Does the CC3200 have an internal antenna? Can it be used without attaching an external antenna?
This thread has been locked.
If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.
Does the CC3200 have an internal antenna? Can it be used without attaching an external antenna?
Since most of us are currently using the Launchpad I wanted to be sure to clarify 1 thing. While the MCU itself does not have an integrated antenna the Launchpad provides one. So when using the Launchpad you do not need to connect an external (to the Launchpad) antenna.
If you design your own board be sure to pay attention to the specifications regarding the antenna. They are very specific to ensure optimal performance.
I read in the Launch Pad design notes that the demo uses the higher price recommend cost Taiyo Yuden (Edge Mount Antenna). But we see that it also recommend the lower cost Walsim RFANT5220110A2T.
There is some design application details details about the Taiyo Yuden (Edge Mount Antenna) used in the demo (Gerbers and matching components etc...).
The Walsim one will work for us, however there is less design info about it. I find a small amount in the Walsim data sheet, which may be enough, I assume there is no impedance matching required. Also it is not edge mounted as TI design guidelines suggests???
1) Do you know how to impedance match the Walsim one (if any)? It looks like they do not use any? Do I use the recommended demo impedance matching for the Taiyo Yuden one. Or is the Impedance match for the WiFi IC not the Antenna (i.e. the antenna is inherently 50 Ohms)?
2) Does it need any matching changes if I change the PCB thickness different 1.6mm PCB or 1mm PCB thickness (I understand the transmission lines change)? The demo is for 1mm PCB.
3) Does this need mounting in the corner as mentioned by TI design notes (The Walsim Data sheet shows non corner mount)? If so, what horizontal distance should I have (above diagram) before we can begin ground plane again? If not what distance before is restored again?
4) The Antenna design is important for two reasons (RF compliance – Bandwidth and filter matching, and Optimum radiation distance – Range). Do you know how important this is in relation to this minimum amount of layout info we have?
5) What is your recommendation regarding this Antenna? How much risk am I taking using the Walsim one?
Thanks, This was helpful. These DN and AN docs help for a good background understanding. However I was hoping for some more specific designs regarding the alternate antenna mentioned in the CC3200 design guide. It is a much lower cost antenna (we are not limited by space). But clearly there are no reference designs available for the amateur (like me).
I have had a RF designer friend answer most of my questions. I will share it here for others to ponder:
----------------
The AH316M antenna relies heavily on the PCB plane geometry as it utilizes the geometry to form the radiating element. A matching network is invariably required to achieve a reasonable return loss.
The RFANT522 device on the other hand is a radiating antenna. The return loss plot suggests up to 22dB return loss which is pretty good for a chip antenna, provided you follow the keep out guidelines. Impedance matching with the WALSIN device (RFANT522) should not be necessary provided the trace widths are impedance defined for your substrate dielectric and thickness. I prefer to fit a PI pad with 0R pass through just in case there is room for improvement. The CC3200 output impedance doesn't appear to be specified in the data sheet. Many integrated transceivers have output impedances which are not 50R so incorporation of a matching network is usually required. The layout guidelines indicate a 50R strip from the transceiver through to the filter so I am leaning towards the CC3200 output impedance being 50R.
So in response to your questions,
1) The Walsin will most likely not require impedance matching if the plane relief is observed, but integration of a PI match is a good idea for optimization. The impedance match of the Demo AH316M antenna will not be suitable.
2) Provided that the line impedances are maintained, then the traces may be scaled accordingly. Be aware however that if traces are reduced in width then etching error and etch factor will affect the tolerance of the impedance.
3) The antenna does not need to be mounted in the corner. Note that the corner mounting advice is specific to the AH316M device specified in the demonstration assembly. The proposed Walsin antenna may be mounted along the edge, corner or within the PCB area provided the keepout areas are observed
4) The chip antennas are electrically small so they will be fairly uniform radiators. Filter matching should be fairly trivial if the filter is 50R. Further harmonic suppression is achieved by the frequency response of the antenna however an intermediate PI network can also be used for additional filtering if required. All the layout information required appears to be at hand. Apart from the specifics regarding the AH316M matching network, all geometries are fairly clearly defined in the data sheets. Risk assessments regarding bandwidth, emissions compliance and optimum range performance all really depend on your specification and what the functional performance targets are. There will always be a compromise. Both of these antennas appear to have the necessary bandwidth requirements for 802.11 functionality.
5) I don't have any reservations against using the Walsin antenna, however it depends on your design objectives. If price point is the objective, then the lowest cost components are a good idea. If PCB real-estate minimisation if the objective, then the AH316M may be a better option. Just remember that any antenna can be matched provided the provision to match it is designed in. The Walsin antenna appears to be a 50R off the shelf device so I believe it would be easier to work with.
--------------
In my re-cad (PCB Version 2), I removed the Pi network (I had a 0R0 resistor). It works just as good (or better).
I also used the more common RF filter (same footprint as the TI recommended one) Taiyo Yuden: FI212B245025-T . It is available Mouser (and some small stock DigiKey) for your prototypes.
Just using the antenna layout on the Walsim RFANT5220110A2T website.
50 Ohm Microstrip, High TG PCB (for RF impedance control). 1.6mm thick PCB, 4 Layer, with GND plane on layer 2 (just below the the top layer Microstrip). Microstrip is 0.495mm wide. Top core is 0.3099mm.
CC3200 (Pin31) => FI212B245025-T => RFANT5220110A2T (antenna layout guidelines).
Layout (pink thin lines are keep out).
PCB Manufacturer's Calculations (Ask your PCB manufacturer for their recommendations for 50 Ohm Microstrip:
My layer stack:
Mani,
These two distances do not matter at all. They are all 50 ohm tracks that can be any reasonable length. Best to keep them as sort as practical, because if there is variations in the PCB track impedance, then the change of impedance is minimized. However I am not an RF expert, I just followed the antenna design guidelines on the Walsin website (as best as possible).
The actual lengths are (even though they are not an important factor):
Chip pad center to filter pad center = 2.075mm
Filter pad center to antenna pad center = 4.975mm
Also the filter I ended up using was a Taiyo Yuden: FI212B245025-T it seemed more available at the time (see Mouser).
Ian
Hi Marni,
I am no expert in this area. It looks similar to my layout. Except you need to remove the GND fill edges/frame (top and right) around the antenna. This is not adhering to the clearance rules for the antenna. Picture it as the antenna needs to radiate out of this area. The antenna only works with GND on one side (bottom). It is the same requirement for any nearby metal (chassis etc...) around the antenna (above and below etc...).
I can't add any more, cause I an not an RF designer.
Hope it works...
Ian