Hi! I recommend using the same trace witdh for V- / GND that you used with the V+/VSYS2BAT Also add a decoupling capacitor there between V+ and V-. You have good space for it in bottom right corner. And tank (electrolytic)capacitor would be also recommended. [https://lcsc\.com/product\-detail/Aluminum\-Electrolytic\-Capacitors\-Leaded\_Xunda\-TP4761EMC117RB\_C399073\.html](https://lcsc.com/product-detail/Aluminum-Electrolytic-Capacitors-Leaded_Xunda-TP4761EMC117RB_C399073.html) [https://lcsc\.com/product\-detail/Others\_Dersonic\-CD1H104MC9BEF4D000\_C263185\.html](https://lcsc.com/product-detail/Others_Dersonic-CD1H104MC9BEF4D000_C263185.html)<br> <br> You have very clearance issue marked here with X  And it is advisable to route the traces straight in 90 degree angles to the pins and not 45 degree. This produces the clearance error just like the one I added to the picture. One more thing: add a bit more trace width to the buzzer minus signal. Currently it is 0.254mm. I suggest to double that. And in schematic it should be H2, pin 12, not pin 1. So there is some routing mistakes with switches and buzzer. Regards, Markus Virtanen HW / Electronics Designer

@f.sofras, I recommend that you read (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) In that you will find two essential checklists (4) and (6) which you should go through before converting a schematic to PCB and before submitting a  design for fabrication.

@f.sofras, * Please also remember to post the url to a public project and to clearly identify which version of the PCB that you want people to make the time to review for you: [https://easyeda.com/f.sofras/test2](https://easyeda.com/f.sofras/test2)<br> <br> * It is not clear but I assume that PCB_test4 is the final PCB that you wish to review: [https://easyeda.com/editor#id=be775e98c633475c9763d38043c074c8](https://easyeda.com/editor#id=be775e98c633475c9763d38043c074c8)<br> <br> * You have several ground pins that are unconnected because you have no tracks or ground copper area to connect them:  * These vias are unnecessary because the OLED is a through hole packaged device:  * Regarding your Schematic, please read Appendix A of (2.2): [https://docs.google.com/document/d/1CU7RuPyFlSZPzWBN-YZ0x87xeAB4xpLdLaIsUwhLj_M/edit#heading=h.xxt5yo1ar0j6](https://docs.google.com/document/d/1CU7RuPyFlSZPzWBN-YZ0x87xeAB4xpLdLaIsUwhLj_M/edit#heading=h.xxt5yo1ar0j6)<br> <br> 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)<br> <br> to understand how to properly deal with off-board components (i.e. H1 and H2 are on-board, the processor is off-board). (Recommend that you read all of that document, (2.2)). * You have one extra switch which is unconnected in your Schematic and which, depending on the PCB versions may be SW8 or SW9 in your PCB: 

Thank you Markus and [andyfierman](https://easyeda.com/andyfierman). I will follow your instructions

@Markus_ee Markus, I thought that traces should not run at 90 degrees. Am I wrong

@f.sofras, What @Markus_ee is referring to is the trace entry to the connector pins to avoid traces getting too close to other pads. Usual practice is to route with the routing angle canvas attribute set to 45 degrees so that tracks route at any increment of 45 degrees i.e. 0, 45, 90, 135, etc. You can use rounded corners with 45 degree routing which likes pretty but has little other effect. You can use free angle routing as you have done here but on crowded boards that can end up wasting a lot of space. If traces on different layers where there is no copper plane separating them (so this always applies to 2 layer boards) have to cross, they should always do so at 90 degrees. Except for synchronous buses, differential traces and broadside or edge coupled striplines, tracks should not be run parallel to each other for any significant length either on the same or on different layers.

Thank you andyfierman

I like it for a First play. Have a look at other Circuits and get a feel for it. get your circuit and look where you can Save SPACE, and costs .. Smaller board is a bit cheaper. <br> Also Windows 7 i think they stopped supporting that From a Crazy Hippy off beat Designer.. some boards are like a work of art, you leave your own mark and style and sign it Ive always wanted to have Sign my Name in Track on a board :) also this Software isnt Perfect

Thank you everybody Today I am a bit perplexed because I think that I wired my LEDs incorectly (anode instead of cathode) Will you have a look at the PCB and tell me which part is Anode? Thanks for your time

Please confirm which PCB version in your project: [https://easyeda.com/f.sofras/test2](https://easyeda.com/f.sofras/test2)<br> <br> that you are asking about.

In your schematic you now have an extra LED9 and an extra switch SW9 which do not appear on PCB_test4. I do not know how you have generated PCB_test5 but it is not by doing Convert to PCB... from your schematic. Many of the component prefixes do not exist in the schematic and two of the LEDs are wired up back to front which will not be indicated in the Design Manager because the netlist is not derived directly from the schematic (which is correct as far as the LED orientation is concerned).

