Maker Pro
Maker Pro

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
smile.gif
Please try to answer all it would really help me.
 
I am not an expert, but:

Make it as small as possible.
Place the components to minimize the distance of all connections.
Use a ground plane.

I have seen old amateur radio circuits that were build on a ground plane on a single sided pcb, with through hole components mounted like surface mount. Today, I would think a 2 sided pcb with ground plane on the bottom and surface mount components on top as you said would be best. And you would use vias to connect to ground.

Bob
 
Hello
You got most of that right apart from the ground plane acting as a capacitor. You will need a power plane above this for this to work. But is does not make a very good capacitor so you still need the standard decoupling capacitors for each IC. The use of a microstrip or strip line is when you need controlled impedances. Transmission lines only need to be used to prevent reflections when the signal trace is over a certain length compared to the rise time of the signal. Some basic things covered by Bod already but to add a couple more.

1. Use multiple vias on ground connection, keep them as close to the pad as possible.Actually via in pad is the best option but PCB assemblers don't like them because of dry joints
2. Avoid trace stubs unless used for tuning impedance in very high speed designs.
3. Avoid swapping layers on high speed traces.
4. Use internal power planes, this is the best thing you can do for PCB. A respin of a PCB that you find needs internal planes is costly. It's the most cost effective thing you can do for a high speed design.
5. Don't use top broken copper 0 Volt planes, bad idea. It may have some shielding properties but does nothing really for EMC.
6. Some designs will benefit from unbroken top and bottom 0 Volt planes via stitched together to form a shield and prevent fringe emissions. All signal traces are routed internally. This is actually the option I take for products that are complex and used in certain harsh enviroments.


You don't say if your 100Mhz signal is a stream of data, a clock or a sine wave. Are you routing this to a connector or another device. Do you have a circuit diagram or a started layout we can look at? If you could explain a bit more about your design then I could go into a lot more detail for you.

Thanks
Adam
 
I put somthing together for you. I will look at you design in due course. Hope it's of some use.
Cheers
Adam

Transmission Lines
What is a transmission line? Well it’s basically any pair on conductors used to guide electromagnetic energy from one point to another. In a PCB the transmission line is the trace above a power plane. This provides closely coupled send and return signal paths, with the return signal being directly underneath the send trace. This reduces loop inductance due to magnetic field cancelation.

Other types of transmission lines
· Twisted pair Cables
· RF Coaxial cable
· Waveguides
· Power traces

What’s happening on this transmission line?

Sometimes it’s advantageous to think of a mechanical transmission line, the simplest I can think of is what we call a newton’s cradle. The transmission line in this case is an acoustic version and Kinetic energy from one ball to the other propagates through the other balls at the speed of sound.

New Picture.png



Figure 1 Newton’s Cradle Mechanical Transmission line
The middle balls don’t move they just compress and expand back again once they have transferred the energy to the other balls. Initially the last ball will swing up as high as the first ball that was released in the first place. In an Ideal world this would carry on for ever, the first and last balls alternatively swinging out as the cycle repeats itself.

Losses in the transmission line prevent this carrying on and eventually this dies out and stops. This is essential the same principle of what happens to an un-terminated PCB transmission line. Energy is reflected back and forth within the PCB trace causing corruption of the original signal. The way to prevent this is to somehow absorb this reflected energy.

New Picture (1).png
Figure 2 Various PCB Transmission Lines Setups
Two common methods of termination that are used are series termination and parallel. Series termination is when the reflected wave is allowed to come back to the source and energy would be absorbed in a series resistor. Parallel termination is a method of using a shunt resistor at the load end which absorbs the reflected energy there and prevents this reflected energy from continuing back up the transmission line to the source.

Tip!
· If the insulating material between the transmission line has a dielectric constant that is constant with frequency then the impedance will be the same at all frequencies.
· If the cross sectional area of the transmission line is constant it will have the same impedance irrespective of length.

This is another good reason not to change layers on a transmission line because the via will contribute an impedance discontinuity and cause some reflection of the signal back to the source which reduces the amount energy transferred to the load which is used to develop the voltage signal at that end.
How do we control this?

If you are dealing with RF signals then there may be only a few lines that need controlled impedances which can be controlled quite easily. But on a high speed digital PCB this is much harder because trying to make sure all traces are matched is very time consuming. So a level of signal degradations needs to be accepted, this is down to the designer and product function. The most effective use of time for this approach is to use internal power planes.

Un-terminated
New Picture (2).png

Figure 3
New Picture (3).png
Figure 4 Response of un-terminated line
Series connection
Notice the reflections bringing back the losses from the potential divider formed by the different impedances.

