Transistor Labels

Bipolar Labels

The "M" text field sets an overall scaling factor for the device model. For example, if the diode connected transistor of a current mirror was set to 1.0, and the output transistor was set to 2.0, the mirror output would be twice the input current. The M (area) factor effectively sets how many parallel devices there are.

The parameter text field may be used to pass extra additional parameters to models, if required, for example:

Parameter text field set to: voffset=1.01

With a model specified as:

.model (... is={2.5e-16*1.01} ...)

This allows the same model to be varied an individual instance basis. Parameter variables may use any user specified name, except for m, area, width and length.

See Bipolar Labels for more information

Use Model Default L & W For Discrete and IC MOSFETS

Check this button to use standard models as supplied by a discrete parts vendor. This is the usual case for discrete components. These models usually assume a fixed W and L of 100u, and therefore do not require L and W to be set. Setting this check will cause the L and W fields to be ignored. AS and AD checks will also be ignored.

Uncheck this button if you desire to set the L and W of the model manually. This is the usual case for i.c. based components.

Mosfet Labels

Set the Width (W) and Length (L) and the number of devices in parallel (M) in the appropriate fields.

See also Device Designer. Device designer allows for the automatic calculation of mosfet values based on desired voltages and currents.

Note: For BSim3 models, M is a true parallel number of identical devices, implemented directly in the engine by multiplication factors in the core code. For other mosfet types, w is simple multiplied by M.

SuperSpice extension parameters are "ws" Width of Source and "wd", (Width of Drain) has been added to the ".model" parameters. Alternatively the length of heavily doped diffusion, hdif can be specified, from which ws=wd=2*hdif. This forces SuperSpice to automatically calculate and include the relevant AD AS PS PD NRD NRS parameters in its netlist line for the device from:

AD=wd * W

AS=ws * W

PD=2*wd + 2*W

PS=PD=2*ws + 2*W

NRD = wd/(2.W)

NRS=ws/(2.W)

"ws" and "wd" are the width of the source and drain area. This area is the region that contains the contact strip to the source or drain. "ws" and "wd" will usually be a little larger then the contact width.

AD=area of drain region

AS=area of source region

PS=perimeter of source

PD=perimeter of drain

NRD=number of squares for drain resistance, this value multiplies the rsh parameter to obtain parasitic drain resistance.

NRS=number of squares for source resistance, this value multiplies the rsh parameter to obtain parasitic source resistance.

W=Channel width

L=Channel length

Enable AD/Enable AS

Un-checking these buttons will disable and set to zero the AD PD/AS PS area and perimeter factors calculated above, respectively. This allows adjacent devices to to be modeled correctly. That is, one device might have its AS enable off, whilst a butting/next to device might have its AD enabled on. This means that the capacitance of the joined region will only be included once, as required.

Reserved Parameters

Models have reserved, key parameters of:

length, width, area, m

These names should not be used for user parameter variables, but they may be used as variables in model functional expressions. They are calculated automatically for ic resistors, ic capacitors, bipolars and fets. The calculation for "area" automatically includes "m", the device multiplier.

Contents