Quick Tutorial: Graphing the Open Loop Gain of a Circuit in PSpice

October 23, 2013 Team EMA

Graphing the Open Loop Gain of a circuit can be a challenging and time consuming task in PSpice because of a few difficulties with the tool that have been overcome in the latest hotfix (V16.6 S017).


Shortcomings of Previous Versions of PSpice


The first problem was the amount of time that simulating the circuit to get all the data would take.  If you want the responses from a wide variety of frequencies and only want to run the simulation once, you can only have one set duration for the simulation which meant that your high frequency signals will have to run a LOT more times than your low frequency signals.  


This means that your CPU will be busy crunching a lot of data cycles for your high frequency signals and the higher you go in frequency, the longer the simulation takes (exponentially).


Once you have all the data collected, the second problem is turning the collected time domain information into something that is quickly readable (ie a Bode plot).  You could make equations and pull data out and have it plotted but this required a lot of clicks and a fair amount of knowledge.


In the latest version of PSpice, these problems have both been removed to make graphing the open loop gain of a circuit a simple and quick operation.


I’m going to be going over the example FRAEXAMPLE.opj in the C:\Cadence\SPB_16.6\tools\pspice\capture_samples\anasim\fra directory (make sure you have hotfix S017 to see this directory) with just a few slight modifications.



Solving with Middlebrook’s Method


By using ‘Middlebrook’s Method’ on linear, closed loop systems, we are able to determine the open loop response.  This is done by injecting small test signals in a point of the circuit where a low impedance drives a high impedance.  A point like this can usually be found in a SMPS design where the power supply drives an amplifier input.  At this point in the feedback loop, the current gain should be zero and the voltage gain can be used as the loop gain.


Using a Text Block as a Simulation Profile

The first new feature in PSpice is the ability to use a text block on your schematic as your simulation profile.  This may seem like a step backwards back to the days of hand entering SPICE netlists but in this case, it gives us the flexibility to add a formula into the total simulation time field.


Taking a look at the simulation profile that’s been set up as a text block in the FRAEXAMPLE file, we see:

.TRAN  0 {5/Freq} 
.options MINSIMPTS = 1000


Where the:


@PSpice: - means that the tool should look at this text block for the profile information

.TRAN 0 {5/Freq} – means that we’re doing a transient simulation with no specific minimum step size (the 0) and a total simulation time of 5/Freq which equates to 5 periods at whatever frequency we’ll be running in a particular sweep case (see next item).  


The ability to put an equation in the value for total simulation time means that it will take just as much CPU time to run the low frequency signals as it does for the high frequency signals because it’s doing just 5 periods regardless of frequency.  This is the first part of solving our first problem of taking too much simulation time.


In the FRAEXAMPLE, it would take about 30 minutes of CPU time and have an extremely large .DAT file without this vs. about 5 seconds to run the complete simulation using this variable total simulation time and a tiny .DAT file that’s consequently easy to manage.


.STEP DEC PARAM FREQ 0.1 1MEG 7 – means that we want to sweep a parameter called FREQ logarithmically by decade from 0.1 Hz to 1 MHz taking 7 samples per decade.


.PROBE64 P(FREQ)- is a new parameter in this latest hotfix that allows the parameter FREQ swept above to be stored in the 64-bit Probe output results as it will be used in calculating the FRA (Frequency Response Analysis) in later steps.


.options MINSIMPTS = 1000 – is another new parameter in this hotfix that is used to force the simulator to take an adequate amount of time points for each simulation run.


Normally the Minimum Step Size is used to accomplish this but in this case, with the frequency constantly changing, that’s not possible without again increasing the CPU simulation time for the low frequency signals that have to take a lot of sample points to keep up the resolution on the high frequency signals.  This is the second part to solving the simulation taking too much time.


Simulating and Viewing the Results

When the simulation is run, the results look pretty meaningless and messy but there is a lot of important details stored in there.  First, you can see that the simulation end point changes with each of the traces, this is what saves us a lot of simulation time.



Let’s take a look at the data from a single simulation sweep, the first simulation run (FREQ=0.1Hz).  You can do this by adding the traces you want to see with an @1 sign afterwards which indicates that you just want the results from the first simulation run.


We can verify from this is that there are only 5 periods of data, next we want to understand the relationship between V(A) and V(B).  V(B) appears to be out of phase by 180 degrees with respect to V(A) at 0.1Hz.


Dividing V(A) by V(B) tells us that it’s 49,751 times larger than V(B) which is the amplification at 0.1Hz.


To collect another sample data point, let’s take a look at the last (50th) simulation run (FREQ=1 MHz) to see what the relationship is there:



V(B) appears to be lagging by 90 degrees with respect to V(A) at 1 MHz.  Dividing V(A) by V(B) tells us that it’s 4.97 times larger than V(B) which is the amplification at 1 MHz.


Frequency Response Analysis (FRA)


We could do this type of individual measurement for all the frequency points or even set up a global measurement that would do it for us at all frequencies but once you have that data, how do you look at it in PSpice?


With the new FRA functionality you can get all the measurements done and plotted in a few mouse clicks without any expert knowledge.


In PSpice, click on Tools > FRA… which will open up this TCL window



The only thing that you should need to set is the names of the nets on either side of your voltage source which in this example is V(A) and V(B).  Hit OK.  It’ll work for a second to do the necessary computations and present you with a new tab containing a blank window when it’s finished.

To show the FRA, go to Trace > Add Trace… and choose Plot Window Templates from the drop down in the upper right corner, then select either “Bode Plot – separate(1)” or if you want to see the results in dB choose “Bode Plot dB – separate(1)” and finally click on the word Gain on the left.  


Those three clicks should result in the Trace Expression at the bottom containing “Bode Plot - separate(Gain)”. Hit OK.



This will give you the Bode plot that you were expecting with the Gain at the top and the Phase at the bottom.



We can verify that it makes sense against our original results obtained above:


  • At 0.1 Hz, the phase shift was 180 degrees and the gain was 49.7k.
  • At 1 MHz, the phase shift was 90 degrees and the gain was 4.9.


If you had picked to see the results in dB instead, they would look like this, nicely showing the 20dB/decade rolloff:



Video Demonstration




Note that this technique can be used for Switch Mode Power Supply designs and nearly any other design that you need to take a look at the open loop gain for, not just OpAmp circuit’s like the one above.


Hopefully this helps you to understand how the new features in PSpice 16.6 S017 can help you quickly and easily plot the open loop gain of a circuit in just a few minutes.  Stay tuned below for a video describing these same capabilities with a few additional details.



Thanks for reading through this post and please add a comment if you have any questions or feedback.

Previous Article
OrCAD Capture 16.6: Catch Design Issues Quickly with Custom DRC's
OrCAD Capture 16.6: Catch Design Issues Quickly with Custom DRC's

Have you encountered hanging wires and overlaps with Capture wires and want to be able to find these quickl...

Next Article
What's Good About PSpice IBIS Model Support? It’s in the 16.6 Release!

PSpice 16.6 now provides IBIS model simulation capability. This often requested feature supports: SPICE cir...

OrCAD Free Trial

Try OrCAD Today