Chip Antenna on Complex PCB Footprint/Layout - Page 1
Forum section: electronics / rf-microwave

author: Bedmonds91
author_rank: Contributor
timestamp: February 09, 2022, 02:45:00 am
content: Hello everyone, this is my first post ever so please let me know if I'm doing this wrong.I am trying to find design a chip antenna into a PCB that is very packed with components and has an odd footprint.It is a 4 layer board and I am using an ESP32-PICO to drive the antenna.Layer 1 (Top Layer) and Layer 2 are both ground planes, while Layer 3 and 4 are for 3.3V and 5V, respectively.The images I have attached will show you how I have laid out the the chip antenna around the other components.The antenna is from Johanson, PN: 2450AT18B100Datasheet:https://www.johansontechnology.com/datasheets/2450AT18B100/2450AT18B100.pdfI have spoken to tech support at Johansen and all they said was that it should be moved to the lower edge of the board (as shown in the image labelled AlternativeLayout). They also suggested a smaller package size (i.e. the 2450AT07A0100) which is shown in the image.I really like my original layout, and I didn't get a clear answer as to why it wouldn't work.If anyone could please take a look at the images and let me know what their thoughts are, that would be fantastic.Thanks,Bedmonds91

author: T3sl4co1l
author_rank: Super Contributor
timestamp: February 09, 2022, 03:22:43 am
content: What's the slot all about? How tall? And does anything go there (mechanical?)?The chip antenna won't be on band because it's the wrong distance from nearby ground, and that distance isn't spanned by bare laminate. Maybe the lower k (air) would account for the shorter distance, I don't know. It's also sprung out on a short distance of the web (arm? loop? slotted-off section? whatever), not projecting off a straight edged ground plane.The long web of board screams PCB antenna, but you'll need to tune that yourself. I mean, it's not so bad, if you have a SNA/VNA, and the time to do it; but lacking just one of those things, good luck, yeah.I imagine all of that can be tuned out [about the chip antenna], too, but again... if you need design assurance? Copy the MFG design, nothing you can do to it.I would anyway leave the rest (bottom) of the arm blank, no point in grounding up in there. Could make things worse by making a stub anyway. Stitching vias along the antenna edge are preferable. I suppose you can't reroute that, what is that, N$30?I don't like the long trace. It might be okay as stripline? Could go straight to layer 3 and calculate it for buried stripline of correct impedance. Maybe there's not even enough room for stitching vias in that web bit there? Hrm.Is there room for a patch antenna, off some tiny coax and a U.FL connector or whatever? And, is the enclosure of recommended material, thickness, distance (clearance), etc. to support one?And I suppose the radio / controller can't go in any other corner of the board, or, not like you have any more room anywhere else anyway?What about backside placement, and could you afford blind/buried vias if necessary to facilitate such a layout?Definitely a challenging situation. Afraid nothing great comes to mind.Tim

author: MartinL
author_rank: Regular Contributor
timestamp: February 11, 2022, 04:00:56 pm
content: There's something that everyone ought to understand about chip antennas, but which nobody really tells you explicitly:A "chip antenna" is not actually a complete antenna.When you look at the reference PCB layout in the manufacturer's datasheet - thatwhole PCBis what's actually the antenna.The driven element (the chip), and the layout & ground plane around it, work together as a unit. When you drive an RF current into the chip, the combination of the dielectrics involved and the geometry of the layout causes RF currents to flow back and forth throughout the PCB, and the whole combination has been designed such that it will radiate effectively at the target frequency. The size and shape of that cutout around the antenna is a critical part of the tuning of the design. The sizing of the rest of the board is less critical, but still important.So why are chip antennas useful at all, if they're so dependent on the reference layout?The answer is that you can take a bunch of extra components and tracks, and lay them out on top of that empty ground plane, and the result will work almost exactly the same as the empty ground plane alone. So you get to use your whole PCB as the antenna, and use all that space for components as well, with the components to drive that antenna - the chip element and matching network - only occupying a small space in the corner (or sometimes a side).But thisonlyworks properly if you keep that big solid ground plane under your PCB, and you keep that precisely designed cutout around the chip element. Otherwise, you're missing most of the antenna.Your board layout is full of slots - it won't behave at the same as a continuous ground plane. And you've got nowhere to put that precisely designed cutout that goes around the chip element. So you're not really getting anything out of using this element. You're basically trying to design a new antenna from scratch, but with no calculations or simulations behind it at all. The whole point of these off-the-shelf chip elements is that someone else has done the work to design an antennaaroundthem which you can can incorporate into your layout.I think the reason Johansen have advised moving the chip to the bottom left corner is that it's at least possible to try to create the necessary cutout around it there. Your original layout didn't try to reproduce the cutout geometry at all, and your alternative still doesn't match the tested geometry in the datasheet.My view is that your layout is sufficiently unusual that to get a really effective antenna then you're basically going to be designing from scratch.My suggestion would be to use a PCB trace rather than a chip element. The "handle" area that you placed the chip antenna on seems like a perfect place to run a trace antenna along. You could tune it experimentally on a prototype by making the trace the full length of the handle, and then cutting away copper millimetres at a time until it resonates at the right frequency on a VNA, with a connector (perhaps U.FL) soldered in at the feed point.Keep the footprints for a pi matching network in there too, and they'll give you more degrees of freedom you can tweak for a good match.For an example of the approach I'm describing, see the latter parts of this guide:https://colinkarpfinger.com/blog/2010/the-dropouts-guide-to-antenna-design/

