Spectrum Software
Industrial Strength Simulation




Spectrum Software has released Micro-Cap 11, the eleventh generation of our SPICE circuit simulator.

For users of previous Micro-Cap versions, check out the new features available in the latest version. For those of you who are new to Micro-Cap, take our features tour to see what Micro-Cap has to offer.




Questions and Answers


Question: When I run AC analysis in a circuit with more than one source, how can I tell which source is providing the AC stimulus?

Answer: In AC analysis each waveform source contributes AC signals as follows:

Pulse Source: Fixed at 1

Sine Source: Fixed at 1

V (SPICE voltage source): Specified by user, defaults to 0

I (SPICE current source): Specified by user, defaults to 0

User Source Value of expression in selected user file

Battery or Fixed Analog Fixed at 0

Typically, only one source is used to provide an AC stimulus and the AC value is set to 1.0. All others are usually set to zero.

Question: How do I plot or print energy?

Answer: Energy is obtained by integrating one of the power expressions. For example, suppose you wanted to see the energy stored in an inductor versus time. Here is the expression you’d use:

Since PS(L1) is the power stored in the inductor L1 we need only integrate to get energy like this:


SUM(PS(L1),T ) integrates the expression P(L1) over time to produce the energy stored in L1.

To see the energy stored in the entire circuit, use the PST (Power Stored Total) variable like this:


To see the energy dissipated in the entire circuit, use the PDT (Power Dissipated Total):


To see the energy generated by all the sources in the circuit, use the PGT (Power Generated Total)


Question: How do I add a new NMOS model with my own parameters?

Answer: First select the DNMOS component for placement from the Component menu / Analog Primitives / Active Devices / DNMOS. Then click in the schematic to place the part. When the Attribute dialog box comes up, enter any model name you wish, like IRF711A. This instantiates a model with default parameters. To edit them manually click on the Edit button and edit the parameters as needed. If you already have a model statement for the part, paste it into the text area before placing the part and the program will pick it up and place its name in the Attribute dialog box’s model list. Click on the name to select the part and its model.

If you select a model name from the list, then edit one or more of its parameters, its modified model parameters become local to the circuit file.

Question: How do I handle a model parameter that uses an expression?

Answer: MC6 can handle formulas or expressions in model parameters if the formula is enclosed in braces ( e.g. VTO={2.5-TEM/100} ), and if the variables used have been created with a .define statement. MC6 cannot handle simulation variables like TEMP (operating temperature) that are only known when the simulation is run. Future versions will be able to do this but MC6 cannot. If you have a model that includes a parameter formula that uses say the TEMP simulation variable, the way to handle it is this. Change the variable name in the formula to TEM. Then add a .define command like this:


Here TEM acts as an alias for the expected temperature of the run.

Each time you run an analysis at a new temperature, edit the command statement to the new temperature value. Of course, you cannot step temperature during the analysis this way, as that would require multiple values of temperature.

Return to the main Newsletter page