On your design, how long is the trace from chip to antenna? If the trace to the antenna is less than roughly a tenth of the wavelength (in this instance, the trace would have to be less than 1.25 cm), if it not considered a transmission line, and its impedance is not a factor. Depending on your answer, it seems likely that your antenna isn't properly matched to 50 ohms. In order to properly match your antenna, as you pointed out yourself, you have to take into account a number of external factors, and it is imperative to place footprints for this match, usually in the form of a pi network. Then, you have to use a VNA to match the antenna. There are too many factors that impact an antenna match to think that it's possible to just plug in values for the filter based on another design. Personally, I wouldn't copy the design of these modules. I have not been impressed with their performance.

@martin thanks for your answer. I measured the trace length from antenna to chip and it comes to some 3.1 cm total. There is some components in between (that I believe make up the pi network) and those are connected by traces as well, so I just added them all up. Based on your comments, you think if I can get the antenna withing the 1.25 cm range of the chip I can mitigate the impedance factor? I understand there would still be other factors involved after that, but unfortunately I do not have access to an analyzer device that would allow me to tune it further :/ I'm just trying to get it good enough, and these off the shelf ones have worked for me before at least.

@b.kruijer, When it comes to doing the PCB, JLCPCBs information about controlled impedances might be helpful: [https://jlcpcb.com/capabilities/Capabilities](https://jlcpcb.com/capabilities/Capabilities)

Bob, if you can shorten the trace, it's one less factor you have to deal with, so I would definitely do that (I do on my RF boards!). In terms of it being good enough, that is really hard to say. In my experience, tuning has been 100% necessary to get good performance. Trying to guess the right LC values for your filter is basically impossible. You might be able to borrow VNA time at a university, or you could do like I did and buy a "good enough" VNA if you're willing to spend a few hundred dollars. I got this guy: [https://xaxaxa-dev.com/xavna.cppsp](https://xaxaxa-dev.com/xavna.cppsp)

Oh, another thing I'd try: don't populate the filtering network. Random values are most likely making the problem worse.

I am trying to make a simple board with a cc2640r2fhbr and a PCB antenna\. The chip has RF\_P and RF\_N\. Is there anyway I can beg\, borrow\, or buy a circuit design and pcb layout that will do the antenna and the pi network? From reading above, it seems that the pi network values need to be determined after the pcb has been built. But isn't this repeatable such that I should be able to use an existing design and just place the cc2640 to the antenna/network layout without adding any trace? The antenna/network combo would specify the board thickness and such. I searched, but I don't see anything like that. I need maybe 1 meter of distance between my bluetooth devices. I don't know squat about these analog circuits and would love to avoid having to learn all that voodoo.

@johntaves, Please have a look through this topic: [https://easyeda.com/forum/topic/Help-needed-with-NRF24-reference-design-fd56c235282a43bbb5dbd2a30c9ea581](https://easyeda.com/forum/topic/Help-needed-with-NRF24-reference-design-fd56c235282a43bbb5dbd2a30c9ea581) which is a more detailed follow-up of this one.

I don't think you can get a good match without taking measurements (a nanoVNA is super cheap!), but your best bet is to exactly follow TI's reference design otherwise: [LAUNCHXL\-CC2640R2 Development kit \| TI\.com](https://www.ti.com/tool/LAUNCHXL-CC2640R2)

Thanks, Martin and Andy. I totally appreciate the help. The topic Andy referred me to seems to indicate it is not easy to duplicate the reference design. I have the 2640 dev kit on the way to me and will use it to prototype. Below is the circuit and pcb for the antenna. TI provided files in some format that I did not find possible to import into easyeda. So, I am not sure how to copy that design. Can you answer these questions to help me understand? 1) This is a double ended circuit, which I read should provide better performance, but will be less forgiving if I have the wrong values. So maybe I should go for a single ended solution? 2) What is being matched to what? Since this sample circuit has 2 different antennas, I conclude that I can copy the circuit from RF_P/N to C24, because that is the same for 2 different antennas. I conclude that the circuit is matching to the chip. It seems like I would pick some C58 to solder in if I was going to use P11. However, A1 is marked as DNM, but there it is in the pcb, and C15 seems to be a part I would pick and solder in, but I don't see it in the pcb and how would I know what to pick? TI made the pcb antenna (A1), right? I would think that they would have some way to disconnect A1, to use P11. Maybe I just destroy C51, if I want to use P11? Oh, and then they have C12 DNM, what's that? Sorry, my head is spinning to understand this circuit and what I would copy. 3) Why not use a chip antenna? Wouldn't that be fewer variables for me to comprehend? The pcb antenna seems to be a bitch with trace width, depth, and coating, all of which I have generally not paid much attention to because I have been dealing with digital circuits. Maybe I should just use one of the pcb antennas in the easyeda library? 

