Ground pour on RF layer - Page 1
Forum section: electronics / rf-microwave

author: Nikos A.
author_rank: Regular Contributor
timestamp: June 06, 2019, 10:08:10 am
content: Hi everyone, I am designing a RF PCB in Eagle using micro strip traces. The RF layer is placed on top of the board.I filled up the layer with ground pour and vias for both better RF performance and heat dissipation as I am using two LNAs across the board.What I am concerning about is the danger to have accidentally "convert" the micro strip line into coplanar waveguide changing the 50ohms impedance. At the moment the ground pour opening is twice the RF trace.The attached image is the first layer in Single Layer Mode.What is your opinion? Should I reduce the ground pour area?Thanks is advanceNick

author: T3sl4co1l
author_rank: Super Contributor
timestamp: June 06, 2019, 10:13:22 am
content: The gap to substrate ratio is the relevant figure; if this is a normal proto with thin e.g. 7 mil prepreg, it's more than plenty clearance that it will be very close to microstrip as such.Tim

author: Nikos A.
author_rank: Regular Contributor
timestamp: June 06, 2019, 10:19:20 am
content: This is a total 0.8mm thickness board with 0.14mm (aprox 5.8mils) prepreg. So this is ok?

author: Nikos A.
author_rank: Regular Contributor
timestamp: June 06, 2019, 11:02:58 am
content: By the way I've found a great article explaining how the impedance of a microstrip is affected by the ground plane.https://www.edn.com/design/analog/4407109/PCB-s-top-ground-plane-and-its-effect-on-a-microstrip-line-s-characteristic-impedance

author: T3sl4co1l
author_rank: Super Contributor
timestamp: June 06, 2019, 11:51:55 am
content: Yeah, or easily enough seen playing with a calculator, or comparing with microstrip:http://www.chemandy.com/calculators/coplanar-waveguide-with-ground-calculator.htmhttp://www.chemandy.com/calculators/microstrip-transmission-line-calculator-hartley27.htmYou'll find the error is well within the fab tolerance, unless you're getting a terrifically precise (10%, even 5% Zo tolerance?) product.Tim

author: Rerouter
author_rank: Super Contributor
timestamp: June 06, 2019, 12:00:04 pm
content: You can use "Saturn PCB toolkit" to calculate what your impedance will be in those scenarios,

author: mc172
author_rank: Frequent Contributor
timestamp: June 06, 2019, 01:38:12 pm
content: You have got coplanar waveguide, not microstrip. You've either got ground copper on the top layer or you haven't.With coplanar waveguide the impedance is also a function of the track width, not just the spacing of the track to ground, so your pads decrease the impedance locally even though the gap is the same.I've attached a picture and highlighted a few areas. They are numbered from 1 to 3. In circle 1, the reduced spacing between the square green pads and the track will reduce your impedance even though the track width has not changed. This region is probably the most significant of the three because it is electrically quite long. I don't know what frequency you are working on but relative to the board length, and because the same happens at the other side, this could be quite major.The local impedance at the input and output pads (Circle 2) will be very low (I assume that's what they are). The fact that the pads are larger than the track width on its own would usually be OK, but because the ground does not expand around the pads in combination, you will be in the low 30s going by the aspect ratio.Circle 3 will also be lower than you expect because the pads are larger than the track and the ground does not expand around the pads. Probably not that important but if it were me, I'd expand the ground around it to match the rest of the clearance.However, that being said, I wouldn't focus too much on trying to make everythingexactly50 Ohms, especially things that are quite short such as the pads of components. The best way is to build one and attack it with a scalpel - cut away some ground where you think there might be a problem and see if it improves. If not, it wants more capacitance or a lower impedance. If nothing happens, it's not really critical.You may want some ground pour between the track above where I've put a number 2 and your "TP PART1" track to reduce coupling. It might not need it, I don't know.Unrelated...Be careful with lots of very closely spaced vias around where you are trying to conduct thermal power away. Lots of vias decreases your conductive surface area. I understand that you are trying to get the thermal power to the bottom layer but in doing so you reduce the cross-sectional conductive area along each side of the board In this case, all you do is just get the power to the other side and not much further. If you can fill them with solder then this problem goes away.I know everyone has their favourite calculator etc. but I really like AppCAD.http://www.hp.woodshot.com/

author: Nikos A.
author_rank: Regular Contributor
timestamp: June 06, 2019, 02:28:05 pm
content: Dear mc172, thank you for your detail reply.QuoteThis is the the SMA connector pads, I cannot avoid this area.. The max frequency I am going to pass is 2.7Ghz. Do you have any suggestion?QuoteCan you give a further explanation? How could I expand more the ground?QuoteYou mean the upper and lower clearance to be same?QuoteThis is LNA component and I consulted the manufacturer to achieve adequte RF and thermal performance. Tell you the truth, he suggests an even denser vias arrangement

