Op Amp Power Supply Connections

Here's a method for setting up power for a dual-supply op amp:

Use the components UA741, VDC, GND_ANALOG, and BUBBLE. Double-click the BUBBLE symbol to name the power nets. Visually disjoint nets with the same name are actually the same net.

"Too Many Opamps"

Designs that use more than about four or five opamp transistor-level models (e.g., uA741) will not simulate due to the device limit in the evaluation version. PSpice does not limit the number of basic devices such as voltage sources and resistors, so an ideal opamp model based on a controlled source may serve your needs just as well. You give up the ability to accurately model saturation and limited-bandwidth effects.

You can replace the uA741 opamp with an ideal opamp model based on a voltage-controlled voltage source (VCVS) called the "E" device in PSpice. Ground the negative side of the output source (as shown below), and use the remaining three pins just as you would for a 3-terminal op amp:

Double-click the symbol to set the gain to a reasonably large value such as 10⁵ or 10⁶ (enter 100000 or 1000000 in the dialog box). Now you have a high gain differential voltage amplifier with infinite input resistance and zero output resistance.

Mutual Inductance

Mutual inductance occurs when two inductors L1 and L2 share some common magnetic flux. The double-sided arrow symbol indicates the mutual inductance M that exists between the magnetically-coupled coils.

The diagrams below show a typical circuit symbol for coupled coils, and its translation into PSpice:

==>

Here's what you do:

1. Place the two inductors as you normally would. The inductor node anchored to the cursor is the dotted terminal.
2. Place the "K_Linear" part.
3. Double-click K_Linear and specify the reference designators for your two coils as the parameters for "L1" and "L2" (in this circuit, L1 in K_Linear happens to refer to an inductor which has the same designator).
4. Set the "COUPLING" parameter of K_Linear to M/sqrt(L1*L2), where M is the mutual inductance.

Frequency Response Measurement

Follow the procedure below to measure the frequency response of a circuit (the results are in the form of a Bode plot):

1. Enter your circuit.
2. Use 'VAC' as the signal source. Set its amplitude to 1.
3. Attach a dB voltage marker to the output node (select 'Markers -> Mark Advanced -> vdb')
4. Open the simulation setup dialog box (select 'Analysis -> Setup') and enable the 'AC Sweep' function. Click the 'AC Sweep' button.
5. Select 'Decade' for 'AC Sweep Type'.
6. Set your start and stop frequencies, then click on 'OK', the click 'Close'.
7. Run the simulation. You should get a PROBE plot of the amplitude portion of your frequency response.
8. If you need the phase response, use the 'vphase' marker on the output node (look for it in the same place as in Step 3 above).