PCB transmission line questions

[[email protected]]

Hi folks,

Let's say I have a 50R termination resistor at the end of a 5 mils
wide 50 ohm line on an outer layer on this particular PCB. Now when
the line hits the pad of the resistor, the impedance of the pad is
lower than the line, since the pad is about 12 mils across (0201
part). Now the signal is "in" the resistor, which has a 50 ohm
resistance, and now the signal goes back out the other pad, back to a
short line, and then ends up in the 18 mil via to ground....

1) What difference does it make if the 3 mil long line that connects
the resistor to the via is a "50 ohm" line or not? The prop delay is
0.3 PICOSECONDS. What frequency does the signal need to be to be able
to "see" the impedance in such a short trace? 100GHz +???

2) Isn't it worse to have 2 steps (pad, 50 ohm line, via) than no
steps (line is as wide as the pad)??

3) Something I never quite "got". Parts must have an impedance as
well, is there such a thing as a 50 ohm 1K resistor? A 0201 1K
resistor is wider than a 50 ohm trace on this PCB, so does the 1K
resistor present an additional mismatch on the line due to the
physical size as well as the electrical resistance? What happens to a
signal that encounters a large part on a narrow 50 ohm line? I
understand that the impedance basically tells me about the ratio of
electrical to magnetic field, or something to that effect, while the
resistance tells me about turning electrical energy into heat.
Question is, if a resistor is sufficiently mismatched, will the
impedance effects dominate the part? Will a sufficiently large (1206
say) part on a sufficiently small (5 mils) trace, reflect most of the
signal instead of actually going in the part??

4) My brain is burnt. It looks like a bowl of oatmeal left in the
microwave for 3 hours then tossed into a volcano. May I ask you to
keep the answers short, with 2 or 3 syllable words? Grunt, or use sign
language if appropriate.

Thanks!

 

[John Larkin]

Hi folks,

Let's say I have a 50R termination resistor at the end of a 5 mils
wide 50 ohm line on an outer layer on this particular PCB. Now when
the line hits the pad of the resistor, the impedance of the pad is
lower than the line, since the pad is about 12 mils across (0201
part). Now the signal is "in" the resistor, which has a 50 ohm
resistance, and now the signal goes back out the other pad, back to a
short line, and then ends up in the 18 mil via to ground....

1) What difference does it make if the 3 mil long line that connects
the resistor to the via is a "50 ohm" line or not? The prop delay is
0.3 PICOSECONDS. What frequency does the signal need to be to be able
to "see" the impedance in such a short trace? 100GHz +???

Depends on the signal bandwidth/risetime. If the structures are a
small fraction of the wavelength or risetime, they become invisible.

2) Isn't it worse to have 2 steps (pad, 50 ohm line, via) than no
steps (line is as wide as the pad)??

3) Something I never quite "got". Parts must have an impedance as
well, is there such a thing as a 50 ohm 1K resistor? A 0201 1K
resistor is wider than a 50 ohm trace on this PCB, so does the 1K
resistor present an additional mismatch on the line due to the
physical size as well as the electrical resistance? What happens to a
signal that encounters a large part on a narrow 50 ohm line? I
understand that the impedance basically tells me about the ratio of
electrical to magnetic field, or something to that effect, while the
resistance tells me about turning electrical energy into heat.
Question is, if a resistor is sufficiently mismatched, will the
impedance effects dominate the part? Will a sufficiently large (1206
say) part on a sufficiently small (5 mils) trace, reflect most of the
signal instead of actually going in the part??

Again, it depends on the signal bandwidth. A resistor is up off the
board some, so its impedance is higher than a trace of the same width.
And the climb over the end cap, followed by a via to ground, adds
inductance. Some people like to load surf mount resistors upside down,
which helps a little.

Figure that you can run a 1 or 2 GHz signal, risetimes 350 to 175 ps
respectively, into a 1206 or 0805 plus a ground via and get a good
termination. A good term for faster stuff would be two 100 ohm 0603's
or 0402's, each with its own via or, better, a big ground pour with
sevaral vias. That might be pretty good up to 10 GHz. At frequencies
like that, the incoming trace will start getting so lossy that an
imperfect ternination hardly matters.

We've done fairly complex circuits, signal shaping, summing,
amplification, with 0603 and 0402 parts down into the 90 ps sort of
range, 4 GHz maybe, on FR-4.

Higher value resistors, a couple of K or so, tend to be dominated by
their shunt capacitance. Caddock makes some axial, leaded resistors in
the 500r-2K range that are remarkably good to 5 GHz or so.

4) My brain is burnt. It looks like a bowl of oatmeal left in the
microwave for 3 hours then tossed into a volcano. May I ask you to
keep the answers short, with 2 or 3 syllable words? Grunt, or use sign
language if appropriate.

Relax. Fast stuff, low GHz range, is easy with cheap surface mount
parts.

John