author: ejeffrey
author_rank: Super Contributor
timestamp: June 06, 2019, 04:38:30 pm
content: Quote from: Nikos A. on June 06, 2019, 02:28:05 pmWhat connector are you using? Do those square pads really need to be that large? At least make them round instead of square!QuoteJust increase the clearance from the top ground pour to the pad to match the clearance to the transmission line. That will reduce the unwanted ground capacitance of the pad, although it will still be pretty high due to the capacitance to the inner ground plane layer.

author: Nikos A.
author_rank: Regular Contributor
timestamp: June 07, 2019, 06:16:28 am
content: Dear all, thank you for your replies.. Finally I decided to remove the ground pour form the top layer as it was changing the impedance around 12%. I placed ground pour only under the active ICs components.Also convert the SMA square pads into circular as correctly recommended.I have got some RF filters and looking the datasheet I couldn't find any reference on vias beneath them. Does it recommended in general vias under passive components?

author: mc172
author_rank: Frequent Contributor
timestamp: June 07, 2019, 08:10:14 am
content: I think the poured ground would be a better solution, but it's up to you.I haven't seen SMA connectors that look like that before. They're normally like this:The holes for the SMA connectors don't have to be in the middle of the pads. This way you could keep the impedance constant through the pads underneath.I've bodged together a picture, attached.In that picture I've attached, can you see how the output pad (I assume) on the far right has the ground plane expanding around it, to keep the gap between it and the ground plane the same size? That's what I was talking about doing around your other component pads.

author: rf-messkopf
author_rank: Regular Contributor
timestamp: June 07, 2019, 08:51:37 am
content: As mc172 already said, the SMA connector footprint looks unusual. And you should avoid the thermals at its THT pads, because you are effectively joining the connector ground through a piece of transmission line. The connector has plenty of thermal mass anyway, so the thermals will hardly improve solderability.

author: Gribo
author_rank: Frequent Contributor
timestamp: June 07, 2019, 04:59:05 pm
content: Can you post the SMA connector's PN? Either you are missing one hole in the center, or you are using edge launch connector. In both cases, your footprint is wrong.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: June 07, 2019, 07:58:57 pm
content: Quote from: rf-messkopf on June 07, 2019, 08:51:37 amIn a 4-layer board, even with solder wave, I think you will find a substantial difference in favor of spokes.The equivalent stray inductance of spokes is easily calculated; it's negligible.By the way, try to maintain copper density on top and bottom -- if you have unpoured top, bottom probably should be unpoured as well. Or pour both.Tim

author: ejeffrey
author_rank: Super Contributor
timestamp: June 07, 2019, 09:43:42 pm
content: Quote from: Gribo on June 07, 2019, 04:59:05 pmI am assuming it is something like the cinch connectivity 142-0761-881https://www.digikey.com/product-detail/en/cinch-connectivity-solutions-johnson/142-0761-881/J801-ND/726108which looks similar to what is drawn. But if you follow the manufacturers footprint, it will preserve the waveguide geometry properly.

author: Gribo
author_rank: Frequent Contributor
timestamp: June 09, 2019, 02:55:32 pm
content: There are other edge mount SMA, with a saner footprint (pads only, no VIAs).Example:https://www.digikey.com/product-detail/en/cinch-connectivity-solutions-johnson/142-0701-841/J630-ND/396573

author: Nikos A.
author_rank: Regular Contributor
timestamp: June 10, 2019, 06:58:45 am
content: Thank you for your replies!! I appreciate that!!ejeffrey, this is exactly the SMA connectors I used ( 142-0761-881). Ok, a few questions regarding the footprint..For my project, I have got design microstrip RF transmission lines but the manufacture suggest coplanar waveguide for its SMA connector footprint..In case I decide to keep these SMAs I must recalculate the transmission line as coplanar waveguide and fill the top layer with ground pour isn't it?If I want to keep the microstrip designing I must select a different SMAs connectors, like this one Gribo suggests?https://www.digikey.com/product-detail/en/cinch-connectivity-solutions-johnson/142-0701-841/J630-ND/396573

