3
\$\begingroup\$

I was designing this PCB below as a watchdog for cutting power in case of missing pulse from Raspberry Pi and manually cutting power via switch. Pulse frequency 30Hz.

In the left side 6 pin connector is connected to a switch to cut power manually, and 4 pin connector connected to Raspberry Pi for watchdog input. Both top and bottom plane has GND pour.

I was wondering how can I improve this PCB, in terms of good design practices. Any idea and critic will be appreciated. This is first time for me in PCB design. Thanks everyone in advance.

PCB Top Plane PCB bottom plane

Bottom Plane

Top Plane

\$\endgroup\$
2
  • \$\begingroup\$ This long comment chain has exceeded what is reasonable for comments. Therefore it has been moved to chat and should be continued there (link below). --- As this bulk moving of comments to chat can only be done once, any further comments posted here which try to clarify the question, might be deleted without notice. Keep it in chat, please! When someone has got enough information from the chat to post an answer, then please do that. Any factual updates to the question which are decided during the chat, should be made via an edit to the question. Thanks! \$\endgroup\$
    – SamGibson
    Jun 11, 2021 at 13:45
  • \$\begingroup\$ Since comments are not for extended discussion; this conversation has been moved to chat. \$\endgroup\$
    – SamGibson
    Jun 11, 2021 at 13:46

3 Answers 3

2
\$\begingroup\$

Suggestions on the silk:

  • Some of the text is close to (or overlapping) holes in the solder mask and most board houses will clip those; text on the upper-right mounting hole is an obvious example, the body outline of the NE555 inside the pads is another. The pin descriptions on the right-most connectors are possibly too close to the board edge and may be clipped.
  • Some lines are too thin (TP3430, pin descriptions on the connectors on the right) that may not print well; double-check the guidelines from your board house.
  • Some components have designators (C6, R5, etc.) while others have the part type (2N3906, 48V-VHR-4N), others are something else (NOT_G, AND_G) and others have nothing at all (connectors on the left edge).
  • The pin labels on the relays will not be visible when those parts are installed.
  • Since the parts are not consistently oriented, having visible hints to orientation is especially important if hand soldering. The TPS3430 for example, is installed "upside down" according to the pin 1 indicator but the part type text is not upside-down. I would suggest the pin 1 indicator be much larger and the "TPS3430" text be flipped to consistently show which way is correct. Even better would be make things consistent by rotating either that part or the NE555. If you're only building 1 or two of these, it is less of a problem.

Suggestions on the copper:

  • Add keep outs (or increase the keep out area) to keep the ground pours away from unconnected pins. This will help avoid shorts if there are any defects in the solder mask as well as making it easier to inspect visually.
  • The whole-board double-layer ground pour is unnecessary and may be counterproductive for a 30Hz digital board. The two ICs are the only part of the board where noise may matter, but the large pour creates an larger antenna to pick up noise, while increasing the possible manufacturing failure rate by having the copper so close to pins you want unconnected from ground.
  • Keep the copper pour back from the edge of the board a bit more to avoid exposing the copper edge when the board is cut.
  • Any reason the ground is connected to one (and only one) mounting hole? Should it be all (or none) of them?
  • Convention usually has pin 1 of the connectors indicated in some visible way; rectangular pads, silkscreen dots or blocks, etc. The connectors on the right seem to show a latch but the JST connectors on the left are ambiguous.
  • The SGN trace is too close to the lower-left mounting hole in my opinion. It is in danger of being shorted to ground if the solder mask is damaged by an overly-large screw head on that mounting hole.
  • I would increase the pad size of the relays to improve the connections' mechanical strength on these large, heavy parts.

Suggestions on physical placement:

  • If possible, I would move the corner mounting holes in to provide more PCB material on the outside of the holes for mechanical strength.
  • Hand assembly will be easier if the components' connection to ground is made with thinner traces. Look for "thermal spoke" settings in your layout software.
  • The board would look cleaner and more professional if some sort of placement grid and consistency were maintained. For example, the placement of C7, C8 and the logic gate ICs seems almost random, along with the IC rotations I mentioned above. The connectors on the left of the board could be centered vertically between the mounting holes.
  • The C7 capacitor is too close to the 24V relay. Moving it would make inspection and rework easier.
  • Without knowing the physical height of your relays and connectors: think of which way the wires will leave the board, especially if the wires leave the side of the connector rather than the top.
  • With the relays installed, will you be able to physically grasp and unlatch the latching connectors?
\$\endgroup\$
1
  • \$\begingroup\$ Thank you so much for your comments and recommendation, you're totally right I'll should try to be more consistent, and should spend more time on thinking before getting started to designing. :), Anyway thank you again for helpful advices. \$\endgroup\$
    – Veysi ADIN
    Jun 11, 2021 at 15:21
1
\$\begingroup\$

There are some acute angle pad entries that might create acid traps during PCB etching.

Take a look at the red circles.

You might also read this Cadence application note:

https://resources.pcb.cadence.com/blog/are-acid-traps-still-a-problem-for-pcbs-in-2019-2

enter image description here

\$\endgroup\$
0
\$\begingroup\$

So after several feedbacks from good people, I made several changes in terms of consistency, naming, placing. Thank you everyone who took their time to help me out. I removed ground plane from top layer, decreased number of connections in bottom plane to one and decrease size of mounting holes to 2.5mm. You can see final layout below.

Final Layout Top + bottom layer Top layer Bottom Layer

\$\endgroup\$
2
  • \$\begingroup\$ Did you get these boards manufactured? If so, are there any lessons learned from them that you could share with those who might find this question later? \$\endgroup\$
    – spuck
    Jun 30, 2021 at 22:06
  • \$\begingroup\$ @spuck Hello, thanks for your comment, sorry I couldn't reply earlier, yes I did manufactured them, and hand soldered parts, only think went wrong in one board was soldering TPS3430 IC, it was suggested to use different IC but I couldn't find equivalent one. So one lesson to take from all this experience will be that for hand soldering try to avoid using QFN packages. That's all I can say for now. \$\endgroup\$
    – Veysi ADIN
    Jul 7, 2021 at 7:40

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.