author: Bedmonds91
author_rank: Contributor
timestamp: February 15, 2022, 10:50:02 pm
content: Thanks for your replies. I understand that these chip antennas are only really half the antenna and require a ground plane. What I can't really find a straight answer to is about where the "reflection" is happening. Like does it matter where the ground plane is relative to a specific orientation of the chip and how big does the surrounding ground plane need to be?The bottom layer of my PCB is carrying 5V but it is a copper fill. Would that still work then if I put the antenna on the bottom or does it half to be connected to ground?The "Alternative" design that I posted I think could hold the shape and dimensions of the "no fill zone" so do you think that would be enough?I have also tried a trace antenna down that right arm of the PCB and it worked but with a high dropout rate. Like I could send simple commands to the ESP32 but I could rarely flash an OTA update.OI also don't have access to a VNA so I'm not sure which option is best.

author: Bedmonds91
author_rank: Contributor
timestamp: February 15, 2022, 10:51:52 pm
content: If anyone on here is familiar in this sort of unique design I would very much appreciate a video call where I could share my work in much more detail.

author: Marsupilami
author_rank: Frequent Contributor
timestamp: February 16, 2022, 04:15:43 pm
content: I know this wasn't the questions, but have you considered not messing with it and having a discrete antenna instead?E.g. Molex flexible flat patch:https://www.digikey.com/short/z012mb3jIf your enclosure can fit it I might recommend this way as the only thing you have to do is put a U.FL connector on your board.Without doing simulation and proper performance characterization I find changing even the smallest detail compared to the reference design very risky. If you want to learn the process you can also make multiple separate antenna part pcb-s also fitted to be connected via the ufl connector, that way you won't have to respin the whole board because your antenna didn't turn out as you would've liked.HTH Good Luck

author: Bedmonds91
author_rank: Contributor
timestamp: February 18, 2022, 01:37:50 am
content: Actually that won't work for this project. The application doesn't actually require an enclosure at all and definitely won't be able to support a discrete antenna.

author: Bedmonds91
author_rank: Contributor
timestamp: February 18, 2022, 03:33:28 am
content: Here is the PCB antenna I designed previously which does work but not very well. It has a trace width of 1.574mm (just as wide as I could get it), and 23mm long.23mm was as long as I could fit on that PCB cutout area, but should it be longer or will I be able to cut it back from 23mm as a tuning method?Does the width matter?Another thing I don’t understand is the length of the antenna. Should I just make it as long as possible? I've seen designs that increase the length by routing through to other layers in order to continue past blocking components but I also read somewhere it should be 1/4 wavelength.How could I test this without a VNA. So far the only way I can really gauge it's performance is whether or not I can complete a large data transfer successfully such as an OTA to the ESP32.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: February 18, 2022, 01:50:12 pm
content: The length is probably about right. I would guess the impedance is too low. So, you have three components (matching network) to solve for, based on that. And, being slightly shorter than 1/4 wave (~30mm) maybe it's reactive. Or maybe proximity effect balances that out and it's near resonant. Unfortunately it's impossible to say without a full-field simulator or VNA.Tim

