Somebody to review my PCB
176 7
Jim Krug 2 months ago
I completed my first PCB. But I really knew nothing when I started. How do I get someone to review what I made and tell me if it can be created or if I have problems? It began as a copy from a PCB by HowToMechatronics, but I ended up completely revamping it (to use a Nano). I want to get it printed, but it needs a critical review first. Can anybody help? Also, I don't know how to publish it so people can review it. And once people tell me it looks okay, how do I get it created? 1. Did I route something wrong? I noticed that the original from HowToMechatronics did not route the GND lines. I didn't understand why, so I routed them. 2. Are any of the lines too close? 3. I intend to power it though the USB port on the Arduino Nano using a Cell phone battery pack. So, no switch...just unplug. P.S. This site ROCKS! Needs better learning tools and help information, but functionality of the site is excellent! P.P.S - I think I made the project public.  [https://easyeda.com/jimkrug/arduino-radio-controller](https://easyeda.com/jimkrug/arduino-radio-controller)  I want "Using Arduino Nano" reviewed. Feel free to review the other one, but GND is not routed and I don't know how it would work. Plus I think RobotDYN's board does not work properly with MISO and MOSI. I have 3 boards...none work. Nano worked on the first try.
Comments
andyfierman 2 months ago
If you read the sticky forum post marked as [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) that will point you to a series of linked documents, two of which are the essential checklists you must go through before you (a) convert a schematic to PCB and (b) submit the PCB produced from that schematic, for manufacture. And yes, you have successfully made your project public so others can look at it. :)
Reply
Jim Krug 2 months ago
@andyfierman Thanks. I was able to correct a number of minor issues. My board has no components & no schematic. I will be soldering everything onto it. The bulk of the instructions are about schematics and converting them to PCB. I think my last item is that I don't know how to get the net for GND to stop having the red X. I will look more for how to get the board created. Still looking for anybody to give it a quick once over and highlight any issues they see.
Reply
andyfierman 2 months ago
I'll look when i have a mo.
Reply
deskpro256 2 months ago
Hey, I finally decided to have a go at this. I'm in no shape or form a design guru or a grand specialist, but an EE student, but doing this a few years I've learned a few things. This will be a bit long, so prepare yourself! :) I'll try to reply to your questions first: > Did I route something wrong? I noticed that the original from HowToMechatronics did not route the GND lines. I didn't understand why, so I routed them Well, you didn't have a schematic here before the PCB so you're all-in I'd say. Either you have the components and their connections correct or not. If HowToMechatronics had a schematic you worked from, it should work. I saw his video a while back if I remember it did work. But from a first look they seem fine. The routing is a bit messy, but we all start somewhere and this also is messy, but works: ![back.jpeg](//image.easyeda.com/pullimage/Il74VlY9F8eniX31DyhwXJ1QwSgXhlNqCRpMmjaj.jpeg) I'd say if the traces are connected to the right components, it'll do the job. The I2C connections look like they are connected correctly, SPI lines too. For your own sanity and wallet, further projects will be a lot easier with a schematic, then the routing is also easier. The ratsnest basically does the hard job for you and you just connect the dots. About the GND. HowToMechatronics doesn't connect the GND pins because he adds a ground pour on the top layer which will connect all the GND connections: [https://youtu.be/-BDCmwNssiw?t=218](https://youtu.be/-BDCmwNssiw?t=218) The error you have is due to the Nano having 2 GND pins but you have them unconnected. The DRC doesn't know that the pins are connected on the module, so it thinks they need to be connected. ![Screenshot_3.png](//image.easyeda.com/pullimage/MV6dJQ8x2komIb9JsmdBCuU8VHDnWm2EcbKbpUpj.png) With the ground pour on the top layer  the error will disappear. But I'd suggest that you put the ground pours on both the top and bottom layers. That will use less etchant in the PCB manufacturers and save copper, as well as remove the possibility that the board can warp due to one side having lots of copper and the other not at all. You can notice this phenomena when you wet one side of a paper sheet, it starts to warp on one side. That can happen with PCB's too. Maybe not this one, but when you later have bigger boards, that may be an issue and you'll know how to fix that. > Are any of the lines too close? To my liking, yes. Some 5V traces near the joystick are too close to the mounting holes. To be on the safe side route them a bit further off for unexpected surprises later :) Also the 5V traces could be a bit thicker. Now you have them with 10mil(0.254 mm) thickness. You could make them 20mil(0.508 mm) for good