Spectrum Software
spacer
Industrial Strength Simulation
select:

divider

 

News:

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.

 

divider

 

Stepping

 

How do I step the duty cycle of a pulse source?

 

There are two methods for stepping the duty cycle: stepping multiple parameters or stepping a symbolic parameter. Let's use a 1MHz pulse source whose model statement is initially:

.MODEL PULSE1 PUL (VZERO=0 VONE=5 P1=100N P2=110N P3=400N P4=410N P5=1U)

Stepping Multiple Parameters
In this case, both P3 and P4 should be stepped. Go to the Stepping dialog box. For this example, the part name of the pulse source will be V1. Parameter 1 should appear as:

Step What V1
P3
From 200n
To 700n
Step Value 100n

Parameter 2 should appear as:

Step What V1
P4
From 210n
To 710n
Step Value 100n

Set the Change option to Simultaneous. Both parameters must have the same amount of steps to step simultaneously. In this case, the duty cycle is being stepped from 10% to 60%.

Stepping a Symbolic Parameter
For this method, the pulse model statement needs to be changed to the following:

.MODEL PULSE1 PUL (VZERO=0 VONE=5 P1=100N P2=110N P3=cycle P4=cycle+10n P5=1U )

A .define statement needs to be added to define the cycle parameter. It should appear as following in either the schematic or the text area:

.define cycle 500n

Go to the Stepping dialog box. Change the Parameter Type option to Symbolic. Step the Cycle parameter such as:

Step What Cycle
From 200n
To 700n
Step Value 100n

This produces the exact same response as the first example.

 

 

 

 

Categories


AC Analysis
Analysis - General
DC Analysis
Dynamic DC
Incompatibilities
Initial Conditions
Miscellaneous
Models
Monte Carlo
Output
Probe
Schematic Editor
Stepping
Transient Analysis