Functional Simulation with Accusim

1.1 Create a directory under your home for the VLSI class and keep all of your work in there:

>> mkdir egre429
>> cd egre429

Be sure and change into this directory after you login and before you create any new designs for this class.

1.2 Create a directory for this lab and move into it. Then start Design Architect (DA):

>> mkdir lab1
>> cd lab1
>> adk_da &

1.2 In DA open a sheet called inv and use the Libraries->ADK Libraries menu item and then click on the SDL Parts item in the palette to bring up the library of transistors that you will use to develop your IC cells. Use your knowledge of DA to create a schematic of an inverter using PMOS and NMOS devices, VDD, GND, and portin and portout components. Don't forget to connect the body contacts of the transistors and change the width of the PMOS device to 10 from the default. The resulting schematic should look like the one below:

1.3 Check and save the sheet and exit DA
 

Accusim is the Mentor version of the Spice simulator and works much like PSpice that you are familiar with. We can use the transient analysis mode to simulate the function of the circuit to ensure that it is performing correctly.

1.1 Create an Accusim viewpoint for your inverter design:
 

 >> adk_dve inv


Note that this viewpoint is created inside the inv directory so you will not see it and this command also creates other viewpoints that you will use later for LVS and SDL.

1.2 Invoke Accusim on your inverter design:
 

 >> accusim inv/accusim &


This will bring up the Accusim window shown below:



1.2 Once Accusim is loaded, you should see your schematic. The first thing that we need to do is to set up the analysis type. Do this using the Setup Analysis icon in the palette menu. Since you will be performing a transient analysis, you need to press the Transient button to get the dialog box for setting up a transient analysis. You should use a time step of 1 ns and a stop time of 500 ns. Leave everything else at its default value. The dialog box should look like this when you are done:



Click the OK button to exit the dialog box.

1.3 Next, you need to set the input forces. Select signal in1 and then use the Add Force icon or menu to add a force. This should be a pulse type force with an initial value of 0 V and a pulsed value of 5 V. The pulse width should be 200 ns with no delay and a period of 400 ns. The Add Force dialog box should look like this:


 
 

Note that the signal that you selected is listed as is the //GND as a reference. Click OK when done.
 

1.4 To trace the input and output values, select both the in1 and the out1 signals and press the trace button on the palette menu. A chart window with an Analog trace of both signals will open.

1.5 Before you can run the simulation, you must tell the simulator what the models are for your FETS. The model names are "tp" and "tn" for the P- and N-FETS, respectively. There is a model file in $ADK/technology/accusim/ami05.mod that you can use for the AMI 0.5 micron process To load a model file, use the File->Auxiliary Files->Load Model Library menu. You can then enter the filename with your models in it. Use the navigator to go to the $ADK directory and navigate into the technology/accusim directory. Load the above file and click OK.

1.6 Now type run in any window to run the simulation (or use Ctrl-F1). The result should be a chart of the values on in1 and out1 as shown below.



1.7 Make the chart window active and print it using the File->Print->Active Window... menu item. Exit Accusim.
 

Like PSpice, Accusim can be used to perform other analysis as well. Here we will examine the voltage transfer characteristic of the inverter using Accusim.

1.1 Restart Accusim on your inverter:
 

>> accusim inv/accusim &

1.2 Select the in1 signal and THEN press the  Setup Analysis icon in the palette menu. Press DC Sweep and notice that the Positive Net and Negative Net are already set to /in1 and /GND already.  Set the From and To values to 0V and 5V respectively. The result should be a dialog box like this:

Click OK when you are done.

1.3 Trace the in1 and out1 signals and load the ami05 model file as before and type run in the window to run the simulation. The result should be a chart window like that shown below:

1.4 Print the chart window and exit Accusim.
 

Based on the tutorial prepared by David Zar.