Hjem

Rom
- DataSaler
- Auditorier

Teknisk
- Linux
- Windows
- Sikkerhet
- Driftslogg

Avdelinger med info
- IFT
- Informatikk
- UB

Laboratory exercise for building and simulating a simple CMOS inverter in Cadence Virtuoso

Olav Torheim, Universitetet i Bergen, Institutt for fysikk og teknologi, February 2005

To invoke Cadence Virtuoso, type the following from unix shell:

ssh -X mikroserver1
cadence-c35d4
(eller source /prog/design_kits/cadence_init/cshrc.cadence.ams)
ams_cds -tech c35b4

Virtuoso Mixed Signal Design Environment should now start up:

In the "icms" dialog box, choose "File > New > Library".

In the "New Library" dialog box, you must give the library a name (for example TORLIB, as I did). You must also specify a technology file. Here you choose "Attach an existing techfile". Then click the OK button. When asked for technology, choose TECH_C35B4.

After successfully creating the new library, it is time to create your first design. In the "icms" dialog box, choose "File > New > Cellview". In the "Create New File" dialog box, you must give the design a name (for example "torcell", as I did). You must also specify which library the design belongs to, and here you specify the library that you have just created (in my case, TORLIB).

Now click OK, and the Virtuoso Schematic Editor should pop up. We will now draw a simple inverter design, as shown in the picture:

To create the inverter design, do the following:

1. Press i or click on the "Instance" icon to invoke the transistors. The "Add Instance" dialog box will now pop up. In the "Library" field, click "Browse" to open the "Library Browser". In the library browser, choose "analogLib" as library, "nmos" (for n-type transistor) or "pmos" (for p-type transistor) as cell and "spectreS" as view. The cell is placed in the schematic by moving the cursor to the desired location and clicking the left mouse button.

1. To insert the voltage sources, pick the "vdc" cell from the "analogLib" library.
2. To insert the ground and vdd nets, pick the "vdd" and "gnd" cells from the "analogLib" library. Here the view name should be "symbol", not "spectreS" (in fact, "symbol" is the only available option).
3. To connect the symbols, press w or click the "Wire (narrow)" icon. Then use the left mouse button to click the nodes togeter, two by two.
4. To remove an instance or a wire, left click at the instance or wire that you want to remove, then press the "Delete" button on the keyboard.
5. To change the properties of the icons, press q or click at the "Properties" icon. Then click at the instances or nets that you want to modify. For the vdc source connected between vdd and gnd, set the "DC voltage" property to 3.3. For the transistors, set the "Width" and "Lenght" properties to "4u" and "1u". For the pmos transistor, set the "Model name" property to "modp". For the nmos transistor, set the "Model name" property to "modn". As we will see later, the "modn" and "modp" models correspond to SPICE simulation models used by the simulator in the Analog Environment.

1. To check and save the schematic, press X or click the "Check and save" icon. Make sure you get no errors or warnings. Then open "Tools > Analog Environment". The "Virtuoso Analog Environment" should now come up:

1. Choose "Setup > Simulator/Directory/Host" and set spectreS as your simulator.
2. Choose "Setup > Model Path" and add directory "/prog/hk_37/spectreS/c35/cmos53/tm" to your model path.
3. Choose "Simulation > Netlist > Create Raw".
4. Choose "Outputs > To be plotted > Select on Schematic". Click at the "vdc" node connected to the inverter input, the drain node of the nmos transistor and the net connected between the drain nodes of the nmos and pmos transistor.
5. Choose "Analyses > Choose". We will now run a dc analysis to obtain the DC transfer characteristics of the inverter. Choose "Component parameter" as your sweep variable. Then click at "Select component". In the schematic, click at the input "vdc" instance. In the "Select Component Parameter" dialog box, choose dc as your sweep parameter. The sweep range should go from 0 to 3.3.

The analog environment should now look like this:

1. Choose "Simulation > Run".
2. After the simulation has completed, choose "Results > Plot Outputs > DC". The outputs should look like this:

To save your simulation settings, choose "Session > Save state" to save your state information under whatever file namn you want. In a later session, you can reload your saved states using "Session > Load state".