## How does Spice think?

You’re
an engineer. Spice doesn't think like you think.

Spice
was written by a group of Professors and grad students at the University of
California, Berkeley, over 45 years ago. So it thinks like most of your college
professors did - it likes theory and ignores reality.

It
simulates by solving matrixes of circuit equations. Circuit equations use ideal
electrical elements: resistance, capacitance, inductance. Things we can't buy.

So
it follows that we need to go back to college thinking to understand Spice. And
that Spice depends totally on us to interpret the physical world into its
theoretical world. This process is called modeling
your circuit for simulation.

###
**You Create the Circuit Model, not Spice **

Consider
your physical circuit on a PCB. It's built of parts you can buy, each of which
if far from a pure electrical element. It has a ground plane with measurable
impedance, noisy power supplies, stray coupling between traces, etc.

Spice
has ideal electrical elements, its ground node connects all ground points with
zero impedance, its voltage sources have zero impedance and are used to provide
the power supply voltages in simulation. Ordinary circuit equations don't
couple to each other.

So
you are the physicist here. How do you take the Physics of your physical
circuit and create a schematic for Spice's ideal world that includes enough of
the real world imperfections to make a
model accurate enough for your needs. But not totally accurate as that
takes forever. This is the major challenge of using Spice.

Keep
this concept in mind to guide you in using Spice effectively.

Given
the above, notice that the Spice schematic is almost always different from the
PCB schematic.

Rule 1
If you find yourself starting to simulate the PCB schematic, stop. You
have brain fade.

### Working with Spice as a breadboard

An
effective way to use simulation is to first gain some understanding of your
area of design - from past experience, reading and playing in the lab with a
real circuit, playing with the program. Then plan a model of the proposed
circuit considering the real world imperfections of the parts you will be
using. Keep the model’s schematic to only the bare essentials to start. Enter
this schematic into the program and do your initial simulation. Now the
important part - confirm that the results of simulation are reasonably close to
the results from your lab circuit. No lab circuit? - do some other form of
reality checking/testing.

Rule 2
Avoid the beginner’s mistake of assuming that since simulation runs
without errors, your schematic accurately models your lab circuit.

Continue
with an interactive process of improving your simulation model of your design
AND your lab design, repeatedly comparing the two. When they match over time,
frequency, etc., you know you can trust your simulation model. Have fun.

### Details of modeling your circuit for simulation

How
is the schematic for simulation going to differ from your lab or production
circuit schematic? Remember that resistors, capacitors, inductors and
voltage/current sources in the simulator schematic are mathematically perfect.
Parts you can buy always are mixtures of resistance, capacitance and
inductance.

Also
remember when using a Spice subcircuit that models a complex part, the
subcircuit may model only a portion of the behavior of the physical device.

Common imperfections of physical devices

Resistors

inductance
for wirewound resistors

Capacitors

series
resistance, especially electrolytics where resistance is large and varies
strongly with frequency and temperature. Also far from perfect are ceramic caps
made from high dielectric materials (Z5u, etc.).

Inductors, transformers

series
resistance, self resonance with the winding capacitance (at surprisingly low
frequencies) and usually a series resonance at much higher frequency. If there
is a magnetic core, it may saturate and has losses that go up very rapidly with
frequency.

Circuit board

Even
the ground plane has significant resistance if you are pumping several amps
through it. Long traces have significant inductance at higher frequencies. And
stray capacitance, etc.

subcircuit limitations

Op Amps

Manufacturers
supply models (in the form of Spice Subcircuits) for many of the Op Amps they
make. Be aware that the models are all greatly simplified in number of
transistors/FET’s compared to the actual Op Amp. They also differ widely in the
amount and accuracy of the functionality they include. If your design depends
on Op Amp input noise, slew rate, distortion, input common-mode rejection
versus frequency, power supply rejection or handling input or output signals
near the supply rails, you need to verify that the manufacturer's Op Amp model
you use

- models these areas
- matches a real world Op Amp in the lab close enough for your purposes

Also note that production Op Amps have wide tolerances on GBW (gain-bandwidth product) from lot to lot. The manufacturer’s model usually has a typical value.

Power FET’s

Manufacturers
use Subcircuits to model Power FET’s. These vary in complexity and accuracy.
See discussion of Op Amp above.

Spice model limitation at High Frequency / fast Rise Time

The
general purpose Spice models (.Model) for diodes, FETs and transistors do not
include any lead inductance. You or the manufacturer can write a Spice .Subckt
which contains the .Model plus lead/package inductances. Power MOSFETs are
modeled using a .Subckt and usually have these inductances.

switching circuits with inductors/transformers

The
inductors and transformers in Spice have no winding capacitance. Switching an
ideal inductor that has current flowing can result in an infinite voltage spike
with zero rise time. Simulation will fail (you can almost feel the simulated
gamma rays coming out of the screen). Add parallel capacitance and/or
resistance to limit bandwidth and limit spike rise time/amplitude during
switching.

Power Supplies

Remember
that Spice voltage sources turn on instantly. Real power supplies do not. This
sometimes results in Spice finding a different DC Bias solution than the actual
circuit has! Fix crazy DC bias voltages by adding NodeSets
to the schematic.

Spice
voltage sources have such low impedance over all frequencies that they will
short out DC drop, ripple and noise that would appear in any real world
circuit. So consider adding series resistance (and possibly inductance) if
using a voltage source to model a real power supply or voltage regulator.

Ground Layout and Impedance.

Spice’s
ground symbol provides the perfect, zero impedance connection between all
points. No real circuit or ground plane is like this. Ground impedance issues
are complicated. See EDN.com for a detailed article on
ground currents and grounding.

Too Much Perfection!

Many
circuits improve in performance as part values match or track each other. You
can get some awesome numbers with Spice's perfect components.

## No comments:

## Post a Comment