High Speed PCB Design

Hello everyone I am looking for considerations to keep in mind while designing a pcb(Only double sided available) with high speed signals (upto 100MHz).
What I know up till know:
1)Using small traces to get low inductance and capacitance.
2)Using a complete layer of the two sided pcb as ground plane to act as a decoupling capacitor.
3)Avoid removing any part from the ground layer so that the return current is exactly under the signal current.

Questions:
4) Would using smds be a better option than through hole components and why?
5) If I use smds, I would have to use vias to provide ground is using vias for ground and also other connections a good option?
6)What other techniques can be used to minimize the stray capacitances and inductances at high frequency.
7)What is with the transmission line termination and control impedance?
8)Microstrip:what is it ? In case of double sided pcb with one ground layer and the other etched part is this microstrip?
9)What should I do with the power should it be provided on the etched side?

Please correct me where wrong Please try to answer all it would really help me.

 

surface mount componants dont have leads, therefore less stray inductance and capacitance. for years am - fm radios used single sided pc boards, at frequencies above 108 mhz. also scanners and tv's did too good layout and practices will work on single sided boards, check the ARRL amature radio handbook for construction.

 

Assuming we are talking digital, not analog. #1 is dubious, you should care more about the proper impedance of the trace, not as much about inductance and capacitance. Maybe true for power supply lines, you want those as fat as possible.
#2 and #3 seem correct.
#4 SMDs are better since they have the shortest leads possible
#5 via to ground plane is much much better then snaking in some trace that is far away connected to ground - much lower inductance with vias
#6 keep traces short and loop areas at minimum
#7 the most critical is the source impedance. You dont need nor want termination at the far end, since it will only reduce the amplitude. The correct matching between source and trace impedance will make sure that all the reflected signals coming back from the far end will not be reflected once again form the source side.
#8 correct, but with added fact that it has closely set impedance relative to the ground plane and it should have this impedance all the way from source to the end
#9 if you really need proper high speed design, then use at least four layers. Especially when considering EMI compatibility you will have hard time getting it right with two layers. Most of the time you cannot physically connect everything on top layer, so your ground plane will get a lot of breaks in it, which might affect the high speed signals. Other thing is that the supply rail will be long and sneaky which will again ruin your EMI emissions.

 

Per kubeek, what are we talking here, analog frequencies up to 100 MHz or digital data rates up to 100 MHz(bits)? The answer has a big impact on the layout.

 

7) Transmission lines only need to be considered if the trace electrical length is greater than about 1/10th of the signal wavelength for sinewaves or about 1/4 of the signal risetime for digital signals. If you do need transmission lines then the source will need to be able to drive the low impedance of the transmission line or microstrip (typically in the neighborhood of 100-150Ω).

 

crutschow, you are my Hero. So many people do not get that it requires at least a 1/4 wavelength before the trace starts to behave like a transmission line. Below that length, the trace is just simple lumped elements.

crutschow, you made my day.

Mark

 

Guys 1/4th of signal risetime would give something in seconds comparing it with the trace length?

 

comparing with trace length divided by propagation velocity, which I think is about 2/3c or 8in/ns.

 

I said "electrical length" by which I meant the trace length for that amount of propagation delay as stated by Kubeek.

 

One thing I do when using SMD capacitors for IC decoupling is the run the power trace form the IC through the pad for the capacitor (in one side and out the other side). That gives the absolute minimum inductance between the trace and the capacitor. The ideal is to then connect the other side of the capacitor directly to a top side ground plane (or ground flood).

 

Check out this book -- it's the standard reference for high speed design considerations. It answers all of your questions, and more.

"Black Magic" book