Why do some PCBs have via stitching only near edge and not througout? - Page 1
Forum section: electronics / beginners

author: matrixofdynamism
author_rank: Regular Contributor
timestamp: July 04, 2023, 12:08:33 am
content: I sometimes see PCBs that have a visible copper near edge with a whole lot of vias around the perimeter of the PCB on this copper. These vias are not very small in size and easily visible.From what I know, we could add stitching vias throughout the PCB to stitch the different ground layers together and provide low impedance path for the currents through the reference plane. But, what does it mean when the stitching vias only exist near the edge of the PCB and that also on what looks like exposed copper?I wish I could attach picture to this question but I don't have it at hand.

author: ataradov
author_rank: Super Contributor
timestamp: July 04, 2023, 12:45:43 am
content: The dense stitching on the edge helps with EMI, it prevents edges of the PCB from radiating. There is likely stitching in the main area a well, it is just not as dense, since it does not make sense and at some point vias are not free anymore.The exposed copper often means that this part would be contacting the case acting as a shield. This is often done though conductive gaskets. Or it can have shield attached some other way and having exposed copper just narrows the gap.

author: mengfei
author_rank: Regular Contributor
timestamp: July 04, 2023, 01:20:46 am
content: sometimes referred to as a Faraday Cagehttps://resources.altium.com/p/building-a-faraday-cage-to-contain-emi-part-1

author: ppTRN
author_rank: Regular Contributor
timestamp: July 04, 2023, 09:29:11 am
content: Quote from: ataradov on July 04, 2023, 12:45:43 amWhat do you mean? Does PCB manufacturer charges some $ per via after a certain amount? Did not know that, is adding vias such a critical job that they want extra money? Of course I am not talking about buried or blind vias, but even for them, once the first is done...

author: Siwastaja
author_rank: Super Contributor
timestamp: July 04, 2023, 09:34:43 am
content: Quote from: ppTRN on July 04, 2023, 09:29:11 amThey do have an actual cost (machine time, drill bit wear), albeit small, so for actual large-scale manufacturing where every penny is pinched and prices negotiated, a design with gazillion of vias will be some cents more expensive. Most prototyping/small scale services do not charge for holes separately; but try to do a 100x100mm board with 10000 vias on it on 1mm grid and place a 10000pcs order on JLCPCB or PCBWay and see what happens.But, 1000 stitching vias on a semi-complex digital board would be still quite normal.

author: ArdWar
author_rank: Frequent Contributor
timestamp: July 04, 2023, 09:38:35 am
content: Quote from: ppTRN on July 04, 2023, 09:29:11 amYes, most fabs charge an extra once you exceed a certain via density per area (or more generally drill/area). Drill bits wears out obviously, especially at the small size of via holes. Drilling is also often done sequentially, so there's cost for fabrication time too.

author: Berni
author_rank: Super Contributor
timestamp: July 04, 2023, 09:48:26 am
content: The edges is where via stitching is most effective, that's why.If you have two large ground fills that are stitched together, then the vias in the middle of it are not actually going to be carrying much current since the currents likely found a closer via before it, distributed itself over the two planes, then flow along the planes.However when you are at a edge, there is a likelihood that that via is the closest one as the ground fill ends there. Any current trying to flow towards the edge of the fill and wants to go between planes will get stopped there if there was no via for it to go trough. Note that i said edge of fill and not edge of board. This edge stitching is often used to join together ground planes that have been cut apart by a trace running trough them. That way a signal trying to cross the cut can jump down to the other plane, continue on it, then jump back up, hence current flows at the edges.For PCB edges it is a bit less critical (since current cant flow over the edge), but you are still going to have traces running close to the edge of the PCB, so you can have ground return currents close to the edge.PCB manufacturers generally let you use large numbers of visas, but if you use an absurdly large number of vias they will sometimes indeed refuse, or charge extra. It also might make a difference when ordering production quantities of >250pcs of the boards.

