Free Trials

Download a free trial to find out which Altium software best suits your needs

Altium Online Store

Buy any Altium Products with few clicks or send us your quote to contact our sales


Download the latest in PCB design and EDA software

  • Altium Designer

    Complete Environment for Schematic + Layout

  • CircuitStudio

    Entry Level, Professional PCB Design Tool

  • CircuitMaker

    Community Based PCB Design Tool


    Agile PCB Design For Teams

  • Altium 365

    Connecting PCB Design to the Manufacturing Floor

  • Altium Concord Pro

    Complete Solution for Library Management

  • Octopart

    Extensive, Easy-to-Use Component Database

  • PDN Analyzer

    Natural and Effortless Power Distribution Network Analysis

  • See All Extensions
  • Live Courses

    Learn best practices with instructional training available worldwide

  • On-Demand Courses

    Gain comprehensive knowledge without leaving your home or office

  • Altium 365 Viewer

    View & Share electronic designs in your browser

  • Altium Designer 20

    The most powerful, modern and easy-to-use PCB design tool for professional use


    Annual PCB Design Summit

    • Forum

      Where Altium users and enthusiasts can interact with each other

    • Blog

      Our blog about things that interest us and hopefully you too

    • Ideas

      Submit ideas and vote for new features you want in Altium tools

    • Bug Crunch

      Help make the software better by submitting bugs and voting on what's important

    • Wall

      A stream of events on AltiumLive you follow by participating in or subscribing to

    • Beta Program

      Information about participating in our Beta program and getting early access to Altium tools

    All Resources

    Explore the latest content from blog posts to social media and technical white papers gathered together for your convenience

    Altium Online Store

    Buy any Altium Products with few clicks or send us your quote to contact our sales


    Take a look at what download options are available to best suit your needs

    • Documentation

      The documentation area is where you can find extensive, versioned information about our software online, for free.

    • Training & Events

      View the schedule and register for training events all around the world and online

    • Design Content

      Browse our vast library of free design content including components, templates and reference designs

    • Webinars

      Attend a live webinar online or get instant access to our on demand series of webinars

    • Support

      Get your questions answered with our variety of direct support and self-service options

    • Technical Papers

      Stay up to date with the latest technology and industry trends with our complete collection of technical white papers.

    • Video Library

      Quick and to-the-point video tutorials to get you started with Altium Designer

    Filter Transfer Function and Pole-Zero Analysis in Altium Designer

    Zachariah Peterson
    |  April 5, 2020
    Filter Transfer Function and Pole-Zero Analysis in Altium Designer

    I remember spending hours on circuit analysis problems in my electronics classes, and I learned to analyze all sorts of filter/amplifier configurations by hand. The circuits were usually tractable with Ohm’s law and Kirchoff’s laws, as long as there was no feedback in the circuit. Circuits for advanced applications, such as wideband or multiband matching circuits for RF components, can quickly become difficult to analyze by hand.

    But as the number of resonant frequencies in a complex filter exceeds 2 or 3, the problem can quickly become intractable. At this point, the problem usually involves decomposition or direct solution of a 3rd degree or higher polynomial, which becomes unmanageable by hand. Even as a math guy, I’m no fan of higher degree polynomial problems. Fortunately, when dealing with complex filters, you can determine many aspects of signal behavior

    Analyzing a Complex Filter Circuit

    The circuit shown in the schematic below is a rather complex filter. While you may not encounter this type of filter in general practice, you’ll come pretty close when you’re designing a matching circuit for a multiband antenna. In this circuit, the source (V2) sends a signal into a bandpass filter, and the output from this portion (the voltage across the capacitor) is input into the bandstop filter. The output voltage from the filter is measured across L3 and C3. This filter circuit was built using the generic components in the Miscellaneous Devices.IntLib library. The sinusoidal source (V2) can be found in the Simulation Sources.IntLib library.

    Schematic for calculating a filter transfer function
    Schematic for a complicated bandpass/bandstop filter.

    A simple analysis of this filter would say that there are two important poles; a peak in the output voltage at the bandpass RLC resonance frequency, and a zero in the output voltage at the bandstop resonance frequency. In reality, this is not correct. This is because capacitor C1 and inductor L1 also participate in resonance with the band-stop portion of this circuit, creating a complicated resonance structure in the circuit’s transfer function.

    As we will see, there are more than two peaks and zeroes in the filter transfer function. This is normally done by converting the circuit and the input signal into the Laplace domain. In general, the transfer function can be written as a fraction of products, as shown in the equation below.

    Transfer function equation
    General form of an amplifier or filter transfer function in the Laplace domain.

    In this equation, each z is a zero in the transfer function, corresponding to some frequency and decay rate where the circuit is not allowed to pass an output voltage. Each p is a pole, which corresponds to a peak in the transfer function. In linear circuits without feedback, poles will appear in imaginary conjugate pairs or as fully complex conjugate pairs with negative real part. The real part of a pole will tell you the transient behavior in the circuit.

    If you try to calculate the resonances by calculating critical points in the output voltage, you’ll find that you need to solve a sixth-degree polynomial for the frequencies to determine the critical points. For the circuit above, you’ll still have to solve a sixth-degree polynomial to determine the poles in this circuit. While this problem is technically solvable, it’s faster to use a SPICE simulator to determine the circuit’s behavior in the frequency domain. Instead of doing this exercise by hand, we’ll solve this problem with a SPICE simulation in Altium Designer.

