Creating Bode plots using PSpice and PSpice A/D with Schematics

PROBLEM:
How do I Create Bode Plots Using PSpice and PSpice A/D with Schematics?

SOLUTION:
In Schematics:

Draw your circuit schematic, including DC power supplies.
Use a Vac symbol as the input (stimulus) source, and edit its attributes to set ACMAG=1.
Double-click the wire that represents the output node and label it OUT.
In Schematics, from the Markers menu, choose Mark Advanced select VCB, then place it on the output wire/node.
Repeat Step 4 for a VPHASE marker.
From the Analysis menu, choose Setup, then click AC Sweep. Define the sweep's type, range, and resolution.
From the Analysis menu, choose Probe Setup, then select Automatically Run Probe After Simulation.
From the Analysis menu, choose Simulate.

When the simulation ends, Probe starts and displays the dB and phase traces. In Probe:

From the Plot menu, choose Add Y-Axis.
Below the x-axis, click the text Vp(out). It turns red when selected.
From the Edit menu, choose Cut.
From the Edit menu, select Paste.

Notes

Markers can be placed or moved on the schematic after simulation.
PSpice is not case-sensitive, so both m and M mean milli (1E-3); 3m, 3M, and 0.003 are all the same. Type Meg for mega (1E6), e.g., 3MegHz.
AC Sweep is a linear analysis, so it is amplitude-independent. If the input is unity with no phase, then the output voltage is the gain, and the phase of the output voltage is the phase response of the circuit. In Probe, dB=20*log10.
To avoid having to repeat the Probe steps after future simulations of this circuit, choose Probe Setup from the Analysis menu in Schematics, and select Restore Last Probe Session.