Via overkill? - Page 1
Forum section: electronics / rf-microwave

author: daqq
author_rank: Super Contributor
timestamp: February 01, 2018, 08:58:05 am
content: Hi,I've been looking through the datasheet of the ADRF5044 (http://www.analog.com/media/en/technical-documentation/data-sheets/adrf5044.pdf, page 11) and I noticed the board in the attachment... Isn't this a tad excessive? I mean, isn't this an overkill? How exactly did they determine that that particular area of the PCB should be so flooded with vias?I mean, sure, stitching, stripline stuff... but it does seem a bit too much.I'm not criticizing, I'm asking, as the realm of 30GHz is a mystery to me...Thanks,David

author: TheUnnamedNewbie
author_rank: Super Contributor
timestamp: February 01, 2018, 10:11:15 am
content: I don't think it's overkill. Using two or three rows of vias is something I've seen before, perhaps more under the motto "if it's worth doing it's worth overdoing" but then again, if you are paying for a more expensive stackup like that might as well go all the way.In the center part I think it's more to keep any odd resonances between input signals at bay. It is a switch so the signals are going to be at exactly the same frequency, so it is easy to imagine that some strange coupling modes start messing up your impedance, especially at lower frequencies.

author: RadioNerd
author_rank: Regular Contributor
timestamp: February 01, 2018, 05:39:06 pm
content: Think about that:1) How many vias would you put on an RF-Board working at 3 GHz to achieve a solid ground connection? Already quite a few I presume... Now you have to increase the via density by a factor of 10 in each direction to achieve the same effect at 30 GHz... Then you easily end up with this kind of PCB layout.2) Vias are virtually for free on a PCB, therefore RF engineers usually put a few more than strictly necessary.3) And last but not least: Esthetic preferences

author: Yansi
author_rank: Super Contributor
timestamp: February 01, 2018, 05:44:42 pm
content: When tinkering with 10+ GHz, one should be aware of not to place vias symmetrically or in any repeated patterns - as that might cause standing waves to exist in between them.

author: TheUnnamedNewbie
author_rank: Super Contributor
timestamp: February 01, 2018, 05:51:28 pm
content: Quote from: Yansi on February 01, 2018, 05:44:42 pmThis is not unique to 10+ GHz. What you should be aware of is that you don't want to place anything repetitively if the order of size of the repeating (Ie, the "period" of the structure) is electrically large. Usually people use as rule of thumb larger than a tenth of the wavelength. It doesn't matter if this is at 100 GHz, 1 GHz, or 1 MHz. It's just that in the latter cases it is much harder to actually have issues with this since 1/10th of the wavelength at 1 GHz is still on the order of a centimeter, but at 10 GHz we are talking about millimeters.Sometimes this is of course done on purpose, to create the classic "voodoo RF black magic" filter structures based on distributed networks.

author: slurry
author_rank: Regular Contributor
timestamp: February 01, 2018, 06:00:33 pm
content: I usually add vias until the board weight has doubled, then it is usually enough vias.

author: daqq
author_rank: Super Contributor
timestamp: February 02, 2018, 06:55:30 pm
content: Thanks guys. So, probably not overkill.

author: dcarr
author_rank: Regular Contributor
timestamp: February 03, 2018, 12:56:13 am
content: Good article on this topic:https://www.edn.com/Pdf/ViewPdf?contentItemId=4406491

author: ogden
author_rank: Super Contributor
timestamp: February 15, 2018, 11:23:09 am
content: Quote from: daqq on February 02, 2018, 06:55:30 pmWorth noting that this is evaluation board which will be used for evaluation and measurements of IC (note "through" calibration stripline on the right side). Obviously manufacturer wanted to ensure that board is as good as it can be. It shall look so as wellObviously when you doyourcircuit, such via stitching could be overkill indeed. Usually at those (> 5GHz) frequencies you would want to run simulation of whole thing anyway - including board layout and it's vias. When you simulate - you see how much stiching is needed to achieve what you want.In short: evaluation boards can be misleading. Better learn from real world devices and also read books

author: ejeffrey
author_rank: Super Contributor
timestamp: February 15, 2018, 05:26:13 pm
content: The reason for double row via fences is the risk of launching waveguide modes which can cause crosstalk.If you have a grounded CPW or stripline transmission line, you have two ground planes. These two ground planes can support propagating modes that do not fall of with distance. To suppress this coupling you need to tie the ground planes together, making it look more like a coaxial transmission line.However, if you have a single row of vias, the gap between vias acts as an aperture in a thin-wall waveguide. Even a lambda/10 or lambda/20 aperture can radiate like a point source.Placing a second row of vias some distance away (say lambda/10), makes the aperture look more like a secondary waveguide defined a group of 4 vias. Assuming you did it correctly, your signal is far below the cuttoff frequency of this waveguide and then the field falls of exponentially away from the signal trace. For this to work, it is actually important that the second row of vias be a reasonable distance away from the first. If they are too close, it still just looks like a thin aperture, and the field doesn't have enough distance to fall off appreciably.The lower density of vias in the far field likewise suppresses travelling modes by effectively creating a band gap.Possibly this is overkill, you can do some quick numerical estimates or you can do simulations to figure that out. But this is an evaluation board for a microwave frequency switch, and isolation is probably the biggest single parameter of interest for a switch like this. It is worth overkill top avoid degrading the isolation even a tiny bit, since customers will be using this board to evaluate whether your IC can meet their performance requirements. Getting 43 dB of isolation on a PCB with a single stage switch an no shielding cans is not something that happens automatically.

author: rfeecs
author_rank: Frequent Contributor
timestamp: February 15, 2018, 05:53:21 pm
content: Quote from: ejeffrey on February 15, 2018, 05:26:13 pmExactly. And tons of vias under the package with good solder coverage to the backside ground pad because any common ground inductance will kill the isolation as well.In an actual application, if this thing is used at 30GHz it will have a cover plate that isolates each channel in a separate cavity.

author: cowana
author_rank: Frequent Contributor
timestamp: February 18, 2018, 10:46:21 am
content: It's also worth considering the wavelength - at 30GHz, it's around 1cm. So You'll want vias to be spaced more closely than 5mm intervals, as that could allow standing waves to form between them.