within SPICELib.analyses; model OP extends src.ANALYSES.OP; annotation ( Window( x=0.03, y=0.02, width=0.24, height=0.45, library=1, autolayout=1), Documentation(info="

OP - Bias point calculation

To calculate the DC response of an analog circuit, SPICELib removes time from the circuit. This is done by treating all capacitors as open circuits, all inductors as shorts, and using only the DC values of voltage and current sources.

The bias point is calculated for any analysis. However, additional information is reported when the Bias Point analysis is made. The following information is reported to the dslog.txt file:

a list of all analog node voltages
the currents of all voltage sources and their total power
a list of small-signal parameters for all devices

Bias point calculation is the most problematic step from the numerical point of view. The nonlinear equations which describe the circuit's static behavior must be solved. SPICELib provides four alterative algorithms for solving the circuit static model (see Table 1). The SOLVE_STATIC parameter determines which of the four algorithms to use.

Table 1. Algorithms for solving the circuit static model.

SOLVE_STATIC=0	Static model iteration The solution of the circuit static model is left in hands of the modeling environment (for instance, Dymola). SPICELib has two symbols to provide an initial guess for Newton-Raphson algorithm: NODESET1 and NODESET2.
SOLVE_STATIC=1	Static model ramping The static value of the independent sources is ramped by SPICELib from zero up to their target values. The clamping voltages of the IC symbols and the capacitor IC property are also adequately ramped. The value of the parameter TIME_SCALE determines the time length of the ramping.
SOLVE_STATIC=2	GMIN stepping GMIN stepping attemps to find a solution for the static model (with power supplies at 100%) by starting with a large value of GMIN, initially 1e10 times the nominal value. If a solution is found at this setting, SPICELib reduces GMIN by a factor of 10 and tries again. This continues until either GMIN is back to the nominal value, or a repeating cycle fails to converge.
SOLVE_STATIC=3	Dynamic model ramping The initial condition to iterate the static model is obtained by simulating the large-signal model. A transient analysis is performed: all sources are ramped up from zero to the desired initial value and this value is held for some time to allow the circuit to stabilise. Then, the voltage values calculated from this transient analysis are used as initial conditions for solving the static model.

Note:
The algorithms static model iteration, static model ramping, and GMIN stepping are supported by PSpice. PSpice first tries to solve the static model of the circuit using the Newton-Raphson algorithm. If a solution is not found and GMIN stepping is enabled, then GMIN algorithm is applied. If it also fails or it is not enabled, then \"static model ramping\" is applied.
The algorithm dynamic model ramping is proposed in \"Cellier F.E. (1991): Continuous System Modeling. Springer-Verlag\".
"), Icon( Rectangle(extent=[-90, -50; 60, 35], style(thickness= 2, color=3)), Line(points=[-90, 35; -60, 50],style(thickness=2, color=3)), Line(points=[60, 35; 90, 50],style(thickness=2, color=3)), Line(points=[-60, 50; 90, 50],style(thickness=2, color=3)), Line(points=[90, -35; 90, 50],style(thickness=2, color=3)), Line(points=[60, -50; 90, -35],style(thickness=2, color=3)), Text(extent=[-90, -50; 60, 35], string=".OP",style(color=1)) )); end OP; model AC extends src.ANALYSES.AC; annotation ( Window( x=0.03, y=0.02, width=0.24, height=0.45, library=1, autolayout=1), Documentation(info="

AC sweep - Frequency response of the circuit

AC sweep is a frequency response analysis. SPICELib calculates the small-signal response of the circuit to a combination of inputs by transforming it around the bias point and treating it as a linear circuit.

Nonlinear devices are transformed to linear circuits about their bias point value before SPICELib runs the linear (small-signal) analysis.
Because AC sweep analysis is a linear analysis, it only considers the gain and the phase response of the circuit; it does not limit voltages or currents.

The best way to use AC sweep analysis is to set the source magnitude to one. This way, the measured output equals the gain, relative to the input source, at that output.

Setting up an AC analysis

To run an AC sweep analysis, you need to place and connect one or more independent sources and then set the AC magnitude and phase for each source. Each independent source in your circuit contains its own AC specification for magnitude and phase.

The parameters defining the frequency sweep are shown in Table 1.

Table 1. Parameters.

TYPE_AC_SWEEP	It defines the frequency sweep type: TYPE_AC_SWEEP=0 - Linear. TYPE_AC_SWEEP=1 - Logarithmically by decades.
POINTS_NUMBER	Number of sweep points: TYPE_AC_SWEEP=0 - Total number of points. TYPE_AC_SWEEP=1 - Total number of points per decade.
START_FREQUENCY	Starting frequency for the sweep.
END_FREQUENCY	Ending frequency for the sweep.

"), Icon( Rectangle(extent=[-90, -50; 60, 35], style(thickness= 2, color=3)), Line(points=[-90, 35; -60, 50],style(thickness=2, color=3)), Line(points=[60, 35; 90, 50],style(thickness=2, color=3)), Line(points=[-60, 50; 90, 50],style(thickness=2, color=3)), Line(points=[90, -35; 90, 50],style(thickness=2, color=3)), Line(points=[60, -50; 90, -35],style(thickness=2, color=3)), Text(extent=[-90, -50; 60, 35], string=".AC",style(color=1)) )); end AC; model TRAN extends src.ANALYSES.TRAN; annotation ( Window( x=0.03, y=0.02, width=0.24, height=0.45, library=1, autolayout=1), Documentation(info="

TRAN - Transient analysis

The Transient response analysis causes the response of the circuit to be calculated from TIME=0 to a specified time (see the note below). During a transient analysis, any or all of the independent sources may have time-varying values.

The parameters defining the transient analysis are shown in Table 1.

Table 1.
Parameters

TSTOP Length of the transient simulation.

SKIPBP SKIPBP=false
The transient analysis does its own calculation of a bias point to start with, using the same technique as described for Bias Point. This is necessary because the initial values of the sources can be different from their DC values.
Two equivalent procedures are provided to specify the analysis initial conditions: the IC symbols and the IC property.

SKIPBP=true
The bias point calculation is skipped and the simulation proceeds directly with transient analysis at TIME=0. The large-signal circuit state is initialised to the IC-property corresponding values. Devices with IC property defined start with the specified voltage or current value; however, all other such devices have an initial voltage or current of zero. IC symbols are ignored.

Simulation time during transient analysis
When the transient simulation is started, the value of Modelica variable time is different from zero. For this reason, a variable is defined to measure the transient simulation time: TIME. "), Icon( Rectangle(extent=[-90, -50; 60, 35], style(thickness= 2, color=3)), Line(points=[-90, 35; -60, 50],style(thickness=2, color=3)), Line(points=[60, 35; 90, 50],style(thickness=2, color=3)), Line(points=[-60, 50; 90, 50],style(thickness=2, color=3)), Line(points=[90, -35; 90, 50],style(thickness=2, color=3)), Line(points=[60, -50; 90, -35],style(thickness=2, color=3)), Text(extent=[-90, -50; 60, 35], string=".TRAN",style(color=1)) )); end TRAN;