PADS Professional Parasitic Extraction (Classic UI)

Abstract:

In this article we will go over how to run Parasitic Extraction with Xpedition AMS. Parasitic Extractions help determine the unwanted or parasitic effects from an electrical design in order to create more accurate models and simulations.

We will provide the steps and an example project which you can use to practice running the process. This project folder can also be found in <AMS installation path>\SDD_HOME\sim\systemvision\tutor\. Copy the folder PCBPowerSupply1 to your working directory.

Link to project folder zip: Data.zip
 

Estimated Time to Complete: 30 to 45 minutes

Version Information: X-ENTP AMS VX.2.13 (should also work with VX.2.5 and later)

---

Prerequisites

Installation and licensing of Xpedition AMS and HyperLynx Advanced Solvers

Download and Use the File

1. Download the attached zip file or navigate to the PCBPowerSupply1 folder
2. Within Xpedition AMS, open the .prj file called PCBPowerSupply1.prj

Run Simulation without Parasitics

First run the simulation as is to observe the performance without parasitic effects.

Open the Netlist Settings dialog box.

1. Go to Simulation > Netlist > Netlist Settings
2. Uncheck the boxes for Include parasitics in netlist and Include IBIS
3. Click OK

Initialize the Xpedition AMS Simulator by opening the Simulation Control dialog box.

1. From the menu, click Simulation > Simulate
2. Within the Simulations tab:
   • Experiment name should be set to expt1.cmd
   • Time-Domain Analysis should be enabled
   • End Time set to 170u
3. Within the Results tab:
   • Under Time-domain Waveforms choose All Waveforms from the dropdown menu.
4. Click OK to start running the simulator. The Waveform Analyzer should automatically open with the results loaded into it once the simulation is done running.

Analyze the results in Waveform Analyzer.

The Waveform Analyzer window should have automatically opened. On the left, under Waveform List, you should see a list of signals.

1. Double-click on the signal names to plot them. Choose A_OUT, FB, FETOUT, and PWM_GATE. Observe the graphs, as seen in Figure 1.

 

Run Simulation with Parasitics

Now, we will run the simulation to analyze the parasitic effects. 

Open the Extract Parasitics dialog box.

1. From the menu click Simulation > Parasitic Extraction > Run Solver
2. From the Xpedition Designer Navigator window, choose the Project tab. Under Nets, choose the following by doing a Ctrl+click operation: A_OUT, FB, FETOUT and PWM_GATE. 
3. Click anywhere within the Extract Parasitics dialog box to load them into the Selected Nets pane, as seen in Figure 2
4. In the Layout section of the dialog box, choose 'Browse for existing layout file (.cce file):' and click the 3 dots to the right to browse for a file.
   1. Navigate to the project directory
   2. Within the PCB folder, open the Output sub-folder
   3. Choose the PowerSupplyBoard.cce file and click Open
   4. Change the Solver and Advanced settings so they match those in Figure 2. The minimum and maximum frequency values define the range in which the HyperLynx Hybrid solver will extract the PCB parasitics.
   5. Click OK to run the parasitic extraction. The Output Window shows messages that describe the status of the extraction.
   
   Figure 2: Extract Parasitics dialog box settings
    
   Open the Netlist Settings dialog box.

   1. Go to Simulation > Netlist > Netlist Settings
   2. Ensure that within Scope, Complete Design is selected
   3. Ensure the Include Parasitics in netlist box is checked
   4. Click OK to close the dialog box

   
   Generate the Parasitic Simulation Netlist.

   1. Click Simulation > Netlist > Netlist
   2. The generated parasitic netlist can be viewed under the Simulation tab in the Xpedition Navigator Window
      1. Click TestBenches > PowerSupplyBoard > Files > Spice Files
      2. Click on the PowerSupplyBoard.cir file to open it in an Xpedition Designer window
      3. There is an entry in the netlist called XParasitics
      Begin the Simulator.
      1. Within the PowerSupplyBoard schematic window, click Simulation > Simulate. This will open the Simulation Control dialog box.
      2. Enter the same settings as before:Within the Simulations tab:
         1. Experiment name should be set to expt1.cmd
         2. Time-Domain Analysis should be enabled
         3. End Time set to 170u
         4. Within the Results tab:
            • Under Time-domain Waveforms choose All Waveforms from the dropdown menu.
      3. Click OK to start running the simulator. The Waveform Analyzer should automatically open with the results loaded into it once the simulation is done running.
      Note: You will notice that the four signal names in the Waveform List now appear with slight changes. The new format is <original net name>_<symbol reference designator>-<symbol pin number>. So "FB_C3-1" indicates the the FB net is connected to a symbol with a reference designator of C3, on pin number 1.
      
      Analyze the results of the parasitic effects in Waveform Analyzer by plotting the following waveforms. 
      
      Plot the parasitic waveforms on to the same graphs as the original circuit waveforms by dragging the name of the parasitic waveform from the Waveform list pane on to the box of the corresponding original waveform's graph.
      
      Plot:
      • A_OUT_U1-2 with A_OUT
      • FB_U4-1 with FB
      • FETOUT_U2-1 with FETOUT
      • PWM_GATE_U2-2 with PWM_GATE
      When finished, your window should look like Figure 3.
       
      
      Figure 3: The parasitic waveforms graphed with the original waveforms
       
      Use the graphs to analyze and compare the results of running the original simulation and the one that included the PCB parasitics.
       

      Search Terms:

      • Parasitic Extraction

      • Parasitic Effects

      • Parasitic Results

      • PCB Parasitics

      • AMS Parasitics Extraction