Greg,

Overall power dissipation depends mainly on component size, placement
and air flow. A few large parts, spread out over the
board, can obviously dissipate more power than smaller parts placed
close together but, if there's no forced or convective air
flow, the eventual temperature rise will be the same. Back in the dark
ages, 10 or more years ago, we would just add a heatsink
and be done with it but, with todays closely packaged tiny parts, that's
no longer an option in many cases.

In the last few years, many semi manufacturers have adopted small dual
and quad packages with a central thermal pin or pad
that's intended to be soldered directly to the board. Quite often these
parts burn so much power that, on the board, the central
pad must be thermally connected to power planes or a solid area on the
reverse side of the board with thermal vias to handle
the dissipation.

Commercial grade parts are typically rated to operate over the 0-70 deg
C range. If you can keep your parts within that range,
you should be good. If not, increase the air flow and/or add direct
thermal connection to a metallic section of the case.

Impedance issues depend on the frequencies involved, not only clock
speed but also edge rates, and the geometry. Low power
CMOS parts generally have edge rates in the 1-10 ns range which, at the
faster limit, still places most of the signal energy below
5 GHz.

Generally, in the digital world, an impedance discontinuity smaller than
1/10 of a wave length can be ignored. A trace on FR-4
will have a propagation velocity, depending on geometry, in the 160-190
ps/in range which makes the wave length, at 5 GHz,
about 1.05 to 1.25 inches. So geometries smaller than 0.1 inch can be
ignored but, if a trace is longer than that, trace impedance
and end terminations start to come into play.

Numerous free impedance calculators and a few field solvers are
available on the web. A few I've found useful are:

Zcalc, a differential pair calculator, can be found at
http://www.jnicolle.com/?page=LVDS

Saturn PCB Toolkit handles single ended and differential pair
impedance as well as a number of other useful things. it can
be downloaded from Saturn PCB Design at
http://www.saturnpcb.com/pcb_toolkit.htm

Trace Analyzer is a handy tool that can handle a number of
conductors, ground planes and grounded shields. It can be
downloaded at http://www.eecircle.com/downloads/download.html

All three of these give answers that agree well (within a few percent).
On the other hand, avoid the Rogers Corp MWI-2008
tool. It tends to give answers 20% - 25% too high. I've bitched at them
but they still haven't fixed it...

HTH.

Bruce

> To what point (or end) should I be concerned with thermal dissipation and
impedance values in the traces on my board? How do I calculate these values?
>
> - The two boards I am designing are 2" x 4" and 2" x 6" in size.
> - I am using some RS-232 and USB stuff mostly.
>
> Greg