PCB Vias - More or less layer changes? - Page 1
Forum section: electronics / beginners

author: tav
author_rank: Newbie
timestamp: February 24, 2021, 09:06:14 pm
content: Hi,I hope you're all doing well.I'm slowly getting into PCB design concepts and practising in the off-hours as a knitting or puzzle substituteLoosely speaking, for non-high speed circuits - analogue audio only, no AD/DA - when routing traces, is it 'better' to use multiple single vias to change between layers multiple times on a 2-layer PCB, compared to using fewer vias and staying on a single side of a board as long as possible?I have a physical copy of the IPC-2221A booklet but it's not on my person currently. Not too sure if it would give me a clear answer, though!My thinking is to use multiple vias and go between layers more times as to reduce breaking up my ground plane; but this is all very new to me!Any pointers would be greatly appreciated.Thanks in advance.Tav

author: Benta
author_rank: Super Contributor
timestamp: February 24, 2021, 09:46:16 pm
content: It's a bit difficult understanding what you mean. First, you write about 2-layer layout, which is fine, but then you suddenly mention "ground plane", which doesn't fit at all.Here's my personal take:Many vias: messy layout.Few vias: nice layout.One of my methods when doing 2-layer PCBs is the E-W, N-S approach. This usually results in nice routing. The idea is having routing on one layer in horizontal direction, vertical routing on the other layer.Lots of exceptions of course, but if it succeeds to 70% it's fine.Cheers.

author: Refrigerator
author_rank: Super Contributor
timestamp: February 24, 2021, 09:52:58 pm
content: Making the effort to route as many traces with as few layer changes is how i do my boards. Also vias can increase the failure rate (although it's negligible for a hobbyist) due to a failed via.But as long as your board layout is neat and efficient it's all fine. Don't forget to take full advantage of the two layered board.In university i've seen people route 2 layer boards as if they were two 1 layer boards stuck together, for example a clock signal going all over the board when it could just make a couple layer changes to make the trace 5x shorter.

author: Refrigerator
author_rank: Super Contributor
timestamp: February 24, 2021, 09:55:26 pm
content: Quote from: Benta on February 24, 2021, 09:46:16 pmI assume he wants to use one layer as mostly ground with as few traces going into that layer to cut the ground up.

author: nigelwright7557
author_rank: Frequent Contributor
timestamp: February 24, 2021, 10:02:57 pm
content: There was a time when pcb vendors asked how many vias and charged accordingly.These days its not so much of a problem.I tend to go for as few vias as possible.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: February 24, 2021, 10:24:07 pm
content: For what purpose?For non-high-speed circuits, it matters very little. You probably still want the ground plane, to provide shielding against external fields. In a 2-layer design, ground can be poured over both sides, and stitched together with vias, effectively averaging out to 1 good ground layer. More signal vias implies more crossings between layers -- implies more cuts through those pours -- causing a knock-on increase in ground vias stitching around those cuts. That's generally a bad thing. But how bad, again, it depends. There's a huge spectrum of "non-high-speed" designs, some of which may be affected, who knows. (I could give an assessment, based on a layout and specification including regulatory requirements; but explaining the process used to make that assessment, could fill a book; you'll forgive me for not explaining in greatest detail here.)Tim

author: penfold
author_rank: Frequent Contributor
timestamp: February 24, 2021, 11:13:16 pm
content: Aim to keep the number of layer changes in any signal as low as possible even if its just to keep it easier to follow when debugging but also using a ground plane on top and bottom layer with "via stitching" between them to bridge any major slices

author: Siwastaja
author_rank: Super Contributor
timestamp: February 25, 2021, 10:00:04 am
content: Dozens of layer hops just to save a few mm of trace length -> nope.Massively long serpentine trace all over the place just to save a few vias -> nope.Traces are OK, so are vias, we wouldn't use them if they were "bad". Balanced design does not go into extremes trying to avoid something that doesn't need to be avoided (and replace it with something else).

author: Terry Bites
author_rank: Super Contributor
timestamp: February 26, 2021, 05:36:45 pm
content: And charged by the hole and number of hole sizes and tinning, leveling, blah blah ...... why did we ever put up with it!

author: tav
author_rank: Newbie
timestamp: March 02, 2021, 09:21:51 am
content: Thank you all for your input, it's greatly appreciated!Lots to follow up on from each of you, I'm glad we're not paying by the via anymore!

author: Rerouter
author_rank: Super Contributor
timestamp: March 02, 2021, 09:41:43 am
content: route as many important / critical signals on the same layer with a nice unbroken ground plane, for anything else use vias when neccesary, but pay attention to how your return currents are flowing and add ground vias where needed to keep the detours short,Placing down vias for sheilding is always valid for designs if you have any concerns about noise, I reguarly test analog circuits in a swept frequency demagnetiser (practically an induction heater), and its impressive how much ground fill on both sides, some fencing around critical signals, and some planning of return currents to keep them near the signal cut that down to near nothing, despite tens of amps from the shorted turn flowing through the board. and the induced magnetism trying to shoot the thing across the roomAlso I have yet to meet a manufacturer who complained about the number of via's, but my usual approach is you don't need to grid the entire PCB, just keep the return paths close to signals, and fence what you feel needs fencing.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: March 02, 2021, 01:26:57 pm
content: Quote from: Rerouter on March 02, 2021, 09:41:43 amI like to place them like this,Mainly around traces, stitching across the gap thus created; placed at peninsulas where the ground impedance will be relatively high thus doing the most work; and three or four where traces/buses cross. Note in the second case, with so much bus width, and a need to cross traces under a row of pins, the vias are staggered to allow bottom ground (blue) to pour between them; a row of vias, inside that pin row, stitches ground back together. Or between C29 and C40, the VCC trace making a jump to allow ground to pour under the bus -- it's not great, but it's better than a full width slot.Tim

author: nigelwright7557
author_rank: Frequent Contributor
timestamp: September 02, 2021, 11:08:21 pm
content: I recently built up a USB scope pcb.It didnt work, I couldnt program the PIC.Tried replacing every basic part and it still wouldnt work.Did visual check for shorts and it was fine.All volts seem fine around the PIC.Had to give up in the end and started building a second pcb using same components and this time it worked.So I am guessing fault is down to pcb, either a broken track or a bad via.The pcb's are tested at the fab so should have been ok.So got a bit paranoid about via's now and try to minimise them in new designs.