Paul,

every bread board design suffers from extreme inductivities of connections from chip to chip. Especially the ground connections are so bad, that extended circuits containing modern fast microcontrollers with buses are impossible to realize! Only smaller circuits, NOT containing address buses and data buses CAN work. But it's always dangerous and does not allow the least mistake...

Have a look at the following simplified equivalent circuit, showing two digital CMOS chips connected with output to input:



Output toggling is represented by a switch in combination with resistance R. If output goes high, switch connects very fast output to Vcc. If output goes low, output is connected to ground. R represents output resistance (source impedance) and is about 50Ohm for fast CMOS chips.

Input of second chip is represented by Cp, which means the parasitic capacitance at input to ground of about 5pF (3...10pF).

L1 represents inductivity of connection from output to input, realized by a piece of wire, how it's used with bread board designs. L2 represents the wire, which connects the grounds of both chips together. And finally L3 represents the piece of wire, which is used to connect the decoupling capacitor Cx (which is located near Vcc pin) to ground.
Although this scheme was explained in combination with breadboard design, it's of general validity. Means, a circuit sitting on a printed circuit board (PCB) can be represented by an equivalent circuit, which looks very similar, even if PCB is mulitlayer type. Only some stray capacitance from copper trace to ground must be added to Cp. And, of course, values of components L1, L2 and L3 are highly different, as we will see now.

Let's discuss this circuit:
When the output toggles from low to high, a current loop is formed running from Vcc through R, L1 and Cp to ground '2', back to ground '1' via L2 and through L3 and Cx back to Vcc. Yes, ground is distinguished into ground '1' and ground '2'!
Why?
Because this current loop will produce a high voltage drop across L2 (ground bounce), and because of this both grounds are not identical!! (But they should, of course!)

Inductivity L2 is a direct measure of height of ground bounce, and if we compare L2 of different designs, we have a measure of quality of each design.

Assume a breadboard design, where both chips are sitting 15cm away from each other, like it can be seen with extended circuits, containing address bus and data bus structures. With the rule of thumb, that inductivity of a piece of wire is about 1µH per meter, we can estimate L1 and L2 to 150nH each.
If we now compare this breadboard design with a simple double-sided PCB, containing a solid ground plane on one side, we get an arrangement, where the signal 'wire', means copper trace, is sitting directly over a solid ground plane. This arrangement forms a transmission line or microstrip line and provides an inductivity, which is extremely much smaller than that of the pieces of wire of bread board design:
Assume 15cm long copper trace of 0.3mm width running over solid groundplane, with thickness of PCB is 1.6mm. Then, according to published formulas inductivity of this transmission line (L1 + L2) is 18nH (!), capacitance is 1.17pF and characteristic impedance is about 125Ohm. This is an improvement in inductivity by a factor of about 17!
The trick is, that the magnetical field is highly concentrated between the current running in copper trace and it's ground return current running in the solid ground plane! This ground return current flows automatically directly under the copper trace back from ground '2' to ground '1', because the condition, where as minimal as possible energy is stored in magnetic field, is highly preferred!
Inductivity is so very small, because magnetic field is NOT wasted over whole space, but highly concentrated 'inside' transmission line!! (Concretely, we should speak about an electromagnetic wave, which is running inside transmission line.)

But the disadvantages of bread board design are even going further: Assume now, that this discussed signal is part of data or address bus, means is a data line or address line. Then you have to multiply voltage drop of ground return currents by 8 + 16 = 24! This is the result of bread board design: When only using this one piece of wire which connects ground '2' and ground '1' all the ground return currents must flow along this wire and all the voltage drops must be added...
Concept of solid ground plane on the other hand automatically results in forming transmission lines for each data line and address line. And because each individual ground return current searches its path directly under the according copper trace, the voltage drops of ground return currents do NOT add in the same way as with bread board design.
Why?
Because the ground return currents split over the solide ground plane located under the bus lines!!

So, PCB design containing a solid ground plane results in an extreme benefit in terms of ground bounce: Firstly, the factor 17 of inductivity improvement, then, secondly, that voltage drops are not multiplied by number of address and data lines as with bread board design!

Up to now, we spoke about double sided PCB, containing solid ground plane. Of course, it's difficult to achieve a solid ground plane over the whole PCB area, when using double sided PCB. But it's often possbile to achieve it at least under the buses, which provides be a tremendous improve!
But if circuits are to complicated, the use of multilayer boards (4-layer, e.g.) will do the job. Then, distance between copper traces and solid ground plane can be even decreased, resulting in a further improve of inductivity.
Nevertheless, if costs are playing a keyrole, even proper designed double sided PCB containing as much as possible solid ground plane, can offer pretty results.

Other disadvantages of bread board design are:

1. Have a look at loop formed by signal wire and ground return wire. Loop area is in the 'many square-centimeter' range! Radiation of magnetic fields and susceptibility against magnetic fields can be extreme. Just the opposite with solid ground plane: Loop areas are extremly small, because each ground return current automatically searches its path closest to signal! Most of electrical and magnetical field is concetrated inside PCB and will not cause radiation. Also, loop area is so small, that susceptibility against magnetic fields is extremly reduced.

2. Capacitive cross coupling between signal traces is minimized with solid ground plane concept, because also electrical fields are concentrated between signal trace and solid ground plane. Quite different again bread board design. Here capacitive cross coupling dominates, because there's absolutely no reference plane, which could work like a screen or shield. Each signal interferes with every other...

3. With bread board design it's nearly impossible to find any quiet ground reference for connecting cables leaving the circuit. Ground noise is extreme and it's nearly impossible to connect cables, without them mutating into heavy radiating antennas! People who want to connect some bread boards containing digital circuits will get problems over problems...

4. Power supply decoupling suffers from inductivity L3. If only a piece of wire is used to connect Cx to ground, decoupling performance is really poor. If instead the connection is provided by solid ground plane, decoupling performance will satisfy. L3 can be observed to be up to ten times smaller, when using solid ground plane instead of simple piece of wire...

5. Technique of series termination is often used to increase allowed maximum trace length of transmission lines, without being limited by reflections. With bread board design characteristic impedance of resulting 'transmission line' is so big, that series termination is impossible. How a bread board design performs in terms of reflections and ringing of signal lines, especially when bus structures are involved, is not predictable...


Again, when you do not use bus structures, means, when you want to build up a very simple stand-alone microcontroller, then using a bread board CAN work. But when building a bit more extended microcontroller circuits, then don't use these bread boards! Only concept of solid ground plane will then work, providing a universe of advantages...

Kai