author: ejeffrey
author_rank: Super Contributor
timestamp: June 10, 2019, 09:39:09 pm
content: Quote from: Gribo on June 09, 2019, 02:55:32 pmThe connectors in question are designed for high performance use on thin substrates or multi-layer PCBs. The center pin is tiny to directly solder to 10-20 mil traces that are typical for 50 ohm microstrips on ~5-10 mil dielectrics. The guide pins help locate them so that the pin lines up with the center trace, which isn't normally required on the kind of chunky edge mount connectors you show. That type of connector will work well on a standard 63 mil two layer PCB but will have too much parasitic capacitance when used with smaller geometry transmission lines.Quote from: Nikos A.You need the ground pads on the top in order to make contact to the connector. So you will be building a GCPW there no matter what. Past the body of the connector you can transition to whatever transmission line geometry you want as long as do the transition properly. GCPW is essentially a continuum between pure microstrip and pure CPW, chances are your modes are going to look mostly microstrip no matter what, so the transition should be pretty easy.Personally, I don't really like those connectors. They are too fragile, have a lot of assembly problems, and don't handle torque well. So I avoid them if at all possible.

author: Nikos A.
author_rank: Regular Contributor
timestamp: June 11, 2019, 10:58:25 am
content: Well some updates, I modified the footprint to match manufactures one.I calculated the transmission line for GCPW and then I transited to microstrip.. For microstrip I re-calculated the trace width and gradual reduced it..Any comments?

author: TheUnnamedNewbie
author_rank: Super Contributor
timestamp: June 11, 2019, 01:28:40 pm
content: I would suggest avoiding the sharp corner on that transition, and instead having a curve. Ideally, you would simulate these things but that is easier said that done. Do it over the same length as you taper the transition of the center dielectric, just to make it a bit more gradual, and avoid radiation losses from those edges. (but all things considered, I doubt you will see much issues at 2.7 GHz)Oh and just a heads-up: These kinds of SMA connectors have quite good performance, but can be an absolute PAIN to solder.

author: Nikos A.
author_rank: Regular Contributor
timestamp: June 11, 2019, 03:05:06 pm
content: Thank you for your reply!!QuoteAre you talking about the ground pad edges?QuoteDo you know any free or low cost software?QuoteCan you give more explanation? What should I do the same length?

author: ejeffrey
author_rank: Super Contributor
timestamp: June 11, 2019, 11:52:39 pm
content: Yes, I am pretty sure he means the ground pad edges. The idea would be to extend them and then round the corner out. It isn't bad practice, but given that this is only a very minor transition and you are operating at relatively low frequency, I doubt you will notice.

author: Nikos A.
author_rank: Regular Contributor
timestamp: June 12, 2019, 12:00:48 pm
content: Reading some papers I found that an acceptable solution it to gradually widen the gap between the ground planes and the signal.. I applied this method on my design.I am really curious to simulate this transition, is there any free software?Quote from: ejeffrey on June 11, 2019, 11:52:39 pmMaybe this changes slightly affect the performance as you mentioned but I prefer to learn the correct designing techniques for future designs.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: June 12, 2019, 12:37:56 pm
content: Wait, why does the trace get narrower, not wider? The ground doesn't look to be receding very "gradually" as shown.A tapered transition between CPWG and microstrip should be long enough for the lowest frequencies of interest, and tapered enough for the highest frequencies of interest to not be reflected. Although as long as impedance is constant, I can't really justify what that means, geometrically.Probably it's more important just that the trace width is tapered to reflect the approach of nearby ground: if you think about a wavefront approaching a "wall" of coplanar ground, it begins to "see" it, and the effective separation distance to CPG varies with distance from the "wall". The trace width would then be tapered to follow this.There will be a reflection angle and distance, important to very high frequencies. The impedance seen by a wavefront becomes dispersive (the wavefront is smeared out somewhat). Which means the impedance is changing, even if you adjust for trace width. Or actually, it doesn't need to be the impedance changing as such, but the transmission and reflection properties of that TL section (since it's a 2-port) can do goofy things, independent of the impedance. Because /an/ impedance is a 1-port and its response is fixed by the Kramers-Kronig relations, but the same does not hold true for a 2-port (more correctly, it does, but the added degrees of freedom (3 unique matrix elements) allows for arbitrary phase shift.)Yeah, so you would have some compromise between funny phase shift, and funny reflectance or transmission, with such a structure I think. And it can be minimized by tapering the ground so that the reflection angle is shallow; it wouldn't be so much a ratio of electrical length, as a geometric ratio to the width and height of the structure.I would guess an exponential or hyperbolic ground profile would be close to ideal: it approaches quickly from a great distance, because the field at a distance is still very small; as it gets closer and the reflected field becomes a greater fraction of the total, the angle gets shallower, reducing dispersion; eventually at the throat of this planar "horn" shape, the angle is so shallow as to be unnoticeable, and it's pretty much identical to parallel CPWG.But again, all of this assumesextremelysensitive analysis -- if you aren't doing <100ps TDR, or precision metrology in the many GHz, you won't even begin to notice this; and compared to a manufacturing tolerance of 10%or moreit's nothing more than academic at best!Tim

