Please review my PCB - Page 1
Forum section: electronics / projects

author: djsb
author_rank: Super Contributor
timestamp: May 17, 2011, 08:14:09 pm
content: I'm a beginner at PCB design and would like to know how I can improve my current PCB (done in Kicad).In particular what is the best way to use a ground plane on this board? The PIC used will have a capacitive sensing module so the ground plane has to take this into account.Any help/advice appreciated. Thanks.David

author: johnmx
author_rank: Frequent Contributor
timestamp: May 17, 2011, 08:49:12 pm
content: Without the schematic it’s difficult to analyze. Also, the silkscreen it’s all mess up.You need to show us some pictures with the following layers (only one visible layer per picture -> without solder mask): bottom, top, bottom silkscreen and top silkscreen.

author: Unknown
author_rank: Unknown
timestamp: May 17, 2011, 08:55:03 pm
content: There are some basic rules that will improve any design.You can segragate sections of the circuit based on the signals they carry. I see you have the analog output from the trimmer running over digital traces.Check your clearances. I see some traces overlap pads.Ensure that there is a current return path nearby every sending path.Width of traces. Make sure they can carry the required RMS current at a resonable temp increase, say 20 deg C.Ensure decoupling capacitors are placed as close to the pin they are to decouple and in series with the trace.Regarding ground planes, a solid ground plane very close to the signal plane would be ideal. THT technology will create gaps in your ground plane, try to keep those as small as possible.

author: metalphreak
author_rank: Frequent Contributor
timestamp: May 18, 2011, 02:04:12 pm
content: Make sure your board house is willing to cut slots and that they get the appropriate file. Otherwise you're going to end up with a DC jack layout that it won't fit intoThe alternative design uses an enlarged hole instead.

author: shadewind
author_rank: Frequent Contributor
timestamp: May 18, 2011, 09:28:08 pm
content: If you by any chance are planning to use iTead (or Seeed Studio who uses the same PCB factory I believe), I know for a fact that they can route slots for power jacks and such.

author: johnmx
author_rank: Frequent Contributor
timestamp: May 18, 2011, 11:10:00 pm
content: Designing a PCB is a form of creating art. Personally I prefer to admire a good PCB than the work of Picasso.Don’t worry about making the perfect board at the first time. There is no such thing as perfect board and even the professional design guys make mistakes. The best board is a compromise of spending time versus better result.First question, do you have all components? Don’t make any PCB without having all components first. Probably you can’t buy/find some and then you will be in a real trouble.Do you plan to make the board at home by yourself or buy outside? Watch out for non-circular drills (DC SKT), some factories don’t accept that.You forgot to disable the solder mask layer! Some traces seem to short-circuit with some pads, but I think it’s the solder mask.The traces are too close to pads and to other traces.Define the route spacing strategy in your layout program and run the DRC (design-rule-check). My advice for this board is to set the minimum spacing to 12mils.Avoid angles in traces with less than or equal to 90º.Don’t place headers, like Molex KK, too close of each other or it will be difficult to remove the sockets later by hand.In general, the routing, i.e. the choose of track paths, looks very good for someone’s first board (for a single side board)!Regarding the ground plane, take a look at AN1102 from Microchip:http://ww1.microchip.com/downloads/en/AppNotes/01102a.pdfAvoid using ground plane where it isn’t really needed.Finally, check the David’s PCB Design Tutorial. It’s a good start for young players.http://www.alternatezone.com/electronics/files/PCBDesignTutorialRevA.pdf

author: pablo
author_rank: Contributor
timestamp: May 24, 2011, 10:55:35 pm
content: I would fill the whole PCB with a layer connected to ground.Not only you save Ferric Choride (or any other etchant) but also your analog performance improves as well.In any commercial product, you always see that, they do not remove unused copper. They tie it to groundas a ground plane.good luck.

author: johnmx
author_rank: Frequent Contributor
timestamp: May 24, 2011, 11:06:45 pm
content: Quote from: pablo on May 24, 2011, 10:55:35 pmThis is not a simple circuit. He wants to use the PIC’s capacitive sensing module. A ground plane will reduce the sensitivity to measure a finger press. The only advantage is to improve immunity to EMI, but I don’t recommend it in this particular circuit.

author: pablo
author_rank: Contributor
timestamp: May 25, 2011, 04:40:19 am
content: QuoteGot it. I didn't read the thread so i just threw a suggestion by the looks of the PCB. But you are right !!!

author: tnt
author_rank: Regular Contributor
timestamp: May 25, 2011, 11:52:10 am
content: Making sure the board passes the automated DRC would be a good start.

author: scrat
author_rank: Frequent Contributor
timestamp: May 26, 2011, 12:46:34 am
content: Quote from: Alex on May 17, 2011, 08:55:03 pmIs there a rule of thumb to obtain such an estimation (for example on a standard thickness 2-layer board)?One should just need electrical resistivity and thermal track to ambient resistivity.

author: Afrotechmods
author_rank: Unknown
timestamp: May 28, 2011, 07:48:47 am
content: An easy rule of thumb for a standard 1oz copper board is a minimum of 10 mils wide per Amp. You can lay the board out with that to start with, then go back and increase the width of everything as much as you can get away with (switching nodes and the like excepted of course).

author: scrat
author_rank: Frequent Contributor
timestamp: May 30, 2011, 10:13:07 pm
content: Quote from: Afrotechmods on May 28, 2011, 07:48:47 amGood to know, thanks.

author: djsb
author_rank: Super Contributor
timestamp: February 12, 2012, 10:04:47 am
content: Here is a quick photo of the final board in situ (on my blog).http://djsbriscoe.co.uk/blog/It's been in use for around 6 months now and has worked flawlessly. Had a few teething problems with the master clear pin A5 and the ICSP pins B6 and B7 but that has been worked around.David.P.S The Jpegs of my schematic and layout have been lost from this post. Maybe they got lost in all the site relocation that occured earlier on?