Chip antenna mounting considerations

Question

I'm using this chip antenna with a 868MHz radio (RFM12B): http://www.johansontechnology.com/datasheets/antennas/0868AT43A0020.pdf

According to the datasheet's mounting considerations there's a trace that's supposed to go out from the antenna. What is the reason for this? Due to tight space i'd have to drop this with a via to the bottom of the board and do this there, is this ok? I guess the via will have quite a big impact on the RF signals. If not, can i do something "similar" with a same length but slightly different shape? Or is it better to leave it out entirely? Are there other ways of doing this to achieve a "decent compromise"?

Related to this the feed line should have 50 ohm impedance. According to this: http://www.eeweb.com/toolbox/microstrip-impedance I've calculated the trace width to be about 115 mil. This seems very big.. I'm using a regular 1.6 mm FR4 board with 1 oz copper. Am I missing something?

Also I'm assuming this should definitely not have sharp corners so the trace is rounded (cannot be perfectly straight as in the datasheet), right?

Answer 1

It's probably a tuning loop or another structure that makes the small chip antenna act "slower" than it really is (i.e. forces it to operate in the 868MHz mode rather than a faster mode). Dropping it will almost certainly compromise it's operation but the only way to measure by how much is with a VNA. Unfortunately this is the common trade-off; lower frequencies make antennas with larger physical features.

Re: 50 Ohm trace and 115mil thickness. Yes, this is correct for a 2 layer 1.6mm FR4 board. And yes, its very wide. I use a 4-layer board on my M12. Typically the thickness between layers 1-2 and 3-4 are close together (approx. 8.26 mil) while 2-3 are far apart (maybe 40 mil). Check the stackup with your pcb manufacture. Anyway, with a smaller thickness you should start to see more reasonable 50 Ohm trace widths.

Answer 2

It is a loading element that affects the matching and resonance at the operating frequency as Mariano Alvira suggests.

You will get the manufacturer specified performance with the commended PCB material, stackup, and layout design, however that doesn't mean that there aren't "equivalent" or better options that could involve different choices in the PCB materials, stackup, and geometric antenna loading / layout. They couldn't enumerate every possible layout, so they suggested something that gives reasonably optimum, easily reproducible results as a design guide.

If you want to change the loading trace's routing shape somewhat that's probably going to be workable. If you do change the design from their reference design, you should characterize the affect upon the S-parameters / antenna return loss vs. frequency over your bands of interest and possibly make minor adjustments to the feed line side matching network to compensate for changes due to the antenna loading side element.

Actually you should do such characterization on your prototype PCB anyway even if you're following the antenna manufacturer's recommended layout since even variations in passive (L,C,R) component parasitics due to different component manufacturers' designs can affect the matching.

If you're not using a well impedance controlled PCB material and manufacturing stackup control process that can change the impedance double digit percentage as well. Even just changing the relative position of the antenna on the PCB or the affect of other factors due to the enclosure, PCB shape, other components on the PCB will alter the antenna tuning and matching performance. So don't be afraid to characterize changes to the antenna design, but realize that you should plan for using a VNA to evaluate and optimize any changes you do make unless you have very loose performance tolerances as to antenna performance and repeatability vs. process changes.

I would avoid putting a via in the antenna loading line or feed line, however, unless such is suggested by the antenna / SOC application engineers, and you should try to engineer the line impedances to be 50 ohms as they suggest. Saturn PCB has a nice calculator that handles trace impedances and so forth for simple stackups, at least approximately.

Avoidance of sharp pcb trace bend corners aren't that important at 868 MHz and FR4 material, so I'd follow the suggested layout (right angles and all) to sub-millimeter precision if possible as a starting point. If you want to characterize antenna performance with different physical PCB dimensions and layouts you might want to fabricate a panel full of test boards with nothing but a SMA connector, the antenna, the feed / matching / loading circuits, and a similar PCB shape / ground plane / keep-out zone structure as might be used in your product.

You can compare the RF performance of the depanelized test boards and even make small changes to the boards with alternative components, copper strip, a utility knife, etc. to try out variations and optimize the overall design. You can always ask their application engineers about some qualitative advice as to the relative risk of doing some kind of change or other.

If you can get access to something like SONNET or Microwave Office or similar you might even be able to model the PCB and antenna combination to look at the affect of different layout and PCB geometric changes but lacking a very good near field / feed / PCB parasitic model of the antenna itself any such models will only be generally qualitative and not totally predictive of all real world physics.

Just trying an characterizing the performance with a test board is often the best way, though doing some kind of monte carlo analysis around multiple varying tolerance related parameters can be fruitful to see the envelope of overall performance you might get in production.