Does a simulator specific for active opamp filters exist? - Page 1
Forum section: electronics / projects

author: KerimF
author_rank: Frequent Contributor
timestamp: October 08, 2023, 09:44:41 pm
content: A few years ago, I downloaded ‘Iowa Hills Opamp Filters.zip’. It is a useful, easy to use, design tool.Lately, I was interested in designing a low pass filter (fo ~= 25 KHz, 3-pole Butterworth, Sallen-Key). But I have LM358 only (equivalent to LM324). The problem is that the fo of the real LPF under test is much lower than 25 KHz.So, I had the idea that a simulator (for Bode plot), made specific for active filters, could help in finding out the real characteristics of the opamp under test by trial and error; that is by varying the parameters that define the simulated opamp (while keeping the values of the R's and C's unchanged) and compare the resulted Bode plot to the real one.I tried searching such simulator on the internet for hours in vain.Thank you.Kerim

author: Benta
author_rank: Super Contributor
timestamp: October 08, 2023, 09:53:16 pm
content: TI's WEBENCH Filter Design Tool is good:https://webench.ti.com/filter-design-tool/A tip from me: stay away from Sallen-Key and go for "Multiple Feedback" or MFB instead.

author: Conrad Hoffman
author_rank: Super Contributor
timestamp: October 08, 2023, 11:17:52 pm
content: IMHO, any simulator like LTSpice will give results that are as accurate as your models. That's usually the catch; the models aren't as good as they should be.

author: mawyatt
author_rank: Super Contributor
timestamp: October 09, 2023, 12:39:25 am
content: TI WEBENCH doesn't seem to support Apple OS, so can't comment on this (seems interesting tho, so may have to pull out the PC laptop), LTspice works fine and is the popular GP version of SPICE for most, and available in multiple platforms including Apple OS.The models we've experienced regarding LM324/358 types, tend to be behavioral models and lack fidelity especially regarding the output structure. This is where a "dead zone" created by 3 Vbe junctions between the NPN source and PNP sink devices exhibits a highly non-linear and unpredictable output Z which can wreak havoc on precision circuits. This also creates excess low frequency noise in the constant jumping back and forth across these 3 Vbes in an attempt to keep a feedback system "closed".Usually one "loads" the output to either sink or source a current under steady state conditions to force the chips' predrive to stay on one side or the other of the 3 Vbe drops relative to the output. These are popular op-amps, we utilize them often, but do come with some serious drawbacks, there are certainly better choices, but the LM324/358 are cheap!!!So take caution when applying various models, especially with unknown characteristics and/or sources. The fidelity of results can't be any better than the models utilized within.Regarding Sallen-Key or VCVS.A general tip from us, they are fine if one knows how to properly apply and design such. They have a basic non-inverting transfer function, whereas the MFB exhibit an inverting configuration and may not be suitable in many single supply applications such as PWM low-pass filtering where one is seeking the average of a PWM pulse train.MFB types also require an extra component for a given LP or HP transfer function, altho for gains >1 the VCVS require 2 extra resistors.Where MFB is generally preferred is bandpass filtering (especially narrow band), this is where we often utilized such.Anyway something to keep in mind when applying various active filter typesBest,

author: mawyatt
author_rank: Super Contributor
timestamp: October 09, 2023, 01:17:46 am
content: Quote from: KerimF on October 08, 2023, 09:44:41 pmFor this LTspice would be ideal, but you don't want to use Bode plots and active filters to expose op-amp characteristics.For example you can drive the output of the op-amp DUT with an AC current source to find the output Z vs. frequency, then load the output with a R and repeat, then with DC bias source and sink currents and repeat.After the above task, then look at the dynamic output Z with the AC current source changed to a step at various +- current steps and check the dynamic response.There are so many tests that can be performed with SPICE regarding op-amp characteristics, it would take too long to describe.Doing some of the above mentioned tasks will reveal the nature of the DUT op-amp; is it device level, behavioral, or combination of such? Then compare with data sheet parameters. This is seriously important understanding that is all too often overlooked, and allows one to "visualize" the results of the simulation wrt the models utilized, and all too often these results are totally bogus!!We've spend almost 5 decades doing this, including writing our own specialized simulators for specific use, and appreciate the only link between achieving a first pass successful complex chip design and fabrication is the models and how one interprets the results. Errors, redesigns, gotchas, value changes, and so on are very expensive and career limiting in chip design, so one quickly learns the value of quality models and when simulations are misleading!!Interesting tid-bit about op-amps. Vaguely remember back in ~1970 Solomon had a IEEE paper about the 741 op-amp, and how the inputs would swap polarity when the output was loaded such that thermal feedback from the output active device caused a swapping of the input diff pair!! This was before Fairchild's George Erdi conceived the brilliant Cross-Coupled-Quad Diff pair which alleviated thermal feedback (as well a process gradients). Solomon measured this by utilizing a somewhat Bode type measurement (DC tho) to resolve the open loop response and expose the polarity swap which looked like an sideways "S" in the transfer curve displaced about zero by a few microvolts!! Of course in actual use the inputs swamped out this tiny reversal as larger signal dynamics took over.Anyway, thought some folks might find this interesting.Best,

author: KerimF
author_rank: Frequent Contributor
timestamp: October 09, 2023, 06:14:33 am
content: Quote from: Benta on October 08, 2023, 09:53:16 pmThank you for the link.Unfortunately, since more than 2 decades, I don't have the privilege, due to world's regulations, to visit the sites of TI.After all, it is a design tool, but perhaps it includes a simulator too.

author: KerimF
author_rank: Frequent Contributor
timestamp: October 09, 2023, 06:41:02 am
content: Quote from: Conrad Hoffman on October 08, 2023, 11:17:52 pmYou are right. And LTspice is the simulator I use in these days. But, as you said, its results depend on how good the models on the simulated schematic are.For instance, by using the LTspice models of LM324, I have, fo on the Bode plots is close to 25 KHz. Perhaps the LM324 ICs, I have, are not genuine and their unity-gain bandwidth is less than 1 MHz. I am afraid that varying certain parameters of an LTspice opamp model, in order to get an fo somehow close to the one of the real test, is not simple. I simply assumed that this may not be the case if a simulator is made for active opamp filters only.

author: KerimF
author_rank: Frequent Contributor
timestamp: October 09, 2023, 06:53:05 am
content: Quote from: mawyatt on October 09, 2023, 12:39:25 amThank you for your interesting tips.For instance, the LPF, I am working on, will be used to filter delta bit streams which are made to generate sinewaves after filtering (about 20 KHz down to 650 Hz). The frequency of the delta clock is 2 MHz.

author: magic
author_rank: Super Contributor
timestamp: October 09, 2023, 07:58:31 am
content: Quote from: KerimF on October 09, 2023, 06:41:02 amI have seen different figures in datasheets, from just above 0.5MHz to slightly more than 1MHz.Some datasheets show dependence on supply voltage - higher voltage is faster.Slew rate is some 0.2~0.3V/μs.Maybe you need to adjust your expectations, or use a faster part like at least RC4558 or TL072.