Simulation eBook - Initial conditions and starting up circuits
Initial conditions and starting up circuits
Some background and basic start-up techniques
There are several important points to understand about what happens at the start of a simulation.
All simulations start at time t=0.
Whatever DC conditions are applied to the simulation at t=0 are considered to have been present for all time t<0.
Even though it is possible to start plotting the results of a time domain simulation at some time after t=0, the simulation itself always starts at t=0.
Even though an AC Analysis has no time duration associated with it, the DC operating point is calculated at t=0.
If there are no .IC statements included in a simulation and the Startup and UIC modifiers are not used, then the initial DC conditions of a circuit are completely defined by the initial levels or DC offsets of any sources present in the circuit and these are treated as having been present at those levels for all time prior to t=0. So for example, a DC power rail that is set to 9V is treated by the simulator as having been applied to the circuit at 9V for all time prior to t=0.
Similarly, a SINE source with a -1V DC offset or a PULSE source with an initial level of -1V are treated by the simulator as having been at -1V DC for all time prior to t=0. Similarly, a COS source with a 0V DC offset would be treated by the simulator as having been at +1V DC for all time prior to t=0.
Therefore the voltages in a circuit, such as bjt base bias potential dividers and so on, will have been set to DC steady state values for all t<0. Consequently, the voltages across all capacitors and the currents through all inductors in the circuit will have reached their DC steady state values prior to the simulation starting at t=0.
Even if the circuit is an oscillator, prior to t=0 it will have been assumed to be in a stable non-oscillating steady state. At t=0 the circuit will then start from those initial DC conditions. It will then either continue in that steady non-oscillating state or will slowly drift away from the steady DC state and oscillations will build up.
The initial state of oscillators based on a tuned circuit such as phase shift, Wien Bridge and Crystal Oscillators will be defined by their DC bias conditions. If there are no noise sources in the circuit (the default state for all components unless otherwise specified such as resistors defined to have noise contributions) then there is nothing to nudge the circuit away from equilibrium and so it may never start oscillating.
Although in most cases such oscillators will eventually start up due to the 'hidden' noise source which is simply due to the mathematical noise generated by the finite resolution and rounding errors of the calculations carried out in running a simulation, this can take a very long time compared to the time taken to run the oscillator in a stable oscillatory state for a few cycles. Crystal oscillators in particular can take many hundreds of thousands of times the oscillator period to start up and reach a stable state.
To minimise the simulation time spent waiting for an oscillator to start, it is useful to introduce some initial start-up condition to 'kick-start' the circuit into oscillation.
The simplest way to kick-start most circuits in LTspice is to run a Transient (.tran) Analysis with the startup modifier appended to the end of the .tran directive. For example:
.tran 1m ; runs a time domain simulation for 1ms starting with the initial DC conditions
.tran 1m startup ; runs a time domain simulation for 1ms starting with the independent sources all set to zero and then ramps them up in the first 20us or so of the simulation.
Another simple way to kick-start an oscillator based on a tuned circuit is to replace a simple DC supply source with a PULSE source set to an initial level of the desired power supply voltage but configured to generate a short pulse of the supply voltage plus or minus some small voltage. So for example a circuit with a 9V supply that is to run for 1ms with a time step of 1us could have a PULSE source set to an initial level of 9V pulsed down to 8.5V for 1us with 100ns rise and fall times. Or an initial level of 8.5V with a delay of 1us before a 100ns rise-time step up to a pulse level of 9V.
The same trick can be carried out using a voltage source inserted almost anywhere in the circuit simply to inject a small step or pulse into a bias voltage but it must be remembered that if the voltage step or pulse does not return to 0 after the kick then it will represent an offset voltage in that part of the circuit.
An example of this is in forcing crystal oscillators to start.
Crystal oscillators take a very long time to start up because of the extremely high Q of the crystal.
The same thing is true of their simulations so, to avoid simulations taking too long to run and generating massive data files, they may need to be run in stages with increasing start and stop times but a small (Tstop - Tstart) value.
