1. global parameter model parameter temperature
Parametric Sweep
global parameter model parameter temperature

2. A parametric sweep allows for a parameter to be swept through a range of values and can be performed when running a transient, AC or DC sweep analysis.
Parameters that can be varied include a voltage or current source, temperature, a global parameter or a model parameter.

3. Global parameter
A global parameter can represent a mathematical expression as well as a variable and is defined using the PARAM part from the Special library.
To define the global variable, you have to add a new property to the PARAM part by editing its properties via the Property Editor.

4. For example, in the resistor circuit shown in the Figure, the value of resistor RL has been replaced with a variable called {rvariable}; you can name the variable anything you like. The braces otherwise known as curly brackets { } are required in PSpice to define global parameters.
The PARAM part has a heading called PARAMETERS: and contains a list of defined variables and their default values. In this case, RL is defined to have a default value of 10 k if no parametric sweep is performed.

5. The global parameter variable name and default value must be added to the PARAM part as a new property in the Property Editor. The PARAM part is found in the special library and is placed anywhere in the schematic page. By double clicking on the PARAM part, the Property Editor will open
When first selected, the Property Editor will open up in one of two modes, displaying the properties in either rows or columns
Change view by double clicking LMB

6. To add a property which allows a global parameter to be swept, select New Row as shown in and the Add New Row dialog box will appear
Add the Name of the variable and the default Value of the variable
Figure shows a parameter called rvariable being defined with a default value
of 10k

7. By default, new property names and values are not displayed on the part in the schematic diagram so they have to be made visible. This is done by highlighting the property cell in the Property Editor and selecting Display. This will open up the Display Properties dialog box as shown in Figure

8. Now we can set up a DC sweep with a Global parameter named rvariable
for a linear sweep from 500  to 100 k in steps of 500 .
Create a new simulation profile, PSpice > New Simulation Profile, and call it anything you like, for example, global sweep.
Select Analysis type to DC Sweep and select the Sweep variable as a Global
parameter with a Parameter name: rvariable. The Sweep type will be linear
with a start value of 500 , an end value of 100 k and an increment value
of 500

9. Place a power marker on the body of RL, i. e
Place a power marker on the body of RL, i.e. in the middle of RL, by selecting
PSpice > Markers > Power Dissipation, or select the icon or
Run the simulation (PSpice > Run) .
You should see the power dissipation curve

10. Another option to use a global parameter:
the current substitution of values in the schema

11. Model parameter sweep
Each component is defined by its model (set of parameters)
Working with models requires knowledge of model type and its parameters
A detailed description of all parameters of the element is in PSpice Reference Guide (Cadence Help)
RMB

12. Model of transistor Q2N2222
Cjc – capacity of junction CB, Bf – h21 , Ise – saturation current of emitter

13. Example of model parameter sweep (h21 = BF)

14. DC analysis setting Type of model: NPN transistor
Name of the model Q2N2222
Sweeping parameter BF
Sweep setup

15. Result of simulation
Uce Ic BF

16. Temperature analysis
The temperature of the circuit is determined by a global variable TNOM which is set in the Options tab of the simulation profile
For semiconductor devices are temperature coefficients included in standard models
For passive elements, we need to enter the coefficients manually

17. Temperature analysis
We can use the library BREAKOUT to enter the coefficients
In this library are „empty“ models: Cbreak, Rbreak, Lbreak, Dbreak etc.
Temperature coefficients

18. Model Parameters for Resistors
Name
Meaning
Unit
Default R
Resistance multiplier 1
TC1
Linear temperature coefficient
°C−1
TC2
Quadratic temperature coefficient
°C−2
TCE
Exponential temperature coefficient
%/°C
Resistor value = R·(1+TC1·(T-Tnom)+TC2·(T-Tnom)2)
Resistor value = R·exp(0.01·TCE·(T-Tnom))

19. Independent sources V – voltage sources I – current sources
An independent source has three groups of parameters:
DC – for DC analysis
AC – for AC analysis
V1, V2, TD, TR, TF, PW, PER, VOFF, VAMPL, PHASE, FREQ – for transient analysis

20. The most commonly used sources - suitable for beginners
VDC – DC voltage source – DC and transient analysis
VAC – AC voltage source – AC analysis (this is not sinusoidal source for transient analysis!)
VSIN – sinusoidal source – transient analysis
VPULSE – pulse source – transient analysis

21. Pulse source

22. Sinusoidal source
VOFF
VAMPL
FREQ TD DF
PHASE