author: Bedmonds91
author_rank: Contributor
timestamp: February 23, 2022, 04:34:25 pm
content: If I bought the NanoVNA (www.nanovna.com), how would I connect it for testing? I would like to avoid designing in a temporary connector. Will it work if I just solder a lead to one of the pads of the matching network?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: February 23, 2022, 05:05:41 pm
content: Does that have enough frequency range? Or dynamic range? The website doesn't say... matter of fact, it doesn't have ANY kind of spec sheet at all, I'm now realizing.Likely a piece of thin coax, surface-mounted to where the radio goes, shield to exposed pad and thus GND, center to antenna pad, will do. Very little unshielded length of the center, no loop height, just straight into the pad. Then you can do an open/short/termination calibration with the first component in the tuning network, and finally, tune the antenna element by these components and/or trimming element length (cutting excess copper if too long, or adding series inductance if too short).Tim

author: Bedmonds91
author_rank: Contributor
timestamp: February 24, 2022, 04:40:01 am
content: Ok so I did some more testing, and the current trace antenna is actually showing some consistency so I think I'm just going to make some adjustments and see if things improve.To do this, I made the antenna trace a little longer by continuing it around the bottom corner to get it closer to the 1/4 wavelength range. This has increased it from 23mm to about 26mm, maybe a little more.I also replaced the previous matching circuit with a single 0603 0 Ohm resistor in order to have a better chance at wiring up a VNA. There are ground vias close enough to complete the PI network with the two capacitors later.If anyone could please let me know if these minor changes are a step in the right direction or not, that would be very appreciated.I've attached an image of the new design.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: February 24, 2022, 05:05:25 am
content: Eh, I'd rather use a narrower, sinuous track, than putting it so close to those LEDs.Note that, within reason, you can make a trace longer by putting an inductor in series with the base, or shorter by cutting the end off.Tim

author: Bedmonds91
author_rank: Contributor
timestamp: February 24, 2022, 06:47:12 am
content: That makes sense. I always wondered if the thickness of the antenna trace mattered. I kind of just assumed it should just be really thick.Is there a minimum trace width if I'm going to it a sinuous path?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: February 24, 2022, 07:14:55 am
content: Like 20 mils is probably fine.Tim

author: Bedmonds91
author_rank: Contributor
timestamp: February 24, 2022, 03:47:45 pm
content: Great, so 20 mil seemed to be just right for me to meander the trace down the same path. Right now it's about 33mm long so I'm guessing that's enough freedom to tune it.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: February 24, 2022, 09:04:26 pm
content: Looks nice.Pull in those GND vias, or make them smaller; they'll surely get clipped by the board edge rout!Tim

author: rfclown
author_rank: Frequent Contributor
timestamp: February 24, 2022, 10:00:45 pm
content: I see that you've gone away from the chip antenna, but FYI...You didn't have the matching network shown on the Johanson datasheet (at least it isn't shown on your schematic). The components that are on your schematic (and on the esp32-pico datasheet) are not a matching network, but a low pass filter. The matching components on the Johanson datasheet, and keeping the same ground structure around the antenna as shown on the datasheet are all essential to making that chip antenna work. Like MartinL said, it's the whole PCB (and matching network) on the datasheet that is the antenna.

author: Bedmonds91
author_rank: Contributor
timestamp: February 25, 2022, 12:05:48 am
content: Quote from: T3sl4co1l on February 24, 2022, 09:04:26 pmThanks for noticing, but those GND vias are actually part of the footprint for the push buttons, which haven't been cut off in previous iterations. I was also going to ask if you think the 0603 pad I'm using to bridge the transmission line is good enough to connect/solder to a VNA connector. I've attached a close up of it to clarify. I tried designing in a UFL connector but there's just no room at all.Quote from: rfclown on February 24, 2022, 10:00:45 pmYes I decided I'd just go for the simple trace antenna instead since the chip antenna needed to be placed a lot further from IC and since it was really difficult to fit the exact dimensions from the datasheet into the bottom corner of the PCB.

