I've checked a PCB board which has designed by very famous company and I saw something weird.They connected two pin to each other 2 times and from the top and the bottom of the board I am going to design the board by myself and I really don't understand what is the main reason which they use these method for connecting this two pins to the each other. Beside of that I have to mention this board is Low flow current and 12 voltage input, in addition this board's utilized 20 mill thickness for these traces which I have mentioned about that.enter image description here (I have uploaded the picture of the PCB here and I have put green circle around the pins, I hope it be clear ).

Thank you very much for your time

  • \$\begingroup\$ Comments are not for extended discussion; this conversation has been moved to chat. \$\endgroup\$ Nov 20 '18 at 1:12

That is a terrible board design. The person who made it clearly does not do it for a living and they opted to just use the autorouter. This is a huge mistake as 90% of the time, if you don't take hours upon hours to set it up properly, it does nothing but make a mess. In some designs routing like this could even lead to electrical problems.

Any real, experienced PCB designer would not route it that way.

EDIT: Further examination has brought even more issues into light, as Marcus has pointed out. There are components whose leads are shorted by traces, parts with their leads shorted to the same ground plane, etc. If the board shown above was actually manufactured, it would not work. It is not a legitimate design.

  • \$\begingroup\$ Comments are not for extended discussion; this conversation has been moved to chat. \$\endgroup\$
    – Dave Tweed
    Nov 20 '18 at 4:39

This is definitely not the case here, I agree with the other answers, this is a pretty bad PCB layout. However, in some cases it makes sense.

  • When you are laying out logic and other ICs with fast transitions, or when some devices can consume enough power that trace widths become an issue, AND you are doing it in a two layer or single layer board or otherwise have no possibility of flowing proper planes for grounds and power in a particular section, THEN you would place a connecting grid of traces in which pins have multiple paths to each other.

That way you get as close as you can to having a plane and provide proper connectivity to avoid ground bounce, supply issues, and EMC problems. However, this is mostly limited to power and ground connections. I have seen what happens when inexperienced designers ignore this and see PCB traces as just ideal wires.

  • In some cases, due to required component placement, there might be no way to place a wide enough trace to handle a large current. THEN you would provide multiple paths so as to accommodate the proper trace width.
  • In some weird cases in which you can foresee a current through a trace magnetically inducing a potential on a trace on the other side of the board which can lead to problems. By laying loops with currents fields flowing in opposite directions with respect to the other trace you can reduce the induced field.

I know of an inexperienced designer who laid out a simple 2-layer board with an operational amplifier and made the mistake of placing the feedback components a few centimeters away from the inputs, leaving high-impedance signals at the mercy of induced fields from the other side of the PCB. His amplifier was a nice oscillator, I fixed it placing a thin wire across a different route.

  • \$\begingroup\$ Thank you very much for sharing your information my friend, I am trying to copy the PCB same as them as much as I can. So, you don't recommend me to I copy these two traces which has been connected to same pin ?. Also I measured current of main board and I saw the was around .3A which was not too much for 20 mill trace \$\endgroup\$
    – a2640
    Nov 20 '18 at 1:07
  • \$\begingroup\$ As I stated my answer. NONE of these considerations are the case here. This is just a sloppy PCB. For starters, there is a ground plane in there. So no, I don't see a point in copying it. \$\endgroup\$ Nov 20 '18 at 1:12
  • \$\begingroup\$ @a2640 really, this PCB is dysfunctional. It doesn't do what the schematic designer had in mind. It has no worth whatsoever. It's bad in every way a PCB layout can be bad. Don't copy it. PLEASE. \$\endgroup\$ Nov 20 '18 at 14:06
  • \$\begingroup\$ As I said in multiple comments, there's components in there that were simply shorted out by traces that certainly shouldn't be there. I'm completely surprised you even think about copying this. It's not worth the pixels on your screen it occupies. This PCB isn't only slightly suboptimal. This PCB is broken. I don't know how you can still believe this should be the "working reference" you should be copying. It's definitely not. \$\endgroup\$ Nov 20 '18 at 14:07
  • \$\begingroup\$ @MarcusMüller shorted components need not be a design mistake. It could be a trace intended to be cut for testing purposes and/or a component that is not intended to be populated. I’ve seen plenty of old designs where jumper options were just appropriately shaped exposed segments of copper. Surface mount 0ohm resistors were not a consideration. \$\endgroup\$ Nov 20 '18 at 14:17

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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