Cadence Design System

Notes on Using Composer and Analog Artist

to set the default unit scale (such as mm instead of meters) go to Tools®CDF®Scale Factors... in the CIW. In the default auto mode, sub-micron gate lengths will be specified in nanometers with significant digits extending into the sub-angstrom regime.

Openbook Tutorial: IC Tools®Tutorials and Flow Guides®Composer Tutorial
Openbook Documentation: IC Tools®Schematic Entry®Composer: Design Entry Help
use Design®Create Cellview®From Cellview command to generate a symbol from a schematic, or vice versa.
parameterized components: use pPar("CDF_parameter_name")in the properties form for the parameter. For example, parameterize the gate width with W=pPar("wp").When Create Cellview-From Cellviewis used, the symbol will contain this parameter, which can be adjusted in the the parent cell. If the cell is used as a top level cell, the parameter can be specified by adding a user property to the Edit®Properties®Cellview... dialog box to give the parameter a value.
dependent parameterized components: use iPar("CDF_parameter_name")to inherit parameters from the instance itself. For example, to make the AD of a MOSFET a function of the channel width, defineAD=iPar("w")*5u
Passing design variables from Analog Artist to components in Composer

in Composer, use a string for the parameter that you wish to vary. For example, specify the width of a transistor to be "wp".
in Analog Artist, go to Variables®Edit... and enter each variable and its value. You can also use Variables®Copy from Cellview to copy any unlisted variable in the schematic to the Design Variable pane.
look under the Analog Artist section to see how to sweep variables (Parametric Analysis)

Openbook Documentation: IC Design®Analog and Mixed-Signal Simulation®Analog Artist Simulation Help, Analog Artist Parametric Analysis Help, Component Description Format (CDF) User Guide
Setup®Simulator/Directory/Host -- be sure to specify the full path for your project; specify what simulator to use here (e.g. hspiceS).
the Save State command doesn't seem to save the path for the project and always defaults to ~/artist.
Model File options:

put each model in its own file (e.g. one file for PMOS, one for NMOS)
name the file nnnnnn.m where nnnnnn is the model name (case sensitive) used by the components in your schematic
inside the file, each line that continues must end with an '&', instead of a '+' on the beginning of the next line; this is Cadence Spice style
remove all extraneous spaces from the model, including around '=' symbols
parameters are passed through '&n' where n is the parameter number. &1 is the model name, so the first two lines of the model might be

.model &1 NMOS &

LEVEL=49 TOX=5.50e-09 &

put the entire path to the directory containing these files in the Setup®Model Path... dialog box. Note that you can specify various simulation corners (such as normal, fast, slow, etc.), and then put the models for each corner in a separate directory.

create an include file that has an .include statement for your model; you can leave your model in standard Spice format

create design variables as described above under Composer
Tools®Parametric Analysis... to set up the analysis
Temperature sweeps: In the variables window define a variable tempdc. Cadence will recognize this variable as temperature and it can then be used in parametric analysis.

put input pins in the schematic wherever you want to put stimulus sources
graphical editor: I always got the following error message: "Could not find source, vdc, in refLibs," which prevents the editor from figuring out how to configure the the dialog box for each type of source. I tried setting up a refLib and searched the documentation, but couldn't figure out how to fix this problem.
text editor:

In schematic, use Check and Save to extract the schematic before running LVS.
In Virtuoso, place pins on nets that leave the cell. These are correlated with the pins in your schematic.