Placing pads directly in the PCB is risky as they may be overwritten when doing Update PCB... or Import Changes... The correct way to deal with all components that or on or form an integral part of the PCB is to include them as symbols in the schematic and then assign Footprints to them from the library. Then when you do Convert to PCB, all the correct Footprints will be pulled into the PCB. Please see the Design Flow and read about Footprint Library and using the Footprint Manager in the Tutorial. Please also see: Project Sharing in the Tutorial and [https://easyeda.com/forum/topic/How-to-make-a-Project-public-and-share-the-links-to-it-9f006513b84b412580910905b0281d20](https://easyeda.com/forum/topic/How-to-make-a-Project-public-and-share-the-links-to-it-9f006513b84b412580910905b0281d20)

That makes sense to ensure there's a component available (or create one of there isn't). I have the resistors in my schematic but these are surface mount ones as I couldn't find my type (i.e. the ones that are mounted via pads). So either I look for the correct ones or create footprints for them - probably a good exercise anyway. I culdn't find the term 'Design flow'. You're talking about the tutorial here [https://docs.easyeda.com/en/FAQ/Editor/index.html](https://docs.easyeda.com/en/FAQ/Editor/index.html), right?

(1) in (2) in the 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)<br> <br> or direct link: [https://docs.easyeda.com/en/Introduction/Introduction-to-EasyEDA/index.html](https://docs.easyeda.com/en/Introduction/Introduction-to-EasyEDA/index.html)

Thanks for the pointers @andyfierman I have just published my PCB ([https://oshwlab.com/tfmeier/esp-dmx-endpoint_recover](https://oshwlab.com/tfmeier/esp-dmx-endpoint_recover)). I think this is good to go for production but would like to get some feedback from you guys. I'm sure this can be improved upon

I continue and try out the workflow to create a PCB. Have created the Gerber file, uploaded to JLCPCB and then ran the Gerber viewer. To my surprise the holes I had on the PCB in EasyEDA didn't show up. I have created them with the 'Holes' tool in PCB tools. Looking at the Tutorial it looks like I should use the 'Pad' not the 'Hole' tool. Is that correct? What is the 'hole' tool for in that case?

The likely reply is "It's not a bug"  Read the manual. I'm over trying to report bugs. Seems they don't exist. Mike.

@tfmeier, There are a number of things you need to fix before sending off for manufacture. * You have something way off the board toward the upper left of the canvas and maybe also not quite so far out in the lower right. When I open the PCB or when I press the K key the view zoom right out with a small board and a lot of seemingly blank canvas:  If you delete everything inside and including the board outline and then press K you'll see:  Mouse-X and Mouse-Y tells you where the rogue object is. Do CTRL-Z to undo deleting the board. Delete the rogue object, delete it then press K and you'll get to see the board properly:  Then Save it. * The antenna on U1 needs to be at the edge of the board and have no copper tracks or planes under or near it. RF does not play well with conductors near the antenna and can induce strange behaviour in stuff near it when transmitting. * It may be a good idea to put low resistance pullup/downs as required on unused inputs to stop stray RF causing trouble as described above. * It's bad practice to put text in copper layers. Put it in the relevant silkscreen layers or into the Documentation layer if it is not needed on the PCB itself. * Check your Gerbers using gerbv or one of the other recommended Gerber Viewers. At the moment it's better not to rely on the JLCPCB viewer: [https://docs.easyeda.com/en/PCB/Gerber-Generate/index.html#Gerber-View](https://docs.easyeda.com/en/PCB/Gerber-Generate/index.html#Gerber-View) In your schematic: 1. You have not placed a GND symbol and have not labelled any of the other nets. This helps make the schematic readable and helps in debugging and Cross Probing between schematic and PCB;  2. You have no decoupling capacitors. Please read and run the simulations in: [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).  You need a minimum of 10uF across the VCC and GND supply input connector and 100nF across all the supply pins (VCC and internal 3.3V pin on U1) to ground on each chip. Consider adding 100pF to 1nF in parallel with the 100nF to improve decoupling at RF;  3. To reduce overall power track impedances and help screen signal traces against RFI, you could put a ground copper area on the whole of the top layer (except around the antenna!) and then route the signal and VCC only on the bottom layer. This also simplifies decoupling cap placement and reduces ground return path impedance so improving decoupling. 4. Make the the dedicated VCC tracks as wide as possible. 5. Maybe even create a VCC copper area on the bottom layer if there is room for this without forcing tracks back into the top layer and so breaking up the GND plane;  6. The RST pin is floating. Is this OK? It might be a good idea to put and RC power on reset network on it to give a clean power up reset. For an active high reset then it's a C from RST to VCC and an R from RST to GND. RC time constant of about 10ms to 100ms should do it. * Recommend you read and go through the essential check lists (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)

Those points aside, your PCB including the holes (which I assume are for mountings) - generally looks OK. If you are socketing the two modules then you might like to follow the links in: [https://easyeda.com/forum/topic/How-to-represent-off-board-and-not-fitted-components-e03ea0937f924ab2a2b447c7445fcecf](https://easyeda.com/forum/topic/How-to-represent-off-board-and-not-fitted-components-e03ea0937f924ab2a2b447c7445fcecf)<br> <br>

Oh yes, nearly forgot. Don't waste your time trying to autoroute this board. Do it by hand: you'll learn stuff and end up with a better layout. :)

Wow, so much to learn. Thanks so much for this elaborate feedback @andyfierman. At the moment this is probably a 5 out of 10 :) Will incorporate these suggestions. Not sure I understand everything yet but have some reading up to do first :) And yes, the holes are for the purpose of mounting the PCB.

@tfmeier, For your first PCB, you're doing OK. Keep going and keep an open mind to absorb new ideas and information. :)