As discussed earlier, injecting a small step into the supply voltage or an internal node of the circuit can help to start the oscillations a little earlier but the idea of injecting a small step or pulse into a circuit to kick it into life is taken to an extreme in the EasyEDA crystal model.
The technique used in the XTALfast subckt is to include a PULSE source internal to the crystal model to introduce a very high amplitude impulse at t=0 inside the model. This starts the oscillator almost instantly and because an impulse with a very wideband spectrum is used rather than a step (or a sinusoidal burst at the crystals natural resonant frequency), the oscillations start at the actual resonant frequency of the crystal in the application circuit.
The start up time of the example below using the XTALfast subckt can be compared with the same crystal model but with an unassisted start simply by editing the name of the crystal model from XTALnokick to XTALkick.
This example also demonstrates a way to use the advanced features of the LTspice capacitor model to create a more computationally efficient crystal simulation but one which unfortunately cannot be kick started like the EasyEDA model.
Crystal oscillator using the EasyEDA quick starting crystal model
The EXP and PWL sources can also be used as kick-starter supply sources.
Most relaxation oscillators such as the classic two transistor astable multivibrator or the 555 timer have two stable states. Oscillation is normally maintained by the circuit switching between these two states however, under DC bias prior to t=0, these circuits often settle into one or the other of these stable states and so are stuck there at t=0. This means that they never start oscillating.
This is an example of a simple RC relaxation oscillator that does not start up by itself:
This type of circuit may need a rather more vigorous kick to get it started. This can be done using a PULSE source but instead of introducing a small step, the supply is ramped up to the desired supply voltage from 0. So, for example, by setting an initial level of 0 and a pulse level of 9 with zero delay time, with a rise-time of 200us the circuit starts up cleanly up from all internal nodes being at zero.
This example also demonstrates starting up the same circuit with only a simple DC simply by adding the startup modifier to the .tran statement to ramp the DC source automatically:
Another possibility - which will be explained in more detail later - is to use an expression that is a function of time in a B source.
For example, this expression in a B source:
V=9*(1-exp(-time/100u))
generates a voltage that starts at zero and rises exponentially to a final value of 9V with a time constant of 100us:
With symmetrical circuits such as the two transistor astable multivibrator, even this may not be enough to disturb the equilibrium enough to get them oscillating. It may be necessary to introduce some deliberate asymmetry or imbalance into the circuit, for example by making a one base pullup resistor or a timing capacitor a fraction different from the other. Even changes of less than the expected real component tolerance can be enough to tip the circuit into self sustained oscillation with a zero to rated voltage ramped supply start-up.
Sometimes complex circuits - or simple circuits with complex models - may fail to simulate because the simulator cannot find the DC operating point prior to t=0. Such circuits will very often simulate fine if the supply (or supplies) are ramped up from 0. In the same way as slightly imbalancing symmetrical components can help start-up, slightly imbalancing the voltages, delay or rise times of the supply voltage ramps may help start-up more 'difficult' simulations.
There is however, a downside of using the start-up from zero supply ramp. As already stated, at the start of a transient simulation, the voltages across all capacitors and the currents through all inductors in the circuit will have reached their DC steady state values prior to the simulation starting at t=0. If the simulation starts with the supply voltages set to zero at t=0 then obviously all the internal voltages and currents must also be zero (except for some small offsets due to the initial levels of any signal sources and sometimes, badly designed sources internal to models that do not collapse to zero with zero supply voltages).
If all the internal voltages and currents are zero at t=0 then it may take much longer than the desired simulation stop time for all the internal nodes to reach their DC steady states.
A simple solution to this is to run the simulation for long enough for everything to have settled but to only plot the results for just long enough before the stop time to show the signals of interest. So, for example a circuit that is driven by a 1kHz source but which takes 95ms to settle could be observed from say, t=98ms to t=100ms by setting the transient analysis to have a stop time of 100ms and a Start time of 98ms, like this:
.tran 0 100m 98m
This solution works very well but, in this example, over 95% of the simulation time is used just to get the circuit to a steady state before any useful results are generated. This is very wasteful of simulation time and for complex simulations such as switch mode power supply (SMPS) simulations - where exactly this situation is likely to arise - can take many minutes of real time.