author: matrixofdynamism
author_rank: Regular Contributor
timestamp: July 04, 2023, 10:43:34 am
content: Alright, so this is related to EMI and not SI or PI. I see.Now a question that arises is that, a PCB is a structure in 3D, it exists in a 3D world. If it existed in a 2D world than the copper on the sides would act as a Faraday cage. However, in 3D world, we get emissions from any direction.If we do not attach a metal container around the PCB and connect it to this exposed copper on the edge that also contains rows of stitching vias, how effective is this exposed copper with stitching vias?Is there a proper name for this "exposed copper near edge with stitching vias"?

author: Berni
author_rank: Super Contributor
timestamp: July 04, 2023, 02:32:30 pm
content: The gap between the layers is only 1.6mm for the regular thick boards (yet they are often thinner than that). So for anything under 10GHz that gap looks like it is not even there. This is the same principle of how you can have a door on a microwave oven that you can see trough, but the microwaves can't get out. It is because the glass door has a mesh with holes that are much smaller than the RF wavelength.The magnetic field coming from your long traces can reach out into space and emit a lot more EMI. Even more so for the wires coming out of your board, they make great antennas. So getting rid of EMI is not just simply about putting your board in a metal box.

author: Kleinstein
author_rank: Super Contributor
timestamp: July 04, 2023, 06:14:09 pm
content: Even if the PCB is only 1 mm think the size of the PCB is usually larger. Without the via stiching around this can act like a slot antenna. For a similar reason a ground plane should be really closed even just a single trace causing a cut in the plane can have quite some effect on the EMI. Single THT pins are often still OK as they are relatively small.

author: matrixofdynamism
author_rank: Regular Contributor
timestamp: July 09, 2023, 06:09:40 pm
content: I really need to find out why something would behave like an antenna in the first place.I know about something called dipole antenna, we have a wire that is not terminated i.e floating and it acts like an antenna. However, what I do not understand is, why a signal trace that is grounded would act like an antenna. I mean the energy goes from transmitter to receiver and is coupled to a ground plane. So why should it radiate into the atmosphere?

author: Siwastaja
author_rank: Super Contributor
timestamp: July 09, 2023, 06:19:52 pm
content: There is no such magical thing as "ground". GND is a conventional net name for a net which is used as "the another conductor", i.e., for return currents, of pretty much everything single-ended on board. As there are currents flowing in the plane, it means voltages due to impedance (resistive and inductive) of the planes. Multiple planes can be at different voltages.Besides, the issue is not just the planes itself acting as antennas. There are switching traces, and the wide gap between the layers allows the energy to go out. Microwave ovens have a protectivegrid, not just parallel lines, for a good reason. The board edge, which is a 2D shape, needs shielding in both 2 dimensions. The ground planes are fine but you need to add the grid of vias for the other dimension, to block the long gap. Because FR4 itself is lossy enough at frequencies like 10GHz or so (and signal edges in usual "mere mortal" designs are limited well below 5-10GHz, too), a via every 10mm or so suffices.

author: Berni
author_rank: Super Contributor
timestamp: July 10, 2023, 05:30:37 am
content: Yeah you still want some vias there to bind the top and bottom plane together in potential. Just that you don't need a dense wall of packed together vias around the edge to stop things radiating out.As for what makes an antenna, nearly everything is an antenna, even a properly impedance controlled trace on a PCB, just that it is a very very poorly performing antenna that radiates a tiny fraction of the energy. In general what makes things perform well as an antenna is forcing the electromagnetic field to go trough free space (like far apart conductors, or coils) along with hitting a resonance at the working frequency (this makes the voltages and currents rise a lot in the antenna, helping them radiate out)

author: LinuxHata
author_rank: Frequent Contributor
timestamp: July 10, 2023, 05:49:02 am
content: I actually had a case with JLCPCB, when they thought that a row of vias on PCB was actually a separator for two PCB designs, which I merged into one, so they wanted to bill me additional fees for that

author: Siwastaja
author_rank: Super Contributor
timestamp: July 10, 2023, 12:12:42 pm
content: Some PCB manufacturers are nearly hysterical with their "no multiple design" rules so such misinterpretations happen. I would solve that by explaining and if that does not work, then taking the business elsewhere, instead of changing the design.