You need to use EasyEDA editor to create some projects before publishing
Ceramic Chip Antenna Advice
36 3
mark.c.beeman 1 week ago
Hi all: Am trying to learn more about ceramic chip antennas. I found this webpage: [Chip Antenna Layout for 802.11 Applications - Johanson Technology]( have seen a lot of datasheets with drawings similar to these. Before I even get to the point of trying to design a circuit, impedance match, design pi filter, etc. I have some basic questions about these datasheets. For example, I see vias which makes me think there is a dedicated Ground layer, but there is also the large "orange" layer in the figures which is labeled "Ground". So is this saying if I have a dedicated ground layer that I should also have a solid "Ground" region on my top (signal) layer and connect them with vias? I am assuming that large orange area labeled "ground" is on the top layer because the microstripline and pads for the antenna are also orange. Or maybe this is just for a 2 layer board? Also, what is the grey area around the microstripline? Any help is appreciated.
andyfierman 1 week ago
In the Johanson pages, the orange layer is the top layer. It also assumes that there is a bottom layer ground plane of the same shape (but with no tracks breaking it up) and that it is via-stitched to the top layer.  A bottom ground plane layer is required because the tracks on the top layer are microstrip: [](<br> <br> Where it says "No ground plane", this applies to all layers. There may also be inner layers, possibly with stripline structures ([]( as well as other non-RF tracks but they are ignored for the purposes of this particular applications note. Please be aware that designing anything with your own PCB design or even an off the shelf ceramic antenna is not a trivial exercise. You also need to be aware of any RF Approvals and Compliance requirements that may apply in your - and any end - location and application. For info: have a look at this topic and the stuff it links to: [](
andyfierman 1 week ago
The the grey area around the microstripline a way to show that you are looking through the PCB core material and is showing that there is a ground plane on the bottom layer.
andyfierman 1 week ago
" this saying if I have a dedicated ground layer that I should also have a solid "Ground" region on my top (signal) layer and connect them with vias?" Yes. The main reason is to screen any signals that may be sandwiched between the two ground layers from the RF being transmitted from the antenna. The top ground plane os a little less important if it's a receive only circuit but even so it is good practice to reduce supply and ground plane impedances for decoupling and crosstalk and to minimise interference to your receive signal from your own PCB. If you venture into coplanar waveguide layouts then you may get away with only one ground plane on the same layer as the feeder line but that is a much more difficult design to achive and manufacture reliably because it requires very tight tolerances and even tighter control of the PCB subtrate parameters than for microstrip and stripline. It depends somewhat on your operating frequency but once you have a design that works satisfactorily (however you decide to define that!) you should also be wary of changing the PCB material or board manufacturer since the PCB material spec may change and hence your matching gets shifted.
Login or Register to add a comment
如果需要转移工程请在个人中心 - 工程 - 工程高级设置 - 下载工程,下载后在 打开保存即可。
有问题联系QQ 3001956291 不再提醒
svg-battery svg-battery-wifi svg-books svg-more svg-paste svg-pencil svg-plant svg-ruler svg-share svg-user svg-logo-cn svg-double-arrow

Cookie Notice

Our website uses essential cookies to help us ensure that it is working as expected, and uses optional analytics cookies to offer you a better browsing experience. To find out more, read our Cookie Notice