Creating a Library and plotting MOS I-V characteristics

In this section you will learn how to create your library and create a simple schematic/cell view to simulate NMOS I-V characteristics and plot various MOS parameters thereof.

1. From File Menu click on File->New->Library, a new library dialog-box appears. Enter a library name, eg tutorial and hit OK. See figure 4 below:

Figure 4. New Library Dialog-box

2. As you hit OK, a new dialog-box appears. Check the box corresponding to "Attach to an existing techfile" and hit OK, as shown in figure 5:

Figure 5. Technology File for New Library File Dialog-box

3. In the new dialog-box which appears choose "tsmc18rf" and hit OK.

Figure 6. Attach Design Library Dialog-box

4. You would see "tutorial" in the list of libraries in Library Manager. Next select "tutorial" library in Library Manager and click on File->New->Cell View. A new cell view dialog-box appears as shown in figure 7. Type in "mosiv" in Cell Name and make sure that View Name is "schematic" and Tool is selected as "Composer-Schematic" and Library Name is "tutorial". Hit OK and a Virtuoso Schematic Editing window will open up.

Figure 7. New Cell View Dialog-box

5. With Virtuoso Schematic Window selected hit 'i' key, an Add Instance dialog-box will show up. Click "Browse" button, a Library Browser window will open up. Select tsmc18rf Library, Mosfets from Category, nmos2v from Cell and symbol from View column. Go back to the Add Instance dialog-box and change l (M) property to 'l' and w (M) property to 'w' as shown in figure 8. At this point you have configured NMOS properties and are ready to place an instance in your schematic. So, go back to Schematic Editing Window and you would see a ghost of the NMOS device symbol, place it anywhere in the dotted black area and hit escape key.

Figure 8. Add Instance Dialog-box for NMOS

6. Following the same procedure, add a voltage source and a ground into your schematic. The voltage source can be found in analogLib->Sources:Independent->vdc->symbol. The voltage source configuration in shown in figure 9. Ground component is available in analogLib->Sources:Globals->gnd->symbol.

Figure 9. Add Instance Dialog-box for DC Voltage Source

7. In order to wire the placed component. Hit 'w' to enable wiring tool. Click on NMOS gate terminal and layout the wire to connect to positive terminal of DC voltage source, finally clicking on the positive terminal of the voltage source to end the wire. Similarly connect NMOS drain and body terminals and negative terminal of voltage source to the gnd component. Finally hit escape key to end wiring. The schematic now looks as shown in figure 10. Save the schematic by clicking the save button (highlighted in figure 10).

Figure 10. Intermediate State of the Schematic

8. Now hit 'c' key and click on gate DC voltage source to make a copy of it. You would see a ghost voltage source symbol. Place the copied voltage source close to NMOS drain. Hit escape key to end copy. Now select the copied source and hit 'q' key. An object property editor window will open up; change the DC voltage property to "vds". You will observe that the object highlight box color changes to pink in the schematic. Make sure that in the property editor window "Apply to" is selected as "only current instance" and hit ok. Wire the copied voltage source as shown in figure 11. Hit check and save button and make sure that CIW window does not show any errors.

Figure 11. Final Schematic

9. From Tools menu select Tools->Analog Environment. A Virtuoso Analog Design Environment (ADE) Window will open up. Click on Setup->Simulation/Directory/Host. In the setup window, make sure Simulator is selected as "spectre".

10. Select Variable->Copy from Cellview, you will see all the variables defined in schematic show up in "Design Variables" section. Double click on 'w' and change its value to 1u. Similarly, set vgs = 1, vds=1.4 and l=180n.

11. Next select Analysis->Choose... . In Choosing Analysis dialog-box select analysis as "dc" and choose other settings as shown in figure 12 and hit ok.

Figure 12. Analysis Setup

12. Next you need to select the variables to be plotted. Select Outputs->To Be Plotted and then click on the drain terminal of NMOS in the schematic. The current through the drain terminal is added to "Outputs" section of ADE. Double click on the output and check the "saved" checkbox and hit "change". Quit the "Setting Outputs" dialog-box by hitting OK. The current state of ADE window looks as shown in figure 13:

Figure 13: Virtuoso Analog Design Environment Window

13.Click on Simulation->Netlist and Run. When the simulation completes, you will observe a plot similar the one shown in figure 14. The axis labels have been intentionally removed because of confidentiality of the values.

Figure 14: NMOS Ids vs Vds

14. Output resistance (ro) of a NMOS is the inverse of the slope of the above plot. This mathematical operation can be performed by using calculator tool. Click on Tools->Calculator... . In the calculator window select "dc" tab and check "wave" checkbox. Now go the plotted waveform and click at any point on the waveform. The waveform expression is copied into the calculator. Next select "deriv" operation from listed operations in calculator, followed by "1/x" operation. Change plot option to "New Win" and click on "Eval" button. A new plot of ro is generated as shown in figure 15b. The calculator window settings are shown in figure 15a. You may want to play around with the calculator utility and try plotting mobility, gm etc of NMOS.

Figure 15a. Calculator Window