New Picture (4).png
Figure 5 Response of series terminated line

Parallel Termination
Noticed the lack of reflection, the output voltage is too small to trigger the 5 Volt logic level on the output. In this case the output impedance of the source must be a lot lower than the transmission line to achieve a logic 1 level on the output of the transmission line.

New Picture (5).png
Figure 6 Response of parallel terminated line
Termination Techniques

New Picture (6).png
Figure 7 Different types of termination and their uses

New Picture (7).png
Figure 8 Termination configurations
Stubs on Transmission lines
Stubs on transmission lines can cause reflections which can cause the intended signal to interfere with itself. A stub can be intentional and is used for matching the impedance of very high speed transmission lines (microwave).

For the majority of high speed designs they cause a problem because they are uncontrolled and variable. How do you accidentally cause a stub problem? Two common mistakes I see quite often is when people change layers on a multilayer PCB which has through hole vias. And also the connecting of the terminating resistor which was fitted to help can actually cause problems.

New Picture (8).png
Figure 9 this is a via stub

New Picture (9).png
Figure 10 R1 has long Stub from signal trace, bad design

New Picture (10).png
Figure 11 Better approach

New Picture (11).png
Figure 12 Quarter wave stub on transmission line. The stub shorts out the incoming signal by phase cancelation.
When do I need a transmission line or terminate an existing one?

Two general thoughts on this and one is when the quality and amplitude of the signal at the receiver end of a transmission line falls below design specifications. The other is when the length of the PCB trace exceeds the TEL (Total electrical length) of the signal.

Let’s put this into context.

A PCB trace will allow the propagation of a signal at approximately 6 inches per nanosecond. So if a trace is longer than 2.25 inches with signal rise times of 1.5 ns then this signal would need impedance control.

Decoupling Capacitors
Decoupling capacitors are used to provide a low impedance source of energy to high frequency high current switching that happens inside most ICs.

Capacitor Types
Aluminium Electrolytic: Large physical size, large capacitance values, High Voltage, Low ESR, degrade over time.

Tantalum: Medium physical size, Medium capacitance value, Low voltage, Low ESR.
Ceramic: Small Physical size, Low to medium values, Very low ESR.

New Picture (12).png
Figure 13 Equivalent capacitor circuit
ESR (Equivalent Series Resistance) Rs
Capacitance XC = 1/2πfC
ESL (Equivalent Series Inductance) XL = 2πfL

Series Resonance
Series resonance occurs at the frequency where XC (capacitive reactance) is equal to XL (inductive reactance). At this frequency, the impedance of the capacitor becomes equal to the ESR. At frequencies above this, the capacitor behaves like an inductor.

Parallel Resonance
The additional capacitance of the PCB and its power planes cause parallel capacitance which increases the resonant frequency of the capacitor. At this frequency the capacitor has much higher impedance.

New Picture (13).png
Figure 14 Parallel equivalent circuit
So it’s important to choose the correct value and type of capacitor for the design. For many years the standard decoupling capacitor has been 100nF. This is the value I use today for low frequency PCBs. For higher frequencies you need to go lower.

Some people say you can use the capacitance of the power planes. Although this is true, it is quite low value doesn’t make a very good capacitor. The best approach is to choose a ceramic capacitor which has the correct value. Bulk capacitance somewhere in the region of 1uF to 10uF would be used to support the supply pin of a microprocessor.

Capacitor example:

IC power consumption = 1 W
Power Supply =3.3 Volts
Decoupling capacitor = 1nF

Support Time for 5% Droop of supply = C*0.05*V^2/P = 0.5 ns
Another method:
dt=rise time
dv=drop in voltage allowed

C=Total I/O current *dt/dv = 100 mA*1 ns/10 mV= 10 nF
Now this small value will work for very short pulses of energy like the switching of internal ports in ICs. But will do nothing to support the power supply from dipping due to loading on the PCB from other parts of the circuitry or small power dips from the input to the power supply. This is why you need some bulk capacitance from larger value capacitors.
 
Last edited:
Just read the comments from the other guys on your schematic. I have given you some help on PCB design but that's about it. I am not going to help you design an illegal transmitter.
Cheers
Adam
 
Adam it's not an illegal transmitter it is a simple amplifier ( an electronics-part 1 university project). Still thanks for the help. Pity I won't be able to benefit from your knowledge anymore.
 
You surely won't see it I even lack the equipment to get to such a high frequency up till know I have access to a 20 MHz function generator but I will be testing using some NI-PXI thing :)
 
Top