1
\$\begingroup\$

I'm currently making a weather station as a personal project. It will consist of one BLE peripheral and one BLE central. I will fabricate both as one PCB, and panelize them with a vcut. As mentioned earlier, this is a personal project, so I would love to get some feedback on the layout so I can improve the design, and myself as a designer.

Some things worth mentioning:

  • 2-layer design
  • Uses Renesas DA14531mod BLE-modules
  • Battery powered (3V0)
  • Will display data on e-paper display through SPI.

Here is the schematic: enter image description here

Here is the top layer: enter image description here

And here is the bottom layer: enter image description here

As I'm using the same ground for both PCBs in the schematic, there is a netline visible in the layout (over the vcut).

\$\endgroup\$
14
  • 4
    \$\begingroup\$ Possibly a personal preference and doesn't have any actual impact on performance, but I very much prefer schematics to have lines connecting parts together. Off-page connections should only be used for well, off-page connections ie. connecting signals to another schematics page. Also, when using off-page connectors you should use a symbol for that (typically an arrow or such), not just a net label. \$\endgroup\$
    – Klas-Kenny
    Commented Jan 5, 2023 at 10:30
  • \$\begingroup\$ @Klas-Kenny This is a good point and something I will take into consideration. The readability of the schematic would be improved. Correct me if I'm wrong, but aren't net labels used for connections within the same sheet, and net ports used for connections between sheets? At least according to this article: altium.com/documentation/altium-designer/… (See the section about flat design) \$\endgroup\$
    – user294957
    Commented Jan 5, 2023 at 11:06
  • 2
    \$\begingroup\$ Lines win every time for me. Boxed-up miniature circuit sections don't work for me. They may work for some folk but, for EE pros, they are just another thing to mess up circuit flow. \$\endgroup\$
    – Andy aka
    Commented Jan 5, 2023 at 11:20
  • 1
    \$\begingroup\$ As for general feedback: don't design RF products on 2 layer boards. Pre-made modules like this might not be as picky, but it's still not a good idea. Ideally don't route any traces underneath RF parts but keep ground pour there. Then connect the ground planes with vias at as many places as possible around the RF parts. \$\endgroup\$
    – Lundin
    Commented Jan 5, 2023 at 13:03
  • 1
    \$\begingroup\$ @Lundin unfortunately I don't agree with the people forming the general consensus you mention because I believe that a schematic, where possible, should all be on one sheet. I think hierarchically distributed schematics are really hard to read; especially so if you have only a PDF output with many sheets. \$\endgroup\$
    – Andy aka
    Commented Jan 5, 2023 at 13:11

2 Answers 2

Reset to default
1
\$\begingroup\$

Feedback on PCB-layout wanted

  1. Reserve the GND flood for the blue side
  2. Minimize the length of any tracks that are not GND on the blue side
  3. Where possible use the red-side flood for power supplies like 3.3 volts
  4. Follow recommendations in data sheets for PCB layout

These are all obvious tracks to move (almost in their entirety) to the red-side: -

enter image description here

  1. Try and place components all on one side of the PCB

Reason: minimize disruption of the GND plane to vastly improve EMI withstand and EMI generation. If that means extra vias that's OK in most cases.

\$\endgroup\$
1
\$\begingroup\$

Just some observations:

  • Your schematic is basically an accumulation of components and net labels. One can make a case for personal preference for sure, but just having a lot of labels makes it very hard to understand signal flow and the basic logic of the circuit. Arrange your components in a reasonable way and connect them with wires instead of labels.

  • You should try to have an as solid as practicable GND plane on the bottom layer. Only route signals on the bottom layer if you absolutely have to. And when you have to, keep them as short as possible.

  • I'm not really a fan of "multiple boards in one" trickery. Your split GND net is an obvious example: Your CAD tool will flag this as an error. Once you start ignoring/disabling design rule checks you are asking for trouble eventually. Also you accidentally created an inside "radius" that needs to be milled. Since that inside radius is zero, the outcome is undefined as it will depend on the milling tool size of your fabricator. Or your order might get "on hold" for clarification. Then you had to come up with weird net names like "SDL_2" or "BME_VDD" to keep the nets of the boards separated. Depending on your fabricator my guess is that a two-in-one board won't provide much cost advantage anyway. Since it appears to be a low volume project, you'll probably order the boards from a pooling service. So the boards will probably end up on the same panel anyway and you can let the fabricator worry about panelizeation.

  • V-Scoring makes sense for high volume production where a whole panel is filled with multiple instances of a single design. Since you'll probably use a pooling service, v-scoring might not make much sense.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.