Modelithics app note. Ground pour - Page 1
Forum section: electronics / rf-microwave

author: dmowziz
author_rank: Contributor
timestamp: August 05, 2024, 02:28:49 pm
content: HiUp till know, I thought RF boards should have "copper pours" for ground on the top where there is no signal tracePlease is this wrong?https://www.modelithics.com/Literature/AN029In the app note above, I attached the pic of the boardThe underside of the board is for ground, but I thought the top for RF should be in coplanar board formSo if adding other parts to 1 single pcb (double sided). LPF, amplifierWould it be necessary to fill the unused top part with ground?I hope the question is clearThanks!

author: ftg
author_rank: Frequent Contributor
timestamp: August 05, 2024, 02:50:39 pm
content: If you use CPWG (CoPlanar WaveGuide), then there needs to be ground next to the traces.But if you use normal microstrip, then you don't want ground next to traces, in fact you want at least a few trace widths of distance between the ground pours and the microstrip lines.And in that design they seem to be using microstrip, so no ground pour on the top is fine.

author: dmowziz
author_rank: Contributor
timestamp: August 05, 2024, 07:31:54 pm
content: ThanksTrying to understand :So if this LPF is part of a big board, I'm guessing the "exposed" part on the above image will be covered with solder mask?Will the mask be covering ground?Still this original question "Would it be necessary to fill the unused top part with ground?"Thanks

author: T3sl4co1l
author_rank: Super Contributor
timestamp: August 05, 2024, 07:41:00 pm
content: Yes, the difference is simply whether the geometry is microstrip or CWPG.Magnitude of edge coupling is quite small: typically on the order of ~10%, at design-rule spacing, for nominal-impedance traces (it increases somewhat for higher impedance and vice versa), so for example you can have a microstrip at 50Ω, bring in pours all around, and it drops to only 45, maybe 40Ω. Or the trace width (to maintain 50Ω) shrinks only slightly (whatever it is, 5-20% ballpark) for CPWG vs. microstrip.There is some effect on radiation. Obviously, the trace is visible from the outside, radiating fields couple to it; the trick is, the coupling is normally quite small. It does vary with frequency and trace dimensions (width, height above substrate, electrical length), but generally it's in the... -40dB or better sort of range, I think? That is, say: comparing the radiation from a trace over ground plane, to a dipole of equal dimensions but the ground plane removed. Despite the trace being line-of-sight visible, most of the field lines terminate into the ground plane, or circle around very near the trace.The effect with ground brought in (CPWG)is likewise fairly modest. I *think* stronger than (but still ballpark comparable to) the edge-coupling (self-impedance) change, but, I haven't seen a reference to this exactly. (There is a NIST(?) microstrip radiation test paper you can find, however, which illustrates the radiative coupling much better than my wave-of-the-hand.)In short, it's a small enough effect that, unless youreally needthat little (10 or 20%) edge in performance -- don't worry about it.Commercial applications these days, rarely if ever use shielding (cans or enclosures), as the radiation from 3.3V LVCMOS traces, with up to 100MHz clock speeds and couple-ns rise times, is modest enough, at least if you aren't running it around and across a big whole board, or between connectors and cables; and LVDS (generally speaking; exact examples including LVDS per se (EIA-644), USB (High Speed and up), PCIe, HDMI..) is used widely for faster rates. As the name suggests, Low Voltage Differential Signaling both uses less signal strength (fractional to 10s mA, 100s mV) and is routed as differential pairs, canceling out noise (and radiation!) and making the small signal level practical for fast and reliable digital transmission. The main exception is when working at serious RF -- microwave frequencies, usually for a radio as such (WiFi etc.), where a can (even without the cover placed) may be needed for adequate shielding of internal elements.For something like an RF amplifier, it might not matter, or the shield can is mandatory for various reasons (interference, coupling to other stages that would otherwise cause oscillation, receiver images, etc., or undesired radiation amount/pattern/etc.) and so the minor effect of CPWG is irrelevant compared to the major shielding of the can/enclosure (>100dB is achievable fairly easily).Tim

author: ftg
author_rank: Frequent Contributor
timestamp: August 06, 2024, 07:27:22 am
content: Quote from: dmowziz on August 05, 2024, 07:31:54 pmYou don't have to put soldermask over the RF traces and that is often avoided as it can detune them and introduce some losses.Under 3GHz for stuff that is not usually a concern. Except maybe for microstip filters.And ground fills for the rest of the board really do depend on the rest of the board and what is there.But with only that one particular low pass filter on the board, there is no particular need to add a ground pour on top.

author: Kean
author_rank: Unknown
timestamp: August 06, 2024, 09:25:57 am
content: Be aware that if you have a full ground plane on the bottom layer, having no fill on the top layer can lead to problems like bowing and warping. How bad this will be will depend on the PCB size, material, and thickness.For more info do a web search for "PCB copper imbalance".

author: vk4ffab
author_rank: Frequent Contributor
timestamp: August 08, 2024, 09:51:51 pm
content: Quote from: dmowziz on August 05, 2024, 02:28:49 pmQuite often it is better to have no copper pour on the signal layer in RF situations. What matters more than anything aside from layout, is the distance between the signal layer and ground layer in getting a more ideal LPF response from the filter at higher frequencies. You would not think that 1mm will make a lot of difference, but a via going from top layer to bottom layer will effect the higher frequency response of a filter greatly compared to a via that goes from signal layer to GND layer in a 4 layer stackup of signal, gnd, pwr, signal where that distance is only 0.3mm ISH.I mostly work with HF where things are much more forgiving, and when cheeping out for 2 layer boards, I end up using via walls and extensive ground stitching to control for things when you end up making swiss cheese of ground pours.

author: KE5FX
author_rank: Super Contributor
timestamp: August 08, 2024, 09:59:51 pm
content: QuoteNah. Don't remove copper unless you actually need to remove it. Keep microstrip traces clear, but other than that, party on with the top copper.Add ground vias until your board house complains. Then add a few more just to remind them who's boss.