MOS Transistor Simulation with Accusim

1. Create a schematic of a MOS transistor circuit with Design Architect

1.1 Make a new directory for your transistor simulations:
>> cd egre224
>> mkdir lab5
>> cd lab5

1.2 Start Design Architect to create the schematic of the circuit for this tutorial:
>> da &
1.3 Use your knowledge of DA to create a new component called circuit1 and construct a schematic for it using generic analog parts that looks like the one below:

Note that the transistor is an NEHN4 component from the Generic Parts library under the MGC Analog Libraries palette. The ASIM_MODEL property on the transistor has been modified to have a value of VN2222LLB and the INSTPAR property has been modified to have a value of L=9U W=13000U. An INST property with the value of NMOS1 has also been added to the transistor in the schematic above although it is not required.
1.4 Check and Save your schematic and exit DA.
1.5 Create a simulation viewpoint for Accusim for the circuit1 circuit with DVE as you did in the previous labs.

2. Simulate your transistor circuit to extract the Id vs. Vds family of curves with Accusim

2.1 Before you start the simulation, you will need to create a model file for the transistor with the Spice model parameters in it. Use the text editor to open a file called VN2222LLB.sp in the same directory where the circuit1 design is located and add the following lines to it:
.MODEL VN2222LLB NMOS
+ LEVEL=1
+ VTO=2.3
+ KP=106U
+ GAMMA=0.4
+ PHI=0.37
+ LD=0.1U
+ LAMBDA=0.0108
Save the file and exit the test editor.
2.2 Start Accusim on your circuit1 design:
>> accusim circuit1 &
2.3 Use the File->Auxiliary Files->Load Model Library... file menu item to bring up the Load Model Library dialog box. Use the Navigator... button to bring up the File Navigator dialog box and select the VN2222LLB.sp file. Click OK in both dialog boxes.
2.4 Select the Vd node in the schematic and use the Setup->Analysis... menu item to bring up the Setup Analysis dialog box.. Setup a DC sweep with Vd going from 0V to 5V and click OK.
2.5 Use the Setup->Results->Define Waveform menu item to bring up the Define Waveforms dialog box. Create a new waveform called Id that is equal to the current going into the drain of the NMOS transistor. Click Close in the Define Waveforms dialog box.
2.6 Use the Setup->Keeps...->Keeps... menu item to bring up the Add Keeps dialog box and click OK to add the default keeps on schematic items.
2.7 Select the 0V voltage source on the schematic and use the Run->Sweep Runs->Property on Instance... menu item to bring up the Sweep Property/Variable dialog box. Click on the Select Property... button and select the instpar=0V property in the dialog box that comes up and click OK. Set the From item to 1.8, the To item to 3.4, and the Step item to 0.2 and click OK in the Sweep Property/Variable dialog box to start the simulation.
2.8 Use the Report->Waveforms menu item to bring up the Report Waveforms dialog box. Click on the top-most ../../results item (probably "/col/run/results (Default)") and click OK. Scroll to the bottom of the results window that comes up and click on the W(Id) item to highlight it.
2.9 Use the Result->Chart->Family of Curves menu item to bring up the Chart Signal from Collection dialog box. Notice that the Signal item is already filled out with the Id waveform we defined earlier. Click on the Choose Collection... button and make sure that the sweep (DCOP) collection is selected in the dialog box that pops up and click OK. Leave the Reference item blank in the Chart Signal from Collection dialog box and click OK in it. The result should be a new chart window like the one below:

3. Extract the Id vs. Vgs curve in saturation for the transistor

3.1 Select the Vd node in the schematic and use the Add->Force... menu item to add a DC force of 3.5V to this node.
3.2 Select the Vg node and setup the analysis for a DC sweep from 1.5V to 3.5V. Click the button to run the simulation.
3.3 Use the Results->Chart...->Chart/Trace Defined Waveforms... menu item to bring up the Chart Defined Waveforms dialog box. Select Id, click on the Trace button, and click OK. The result should be a chart like the one below:

3.4 Select the Id wavform and generate and save a list file of the data as you did for the diode current Id in lab 4.
3.5 Exit Accusim.