No idea what your associate means about there not being any pads: your footprints all look OK. You should add some bulk decoupling (electrolytic between 10uF and 100uF) across VIN and GND by connector J1 and local decoupling (ceramic multilayer chip capacitors - MLCC - for preference rather than leaded) in the region of 100nF to 10nF region across VCC and GND and 3V3 and GND at the pins to every active device. The internal supply decoupling of the Ublox Neo-6M module looks to be done OK but some extra on the board would do no harm. [https://www.electroschematics.com/neo-6m-gps-module/](https://www.electroschematics.com/neo-6m-gps-module/)<br> <br> In general, your tracking could be much less spread out. With almost all your components (except the MLCC decouplers!) being through hole, the board is simple enough that you can very efficiently route everything by hand. Autorouting it will just make a mess for you to then have to try to tidy up by hand anyway. By routing between some of the pins where you have plenty of room, you could probably route the whole thing on one layer and have a completely uninterrupted ground plane. You could probably also then have split 5V and 3.3V planes on the top layer with your signal tracks breaking them up a bit but as long as all the parts of the 5V and 3.3V plane areas are connected to each other (at their respective voltages obviously) then that would remove the need to manually route the 5V and 3.3V supplies as dedicated tracks. This might then free up more even more routing space for the signal tracks. Lastly I would put the ground plane on the top (component side) layer and the supply plane areas and signal tracks on the bottom layer.

One thing to note is that although the Neo-6M runs off 3.3v the module is a 5v device. That module has an on-board 3.3v LDO regulator so no need to add one, just supply 5v to it. This should be a relatively easy edit. Using 3.3v will most certainly degrade the operation. _ Regards.

@mrtom528, Good spot: I'd missed that and thought it was already on the 5V net.

@andyfierman , Thank you very much for your answer. I will rework the design and come back to you, if you don't mind. To make sure I understood correctly: ground plane on top layer and split 5V and 3.3V planes and signals on bottom layer. Is that correct? As for the capacitor, can I use this type? My soldering skills are not very good and these are much easier.  Best regards.

@mrtom528 Thank you very much for your remark.

@andyfierman, It catches a lot of people out, me included, and gives the impression the device is faulty or just not good at it's job...whereas it's the most awesome module I've ever had the pleasure of letting the magic smoke out of. (Except the DS3231) _ Regards.

@jluquedz, You can use those for the ceramic parts. Keep the tracks to the GND and supply copper short and wide. This is why having supply and ground planes can help: as long as the supply planes are well connected, it reduces the impedance between the supply pads of the devices and the nearest capacitor pads.

For background, this may help you: [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)

@andyfierman Thank you, Andy.

@andyfierman Hi, Andy: I've done the rework you suggested. Is this what you meant? [https://oshwlab.com/jluquedz/quadcopter/](https://oshwlab.com/jluquedz/quadcopter/) , the updated PCB design is Quadcopter_v2. Some additional questions:    - Must 3V3 and 5V suppy planes cover all the board, even in places where no components use it (even under J1 connector)?    - Should the trace-power plane spacing be 0.65 because the trace width is 0.65?    - How much spacing do I need between both power planes? The 3V3 and 5V pads are very close in the arduino.    - Should the GPS antenna (which is mounted on top of the component have no ground and supply plane under it?    - Are the capacitors in the 5V-3V3 level shifter necessary?    Thank you very much in advance.

@jluquedz I do volunteer to make a finishing touch to your project if you need? Can make this pro bono, seems easy project to me.... Answers:     - Yes, it is advicable to have it all around the PCB, this way helps with signal integrity and this configuration also forms a low value capacitor between the ground plane.     - Trace-power plane spacing? Hmm..... Do you mean clearance value? I usually keep that around 0.012" / 0.305mm. Power trace width 0.032" / 0.813mm     - Clearance between two different power plains = 2 x 0.012" / 2 x 0.305mm     - This is GPS antenna connection point on an add-on module. So, no this is not critical to remove copper. Only if its a WiFi application but this is GPS.     - Capacitors are always welcome :-) Helps alot in transient responds of current flow on a voltage rail. Regards, Markus Virtanen HW / Electronics Designer

@markus_jidoka Hi, Markus: thank you very much for your answers and your offer! I'm willing to pay for that final touch, I understand your time is valuable. I'm going to change the spacings to the values you suggested. When it's done, can I PM you for a final review/touch? Regards, Javier Luque

@jluquedz Hi! Please do PM me once you are finished on your part. We can then later discuss review/touch privately. Regards, Markus Virtanen HW / Electronics Designer