Peer Review Of PCB design

I have designed a PCB with KiCAD and am ready to produce it, but would like some feedback before I have it made. I’ve tried my best to follow some best practices, but it’s my first one!

Is this a good place, or is there a place for peer review PCB layout/design? If so, what files are needed for review? Schematic and screenshots of PCB?


That would be an off topic discussion. Are you using a GHI product in the design?

Of course…I’m plugging a GHI board into this PCB.

Post the design files and those that want to chime in will.

To check your gerber output files there are a number of free tools.

Gerbv works for me.

But the best way i know of is to use the PCB checker on Eurocircuits. This will check all the spacings, thru hole platings etc etc. I can almost garantee it will find something you didnt notice. Fix all the errors in your design and check again. Its free and you can buy from someone else if you prefer, but the tool is excellent.

Post the images of the PCB of decent size (2 x should be enough) and a PDF of the schematic somewhere and link them here and we will have a look. A few have done this before and we’ve spotted issues that helped them.

I’m using a CERB40II for this board, but it’s rendered at a DIP40 chip. I’ve attached some screenshots of the PCB and included a PDF of the schematic. I’m using some optoisolators for pulsed inputs;The Tach IN is a 12v square wave signal, the speed signal is an open collector signal/sensor. The GLCD display and eeprom are SPI on SPI1. The temp sensor is a voltage divider on analog input, and the rotary encoder and push button are hardware debounced user inputs.

I’m using a 12v input to get 3.3 volts via an MCP16301 using the diagram on page 27. I’ve tried to layout the setup like they describe, but also would like confirmation that I’m using this part correctly as well.

Schematic: - page 27

@ Gismofx - Are you going to post the artwork for the copper layers as well?

Strange PCB software as I don’t see any pads for the 40 pin device on the underside of the board.

Anyway, a few things to think about.

Power rails are too thin. You really want to try and use heavier tracks for carrying power. On 2 layer designs and depending on the needs of the devices, I run 40 or 60 mil power rails for both GROUND and VCC (3.3, 5.0 etc)

Add a decoupling cap (0.1uF) next to U1

I can’t see any tracks from from one side of L1. Keep these are short as possible and heavier (same as the power rails) between the inductor and the MCP16301.

I assume this is for a motorbike so there is no radio to worry about causing interference to. If so you need to add a filter on the input as the power rails could potentially generate a lot of EMC. Murata do some very nice automotive spec inlet filters for this purpose. Using a spectrum analyser and some EMC test kit I saw a huge drop in the transmitted signals on the power rails. All my designs now include these :slight_smile:

What is the reason for the 10K pull up and 10K pull down on the ENC inputs? With no signal on these, the voltage on the input will be around 1.65V. Is there a reason for this? You really only need one of the other depending on how the encoder works.

@ Mr. John Smith -

Dropbox - MOTOGAUGE PCB SVG - Simplify your life SVG files of the layers

@ Dave McLaughlin -

I’m using a surface mount DIP40 socket so I can flush mount the GLCD to the opposite side of the board.

Not sure this matters, but I’m using the bottom of the board as a power plane/filled zone at 3.3v and top layer filled zone as ground plane.

I can do that, but are you saying that even though the regulator should supply “clean” power, the power traces can induce noise?

Here’s a zoomed version of the copper for the MCP16301 circuit:

C2 and C3 are the inlet filters, but are you saying I need an additional filter here on the 12v signal?

It’s a simple rotary encoder for the user to be able to navigate menus and settings. It’s also how I’ve had it connected on the breadboard. Image attached. If there’s a refinement or better way to debounce it, I’m open to it.

OK. That would explain it. :slight_smile:

Beef up any power tracks anyway. As your 40 way is top connection only, you need a connection to the lower plane so keep this track heavier. Trust me, doing this before you make the board will pay off with a working system and no issues.

Yip. Your biggest issue with anything switching is power dips. These might only be a few ns or even ms but they can disturb your system. Best practice is to fit one 0.1uF cap at every device. The datasheet will always tell you this anyway.

Only comment here is to beef up the track to the inductor on pin 6. Make it as large as you can. Have a look at the datasheet for the device. There is a section on the layout for the device. It should be at least 80 to 90% of the pad size at best. Your 12V rail looks fine. Use the same size as this.

If you want to keep it quiet for radiated emissions include an inductor filter on the input.

Try this. THey are not cheap but if you need to have EMI/EMC free design these work wonders.

Recheck your design. It is not the same. You R10 goes to ground and your R11 goes to 5V. R10 should be in series with the input signal and R11 should pull up the signal on the incoming side. Make sure the cap is on the output side that goes to the CPU.

@ Dave McLaughlin -

Thank you.

I’ve widened up all of the POWER traces to 25mil and revised the regulator section of the circuit:

Bypass Cap:
So, I’ll add a .1uF bypass cap to the EEPROM Vcc pin. Could it just be an 0603 SMD ceramic cap?

Debouncer circuit:
Thanks, It was modeled wrong on the schematic. I looked at my breadboard circuit and corrected the schematic, but now I’m doubting myself.
Here’s the old/incorrect schematic:

Here’s the revised schematic:

Still wrong on the encoder. The 2 caps go on the PINA and PINB side.

For decoupling 0603 is fine. If need small even 0402 works.

For your regulator, can you increase the GND trace on pin 2. Remember this has to provide up to 600mA although you are unlikely to be using this much, you still need a good gnd path for this IC. I would also make sure that the large ground plane on the lower left of your board has a good connection to the rest of the ground plane via a suitably heavy track on the other side of the board. Can’t see this in your capture.

@ Dave McLaughlin -

Attached screenshots of the debounce circuit and the regulator. I made a larger ground zone and trace around the regulator.

Encoder looks spot on this time. :slight_smile:

Power also looks better. Nice work.

I’ve finally ordered the board via OSHPark! I had to make a few tweaks to some pins and footprints that I use and move the regulator to the opposite corner of the board. I will post some pictures once I receive the board! (hopefully I connected everything else correctly)Thanks!

Looks good. Your text for D3 will be missing when you get the baord back as it covers the pins of another device.

Look forward to seeing the finished boards.

Thanks. Regarding that D3, it’s actually a 5 pin device. That middle pin is actually gone where the text is, but D4 in the power supply area overlaps a little and might be weird.

I’m excited!

PCBs arrived! Components were supposed to arrive same day, but didn’t :confused: Hopefully tomorrow…