0
\$\begingroup\$

I am trying to simulate a 100 kHz FitzHugh-Nagumo oscillator in OrCAD Pspice capture (this paper gives the motivation for the configuration, but is for a 180 Hz oscillator, https://ieeexplore.ieee.org/abstract/document/6313098). I have built this oscillator and have the differential equations, but we are trying to troubleshoot some discrepancies between experiment and simulation at a high level. The ODEs look okay for an individual oscillator, so I want to reproduce a single oscillator in PSpice. We are using a fancy op-amp with a 50MHz bandwidth, AD844 (datasheet: https://www.analog.com/media/en/technical-documentation/data-sheets/AD844.pdf) which does not appear as a simulate-able component in Pspice.

I am not an electrical engineer, so please humor me with what I hope are reasonable questions. I am pretty new to PSpice as well.

First question: what is another high bandwidth op-amp that does appear in Pspice? I have been hunting for an hour and I'm not getting any closer.

Second: if there isn't a suitable built in op amp, is there a way I can enter values from the datasheet into a generic op-amp shell? There appears to be this kind of a method for Multisim, but I can't find this interface for OrCAD Pspice.

FHN oscillator

My FHN: C1=13 nF, R3=100 Ohm, R1=110 Ohm, R2=100 kOhm, L1=100 uH.

Edit: I should comment that we are using AD844 rather than LM358, a more normal 1.2 MHz bandwidth op-amp, because the LM358 doesn't seem to support oscillation. I don't know why that is--I wouldn't be surprised if the LM358 clipped the waveform a bit, but it doesn't move at all. This is a separate mystery that I also welcome commentary on.

\$\endgroup\$
1
\$\begingroup\$

Pick an appropriate op-amp, download the Spice model from the manufacturer and install it in Orcad.

This TI document Using Texas Instruments Spice Models in PSpice covers it, with the specific example of the THS4131 145MHz fully differential op-amp.

Follow all the instructions-- you need to add the library as indicated or you'll just get errors.

\$\endgroup\$
0
\$\begingroup\$

The oscillator builds in amplitude, until R3 dissipates just as much energy as provided thru R1.

Does the LM358 have enough gain-bandwidth to support an oscillation at your Fres? And to drive a 100 ohm load (R1).

I'd also look carefully at the phaseshifts on the Vin- pin. 100Kohm seems way too high for operation with 1uS (100Kohm and 10pF or more Cin of the opamp).

Regarding the opamp model: edit the unity gain bandwidth of the PSPICE model. There likely is an R+C in the 4-terminal gain element used in the opamp. Adjust that tau to match the 844.

Also consider changing the Rout of the 844 model.

And slewrate.

\$\endgroup\$
  • \$\begingroup\$ I am using 100 kOhm because the original (180 Hz) paper used that value with an LM741 opamp. I retained a value of 100 kOhm because....... it oscillated when I hooked it up. Could you briefly give an insight into the role of that resistor? That paper used R1=2.4k, R3=1k, and R2=100k. Since I am cutting the other resistances by ~10x, would I want to cut R2 by 10x? Or what should I do instead? Thanks very much. \$\endgroup\$ – KBL Dec 18 '18 at 18:38
  • \$\begingroup\$ At 100K || 100K, and 10pF assumed opamp+parasistic capacitance, you'll have about 0.5microSecond delay and 45 degree phaseshift at 300KHz, thus about 15 degree phaseshift at 100KHz. Given the phaseplane trajectory is part of the successful behavior, I'd cut the R2 (and R2) down to 10Kohm, so the phase shift is about 1 degree at 100KHz. By the way, these beasts need a non-linearity. Is that the current-limiting, or hitting the VDD, or slewRate? or what? \$\endgroup\$ – analogsystemsrf Dec 19 '18 at 3:55
0
\$\begingroup\$

At its bare simplest, an ideal opamp is a high gain VCVS, or VCCS with proper termination. To mimic some gain bandwidth, use the VCCS with a parallel RC at the end, here's the netlist:

G1 0 out in+ in- {Aol/Rout}
C1 out 0 {Aol/(2*pi*GBW*Rout)}
R1 out 0 {Rout}

Where Aol is the open loop amplification (linear, not dB), Rout is the output resistance/impedance, and GBW is the gain-bandwidth product.

This has no limits, so it will happily simulate kV and up. You can add two anti-series Zener at the end for that, or a more involved commanded JFET circuit. If you also want input impedance, add a resistance, or a complex network of RLC, if you want... Here's the part where I stop and point out to @Spehro Pefhany's answer if you want more finesse.

\$\endgroup\$
0
\$\begingroup\$

So along the lines of @Spehro's answer, I didn't realize that companies released these files for download. It was pretty easy to find the file, with that insight. Installation was still non-trivial, but this youtube video showed it in exact detail:

https://www.youtube.com/watch?v=t5cQIFGpuNs

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.