- Mon Oct 13, 2014 3:56 pm
#1579
I don't consider myself as an RF guru, so take my advice with caution.
Unlike some other PCB artwork, RF PCB design is not just a matter of copying a known-to-work existing design: there are so many parameters to take into account, you are likely to underestimate some and get a non-working or far from optimal antenna this way.
For best performance, impedance-controlled PCB are required, please note that the ones from dirtypcbs.com have a Z0 impedance tolerance of +/- 15%! From experience, the kind of cheap material used will give you an Er ranging from 4.0 up to 4.6... You now understand why computing an accurate impedance in these conditions is just pure fantasy
Here are some interesting links on ceramic antennas:
http://www.johansontechnology.com/techn ... 80211.htmlhttp://electronics.stackexchange.com/qu ... iderationsAnd here is one on PCB trace antennas:
http://colinkarpfinger.com/blog/2010/th ... na-design/As you said in your OP, you will need a 50 ohms matched impedance feed line, and even with the tolerances stated above, approaching the correct value should still be your main goal. What you are looking for is called a "coated coplanar waveguide with ground 1B" configuration. "Coated" because of the covering solder mask, "coplanar waveguide" because you will have your RF trace on the same plane as ground all around it, and "ground 1B" because of the underlying single ground plane below it.
There are some more or less accurate tools to compute the impedance of such a passive circuit; AppCad (
http://www.hp.woodshot.com/), the Saturn PCB Toolkit (
http://www.saturnpcb.com/pcb_toolkit.htm) is a good free choice, but the definite tool is the expensive Si9000 field solver from Polar Instruments (
http://www.polarinstruments.com/products/si/Si9000.html) which is used by most Chinese RF PCB manufacturers for good reasons...
Of course, I don't have this software, but here is a screen capture from a previous 0.8 mm thickness design that I received from my Chinese PCB manufacturer:
0.8mm 50 ohms CWG1B.PNG
Basically, the PCB manufacturing limits are first considered (mainly the 6 mils min. trace width and clearance), along with Er +/- tolerance, substrate thickness, trace thickness, coating thickness above trace and substrate, and coating dielectric, with the trace profile being considered as trapezoidal due to etching...
In this case, it resulted in a 25 mils RF trace width with 6 mils ground separation around it, but YMMV.
FYI, here are the results I get with my Saturn PCB toolkit for the same parameters:
0.8mm 50 ohms CWG1B Saturn.PNG
The actual 50 ohms value is obtained for something really close to 25 mils, not 34 mils... But again, given the +/- 15% tolerance on Z0...
You do not have the required permissions to view the files attached to this post.
but soon 
