Simulation is a design analysis, which replaces design symbols with their simulation models and provides a detailed analysis of their behaviour. For simulating a designed circuit, the model of the real circuit is created taking all factor into consideration and the appropriate inputs are given. Then the outputs at each level are checked and corrections or modifications are made. Hierarchical simulation has been implemented in EDWinXP Mixed Mode Simulator. The Mixed Mode simulator now supports simulation of hierarchical databases.

Steps for Mixed Mode Simulation

Preprocess the circuit

The simulator analyzes the schematic first and checks for the simulation function. It generates the data along with the statistics of the circuit. Data includes the number of digital and analog nets, list of symbols, which may be simulated along with their simulation functions, number of digital inputs and outputs, number of A/D input/ outputs. This is presented as a dialog box. Observe that the analog primitives are assigned negative simulation function.
Click the OK button to close this dialog box. The simulator is now ready for making further analysis on the circuit.

Note: Any change in the circuit element values or topology gets implemented only if the preprocess is invoked. Preprocess menu is invoked from Simulation menu. Preprocessing the circuit resets the values set.

Assign Component Parameter Values

1. Select Component Properties (function tool) --> Change Simulation Parameters (option tool).Click on the component
2. Component Parameter Setup window opens.
3. Change the parameter values.
4. Click Accept.

Analysis

For setting up simulation time and Start analysis types,

1. Select Simulation -->Analysis.
2. Set the parameters by selecting General settings from the tree view on the left side of the window.

3. Set the values as

Simulation Limits:

Ambient Temperature	25
Max. Iteration Error	100m
Iteration Limit	100
Floating No. Precision	4

Min. Displayable Unit:

Voltage	mV
Current	μA

4. Click Accept button to accept the changes and to automatically switch to Analysis option.

Bias Point Calculation

Bias Point Calculation is used to determine the DC behavior of the circuit.
1. Inorder to view the DC values, fix the test points at the base, collector and emitter of the transistor as shown below. To place the test points, select Tools --> Instruments-->    Test points -->   Voltage TP

2. Select Simulation --> Analysis.
3. A window Setup Simulation Parameters opens with the option Analysis being highlighted on the left side of the window by default.
4. Check Bias Point Calculation check box.

Click Start button, and observe that the node voltages are displayed at the locations where test points were placed. Similarly current values can also be viewed by placing the test points at the required nets.

Transient analysis

Transient analysis is used to view the input and output with respect to time. Inorder to view the performance of the circuit in time frame run transient analysis.

1. Select Simulation --> Analysis.
2. Select Transient analysis from tree view.

Analog Sim Step time: Allows setting the step time for TD analysis.

Simulation Time Limit: Allows setting the final time till simulation is to be performed.

Initialize LC: Allows manipulating the initial values of the state variables (capacitor voltages and inductance currents).

Solve: The circuit solves the initial conditions using the supply voltage and current set in the circuitry.

Clear: The initial conditions set using both the component parameters and the circuitry gets cleared. The initial capacitor voltage and the inductor current are set to zero.

Set: The initial conditions set using the component parameters (To do so, select Component/Comp.Params from the menu of Mixed Mode Simulator. Click on the capacitor or inductor for which the initial value is to be set. The window that pops up allows changing/setting the initial value.) are recognized as the initial values for the analysis.

Display Waveform: Displays the simulated result as a diagram if enabled.

Transfer Function: Enable it to include transfer function analysis.

3. Enter following values:

Analog simulation step time:	2μ
Simulation time limit:	1m

4. Check Display waveform check box.
5. Click on Accept to switch into the Analysis option
6. Click Start to begin the analysis.

Parameter Analysis

Parameter analysis helps to study the effect of variation of component parameters on the circuit. This analysis calculates the change in the output of a given circuit when a selected parameter of a particular circuit element is varied over a range of values.

1. Select Simulation --> Analysis.
2. Select Parameter Analysis from the tree view.

Sweep Variable: Allows setting either temperature or component parameter as the sweep variable, while conducting analysis. Select either Temperature or Component parameter from the drop down list. To select a component parameter as the sweep variable - point the cursor to the desired component on the workspace and press the left mouse button. The component name, parameter name and parameter value get loaded. Use the drop-down list for Parameter name to choose the desired component's parameter.

Analysis Type: Allows setting the type of analysis to either Sweep or Step. Select either Sweep or Step from the drop down list. If Sweep is selected, set the Start, End values and Step. If Steps is selected, set the value for steps.

Sweep Mode Allows choosing between linear and logarithmic sweep modes. Select either Linear or Logarithmic from the drop down list. Logarithmic requires both start and end values of the sweep variable greater than zero. The end value may be less than start value - in this case the sweep variable will be decremented. Several rounds of analysis may be done with various component parameters set for each component.

Start & End Value, Steps The difference between start and end values denotes the number of outputs of analysis to the Waveform Viewer (If Display Diagram option is checked). Step denotes the incremental factor of the scale.

Step Value Denotes the values for which analysis is to be performed.

Display Waveform Displays the simulated result as a diagram if enabled.

3. Select Sweep Variable as Component Parameter type.
4. Move the cursor over the resistor and click on it. Selected component name and parameter name appears in the dialog box.
5. Set the values for the following parameter as

Start Value	1KOhm
End Value	3KOhm
Steps	750Ohm

6. Click Accept to switch into Analysis option.
7. Check Parameter analysis check box.
8. Now click Start button for analysis to take place. The result may be viewed in the Waveform viewer.

Fourier Analysis

Fourier analysis helps to calculate the total harmonic distortion of analog waveforms generated during transient analysis.