    Calculating the Filter Transfer Function

    To calculate the transfer function for this circuit, I’ve placed two probes (I and V) at the input and output. The input current will just experience some attenuation or amplification whenever the circuit resonates at its bandpass or bandstop resonances. A comparison of the output voltage measurement (V probe) is compared with the input voltage at a specific frequency to construct a transfer function (see the above equation).

    To get started, create a MixedSim profile and enable the following analyses:

    • AC Small Signal Analysis: Initially, I’m going to sweep the input frequency from 1 kHz to 5 MHz. I’ve set 5000 sample points on a linear scale.
    • Pole-Zero Analysis: Set the input node to the net with R1 (NetR1_2) and the output node (NetC2_1). Make sure to leave the reference node options set to “0” as this will take voltage measurements with respect to ground. Note that, if there were a component somewhere on the net connected to ground, then you would need to change these options. My settings are shown in the image below. Take a look at this article for more information on interpreting pole-zero analysis results.
    • v2[z] (impedance calculation): In the Active Signals portion of the Analysis Setup window, you can enable the v2[z] signal to see the input impedance of this circuit. Alternatively, you can take the ratio of the input voltage to input current to see the voltage drop across the entire filter network. Be careful when interpreting this calculation in the time domain when working with reactive circuits.
    Filter transfer function calculation setup
    MixedSim settings for calculating a filter transfer function and pole-zero analysis.

    Filter transfer functions are usually shown in a Bode plot. Note that you can extract the transfer function directly, or you can extract the complex transfer function from an AC sweep. A Bode plot is convenient as it shows the magnitude and phase of the transfer function in the frequency domain and in the steady state (after all transients have decayed); this allows you to see how the filter affects both important aspects of input signal behavior in a pair of plots. To enable Bode plot visualization, click on Simulate → probe manager. Make sure the “Complex Function” option for each probe is set to “Bode plot”.

    Filter transfer function and Bode plot setup
    Bode Plot setup in the Probe Manager window.

    Analyzing Your Filter Transfer Function Results

    Once you’ve finished the above setup, you’re ready to run your simulation. Hit F9 on the keyboard or click Simulate → Run Simulation. You’ll see a number of plots in the AC sweep results, and a separate window will appear, which shows the pole-zero analysis results. The circuit above contains 6 poles and 2 zeroes. These are shown in the image below. Note that the units on each axis are in units of angular frequency (rad/s). If you want to examine the behavior in the AC sweep results, then you need to convert to frequency values.

    Two of the poles lie along the negative portion of the real axis (i.e., they have no imaginary part). These values show that you can place a momentary output from the circuit when sourcing with a step function or impulse. However, the output will quickly decay with two superimposed exponential decay rates. The other poles and the two zeros correspond to specific frequencies, the behavior of which can be seen in the AC sweep results.

    Filter transfer function poles and zeros
    Pole-zero results, showing 6 poles and 2 zeros in the filter transfer function.

    The graphs below show the behavior of this circuit in the frequency domain. The zero at 1.453 MHz and the poles at 800.7 kHz and 2.885 MHz are clearly visible in the Bode plot (blue curve in the top graph). The bottom graph shows the phase of the transfer function, however, the zeroes can’t be seen in the output voltage plot (overlaid in the top graph, purple curve). The output voltage graph shows that poles 3 and 4 have gain of ~2.3, and poles 5 and 6 have gain of ~6.

    Bode plot showing the filter transfer function
    Filter transfer function results shown in a Bode plot.

    If you want to go further with this simulation, you can set the input frequency to any of the values for the poles shown in the Bode plot and run a transient analysis. This circuit shows some interesting transient behavior due to the complex resonant behavior for the two portions of this filter circuit.

    You can also see how the impedance varies in time with a transient analysis simulation. An example is shown below. However, an important point to remember here is that this is an LTI circuit: the impedance does not actually vary in time. To calculate the impedance of the entire circuit from simulation data, simply take the input voltage across the circuit divided by the current. Because of the phase difference between voltage and current in this type of reactive circuit, you may need to separate the terms into magnitude and phase, just like was done in the Bode plot above.

    Filter transfer function simulation results showing transient behavior
    Apparent time-dependent impedance and output voltage across inductor L3/capacitor C3 (in series) showing the transient behavior in this circuit for poles 5/6.

    The pre-layout analysis tools in Altium Designer® let you do more than just analyze filter transfer functions for linear circuits. You can examine noise immunity, transient behavior, temperature effects in your circuits, and much more. You can then capture your schematic as an initial layout and design all aspects of your next PCB. You’ll also have a complete set of tools for documenting all aspects of your project, managing your supply chain, and preparing deliverables for your manufacturer.

    Now you can download a free trial of Altium Designer and learn more about the industry’s best layout, simulation, and production planning tools. Talk to an Altium expert today to learn more.

    About Author

    About Author

    Zachariah Peterson has an extensive technical background in academia and industry. He currently provides research, design, and marketing services to electronics companies. Prior to working in the PCB industry, he taught at Portland State University. He conducted his Physics M.S. research on chemisorptive gas sensors and his Applied Physics Ph.D. research on random laser theory and stability. His background in scientific research spans topics in nanoparticle lasers, electronic and optoelectronic semiconductor devices, environmental sensing and monitoring systems, and financial analytics. His work has been published in over a dozen peer-reviewed journals and conference proceedings, and he has written hundreds of technical blogs on PCB design for a number of companies. Zachariah currently works with other companies in the electronics industry providing design, research, and marketing services. He is a member of IEEE Photonics Society, IEEE Electronics Packaging Society, and the American Physical Society, and he currently serves on the INCITS Quantum Computing Technical Advisory Committee.

    most recent articles

    Back to Home