really considered it, but I don't need wide range and have already bought the nrfs. But thanks for the suggestion.

@andyfierman [https://components101.com/sites/default/files/component_datasheet/nRF24L01%20Datasheet.pdf](https://components101.com/sites/default/files/component_datasheet/nRF24L01%20Datasheet.pdf) Yeah, I was wondering whether I should put it on the edge whether there is no need to do that.

@andyfierman [https://components101.com/sites/default/files/component_datasheet/nRF24L01%20Datasheet.pdf](https://components101.com/sites/default/files/component_datasheet/nRF24L01%20Datasheet.pdf) Yeah, I was wondering whether I should put it on the edge whether there is no need to do that.

@Hana Šustrová a couple quick comments, haven't looked deeply into your design. 1\. Yes\, the NRF module needs to be away from everthing \(case\, board\)\. If you can have it stand in free air\, do so\. These modules' antennae aren't well\-tuned to begin with\. Ask me why I moved from exactly those to making my own sub\-G\! Just sitting it on top of FR4 \(no ground\, even\) will result in pretty poor performance\. 2\. Ensure the ATmega328 \(haven't looked at its specs\) can source enough current for every led\, but more importantly\, can sink current for 8 of these\, as you are driving your 7\-segment display directly\. 3\. You board layout could use a bit of cleaning up\, imho\. You can use less space\, and maybe consider aligning parts on the X and Y axes? 4\. Use a ground pour on both sides and make use of GND there\.

@martin thanks for the answer I've moved the NRF more to the edge and tried to make the wiring a bit cleaner, I've also put all of the resistors in one line. I tried the circuit consisting of Arduino, 4 digit 7 segment display and the 2 shift registers and it worked fine. I tried using the ground pour, but every time I right clicked to finish the rectangle, nothing happened, there wasn't any filling only the dotted edge.

"I tried using the ground pour, but every time I right clicked to finish the rectangle, nothing happened, there wasn't any filling only the dotted edge." You have to give the copper area the same net name as the net you want it to connect to. The problem is that you have assigned a GND netname for you ground nets so (a) your copper area cannot not fill and more importantly, (b) you have at least 2 separate nets that you are using for ground **but which are not connected to each other.** Look at the highlighted ground net and then at pin 2 of H2:  * I strongly suggest that you read (2.2), (4) and (6) in (2) in: [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) before you go any further.

You also have no decoupling capacitors! Please see: [https://easyeda.com/forum/topic/UPDATED-Power-supply-decoupling-and-why-it-matters-30a39d0a77f34d5d8dc77e37c035b3d3](https://easyeda.com/forum/topic/UPDATED-Power-supply-decoupling-and-why-it-matters-30a39d0a77f34d5d8dc77e37c035b3d3)

As there's 2.4GHz RF in very close proximity to your devices, you should probably insert something like 100R resisotrs in series with all your device input pins and decouple each one to your ground plane directly at the input pins with something like a 100pF C0G or NP0 ceramic capacitor. Failure to do things like that are inviting RFI from your own transmitter to go round apparently randomly waggling your pins. Consider tying all unused pins to ground or supply where appropriate instead of just leaving them unconnected. Yes: they may have internal pullup/down but again those pullups could be overwhelmed by RF from you module. You will need to add copper areas for ground and for VCC. Probably doesn't matter which of top or bottom layer each is on but put GND on one layer, VCC on the other. I tend to prefer GND on the component side and VCC on the other as a short to GND when debugging is usually less spectacular (and more survivable by the components) than a short to VCC.

You may find adding a GND to your schematic will improve matters. I just threw one in, saved, updated the PCB, drew a copper area, assigned it to the GND net (default when prompted) and it worked fine.  Once thats sorted you can carry on with the sound advice already given. Regards.

@andyfierman @mrtom528 Thank you for the help, I managed to make the GND copper area on the component side, but I don't think it's necessary to ad VCC copper pour on the other side, because there aren't many VCC connection on the PCB. I've also seen a project, where almost all the same components were used and there was only one copper pour for GND. Here is link to the project: [https://howtomechatronics.com/projects/diy-arduino-rc-transmitter/](https://howtomechatronics.com/projects/diy-arduino-rc-transmitter/) But maybe I'm wrong. In case I'm right, how thick should be the VCC wires? After doing a little research I tried to add decoupling capacitors. I've read that there should be about 100uF capacitor on power source and that there should also be one 0.1 ceramic capacitor. I read about the NRF24L01 and there was written that 10uF electrolytic capacitor should be used, but I'm not sure if the ceramic 0.1 capacitor should be used there as well. "Consider tying all unused pins to ground or supply where appropriate instead of just leaving them unconnected. Yes: they may have internal pullup/down but again those pullups could be overwhelmed by RF from you module." Which pins do you mean exactly?

A VCC plane will ensure that you decoupling caps have the lowest possible impedance paths to both the VCC and the GND pins of your devices. Also. @MikeDB has written elsewhere about the fact that CMOS devices are effectively symmetrical about their mid swing voltage so they are best treated as needing the same low impedance path to VCC as to GND and therefore should, where possible, have the same type of copper plane for both GND and for VCC. "I'm not sure if the ceramic 0.1 capacitor should be used there as well." Since the internal circuit of the NRF24L01 module is not given, it would advisable to include the 100nF anyway. Don't forget that the smaller the value of the decoupling cap, the closer to the pins it is decoupling it should be. "Which pins do you mean exactly?" My bad: inputs. The D2 - D5 inputs presumably rely on internal pullups in the ARDUINO_NANO module? At the expense of a few mA more battery drain it would be wise to at least make provision for if not actually fitted some pullup resistors from the switches  to VCC and feeding from there through the series 100R and parallel 100pF to and located at the ARDUINO_NANO module input pins.

@andyfierman "The D2 - D5 inputs presumably rely on internal pullups in the ARDUINO_NANO module?" Yeah and I think it should be okay, because in the project to which I sent link earlier there are also button that use only internal pullup resistors. Could you please also have a look at the receiver, I'm not sure, whether there should some more capacitors near the MPU6050 or l298n motor driver [https://easyeda\.com/editor\#id=\|431bdb19c8a34d83827c5cd02a52f75c\|e2d1da72eb1a4ca3931d70e9b03835c7](https://easyeda.com/editor#id=|431bdb19c8a34d83827c5cd02a52f75c|e2d1da72eb1a4ca3931d70e9b03835c7)

Oh, and I forgot to ask how big should I make the clearance on the copper pour?

Every individual supply pin of every device should have its own decoupling capacitor. Please follow the guidelines given in the device datasheets. :)