1. Select Simulation --> Analysis.
2. Select Fourier analysis from the tree view.

Fundamental Frequency Specifies the fundamental frequency of the waveform whose distortion is being computed. Enter a desired value in the text-input box.

No. of harmonics Indicates the number of sinusoidal components of frequencies that are multiples of fundamental frequency, i.e., harmonics. Enter a desired value in the text-input box. As value for number of harmonics increases, computation time and accuracy increase accordingly.

Deg. Of Polynomial Specifies the degree of the polynomial used to interpolate the waveform. Enter a desired value in the text-input box. As value for degree of polynomial increases, computation time increases. But accuracy also increases accordingly.

3. Set the parameters in the box as

Fundamental Frequency	10K
No of harmonics (nfreq)	10
Deg. of Polynomial(polydegree)	2

4. After setting the parameter click Accept button to accept the parameters.
5. Check Fourier Analysis and click Start button. Fourier analysis results are displayed in a text format.

DC Sweep Analysis

DC Sweep analysis mode allows to study the effect of variation of parameters of circuit elements when the parameter of one circuit element is varied keeping the parameter of another circuit element constant, through out a range of values. This also helps to set up the best operating conditions for the design, before detailed functional analysis is made.

1. Select Simulation -->Analysis.
2. Select DC Sweep Analysis from the tree view.

Sweep Variable Allows setting either temperature or component parameter as the sweep variable, while conducting analysis. Select either Temperature or Component parameter from the drop down list.
For analysis of a single component - point the cursor to the desired component on the workspace and press the left mouse button. The component name, parameter name and parameter value get loaded. Use the drop-down list for Paramter name to choose the desired component's parameter.
FFor analysis of two components - point the cursor to the desired component on the workspace and press the left mouse button. Click FILL COMPO(1) button to load the first component. Repeat the process and click FILL COMPO(2) to load the second component.

Start Value, End Value, Steps The difference between start and end values denotes the number of outputs of analysis to the Waveform Viewer (If Display Diagram option is checked). Step denotes the incremental factor of the scale.

Sweep Mode Allows choosing between linear and logarithmic sweep modes. Select either Linear or Logarithmic from the drop down list. Logarithmic requires both start and end values of the sweep variable greater than zero. The end value may be less than start value - in this case the sweep variable will be decremented. Several rounds of analysis may be done with various component parameters set for each component.

Display Waveform Displays the simulated result as a diagram, if enabled.

3. Move the cursor over DC supply and click on it. Selected component name and parameter name appears in the dialog box.
4. Set the sweep limits as

Start value	0V
End value	15V
Steps	1V

5. Check Display Waveform check box to display the waveform.
6. Selectt Accept to switch into Analysis Option.
7. Check DC Sweep Analysis check box.
8. Click t.

AC Sweep Analysis

AC sweep analysis is used to calculate the small signal frequency response of the circuit assuming its current biasing.

1. Select Instruments --> Set Reference Points (function tool) --> AC IN+ and click on the input net.
2. Select Instruments --> Set Reference Points (function tool) --> AC IN- option tool and click on the input net.

This tool specifies the input given to the input side to be a voltage source or a current source for running the AC Sweep Analysis.

3. Select Instruments --> Set Reference Points --> AC OUT+ and click on the load net.
4. Select Instruments --> Set Reference Points --> AC OUT- and click on the load net.

This tool specifies the output variable taken from the output side to be either the open voltage or the short current.


5. Select Simulation --> Analysis.
6. Select AC Sweep Analysis from the tree view.

Start frequency	Allows entering the start value for frequency, for which the simulation may be carried out.
End frequency	Allows setting the end value for frequency, for which the simulation may be carried out.
Points per Decade	Specifies the number of points per decade for which analysis is conducted.
Phase Range	Allows selecting the phase difference of the output curve.
In Source	Allows specifying whether the input source is voltage or current.
Out Variable	Allows specifying whether the output is open voltage or short circuit current.
Output	Provides a list of options, any of which may be chosen for outputting the results of simulation.
Display Waveform	Displays the simulated result as a waveform in Waveform Viewer, if enabled.

7. Set the values for the following parameters as

Start frequency	100 Hz
End frequency	1GHz
Points / decade	100
Phase range	[-180, +180]
IN source	voltage
OUT source	Open voltage

8. Click Accept button to switch into Analysis option.
9. Check AC Sweep Analysis check box.
10. Click Start for AC Simulation Pass to take place.

Monte Carlo Analysis

The Monte Carlo analysis is used for simulations with a given error on different components. This test is very useful for visualizing how the circuit will run with imperfect components as are used in reality.

1. Select Instruments --> Set Reference Points --> Monte Carlo voltage and click on any of the nets.
2. Select Simulation --> Analysis.
3. Select Monte Carlo Analysis from the tree view.

4. Select the component at which the analysis has to be done, by clicking on it.
5. Enter the parameters and click Accept to accept the parameters.
6. Click Start.
The result is displayed in a text file.

Sensitivity Analysis

Sensitivity Analysis is used to calculate the component that is most sensitive to an output reference point.

1. Inorder to determine the sensitivity of a component with reference to a net select Instruments --> Set Reference Points --> Sensitivity voltage
2. Click on any of the nets and place the reference points.
3. Select Simulation --> Analysis.
4. Select Sensitivity Analysis from the tree view.
5. Specify a value of tolerance for which the analysis is to be carried out. This is the common tolerance value for all parameters of all components.

6. Click Accept button to switched into Analysis option.
7. Check Sensitivity Analysis check box.
8. Click Start button, result is displayed in a text file.