This is where another technique for setting initial conditions in a circuit can sometimes be useful.
Setting initial voltages on nets and currents through components
There are occasions where it is required to start a simulation in some predetermined state. For example, a capacitor may be required to start a transient simulation at time t=0, precharged to some given voltage. Similarly the current in an inductor may need to be specified at time t=0. In a larger simulation it may be helpful to precharge the output smoothing capacitor of a power supply to approximately the right voltage to save the time taken for it to be charged up from zero. If the capacitor is at the output of an SMPS then it may be useful to charge the inductor(s) in the SMPS to their average operating current(s) too.
Using the .ic spice directive to set an initial voltage condition on a net
For more information about the .ic spice directive see:
Use of the '.ic' spice directive is illustrated in these two examples:
This approach is not recommended but an alternative to using the .ic statement is shown in the these next examples show two ways to use append the 'uic' option to a Transient Analysis but for the reasons already given in the description of the 'uic' option in the section on 'IC: Set Initial Conditions' in 'Setting up Analyses', care should be taken in using this option.
Using a current source to set an initial current through an inductor
In LTspice, the .ic spice directive can be used to set initial current conditions through one or more inductors. This is illustrated in the following example:
Setting the initial voltage on a capacitor
This approach is not recommended but an alternative to using the '.ic' statement to set the initial voltage across a capacitor is to append ic=<voltage value> to the capacitor value and uic to the .tran statement:
Setting the initial current through an inductor
This approach is not recommended but an alternative to using the '.ic' statement to set the initial current through an inductor is to append ic=<current value> to the inductor value and uic to the .tran statement:
Some circuits may start up on their own but simply changing a component model may cause it to fail to start-up. Don't be afraid to try these techniques before spending ages trying to find some other obscure cause.
Using a 1V source to help start-up
This is an advanced technique which has limited application but which in the right circumstances can be very useful.
By placing a 1V voltage source in a schematic, naming it's output as, say, 'unity' and then multiplying using expressions in B Sources by V(unity), it is possible to force all the B sources in the simulation to start from zero during the early DC operating point parts of a transient simulation.
This can sometimes help produce a clean startup from zero internal initial states.
It must be borne in mind however, that as with other techniques that bring a simulation up from zero, any attempt to run an OP, TF or an AC simulation will usually return zero results because all the internal states and in many cases the gains of B sources will have been forced to a zero initial value.
Replacing ideal and Thevenin voltage sources with band-limited Norton Sources to help start-up
This is technique is very widely applicable since it helps improve the overall convergence of simulations and not just their startup behaviour.
Ideal voltage sources in simulations are capable of producing infinite currents so a load which looks capacitive at any point during the simulation has the potential to cause an instantaneous infinite current flow. This can cause a simulation to go into overflow or to fail to find a valid next step from which to proceed. In either case, the simulation will fail to converge. To prevent this it is good practice to always include some resistance in series with every voltage source, whether that is an independent V, dependent E or H source or a dependent B source configured as a voltage source.
This turns all ideal voltage sources into Thevenin Sources, i.e. voltage sources with a finite source resistance.
Internally, however, the simulator is actually more efficient at calculating the currents and voltages around a Norton Source than a Thevenin source. So, the next step of the process is to convert all the Thevenin sources in a simulation into Norton Sources.
A Norton Source is the exact equivalent circuit of a Thevenin Source. To convert a Thevenin source to the Norton Equivalent source, the voltage source of the Thevenin source is replaced with a current source equal to the short circuit current of the Thevenin source and the series resistance of the Thevenin source is reconnected in parallel with this current source. Both sources than have identical source resistances, open circuit voltages and short circuit currents. So far these steps of converting ideal voltage sources to Thevenin sources and then to Norton equivalent sources generally increases the simulation speed of most simulations but the final step of limiting the bandwidth of the Norton sources can significantly improve the start-up and convergence of many simulations.
