2
\$\begingroup\$

I am looking to dabble into some RF PCB design with a microstrip line to a WiFi chip antenna, and I am trying to understand if my intuition is correct.

I have used various calculators to determine the width of the trace I need for a 50\$\Omega\$ \$Z_0\$ on a 4 layer PCB -- all agree with roughly 18 mils on FR4.

Since the transmitter, transmission line, and chip antenna are all 50\$\Omega\$, there should be no standing wave pattern along the line and \$V(x)\$ and \$I(x)\$ (where \$x\$ is the position on the line) should be constant.

Aside from ohmic losses and parasitics (which the latter can be tuned out), does this imply that the length of the line can be arbitrary? i.e., the trace does not need to be a specific electrical length such as \$\lambda/4\$?

I am leaning towards that it isn't, but I've reviewed some reference designs from TI (the CC3100BOOST and the CC3200 Launchpad) that have caused some confusion. The CC3100 uses a trace length of 660mil from chip to antenna, which is almost exactly \$\lambda/4\$ at 2.4GHz, and the CC3200 uses a 1200 mil line, which is very close to \$\lambda/2\$. I'm not sure if this is intentional or a coincidence.

I'm looking for a (perhaps tediously) clear answer before I make any mistakes.

\$\endgroup\$
  • 2
    \$\begingroup\$ Your intuition is right. \$\endgroup\$ – Enric Blanco Mar 27 '17 at 15:20
  • \$\begingroup\$ ... although if you do make the line \$\lambda/2\$ long, the system overall will be less sensitive to any manufacturing tolerances on its actual \$Z_0\$. \$\endgroup\$ – Dave Tweed Mar 27 '17 at 15:27
  • \$\begingroup\$ @DaveTweed how's that? \$\endgroup\$ – Enric Blanco Mar 27 '17 at 15:47
  • 2
    \$\begingroup\$ Not sure, but I think that there is a special case when the transmission line is exactly \$\lambda /2\$ : No matter what is the characteristics impedance of trans. line \$Z_{in}=Z_L\$, where \$Z_{in}\$ is the equivalent impedance. \$\endgroup\$ – Marko Buršič Mar 27 '17 at 15:51
  • 1
    \$\begingroup\$ @EnricBlanco: What MarkoBuršič said, and it applies for any length that is a multiple of \$\lambda/2\$. \$\endgroup\$ – Dave Tweed Mar 27 '17 at 16:01
4
\$\begingroup\$

In the ideal case, where source, line and load all have the same impedance, there is no significance to the length of the line, other than loss (shorter is better).

Where tolerances make the impedances depart from ideal, there will be small effects, but unless you know which way the departures are going, it's not possible to say whether you will be better off with any specific length.

If the source and load are well controlled, and the line is poorly controlled, then you will be better off with multiples of \$\frac{\lambda}{2}\$ line length. This length transforms the impedance at one end of the line into the same impedance, regardless of the line impedance.

If the source deviates down, and the load deviates up, or vice versa, then an odd multiple of \$\frac{\lambda}{4}\$ would be better, as that length of line transforms Zload into \$\frac{Z_{line}^2}{Z_{load}}\$ at the source end.

However, for either of these cases, you need to have enough control over the impedances to know how wrong they are, and if you know that, you might as well make them correct, or tune for them properly.

The only other case to note is that if the connection line is very short, say less than \$\frac{\lambda}{10}\$ (and the shorter the better), errors in the line impedance will have little effect.

To check your line width calculations, a 50ohm microstrip on FR4 is roughly 2 substrate thicknesses wide.

It's worth noting that the impedance can be fairly wrong, before significant reductions in power transfer between source and load occur. A quick simulation on SPICE may be worth doing to give you an idea of the permitted tolerances.

\$\endgroup\$
0
\$\begingroup\$

You say that all the parasitics can all be tuned out. But the complex materials and geometries of the die to package to board interface and within the antenna mount and connector(s) make that moderately difficult in practice. Thus, a half wavelength (or an integer multiple thereof) might help minimize the effects of any line-end reflections that were missed in your "tuning out" process.

\$\endgroup\$
  • \$\begingroup\$ I guess this applies to the transmission line between the transciever input/output (e.g. BALUN) and the feeding point of the antenna (i.e. on-board, like chip or PCB trace). What if the board only features an SMA connector? Does the half/lambda optimization still applies? \$\endgroup\$ – Guillermo Prandi Mar 28 '17 at 3:19

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.