@johntaves It _might_ just be your lucky day today. I had a look at: [https://www.ti.com/tool/LAUNCHXL-CC2640R2](https://www.ti.com/tool/LAUNCHXL-CC2640R2)<br> <br> and found: LAUNCHXL\-CC2640R2\_1\_0\_Layout\.pdf in: [https://www.ti.com/lit/zip/swrc335](https://www.ti.com/lit/zip/swrc335)<br> <br> The antenna in this looks very much like the antenna originally created by a user and then modified by mein this bug report: [https://easyeda.com/forum/topic/Inconsistent-connection-to-pad-on-single-numbered-multi-padded-footprint-40071cd5cf5a478cac7be7d4334a02a1](https://easyeda.com/forum/topic/Inconsistent-connection-to-pad-on-single-numbered-multi-padded-footprint-40071cd5cf5a478cac7be7d4334a02a1)<br> <br> The reason I converted the footprint into something _with the same dimensions as the user footprint_ was so that it meets the requirements set out in: [https://easyeda.com/forum/topic/How-to-avoid-DRC-errors-when-connecting-to-PCB-Footprints-a-k-a-PCB-Libs-90bf944fe3644b21a7d27a9e9d8df8d6](https://easyeda.com/forum/topic/How-to-avoid-DRC-errors-when-connecting-to-PCB-Footprints-a-k-a-PCB-Libs-90bf944fe3644b21a7d27a9e9d8df8d6)<br> <br> That modified footprint is this one in the Library:  I have no idea how accurate the dimensions of the user antenna above were to the TI design but my edited version has the same dimensions as the user design. If you open the Gerber files in the zip from TI, you can make some measurements of the antenna dimensions and check the EasyEDA footprint above against them. Note however that the any PCB antenna design is only going to work as in the original reference design, if it is not only: 1. the same dimensions as the original but also that: 2. it is constructed on the same PCB substrate material (in terms of dielectric constant and loss tangent) and that: 3. the PCB has the same stackup and vertical dimensions as the reference design. You will therefore need to check these parameters against the information given in: [https://jlcpcb.com/capabilities/Capabilities](https://jlcpcb.com/capabilities/Capabilities)<br> <br> and: [https://cart.jlcpcb.com/impedance](https://cart.jlcpcb.com/impedance?_ga=2.58254058.1981965559.1618510752-1481376643.1615813773)<br> <br>

"Why not use a chip antenna? " * If this is a small quantity project than that might be your best solution but you still need to match the chip to the trace and then the trace to the antenna (unless the trace is less than about 0.1 of a wavelength in length in which case you need to match the chio to the antenna). Note that wavelength shorter on the PCB because wavelength = (propagation velocity)/frequency and the propagation velocity is slower on a board than in free space! Note also that your design is based on microstrip and that propagation velocity of microstrip is reduced by a mixture of the dielectric constant of the substrate under the trace (FR4 in this case) and the air above the trace. There are formulas for this. For RF designs tracks and particularly antennas are left as exposed metal (i.e. no solder resist over them) and so, to maintain a controlled exposed surface, the PCB finish is ENIG and not HASL or Pb-free-HASL. * If this is to be a commercial product then a chip antenna may be an expensive solution and you probably need to be enlisting the services of someone like: [https://radtenna.com/about](https://radtenna.com/about)

Again, thanks for the answers. This is a small qty project, so I am thinking the chip antenna might be easier to deal with than using your antenna, and smaller too. 2.45Ghz is 122mm so, I should have no problem placing a chip antenna within 12mm of the chip. However I'm totally confused about how to match chip to antenna. Is there a solution somewhere between radtenna and me doing this? Can I make my schematic and pcb editable by you, have you plop down some circuit and pcb layout, and I paypal you some $? If the first iteration of the board isn't good enough, I am OK getting the nanoVNA as Martin suggested and providing some measurements from it and paying for adjustments. My problem is that I have way too much to learn to have a chance at making that first version that would be measured to make the final. And of course, it would be really cool if a first version would work. I need to transmit between an RV floor, which is a layer of metal and an inch of foam and some wood. All the cells are within say 2 meters of the receiver (an ESP32 VROOM, but if this works, I would probably redesign that to be another cc2640). I am making a lithium battery management system. I have a wired version working nicely in my RV. I am sick of the wires and thought it would be very cool to make this wireless. So this is a hobby, but still, if this works nicely I think I will open source the design. I have 8 cells, so I just need 8 of these. (Below is a failure, where I chose the cc2541 which requires me to purchase a software development environment, and I had no clue of the difficulties with respect to the antenna, so the odds that this would have worked seems low.) 

