Spice Models

SuperSpice may not load in all of the supplied model files. Manually load these in by drag dropping them from the Windows Explorer file manager, or by navigating from the model folder with a right button click. These models are located in the \SuperSpice\System folder.

Not all of the SuperSpice symbols are attached to spice models so some symbols placed on the schematic will not initially simulate. Standard Spice models and sub circuits (subckts) are freely available from all the main semiconductor manufactures web sites. e.g. On-Semiconductor, National Semiconductor, Texas Instruments etc. These models are easily attached to existing symbols in SuperSpice by button clicks.

SuperSpice has a model library manager which mangers the models and subcircuits that are in these model text files. Often each manufactures model/subcircit file contains just one model, so it might be better to copy all the models of similar function into one big file. Just make sure that the file has an extenuation of .mod or .lib. Drag the model file from the Windows Explorer to the SuperSpice main window for it to be added to the SuperSpice library manager. You can then place any existing symbol and double-click or “q” it to attach the model in the library to that symbol.

PSpice Models

PSpice is not always compatible with the industry standard Spice3/XSpice syntax. See PSpice for more information

BSim3.3.2.4

The BSIM model supported in this version of SuperSpice/XSpice is the BSim3.3.2.4 version released by Berkeley on 21st December 2001. The BSim3.3 version is currently the industry standard, supported by most i.c. fab houses. The BSim3 model is selected by the LEVEL=8 setting in its .model statement. This is equivalent to HSpice Level=49. SuperSpice will convert the level number automatically, however, specific HSpice extensions to the BSim3 model are ignored.

The "M", number of devices in parallel extension to the BSim3 model has been implemented in SuperSpice. In addition to Length and Width, the parameter "M" has been added to the mosfet parameter list. This parameter is the number of devices in parallel. The mosfet setup dialog allows direct setting and display of L, W, and M.

The BSim3 model was redeveloped by the BSIM3 group of the University of California At Berkeley, http://www-device.eecs.berkeley.edu/bsim/?page=BSIM3

BSim4 Version 4.8

This version also includes the November 1st, 2013 Berkeley release of the BSim4 code. This is model level=14. The "M", number of devices in parallel extension to the BSim4 model has also been implemented in SuperSpice.

The BSim4 model was redeveloped by the BSIM4 group of the University of California At Berkeley, http://www-device.eecs.berkeley.edu/bsim/?page=BSIM4_LR

BSIMSOI2.2.2

The Berkeley BSimsoi (silicon on insulator),15th Feb 2001 model code has also been implemented as of 16th October 2001. This is Level=9.

MOSFET AS AD PS PD NRS NRD SuperSpice Extension

Extra parameters "ws" Width of Source and "wd", (Width of Drain) have been added to the ".model" parameters. This forces SuperSpice to automatically calculate and include the relevant AD AS PS PD parameters in its netlist line for the device. Alternatively, if the HSpice length of heavily doped diffusion parameter "hdif" is given, ws and wd will be assigned the value of 2*hdif. More information is at Mosfet labels

These parasitics can be selectively enabled/disabled in the mos setup dialogue so to account for "butting" or adjacent devices. That is, so that the parasitics are not included twice.

Note: Serious mosfet i.c. design usually requires support of the above parasitic parameters. High frequency response can be in error by as much as a factor of 3. That is, a simulation might indicate a response of 3Ghz, when in fact it is only 1Ghz if these parasitics are not included..

Mosfet Binning

SuperSpice supports automatic selection of mosfet models based on the model parameters WMAX, AMIN, LMAX, LMIN. These parameters specify over which rang of Length and Width each model is valid for. To use this feature, models must have names in the following format.

model_type_name.1_xn

model_type_name.2_xn

model_type_name.3_xn

That is, the part of the name before the period is that main model name. Excepting for the the last 3 characters, in this case _xn, the characters after the period identify each separate model. Theses characters do not have to be numbers. The Last 3 characters are the selection of models based on week/slow, nominal, strong/slow types, and are described in the section on worst case analysis.

SuperSpice will examine the width and length for each model on the schematic, and search the model files for a model that will match.

Model and Sub Circuit Attachment

Contents