Thoughts or comments on this layout? - Page 1
Forum section: electronics / projects

author: mayor
author_rank: Regular Contributor
timestamp: December 21, 2023, 02:25:23 am
content: This is a four layer board, signal on top, ground, power, then ground. Unfortunately, the CAN (500 KHz) connector can't be changed so CAN H and CAN L must somehow cross.I'm wondering if there is a better way than this.

author: PCB.Wiz
author_rank: Super Contributor
timestamp: December 21, 2023, 03:22:41 am
content: At 500kHz it really does not matter.I'd be more focused on the other details like* teardrops on the connector pads ?* avoiding top-side connect to a mechanical hole, as stress can fracture plating**. (you can add a redundant via, so hole plating does not matter)** Addit: With plated holed, and manual soldering, and stress, sometimes the top-side plating can be left as the 'lone soldier' - no solder fillet and all the loads and so it gains a hairline fracture.that gives hard to find intermittent failure. Solution can be simple : donotrely on asingletop-side plating.On high current cases, we now add a ring of vias, to any top-side-trace mechanical holes.

author: aeg
author_rank: Regular Contributor
timestamp: December 21, 2023, 06:05:49 am
content: It's not really going to make a difference, but there's enough room between connector pins 3 and 4 to snake CANH around.

author: coppercone2
author_rank: Super Contributor
timestamp: December 21, 2023, 06:08:49 am
content: the 20ghz high speed can bus?

author: mayor
author_rank: Regular Contributor
timestamp: December 21, 2023, 10:33:48 am
content: Quote from: coppercone2 on December 21, 2023, 06:08:49 amHaha, no harm in checking right? Figured as much, but some manufacturer app notes are pretty paranoid even at these low speeds.

author: ArdWar
author_rank: Frequent Contributor
timestamp: December 21, 2023, 11:42:38 am
content: By the way, is that a 0402 resistor for bus termination?It's fine for most designs, but I usually prefer to use larger size there. Both for power handling (0402 is fine for the usual 2Vpp signal, but some overzealous device sometimes drive the full 5Vpp) and ease of [de/re]soldering when you shuffle around your device and it no longer at the end of the bus. Things can be a bit trickier still if you want to tolerate even more mode of faults.

author: mayor
author_rank: Regular Contributor
timestamp: December 21, 2023, 01:10:57 pm
content: Quote from: ArdWar on December 21, 2023, 11:42:38 amThanks for the tip, sized it up to06030805.

author: bson
author_rank: Unknown
timestamp: December 23, 2023, 08:07:45 pm
content: That's just fine. A short via is nothing compared to the 0.100" connector and will make zero difference. You could also mount the SMT components on the other side if you're OCD enough.I'd neck down the CANL/CANH traces at the pads though; they're a little too wide to fit.

author: SiliconWizard
author_rank: Super Contributor
timestamp: December 23, 2023, 08:25:26 pm
content: It's fine. It would also work just fine for USB HS given the limited length of the traces here. You may indeed start questioning that for anything higher than a few GHz, or non-differential signals above maybe 100 MHz, and if phase difference is critical, to get rough numbers.

author: oz2cpu
author_rank: Frequent Contributor
timestamp: December 23, 2023, 10:58:27 pm
content: keep CAN on top onlylike this

author: coppercone2
author_rank: Super Contributor
timestamp: December 23, 2023, 11:01:22 pm
content: the single side design makes sense its unlikely to effect the signal but you don't have a via that can break. reliability is increased. Especially a via near a connector. It could be a high stress shitty plate job screw up near a pug in connection.especially for a automotive component that might have forces on the cable from breaking and stuff.you could probobly rotate it too and keep the SMT package even further from the cable connector and its probably going to have 0 effectand wanna bet that connector is gonna get stuck eventually and someone is gonna knock off the resistor and destroy the PCB with a pliers or screw driver? good to keep the area near connectors clean because you know whats gonna be there, heavy tools.Optimally you want a big keep out around connectors, for durability reasons and ease of maintence by the clumsy. When a psycho car mechanic only has a 18 inch channel lock and a full sized crow bar near him (he is already past wits end because he had to remove the engine, dashboard and drill into the transmission to access the board).if you want cred with modern car manufacturers make sure you make the middle of the board flat flex, so you can stick it into a hole and then it opens up inside like a butterfly, so you need 4 trained ant eaters and a japanese basket maker to remove it.the manual should just feature a picture of a circus on the page of instructionsalso, this is the future of the tektronix DSO?

author: ArdWar
author_rank: Frequent Contributor
timestamp: December 24, 2023, 01:14:59 pm
content: Quote from: coppercone2 on December 23, 2023, 11:01:22 pmIf your design is intended for actual commercial automotive product you probably should pick connector where the working/mating area is nowhere near the PCB itself in the first place. Either through generous standoff, right angle for stress relief, preferably shrouded, and generous amount of anchor...