User Guide

Chapter 13 Analyzing waveforms
338
3 If the file has multiple sections of data for the selected
analysis type, the Available Sections dialog box
appears. Do one of the following:
• Click the sections you want to use.
• Click the All button to use all sections.
4 Click OK.
Adding traces from specific loaded waveform data
files
If two or more waveform data files have identical
simulation output variables, trace expressions that
include those variables generate traces for each file.
However, you can specify which waveform data file to
use in the trace expression. You can also determine which
waveform data file was used to generate a specific trace.
To add a trace from a specific loaded waveform data file
1 In PSpice, from the Trace menu, choose Add Trace to
display the Add Traces dialog box.
2 In the Trace Expression text box, type an expression
using the following syntax:
trace_expression@fn
where n is the numerical order (from left to right) of
the waveform data file as it appears in the PSpice title
bar, or
trace_expression@s@fn
where s is a specific data section of a specific
waveform data file.
3 Click OK.
To identify the source file for an individual trace
1 In the trace legend, double-click the symbol for the
trace you want to identify (Figure 93).
The Section Information dialog box appears,
containing the trace name and—if there is more than
or press UI
The Simulation Output Variables list in the
Add Traces dialog box contains the output
variables for all loaded waveform data
files.
Example: To plot the V(1) output for data
section 1 from the second data file loaded,
type the following trace expression:
V(1)@1@f2
You can also use the name of the loaded
data file to specify it. For example, to plot
the V(1) output for all data sections of a
loaded data file, MYFILE.DAT, type the
following trace expression:
V(1)@"MYFILE.DAT"
Figure 93 Trace legend symbols.
trace symbols
Pspug.book Page 338 Wednesday, November 11, 1998 1:14 PM