Transmition Line Design

[Elektrofreak]

Hello at all,

i am designing a bluetooth audio device with the TI's CC2560 and want to connect the bluetooth-antenna via an sma-connector. I already had kind of HF-stuff at my university but didn't use it until now in practical applications.

I have calculatet a W/d of 1.787 (where W is the trace width and d is the thickness of the board) for FR4 and it seems to be comprehensible from the plots but the trace is then much bigger than the trace in the routing guidelines of the chip (i expect because i only have 2 layers and they use 4 layers).

The antenna is only ~ 6mm away from the chip pin including a bandpass filter. I have to route the trace between two other chip pins so i am wondering if it makes sense to do as an example first a 6 mil trace to get from the chip to the bandpass filter and then continue with a 54.7 mil trace (calculated width using a 0.8mm thick board). For me it seems very strange...

I have added an image of the actual board to show what i mean 

Could you please bring me some enlightenment? 


Thanks in advance
Elektrofreak

[cthree]

Take a look at the reference designs ti publishes. They have very specific instructions and designs for the front end.

http://www.ti.com/lit/an/swra420/swra420.pdf

[lgbeno]

I had the same problem with a cc2500 board that I built at 2 layer, 0.8mm.  I used a  ceramic balun from Johanson for the front end, routed from chip to balun with very short, 8mil traces and then that huge 50 some mil trace to the antenna.  All I can say is that it works, never really got an opportunity to make any other measurements due to lack of equipment.

I would say that your assumptions are correct.  Obviously a 4 layer board with a thinner dielectric would be better but I'm sure you are like me and trying to do it on a low budget.  The only other thing that I could suggest is skipping the board mount connector and making a footprint to solder a coax pigtail directly to your board.  Semi rigid coax works great for this.

[WarSim]

You can't exit the way you did in you layout unless the two pins on either side are guards. 
Remember the transmission line self radiant requirements. 
Also the next layer has to be a neutral or you calculations won't work. 

Unless you can accept over 10db loss that is. 

At first the pin assignment seemed very odd. 
But in the link supplied I saw their intent, to maintain pin count. 

[TommyGunn]

This should not cause too much of a problem. As a rule of thumb you only really need to start worrying about your creating a matched transmission line for distances over 1/10 of the wavelength of your signal. Since you are using Bluetooth (2.4Ghz) and fr 4 the wavelength is about 6.25cm and so 6mm is close enough for the radiation of your transmission line to be negligible.

I would keep the design exactly the way you have it.

It would work fine with or without the 57mil line after the filter. But it doesn't hurt to have it.