Stripline, PCB waveguides, etc - online calculators...

[westfw]

So I've been looking at TI's CC3000 WiFi module.
AFAICT. it's only critical RF connection is the 2.4GHz antenna output.
TI has several app notes that describe the desirable characteristics of the PCB design for that output, including a bunch of parameters that supposedly yield a track with 50ohm Z0.

There are a bunch of online calculators that also claim to show Z0 for a particular trace configuration.

I can't get them to match !  If I plug in the recommended numbers, I'm not getting anything particularly close to 50ohms...
For instance, SWRU331 The CC3000 BoosterPack Module has a nice 2-layer design with 20mil trace, 5mil separate to ground, and 52.2mil dielectric thickness (!).  I get closer to 60 ohms using http://chemandy.com/calculators/coplanar-waveguide-with-ground-calculator.htm

Then there's the SWRU326 CC3000 Eval Board, which is four layers 14.3mil trace, 10mil sep, 12mil thickness, which I get to be something like 62 ohms...

I'd like to make an equivalent design for a two-layer board with a more standard thickness.  But if I can't duplicate the current calculations, I'm a bit lost...

Does anyone have ideas WTF is going on?  Or have a particular online stripline/waveguide/etc calculator that they trust and have proven to work?

[Neganur]

Judging by their return loss measurement from the antenna and matching circuit, their specific configuration has a VSWR of 1.10:1 at 2.45 GHz and VSWR of 1.90:1 at 2.5 GHz and 2.405 GHz.

Those trace impedance calculators are only approximations and even 60 ohms isn't half bad (VSWR of 1.2:1 is reasonably good). You would have to do a lot of re-spins of your board and measure the trace with a network analyser if you want it to be precise. It's impractical though since you're really much more interested in the system as a whole (antenna+matching circuit+trace) and the trace will be in the ballpark of 45...55 Ohms. You can see the extra micro-FL connector (second picture, red circle) next to the CC33000 which they used to find the values for their matching circuit.

The manual for the antenna (AT8010) shows some example layouts but always points out that the actual trace should be designed to match depending on PCB material and thickness.

Side notes:
-The document from TI may contain errors. The component values for the matching circuit in the schematic is different from matching circuit on page 10 of TI's document.
-They list the impedance of the trace as 47.57 Ohms and I wonder if the guy who wrote that value took it from the smith chart for the whole matching circuit at 2.45 GHz (about 45 Ohm).
-The solder mask may have an impact on the impedance.

[enz]

Don't forget that the dielectric constant (epsilon-r) of the PCB material can vary quite a lot between different brands, charges, etc.
The assumption that it is always the same leads often to wrong results. But of course, until you get valid data from the pcb manufacturer, or from own measurements, you only can assume that value.
But be aware of this uncertainty. In "swru326.pdf" it seems that they use a value of 4.3 for epsilon-r.

Martin

[westfw]

My impression is that "FR4" is pretty consistent stuff.

It wasn't clear whether they had designed the PCB for 50ohm impedance, or PCB+matching circuit+Antenna to be 50 ohms. :-(

I guess that for "short" trace lengths (compared to wavelength), it is less relevant?  2.4GHz is about 5 inches, though, and people certainly seem to worry at well below that length...

[Jay_Diddy_B]

Hi,
Another consideration is the etching process. You can assume the traces widths will shrink and the gaps will increase when the board is etched.

Jay_Diddy_B

[westfw]

Yeah, there are lots of things that can go wrong.  But I ought to be able to get calculated results that come pretty close to matching, given the same inputs.  I don't think "20+% different" is very close!

[Russ.Dill@gmail.com]

Er varies by frequency, 370HR

100MHz = 4.24
1GHz = 4.17
2GHz = 4.04
5GHz = 3.92

Er varies by chosen FR4 material, FR408@1GHz Er is 3.66

Er is affected by soldermask

Impedance is affected by nearby traces/groundplanes

Some board designers take into account know etchback when choosing a trace width

And of course, many impedance calculators provides estimates, whose error increases the further you get from the ideal range for that estimation.

2D simulators are better, but different simulators will still give you different answers

[mamalala]

For "simple" stuff like having a trace to connect to an antenna, i think it's not all that important to get a SWR of 1.0. Just look at what a given SWR translates into regarding losses:

http://www.firestik.com/Tech_Docs/SWRLOSS.htm

Combine that with the fact that you need 4 times the output power to increase the received signal strength by one S step (6 dB), and you get the idea.

This is not meant to say that one should not care at all about the layout. But there are many, many other factors in the whole system/signal-path that have a far bigger impact than a difference between SWR 1.0 or 1.5, like placement and positioning of the antenna, etc.

Greetings,

Chris

[thmjpr]

So its given that conductor backed coplanar waveguide includes appropriate use of via's. Do they need to be factored into the calculator equations at all?

Vias bracket the signals to connect the adjacent GND area on the surface to the GND plane underneath the signal traces. The exact placement of the vias is not critical, but care is exercised to keep them close to the edge of the GND plane. Their lengthwise spacing is anywhere from 1/10th to 1/4 of the wavelength of the signal they bracket.

edit: some more discussion/caculations:
http://electronics.stackexchange.com/questions/39834/placement-of-vias-to-connect-ground-planes
http://www.rogerscorp.com/documents/2311/articles/Comparing-Microstrip-and-CPW-Performance.pdf