@johntaves I meant "transmit through an RV floor"

@johntaves "I need to transmit through an RV floor, which is a layer of metal and..." Stop right there. Radio does not pass through metal. End of. That's why screened rooms are made from sheet or mesh metal.

Besides transmission issues through the floor, and antenna matching, your next challenge is learning the TI SimpleLink stack. As a hobby, all of this amounts to months of work. But if I may, I have a project based on the TI stack for long range (CC13X2), that is built as a pluggable uController/Radio stack here on EasyEDA. The antenna is matched to the board (in free air, so can benefit from re-tuning when in a system, but will work nonetheless). This is a project that is used daily for a number of devices, and tested to ~600 meters LOS (ran out of space, but way good enough for my purposes!). See here: [CC1312 Breakout - EasyEDA](https://easyeda.com/martin/cc1352-breakout_copy)<br> <br> Happy to discuss/lend a hand offline.

@martin, I thought you might have something up your sleeve... :)

@andyfierman: Heh! Here to help!

Oh, and if you MUST use Bluetooth at the other end, I also have a CC1352 version (long range + BT) here: [CC1352 Breakout - EasyEDA](https://easyeda.com/martin/cc1352-breakout)<br> <br> :-)

@andyfierman "Radio does not pass through metal." OK, but I just put my phone where I prefer my controller to be and then stuck my head with bluetooth headphones where the batteries are an didn't miss a tune. And it doesn't really matter because I can mount my controller with the batteries and run a wifi antenna up to the interior. So, I suspect a reasonable performance will work and the backup is fine too. I doubt that the failure to go through metal barriers will bother too many, if I open sourced it. So, I still want to proceed. "TI SimpleLink stack. As a hobby, all of this amounts to months of work." I am a pro software developer. If this takes me more than a few days, I will be very surprised, and very pissed off. If that stack requires months to use, TI needs me to make a better stack. I am not going to bet my life on it, but I am not deterred in the least. @martin, I don't need Bluetooth. I tried to get the cost using the "order at lcsc" for both of your designs, but most of the components were out of stock or obsolete. 1) I assume I can modify the PCB, removing the unused connector, adding an LED and plug for a thermistor, and changing the layout to make it the cool bolt on thing shown above, right? 2) What development environment does the cc13x2 use? Is it the free TI thing (I can't remember the name)? 3) I don't see either cc13x2 as a jlcpcb part. I am confused? "Happy to discuss/lend a hand offline.", unless Andy responds with some better thoughts, I am thinking I should contact Martin and have him help finish the radio portion of the cc2640 design I have started. I picked the cc2640 cause jlcpcb has them in stock and I can use the free TI dev environment.

"unless Andy responds with some better thoughts, I am thinking I should contact Martin" Martin is better set up to help you out on the antenna and if necessary, software on this one.

John, 1) The point of my project is to add a mating connector to your specialized board, and not modify the radio module at all. For example, here's one of my specialized boards, which mates with the radio board: [Temp logger for CC13X2 - EasyEDA](https://easyeda.com/martin/Temp_logger-JFDZywSQc)<br> <br> Changing the layout would mean having to re-match the antenna (no point using my project at all, then). If you DO decide to go ahead with your board, I suggest replacing the front-end passives with a ready-made balun (Johanson 2450BM14G0011); this will greatly simplify your design. Also, I'd take a close look at your pi network layout and location, and as stated before, you should get a VNA and semi-rigid SMA cable. I assume you are able to solder 0402 components. 2) CC13X2 refers to the broader family (ie, CC1312 or CC1352). The suggested IDE is Code Composer Studio. TI has a SimpleLink SDK variant for all of these chips, so code of largely portable. In terms of time spent, there are a lot of concepts to master if you want to gain a deep understanding, so it doesn't have much to do with your coding abilities. If you just want to modify provided examples, you can probably do so fairly easily. And last, I always order from DigiKey, as some parts have not been available at LCSC (TI chips, the Johanson balun, an in-spec crystal, RF-rated passives, etc).