Lab 2: Analog Simulation of Passive Circuits

(Using Analog Artist / Waveform)

Before starting the simulation, make sure that your test_rlc schematic is open.

In the test_rlc schematic window, select Tools => Analog Environment

• The icons on the right provide quick access to frequent commands/menus.

• The Design Area: Lists the Lists the Library, Cell, and CellView of the design being simulated.

• The Analyses Area: Lists the types of analyses, any arguments (i.e. time interval), and weather it’s enabled to perform the simulation in the current run.

• The Design Variables Area: Lists components set as variables, i.e., a Capacitor, C1, varying from 1uF to 1pF.

• The Outputs Area: Lists names of nets/signals/expressions/ports to be plotted on the output waveform window.

• The Sub Menus: Essentially, following the menus from the top-left selection to the bottom-right one guides you through the steps required to perform a complete simulation cycle. The following sections will provide more detailed descriptions.

1. We’ll select the simulation engine to be SpectreS. In the Simulation window, select Setup => Simulator/Directory/Host

2. Ensure the Simulator cyclic field is reading spectreS

3. Change the Project Directory to read ~/cadence/simulation. This creates a new directory under your cadence folder.

4. If you’re prompted to "save the current state". Click Yes, and confirm the name as state1 in the form that opens afterwards. Click OK.

In the Analog Artist Simulation window, click the Choose Analysis icon. Instead, you could select it from Analysis => Choose pull down menu. The form appears.We’ll simultaneously setup several analyses modes.

• Transient analysis: This provides the transient output response of the circuit with respect to time. The user specifies the time period and the time variant input waveform while the simulator calculates the output response.

• AC analysis: This simulates the AC performance of the circuit as a function of frequency, and is based upon the small-signal frequency response model.

• DC Operating Point: This analysis simply determines the D.C. operating point of the circuit based on the parameters present on the schematic assuming all capacitors opened and all inductors shorted. It is the default mode and is automatically performed before any other analysis in order to determine the initial state of the circuit.

•DC sweep mode: This generates DC transfer characteristics for the circuit by varying a user specified independent source over a range of values.

Notice that in the Analog Artist Simulation Window, under the Analysis Section, a line was listed to describe this analysis.

•  In the Analysis Section, select ac (refer to next figure).

•  Set the Sweep Variable to Frequency (note the other sweep variables).

•  Set the Sweep Range to Start-Stop. (Start: 0.01k, Stop: 10k).

•  Set the Sweep Type to Logarithmic with 20 Points Per Decade.

•  Turn on the Enabled field.

•  Click on Apply.

Notice in the Analog Artist Simualtion Window, under the Analysis Section, a line was added to describe this analysis. When done, the form should appear as shown in the next figure.

1. In the Analysis Section, select dc.

2. In the Sweep Variable section, select Component Parameter.

3. Click on Select Component. This allows for selecting the instance on the schematic.

5. A form appears listing all the instances parameters. Select the dc parameter. Click OK.

6. In the Sweep Range section, select Start-Stop. (Start: 0, Stop:100)

7. Turn on the Enabled field.

8. Click OK this time.

Notice in the Analog Artist Simualtion window, under the Analysis Section, a line was added to describe this analysis. When done, the form should appear as shown next.

The final look of the Analog Artist Simulation window should be as shown below.

The simulation environment is configured to save all node voltages in the design by default. You can modify the default to save all terminal currents also, or you can select specific set of nodes to save. We’ll select these nodes from the schematic window.

1. In the simulation window, select Outputs => Save All.

2. Select Output => To be Plotted => Select on Schematic.

Node voltages can be selected by clicking on the wire on the schematic window, and currents by clicking on the terminals. Unselecting can be performed either by clicking on the terminal/node again, or by selecting the corresponding line in the Outputs section of the Simulation window and clicking on the Delete icon.

Select the input and output wires to the rlc circuit. Observe the simulation window as the wires get added.

Click on the Run Simulation icon. When it complete, the plots are shown automatically. The 3 Analysis Responses are shown in separate windows. The DC response is not clear due to the voltage divider effect.

We’ll next modify the appearance of the displayed waveforms.

1. Click anywhere in the DC Response area to work in this section. Notice the highlighted box reading "3" at the top-right corner of the section.

2. Select Axes => To Strip, or click on the Switch Axis Mode icon on the left. Observe the 2 separate plots displayed. Repeat for the 2 other plots(1, 2).

3. Double-click on the y-axis label of the Transient Response. A form appears. Fill in the Label field Vout. Click on OK. Observe the label change. Repeat for the other labels.

4. Use the Markers (A, B) to measure the output peak-to-peak amplitude of the Transient Response signal. Click on the Crosshair Marker A icon on the left. Click on a negative peak of the output waveform. Repeat for Marker B, at a positive peak.

5. Read the markers data at the bottom of the screen. Look at the delta field (time, volts).

6. Select the AC Response section. Click on Marker A. Pull it up, till it can’t go any further. Read the resonance frequency from the data at the bottom of the window.

7. To delete the bottom Vin-Vin plot in the DC Response section, click on the bottom waveform, and press the Del key on your keyboard. Finally, the Waveform window should appear.

1. In the test_rlc schematic window, move over the RLC symbol, center-click then go down to select the Descend Edit...

2. A form appears. In the View Name, make sure it reads schematic, then click OK. The rlc schematic is displayed.

3. In the Analog Artist Simulation window, select Results => Annotate => Transient Operating Points.

Lab Report

This lab report is due by the end of next lab.

You need to turn in the printout of

1. rlc schematic view

2. rlc symbol view

3. test_rlc schematic view

4. final simulation waveform.

Please write down the following results for your simulation.

What's your marker data for negative peak and positive peak in transient response analysis?

What's your marker data for peak frequence of AC response.

In transient response simulation, what is your output peak-to-peak amplitude?