Take into account layout considerations for RF


There are a number of layout considerationg when designing RF systems
that were not taken into account or not quantified when making the
first design.

- transmission line width

  The microstrip [1] transmission line connecting the balun and filter
  circuit with the antenna must be impedance-matched with the antenna.
  The rule of thumb according to [2] is to make its width twice the
  board thickness, in this case 0.8 mm or 31.5 mil.

  The microstrip calculator at [3] also takes into account the
  thickness of the copper, 1 oz, and yields a slightly narrower 57.5
  mil or 1.46 mm.

  A more elaborate calculator can be found at [4].

- via spacing

  Section 4.2 of [5] recommends a via spacing of no more than
  Lvia = C/sqrt(Er)/Fres
  where
  C = the speed of light, 3*10^8 m/s
  Er = the board's dielectric constant, 4.5 for FR-4
  Fres = the resonance frequency, at least 24.5 GHz

  We thus obtain Lvia = 5 mm.

- component placing

  [5] places DC blocking, balun, and filter close to the transceiver,
  with only the feed line between the RF circuit and the antenna. Thus,
  no changes are needed.

- feed line termination

  Point 12 of [6] warns us that we may need to terminate the
  transmission line if it is longer than 20% of the signal's rise time.

  Point 1 of [6] gives the rise time as 1/(10*Fclk), which looks as if
  it's meant for digital signals. But we'll use it anyway.

  [2] gives us the typical propagation delay for a microstrip as
  150 pS/in.

  This means that Lmax = 0.2*tr*v
  with
  tr = 1/24.5 GHz
  v = 1 in/150 pS

  We thus obtain Lmax = 1.4 mm

  [2] suggests that the maximum unterminated stub is L(in) = tr(nS).

  With tr = 1/(10*Fclk), we thus obtain Lmax = 1.04 mm.

  Not sure if all this even applies to antennas. This needs looking to by
  someone who understands about RF.

[1] http://en.wikipedia.org/wiki/Microstrip
[2] http://www.hottconsultants.com/techtips/rulesofthumb.html
[3] http://www.cepdinc.com/calculators/microstrip.htm
[4] http://mcalc.sourceforge.net/
[5] http://www.ti.com/litv/pdf/swra236a
[6] http://www.pcbmotif.com/home/index.php?option=com_content&view=article&id=104&Itemid=137


Conclusion: the antenna feed line needs to be revised. The via spacing
of the RF area needs to be examined. The recommended spacing may be
beyond the capabilities of a DIY process, though.