author: cdev
author_rank: Super Contributor
timestamp: February 25, 2022, 01:42:17 am
content: Is the gold color grounded? If so, I suspect it will interfere with the "meandered" antenna trace no-matter what the intent is. It would be better to end the use of any ground plane in the entire "handle" area Cut it off in a straight line so that the monopole antenna is in the clear.UFL connector doesnt need to be very wide, and its useful to have, I would try to do it.I hope I'm clear in that I think the wavy red trace antenna should be the only metal on the handle shaped part of the PCB. The ground should end at a straight line so the antenna can be in the clear.Almost any device can benefit from an RF connector. Keep in mind that ufl connectors are only meant to be connected and disconnected a few times in their lifetime. (25 max?) If its an antenna that you want to disconnect and reconnect, try to use an SMA instead.I have a router that uses almost this exact same layout, it has a UFL connector inside out of sight. it works fine at 2.4 GHz.

author: cdev
author_rank: Super Contributor
timestamp: February 25, 2022, 02:01:43 am
content: Quote from: Bedmonds91 on February 23, 2022, 04:34:25 pmBuy a piece of the very tiny 52 ohm teflon coax and strip and tin the end very carefully. Keep that part very very short. Then solder that to the transmission line. Measure its electrical length in your VNA. Make a note of it. That will be your calibration plane. I was sure I would fuck up on that but surprise, as long as both ground and center lead are super short, it works fine. At least it does for me. I'm not saying there are no blips or no loss, but its not bad. Its sure better than what you might do without the VNA to tell you how you're doing.If you were looking into some kind of balanced (coplanar waveguide) antenna you could also use a tiny balun (transformer) there, a 1:1 transformer if you want. In some situations with a PCB that might be appropriate. But I see no reason to, given your antenna is a monopole, i.e.unbalancedis what you want, and you've already got it. A transformer can be useful for measurement but the higher you go in frequency the more lossy it might be. A tiny broadband ferrite starts to get too lossy to work well at around 1.5 - 2 GHz.

author: Bedmonds91
author_rank: Contributor
timestamp: February 25, 2022, 03:31:36 am
content: Actually if you see my previous response, I posted an image with the copper fill which shows the cutoff point you're suggesting. As for the UFL connector, this is just for testing and won't be used more than a handlful of times. I also checked, and the connectors are at least 3mm x 3mm and I only have about a 2mm x 2mm area to work with.And thanks for the VNA tip! I'm just making sure I have enough copper to work with for testing.Which pad of the bridge resistor would I solder the coax to? Directly to the antenna, or to the IC side with the 0 Ohm resistor soldered on?I also made sure those two pads were close to the GND vias so I could potentially add a parallel capacitor to each side to complete the PI network.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: February 25, 2022, 10:16:58 am
content: Quote from: Bedmonds91 on February 25, 2022, 12:05:48 amOh, those are thru holes?Hmm, probably fine. Not great, but mainly that kind of thing serves to key the switch in place, not necessarily so much to adhere it. Does mean it's easier to tear out, of course that's only going to happen after the SMT pads tear off, and all of that would be really strange for a pushbutton. (So, maybe something to keep in mind for a header or connector.)Yeah, coax right to the footprint, like this:Tin the shield all around, and solder that to the radio footprint. DNP or remove the chip beforehand. You don't have any other good enough grounds around to do this. Even then it's not perfect: with the vias being pulled in from the edge of the pad, there's still some distance around the edge before current can return to the bottom side ground plane. Hmm, there's nothing under that (bottom side) right? Probably better to put the vias closer to the edge than in the middle of the center pad.Then use a 0 ohm jumper or relatively large cap (100pF+?) in the footprint there. This keeps the unshielded coax length absolutely minimal. You don't have many mm to spare before the impedance starts to go wonky.Be careful about soldering the coax; polyethylene melts easily and can short to the shield. Teflon should be easy to handle here.Also slide a few ferrite beads onto the coax before assembly. Doesn't hurt to have a bit more isolation. Remember, the board is reaction mass, serving as a "too large" counterpoise; it will have little common mode voltage, but not zero. Which in turn means the coax cable will affect the measurement -- its (outer shield, CM) impedance will load that voltage.This effect will be worse if the coax isn't solidly grounded to the board, which is why the ground should be very good.So, some FBs to increase and stabilize that impedance, is cheap insurance. (If you don't have any, or don't know what kind you do have, specifically high frequency #61, #67, etc. types should be fine.)Tim

author: Bedmonds91
author_rank: Contributor
timestamp: March 01, 2022, 04:29:35 am
content: Unreal feedback! That drawing clears a lot up for me as well.I think I am going to purchase the LiteVNA which has a working range up to 6Ghz so it should be fine.