PCB mount antenna design - Page 1
Forum section: electronics / beginners

author: Silenus
author_rank: Contributor
timestamp: February 01, 2015, 01:40:27 am
content: Not sure if this is a beginner topic, but still. I am looking to mount a2.4 GHz antenna chipon my pcb and am a bit stuck on the placement of the antenna. On the first page they talk about two instances, with matching circuit and one without. When and why do you use a matching circuit over not having it? It also says "trace width should be designed to provide 50 Ohm impedance". Why isn't trace length also a factor for selecting 50 Ohm impedance? How do I go about designing a trace to match 50 Ohm impedance?Sorry for the barrage of questions, just trying to wrap my head around some of these concepts.

author: VK5RC
author_rank: Unknown
timestamp: February 01, 2015, 05:07:39 am
content: If properly shaped and the feed point correctly positioned the pcb antenna should have a 50ohm feed point input impedance, the output from the ic is very likely not 50ohm. To get maximum energy transfer, the impedances must match to avoid reflections which cause standing waves, and if at modest power can damage the amplifier. Hence often an impedance matching circuit is required, it 'looks' like whatever impedance the amplifier is to the amplifier but presents 50ohm impedance to the antenna.At high rf frequencies you must remember that a straight line on a pcb is often a substantial fraction of a wavelength so it can 'look electrically' like an antenna (eg 1/4 wavelength) and radiate IF there is impedance mismatch and not act as a transmission line. If no mismatch there is no reflections so its length is not relevant.A lovely video from bell labs shows the importance of impedance matching and reflection at impedance mis-match.

author: theatrus
author_rank: Frequent Contributor
timestamp: February 01, 2015, 05:25:54 am
content: There are two ideal ways of putting 2.4GHz RF lines and matching networks on a PCB:Copy a reference designexactlyBuy/rent a VNA and learn a lot about how to read a smith chart

author: ConKbot
author_rank: Super Contributor
timestamp: February 01, 2015, 05:47:11 am
content: Look further down the datasheet for the with and without matching network return loss and smith charts. Without its 2.76 GHz center frequency, and a ~150 MHz wide for a 2:1 VSWR. With the matching network, its 2.47 GHz, and 230 MHz wide for a 2:1 bandwidth. ~-10dB return loss corresponds to a 2:1 VSWR, and usually an antenna bandwidth is specified as where its VSWR is below 2:1.Return loss is measuring the ratio of how much power comes back on the same port when you send power down it, in db. I.e. you send 0 dBm down a transmission line to a device on the end and -10 dBm comes back, the return loss is -10dB. Since you know how much comes back, you then know that the rest is either radiated as your EM waves (good!) or turned into heat by dielectric loss, resistance in the antenna, etc (bad). But a return loss plot wont tell you which.VSWR is from when you would literally move an RF volt meter down a transmission line, looking for standing waves, and it was the ratio of the peaks to the troughs. So literally the Voltage Standing Wave Ratio. Its not measured like that, typically anymore, but the unit is still used.If your transmitter is at 2.45 GHz, then it looks like a -2.5dB or so return loss, so less than half your power will be radiated, and the majority of it will be reflected back into the transmitter. So put in the matching network and the antenna will shift down in the frequency, open up the bandwidth a tad.TLDR; if its a 2.45 GHz device (or 2.5) then the antenna will be on the wrong frequency without the matching network that they specified.

author: Silenus
author_rank: Contributor
timestamp: February 01, 2015, 09:13:11 am
content: I am looking to use theRN-171wifi module. For a PCB trace antenna it says I need a 4 layer board which is unnecessary for my project plus more $$ (so im guessing I can't go with that option). For the chip antenna, it gives achipwhich I can't source from my supplier, nor will I have a 4 layer board that they used to test it or the pi network. If I say, just went with a 2 layered board, used a similar antenna chip and copied the pi network in the datasheet, would it be close enough or will a small change degrade the performance significantly?

author: Codemonkey
author_rank: Regular Contributor
timestamp: February 01, 2015, 09:36:17 am
content: They're probably specifying a 4 layer board so that the thickness between the top copper layer and the ground plane on the layer below is very little (<1mm). The thickness of the board between top and gnd plane defines the trace width required to get a 50 ohm impedance. You really need to read up on this stuff a bit more to get it to work. Either copy their reference design EXACTLY (including positions and orientations of any inductors etc in the RF path), or get a contractor in who knows this stuff. A poor match on the RF stuff could result in your product failing FCC/CE whatever approvals.

author: Howardlong
author_rank: Super Contributor
timestamp: February 01, 2015, 10:14:55 am
content: Quote from: Silenus on February 01, 2015, 09:13:11 amLooking at the RN171 datasheet, there are three antenna examples given. It also states that the RF port is 50 ohms, so any 50 ohm solution should work.For ballpark 1.6mm FR4 with an Er of, say, 4.2 at 2.4GHz, a 50 ohm microstrip transmission line is about 3.1mm wide. Due to the close pin spacing, physically this is not going to work right off the bat, which is why typically multi layer is used so the distance between the ground plane and the transmission line is much less, leading to more reasonable track widths. It'll probably work well enough though. You can of course reduce the width by using a thinner substrate, but with a loss of physical board rigidity. 1mm substrate is about 1.9mm track at 50 phms, 0.4mm is about 0.75mm width for example.FR4 is a bit lossy up in the GHz, so keep the transmission line short, and avoid turns and kinks which themselves can add impedance bumps if not done properly.I am not necessarily recommending that you do do it this way, but if from an engineering cost perspective if you need to keep to 2 layer it will work. You should also check with your board house what the Er is at 2.4GHz.

author: Silenus
author_rank: Contributor
timestamp: February 01, 2015, 10:43:37 am
content: Thank you all for the replies. A few more questions: what if you connect the end of your antenna directly to the pin of the wifi module (in other words can you remove the transmission trace altogether)? Also could you bring a top layer ground plane close in proximity to the transmission trace on the same layer enough to reduce the thickness of the transmission trace? or does the distance to ground only work with the ground directly below it?

author: KJDS
author_rank: Super Contributor
timestamp: February 01, 2015, 10:50:24 am
content: Quote from: Silenus on February 01, 2015, 10:43:37 amThat then becomes grounded coplaner waveguide.Appcad is a readily available bit of freeware from agilent that will calculate line widths for given impedances.

author: Howardlong
author_rank: Super Contributor
timestamp: February 01, 2015, 11:10:45 am
content: Connecting the antenna directly to the pin would work, for example a 1/4 wavelength (30mm including end effect adjustment) of wire would match reasonably well, but resist the temptation to have anything other than a 1/4 wavelength of wire mounted perpendicularly, either directly up or directly away, keeping it in free-air