Thank you andyfierman. As you correctly guessed the "final" working version is **PCB_test5.** Although in the beginning I used the schematic, from some point onward I directly used the PCB so that I can put the components at the place I wanted. I turned off ratlines as they are confusing and manually drew the traces. I then had to move the resistors to the front so that the production service can solder them (they only solder ONE side!!) and I was not sure which part of the led was anode. I have sorted things now. You must admit not too bad for a week's work (from starting with easyEDA) from a retired surgeon! Thank you for all your comments and kindness

@f.sofras, Well done but I recommend for your next projects that you study the EasyEDA Tutorials (and the links in the documents I pointed you to earlier) and follow the Design Flow to avoid most of the problems that you have encountered in this one. Because you have gone so far off-piste by decoupling the layout from the original schematic you must check everything very carefully as the Design Managers are now operating from two different designs so they will be of little help in checking the layout to the original schematic. And therefore the scope for mistakes in both going undetected is much greater. "I directly used the PCB so that I can put the components at the place I wanted." I don't understand the problem here: When you do Convert to PCB... all the footprints are pulled into the PCB and placed in a grid. Thereafter you just place them where you want by dragging them. The Ratlines show you connectivity, not routing but they do show the shortest direct line between nodes that are connected together so you can use them to show you the best placements to simplify the routing. That minimises the effort needed for both manual and autorouted layout. I recommend that you read: [https://easyeda.com/forum/topic/Understanding-Ratlines-371bdbf646c54b23a57451eb05b2026d](https://easyeda.com/forum/topic/Understanding-Ratlines-371bdbf646c54b23a57451eb05b2026d)<br> <br> and this handy trick to help with component autoplacement: [https://easyeda.com/forum/topic/Component-autoplacement-into-PCB-3f0f310db0d74a9bbf848953c4c8048d](https://easyeda.com/forum/topic/Component-autoplacement-into-PCB-3f0f310db0d74a9bbf848953c4c8048d)<br> <br> <br> <br>

@f.sofras, Um, I hope you have not ordered this PCB yet. I've just had another look at your PCB_test5 and can see several errors in it. 1) In the schematic you have effectively numbered H1, 1 to 20 then H2, 1 to 20 in an anticlockwise sense (starting at H1 pin 1 then going to H1 pin 2 etc.). On the PCB you have numbered them (looking at them through the board because they are on the bottom layer) and going anti clockwise from pin 1 of H1, so that H1 goes from 1 to 20 but then H2 goes from pin 20 to 1. I can't easily work out which of H1 or H2 it is but one of them has is the wrong way round with respect to the schematic. As I have pointed out earlier, this is because you have not created the PCB by doing Convert to PCB... from the schematic. Hence there is no way to check your PCB connectivity against that of the schematic. As it happens I think you have reversed the orientation of H2 w.r.t. the scheatic but have also reversed the connections to it in the PCB so in fact the connectivity is correct but it's very hard to tell when you're looking at it through the PCB. Also because you turned off the Ratlines you have limited visual feedback while you are connecting things up. 2) In both the schematic and the PCB there are several ground pins that you have left unconnected. Please check the incomplete nets in the PCB Design Manager. 3) You have not added any of the decoupling capacitances that Markus recommended. Please see -  and run the simulations in - this project: [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)<br> <br>

@f.sofras Hi Frank! I could volunteer to make a few "touch ups" before ordering this PCB, if you want to invite me to your project? Let me know if you are interested.... Regards, Markus Virtanen HW / Electronics Designer

@andyfierman Thank you Andy for taking the time to check the PCB Regarding the H1 and H2 component, they are there so that I can insert a raspberry PICO **board.** The connections have been made with this in mind and I have triple checked that they correspond to the PICO pins. You are right about the GND pins, maybe I should connect them all to GND(?) but what if they are not be used? Regarding decoupling, if I use a regulated 5V or power the whole project from the pico board, do I still need to decouple the power supply? Thanks for your help

@markus_jidoka I would appreciate your help How do I invite you to participate?

@f.sofras, GND pins should always be connected to GND. Supplies should always be decoupled by a minimum of about 10uF where the connections enter the PCB and 10pnf where they enter a device, chip or module. You are in good hands with Markus to help you and I think you will be pleasantly  surprised by the results...

 write my user name to search field "markus_jidoka" and click add  Then change my roles / rights to "developer"  -Markus

Hi Andy! Thank you for your kind words :-) -Markus

@markus_jidoka Markus I am sorry but I can't (for the life of me) find the page you showed. Maybe it's my Win 7? <br> <br> 

Hi! right click on top of your project folder  -Markus

Hello! Why is the resistance R1 seen in "TopLayer" and not seen as capacitor C1? In "BottomLayer" it looks normal. It's a problem? 

@va-cristi WHICH pcb ARE YOU LOOKING AT?

@Frank Sofras ``` I haven't opened another topic. It's a project of mine. ```

@va-cristi I think you should open a topic with new your question

@va-cristi, 1. Please do not hijack other people's topics;  2. Please post your question as a new topic with enough supporting information to allow others - who know nothing about your project - to offer helpful advice. 3. Please 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>

Hi! Project has advanced to v2.1. And hopefully this is completed version as well..... Corrected fabrication files has been added to attachments. All other parts on top, headers and buzzer at bottom. C5 is practice area where you can add your own 100nF - 1uF / 1206 capacitor just for good measure. Hopefully Frank and others are pleased with this game PCB :-) Regards, Markus Virtanen HW / Electronics Designer