Limiting the bandwidth (or band-limiting) a Norton Source is easy: all that is required is to connect a capacitor in parallel with the source resistance that has already been connected in parallel with the current source. This creates a lowpass filter across the output of the Norton source which reduces the output at high frequencies. This means that even if the source is passing or generating highly non-linear signals that can produce exactly the kind of very fast and even discontinuous signals that spice struggles to deal with in its internal calculations, as the frequency content of these signals and transitions exceeds the lowpass filter cutoff frequency, they are reduced to relatively slower edged (i.e. reduced high-frequency content) signals. Such signals then have finite rise and fall times and so spice no longer struggles to deal with them. They become much more spice friendly continuous signals.
Even better is that if there are several such band-limited sources sprinkled around the circuit (such as the input signal sources) then very often the derivatives of these signals also become continuous. This is also a big help to spice because much of the internal calculation in spice is in estimating not just where a signal is but also making estimates about where it is going and how fast it is getting there.
Some words of warning are needed here though. Replacing Thevein voltage sources with band-limited Norton sources is a great technique but it requires a high degree of understanding of what is really going on in a simulation circuit.
The statement above about:
"...all that is required is to connect a capacitor in parallel with the source resistance that has already been connected in parallel with the current source. This creates a lowpass filter across the output of the Norton source which reduces the output at high frequencies."
is all very well but it skirts around the question of what should the value of this capacitance actually be? There is no single answer to that question because the cutoff frequency required to avoid convergence or start-up problems will vary from one circuit to another and even from one location to another in a circuit. The single biggest factor affecting the value is simply that the cutoff frequency must be much higher than the working frequencies of not the circuit itself but of the devices in it. So for example, an audio amplifier circuit designed for a bandwidth of 20kHz may use an opamp that is operated with a closed loop bandwidth that is 200kHz but which internally may have a gain bandwidth of 2MHz or even 20MHz.
In practice, setting the cutoff frequency with an RC time constant of 1ps (1e-12s) i.e. a cutoff frequency of approximately 160GHz, should be safe for most 'ordinary' simulations of amplifiers, linear and switch mode power supply circuits but for high frequency and RF circuits the band-limiting must be increased accordingly.
The value of the resistor in this parallel RC circuit can be also be very tricky to decide. For many lightly loaded voltage sources, a value of 1 Ω is OK and simplifies the calculation of the parallel capacitance to 1pF. In some sources, however, it may be necessary to use a higher (or lower value) of parallel resistance. This in turn will require the use of a proportionately smaller (or larger) capacitance for the same cutoff frequency. This will also require that the current value of the source is reduced to maintain the same open circuit voltage (calculated from V=I*R).
This band-limiting technique should generally not be applied around any existing current sources in a simulation circuit. Placing an RC circuit in parallel with a pure current source may do more damage to the operation of the circuit by reducing the in-band source impedance of the current source than the band-limiting avoids!
Although not an example of a start-up or initialisation problem, the Ideal and Thevenin to Norton Source conversion is demonstrated in steps (i), (ii) and (iii) of this simulation:
Using the 'OFF' option to help start-up
Some components, such as switches, bjts, jfets, MOSFETs and MESFETs have an 'OFF' option to specify the device to be in an initial OFF state.
Switches also have an 'ON' option to specify the device to be in an initial ON state.
This option can be very useful to ensure that for example, one side of a two transistor bistable or monostable circuit or an astable mutlivibrator is off, so avoiding the situation described above where both transistors are on in the initial state. Whilst this does not in itself guarantee that the circuit will start up from t=0 but it may simplify any other measures that have to be taken to ensure it does.
These states are simply invoked by appending the keyword OFF (or, for switches only, ON) after the device name. This can be done either by directly editing the name in place in the schematic or via the right hand panel Properties dialogue. For example, to set a switch with the name MYSWITCH to be initially ON the name should be edited to:
MYSWITCH ON
Similarly, to set a bjt with the name 2N2222 to be initially OFF the name should be edited to:
2N2222 OFF