author: Nikos A.
author_rank: Regular Contributor
timestamp: June 12, 2019, 01:40:41 pm
content: Are you an electronic guru or something like that??? Thank you for your detailed once answerQuote from: T3sl4co1l on June 12, 2019, 12:37:56 pmIs there any book reference / guidance of designing the tapered transition geometry?Quote from: T3sl4co1l on June 12, 2019, 12:37:56 pmI calculated the trace width in both cases (GCPW and microstrip) in order to keep the impedance as close as to 50ohms and the trace width of GCPW is slightly wider. Do I missed anything?The maximum frequency of interest is 2.7Ghz, do you believe that I am going to face any serious signal distortion?By the way I suggested the attached paper to implement the transition.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: June 12, 2019, 02:03:46 pm
content: Your screenshot shows a negative angle compared to the diagram in the paper.2.7GHz is like "DC", see the axes in the paper!Actually, why are they showing transmission loss at DC? Is this not the entire structure, are they missing something?It's also written specifically about monolithic structures (high resistivity Si, SiO2 insulator, micron measurements), so who knows what everything they were doing was. Maybe it's part of a planar transformer structure, and that's why the low frequency response drops off.Tim

author: schratterulrich
author_rank: Regular Contributor
timestamp: June 12, 2019, 02:13:55 pm
content: I am also of the opinion that the trace width of the microstrip section must become wider than the coplanar waveguide section.This is due to the increased capacitance of the coplanar section. So with same trace width the coplanar section would show smaller Z0 (Z0=sqrt(L/C)).I think formula based calculations of trace width has limitations on accuracy. I would prefer TNT for example. It's a free FEM based Transmission line solver. You can find it athttps://sourceforge.net/projects/mmtl/I don't know free simulation tools capable of simulating the transition from Coplanar to Microstrip. But there are models for tapered lines, corners and pads in Ansoft Designer SV. It's a obsolete free student version of a very comprehensive RF suite.You can find it athttp://www.gunthard-kraus.de/Ansoft%20Designer%20SV/English%20Tutorial%20Version/DesignerSV050610.exeYou can find a good introduction somewhere on this homepagehttp://www.gunthard-kraus.de/

author: Nikos A.
author_rank: Regular Contributor
timestamp: June 12, 2019, 02:28:44 pm
content: Quote from: T3sl4co1l on June 12, 2019, 02:03:46 pmPlease see my calculations (attached files) for microstrip and coplanar trace width.. The coplanar is wider.. Do I have anything wrong?Quote from: schratterulrich on June 12, 2019, 02:13:55 pmThank you for you links!!

author: T3sl4co1l
author_rank: Super Contributor
timestamp: June 12, 2019, 10:16:32 pm
content: Yeah, going to guess Saturn's CPWG formula is wrong.Again, while theoretically amusing, these tweaks are way, way down in the noise of practical engineering.Tim

author: TheUnnamedNewbie
author_rank: Super Contributor
timestamp: June 13, 2019, 07:01:26 am
content: I stuffed both into HFSS real quick. Take these results with a grain of salt, as I didn't solve it the 'right' way for such low frequencies:Modes from modesolver below. I think the problem here is that the distance to your gap is significantly larger than the thickness of the PCB. As a result you pretty much get a microstrip, with some additional metal on the side that results in more fields going through the air. This in turn results in somewhat lower capacitance. This is also seen in the simulations - the CPW has higher impedance.(note that while the impedance are not exactly equal, they are within what you can expect from standard FR4 tolerances).If I have time later, I might actually try and giving you the design of a quick taper from HFSS too, and compare results of what you had as well as with/without taper.

author: schratterulrich
author_rank: Regular Contributor
timestamp: June 13, 2019, 11:23:23 am
content: Did you connect the "coplanar" planes to ground at the waveport entry in your HFSS simulation?

author: TheUnnamedNewbie
author_rank: Super Contributor
timestamp: June 13, 2019, 11:51:04 am
content: Quote from: schratterulrich on June 13, 2019, 11:23:23 amI forgot! re-did the sweep, same shape, but now around 49 ohm instead.In other words, the two give pretty much the same impedance indeed, just with a slight offset found in the saturn pcb calculator tool. Doing a full s-parameter simulation gives me the same results within a fraction of an ohm.

author: Nikos A.
author_rank: Regular Contributor
timestamp: June 13, 2019, 01:09:45 pm
content: Thank you guys for your help, so I am going to proceed with this design and will reconsider after testing the completed board.