NI Multisim and Switch Capacitor Filter Design

Hello all,

I am wondering if someone could help me with designing a 5th Order Butterworth LPF using a Switching Capacitor topology in NI Multisim 13.0?

I am trying to replicate a design used in "Design with Operational Amplifiers and Analog Integrated Circuits" by Sergio Franco in Figure 4.33 using Ideal components, where the component values have been worked out in Example 4.13 for f_c = 1kHz at a f_ck = 100kHz and providing the following capacitor values:

C_Ri = C_Ro = C_0 = 1pF, C_C1 = C_C5 = 9.84pF, C_L2 = C_L4 = 25.75pF, and C_C3 = 31.83pF.

The circuit looks like so (note all components are Ideal):

View attachment SC 5th Order Butterworth - Circuit.pdf

With the heirachal inverting blocks implemented like so:
View attachment SC 5th Order Butterworth - Circuit - Inverting Switch Block.pdf
View attachment SC 5th Order Butterworth - Circuit - Inverting Switch Block 2.pdf

The resulting Bode Plot is nothing like a LPF:
View attachment SC 5th Order Butterworth - Bode.pdf

The Transient @ 100Hz looks somewhat reasonable, though it is clipping on the negative swing:
View attachment 5th Order Butterworth - Transient @ 100Hz.pdf

And the Transient @ 1kHz is starting to go wrong:
View attachment 5th Order Butterworth - Transient @ 1kHz - 2.pdf

But then @ 10kHz, it completely disappears:
View attachment 5th Order Butterworth - Transient @ 10kHz.pdf

For reference, here are my clock pulses (clk_phi and clk_phi_bar):
View attachment SC 5th Order Butterworth - Clock.pdf

Can Switched Capacitor circuits be simulated in NI Multisim 13.0?

As it is, I had a convergence problem and needed to relax ABSTOL to 1e-008A and VNTOL to 0.0001V in order to simulate the results. Someone had mentioned that because the convergence is being done at specific points in time, that a switched capacitor system might not be able to simulate correctly, and especially wouldn't bode plot correctly.

Eventually I want to implement this circuit topology with a 7th Order Butterworth and a clock that is upwards of 10MHz, but for the present, I would be satisfied with just getting this circuit to work as expected.

Multisim Circuit Files can be found in the zip file below:
View attachment SC 5th Order LPF.zip

Thanks for the time and assistance.

In general you should be able to simulate a switched-capacitor circuit in any Spice simulator but it may take a long time for each simulation, especially for high clock speeds. And yes, since the Bode plot assumes linear components, that simulation mode won't work to plot the switched-cap frequency response. You will have to use various fixed frequencies at the the filter input and use the Transient Response mode to plot their corresponding output values.

Switched-capacitor circuits can be simulated in the time domain (TRAN analysis) only, unless the S/C blocks are replaced by time-continuous equivalent blocks. Based on these linear replacements it is possible to display the frequency-dependent transfer characteristics (BODE plot).

For SC verification there are analysis such as pss, pac, pnoise ... https://www.designers-guide.org/analysis/sc-filters.pdf, which are available with spectre. I don't know what is available in spice and MULTISIM, but I am almost certain that there should be something similar.

PS: The final verification is always done with transient analysis, at least in my cases.

BR Jerry

helpmejerry said:

For SC verification there are analysis such as pss, pac, pnoise ... https://www.designers-guide.org/analysis/sc-filters.pdf, which are available with spectre. I don't know what is available in spice and MULTISIM, but I am almost certain that there should be something similar.

Click to expand...

No - there are no Spice-based simulators that can create a BODE plot for S/C circuits without prior replacement of the time-dependent parts.

No - there are no Spice-based simulators that can create a BODE plot for S/C circuits without prior replacement of the time-dependent parts.

Click to expand...

While not being a spice expert, a quick look at hspice manual https://cseweb.ucsd.edu/classes/wi10/cse241a/assign/hspice_cmdref.pdf

.HB Invokes the single and multitone harmonic balance algorithm for periodic
steady state analysis.

.HBAC Performs harmonic-balance–based periodic AC analysis on circuits operating
in a large-signal periodic steady state.


From my understanding these two analysis should suffice to perform periodic ac analysis on an SC circuit and create the bode plot. I was able to do this in spectre so it realy shouldnt be an issue.

BR Jerry

Hi Jerry - thank you for the info. It`s new for me - however, it`s never too late to learn. I did a lot of S/C ac analyses (Bode plot) with PSpice, but always based on time-continuous S/C replacements.

Happy to help. I am not sure that PSpice has .HB and .HBAC analysis so if anyone has more info please let us know.

BR Jerry

Simple AC analysis wouldn't work for bode plots in case of SC circuits because of varying operating points.
There is an analysis called FRA (frequency response analysis) available in Pspice which allows calculating frequency response by means of transient analysis. This requires inserting small amplitude sinusiod in the loop.

mvaseem said:

There is an analysis called FRA (frequency response analysis) available in Pspice which allows calculating frequency response by means of transient analysis. This requires inserting small amplitude sinusiod in the loop.

Click to expand...

I suppose, it is a rather new feature, isn`t it?

Yes it is new feature. I observed it in recent ISR of 16.6 release.