Post Go back to editing

Simulating ADA4505 noise against datasheet specifications

Category: Datasheet/Specs
Product Number: ADA4505

When reviewing the ADA4505 datasheet there are many different noise specifications (peak-to-peak voltage noise, voltage noise density), what is the best way to review /simulate these in LTspice?

  • From a datasheet, you can usually get information about different types of noise, the terminology spectral noise density, RMS noise or peak to peak noise can usually be found.

    Lets use the following schematic to work through this in ltspice.

    Run a '.noise' simulation using the following command .noise V(VOUT) V1 dec 100 1 1MEG

    The datasheet for the ADA4505 provides the following information:

    •  voltage noise density of 65 at 1kHz
    •  peak-to-peak voltage noise of 2.95µV from 0.1Hz to 10Hz


    To capture the 'voltage noise density' from ltspice

    1.  Run the simulation
    2. Display the 'Vout noise' by clicking on 'Vout'
    3. Add a cursor
    4. Drag the cursor to the 1kHz frequency
    5. The noise is shown as Voltage Noise Spectral Density (NSD) and is 65nV/. This corresponds to the datasheet specification.

    To capture the 'p-p voltage noise' you first need to capture the 'RMS noise'

    1. Modify the command .noise V(VOUT) V1 dec 100 0.11 10 to display the output between 0.1Hz to 10Hz as stated in the datasheet.
    2. Run the simulation
    3. Display the 'Vout noise' by clicking on 'Vout'
    4. Hold the 'ctrl' button and left click on 'V(onoise)'. The corresponding 'VRMS noise' in the 0.1Hz to 10Hz frequency band is displayed.
    5. To calculate the 'peak to peak noise', take the 'RMS noise' already captured and multiply it by 6.6.


    For more details on different types of noise, read the article, or check out these videos Calculating Spectral Noise Density to RMS Noise - YouTube & Calculating RMS Noise to Peak-to-Peak Noise - YouTube


    When should noise simulations be carried out?

    • Noise analysis should be carried out to understand the overall noise performance of a complete circuit.
    • Check the performance of individual components and easily verify with the datasheet specification for components.
    • Use the '.NOISE' command when simulating in LTspice to carry out a noise analysis of your circuit, allowing the noise spectral density to be extracted from the circuit shown.
    • The noise simulation covers random noise (e.g. thermal, flicker, shot) that is generated by the components within  a circuit, thus the noise simulation does not comprise of any kind of coupled interference, out of band signal components, crosstalk, power supply harmonics and such.
    • It is important to point out that this kind of analysis is a particular case of small-signal AC analysis, independent from TRAN and AC ones. That is, even though our noise analysis will reveal the existence of noise voltage in our circuit, those voltages can’t be observed in the time domain through a transient simulation or have any effect on a small signal analysis.
    • We are required to specify both an output and an input. The output will be used to indicate where we want to measure the noise and the input where we start to add the noise.

    If you want to learn more or get some additional insights why not check this video out LTspice IV: Noise Simulations - YouTube