In electrical mode, only properties with certain values and data can be entered, and only to objects corresponding to library devices or subcircuit instances.
These properties can be applied to devices and subcircuit instances:
name | the device name given to SPICE |
---|---|
param | the device initial condition and other parameters for SPICE |
other | anything, not used internally |
nophys | always ``nophys'' |
These properties can be applied to device instances only:
model | the name of a SPICE device model |
---|---|
value | the device value as given to SPICE |
In addition, internally generated properties, such as node numbers, are listed in the display. There can be only one name, model, value, param, and nophys property, but arbitrarily many other properties per device. The name property will always be present. Assigning a name property means that the assigned name will be used in SPICE listings, otherwise Xic will generate a name for the device. Deleting a name property simply deletes the user's name, if any. The other properties are not used internally, and the text can be any string. They are often useful for storing alternate strings for the model, value, and param properties. The nophys property is a flag to indicate that the device or subcircuit has no physical representation in the layout, and will be ignored in LVS testing.
The device line in a SPICE file looks like:
(name) (nodes ...) (value or model)
(param)
The name field is either the name property given, or an internally generated name. The nodes field is internally generated, but optionally passes through a node name mapping as described in 4.14.1. Only one of the value or model properties is used. If both are set, the model has precedence. This is followed by the param (initial condition and parameters) string, if present. The precise format of the strings for each of these properties is determined by the device being set, and the details of the version of SPICE being used. The first letter of a name property should be the character used to key the device type to SPICE. The user should be familiar with these requirements.
In addition, it is possible to apply the param property to subcircuit instances, and also to the current cell with the Cell Properties command. This provides support for subcircuit parameterization, which is available in WRspice and some other simulators.
Unlike all other properties, after changing a param property of a cell, using the Cell Properties Editor or otherwise, all instances of that cell are examined and the param property of the instances may be updated.
Here is a brief description of how to use parameterization. Suppose that you are editing a cell that contains a resistor, and you wish to parameterize the resistor. Give the resistor a value property consisting of some word, say ``rshunt''. Using the Cell Property Editor, give the cell a param property something like ``rshunt=2.5''. This will give the resistor a default value of 2.5 ohms. Editing another cell, place two instances of the previous cell. Note that ``rshunt=2.5'' appears in a label next to each instance. Select one of the labels, and using the label editor change the string to ``rshunt=1.25''. This will change the resistor value in that instance (only) to 1.25 ohms.