measure. That will make sure you can have more than 1A could flow through them without problems. For trace width and other PCB calculating stuff, there is a great tool: Saturn PCB Design Toolkit It is free to use and makes your life easier. > I intend to power it though the USB port on the Arduino Nano using a Cell phone battery pack. So, no switch...just unplug. Make sure your power bank doesn't have that annoying low current shut-off thing. You know, when it detects a high current device it gives out the 5V, but when you plug in your low power project, it turns off after a while. For the GND error fix: Double click on the crossed GND under Nets. It will pop up a message asking if you want to unroute this net. Select unroute. ![Screenshot_4.png](//image.easyeda.com/pullimage/eE9m5KpAANLHX5zkbspOPvHfT3c6HHXBwEHYKf7y.png) Then select the top layer, and use the Copper area tool, click OK: ![Screenshot_5.png](//image.easyeda.com/pullimage/2X15HaI95ECQi5HiOrlsCV4A2XVW43k3Twkcz2eV.png) Then draw a figure around the PCB so it overlaps it everywhere and do the same for the bottom layer: ![Screenshot_6.png](//image.easyeda.com/pullimage/LUgWxR8wGupbWnGzmlTq9qmzsCJZ8udfLf3lhz93.png) Here are some images from the traces that in my opinion are too close. You can recheck other traces too. ![Screenshot_9.png](//image.easyeda.com/pullimage/tCasLcklXwd9VdHWDbKGNu3Rm6NOKyChycYoKi57.png) **Now for your PCB ordering.** When you finish the board layout and you are happy with how it looks and think it's done, leave it to sit there for a few hours or the next morning. The come back and look at it again. See what it feels like then. If its OK, then generate that gerber file for the PCB manufacturer, which in this case will most likely be JLCPCB. ![Screenshot_11.png](//image.easyeda.com/pullimage/Ektku7pgC2txMSrosUoPBwHdi8jI4fPCwWmhkUcP.png) Here I had some incomplete connections and it asks me to check if everything is alright. Let it do it, it knows a thing or two and is there to save you from disappointment later :) ![Screenshot_12.png](//image.easyeda.com/pullimage/TwGXNOrZ4fBMCdF8ZraBlgoahHCE0p5d06IsaMwB.png) This will also check if you have some Design Rule errors you may have missed. Let it check and if there are errors, fix them, if not, noice, you get the next screen. ![Screenshot_13.png](//image.easyeda.com/pullimage/bzfxU09a6gb19HnFeoEsqgUcsTE7pbJUnliCQMlZ.png) You can either order them by pressing the button or saving the gerber file onto your PC, so you can order the PCB's later or from other PCB manufacturers. You can then go to [https://jlcpcb.com/](https://jlcpcb.com/) and press Quote now and there you will find the ordering form. But please don't make the same mistake I and many others have done in our times. **DO NOT ORDER YOUR BOARDS AT 3AM OR ANY HOUR OF THE NIGHT, GO TO BED!!!!!!!** You may think they are good, but that's why I told you earlier to make the design sit there for a while. Go eat, sleep or do something else that won't spend your money. Learned that the hard way, now I have some 30 failed PCB's sitting there looking at me each time I open that drawer :D But I have left them to see where I have come from and see the improvements. Feel free to look at my projects. Open up your electronics and look at the PCB's, see what others have done and think why have they done it that way. I hope this wasn't too long and you learned from this! Cheers!
Reply
Jim Krug 2 months ago
@[deskpro256](https://easyeda.com/deskpro256) You are totally awesome! This is what I needed. And much more than I expected. I love you!!!! I will investigate this "ground pour" you mention. I wondered what that copper area tool was for. If I do that, then I can remove all the ground lines (that I worked so hard to add). At this point I may just leave this board the way it is. I can look into enlarging the lines. I made them the same size as the ones from HowToMechatronics since he knows more thane me. When, doubt, copy off somebody better :) If I do a ground pour, I should have more room for the thicker 5V lines. Thanks for catching the bad lines that are too close to the joystick holes. I will move them. You rock! jim
Reply
Jim Krug 2 months ago
@deskpro256 I got everything tweaked per your suggestions and I understand the GND pour now. Last question...with the 5V line increased to 0.508mm, I assume I need to increase the size of the VIA. What diameter and hole diameter should I use? Thanks, Jim
Reply
deskpro256 2 months ago
The way they are now is good enough. Should handle about 2.8A. I doubt you'll have even an amp, so you should be alright.
Reply
Login or Register to add a comment
goToTop
你现在访问的是EasyEDA海外版,使用建立访问速度更快的国内版 https://lceda.cn(需要重新注册)
如果需要转移工程请在个人中心 - 工程 - 工程高级设置 - 下载工程,下载后在https://lceda.cn/editor 打开保存即可。
有问题联系QQ 3001956291 不再提醒
svg-battery svg-battery-wifi svg-books svg-more svg-paste svg-pencil svg-plant svg-ruler svg-share svg-user svg-logo-cn svg-double-arrow
We use cookies to offer you a better experience. Detailed information on the use of cookies on this website is provided in our Privacy Policy. By using this site, you consent to the use of our cookies.