Advertisement

Article

Use PSpice models to estimate amplifier noise

While it may be relatively easy to estimate amplifier output noise in cases involving simple amplification or where noise is dominated by flat-band noise, it is fairly complex to do so when the individual noise sources (i.e. thermal, device 1/f, and so on) operate over varied bandwidths and / or where noise is not dominated by the amplifier’s flat-band region.

PSpice is a good tool for computing output noise in these cases and it also simplifies “what if” investigations. This article outlines proper PSpice techniques to simplify the task and shows an example which would be inherently more difficult using other estimation techniques.

Using PSpice to estimate noise
For more complex amplifiers, various estimation techniques such as PSpice analysis may be employed to obtain the expected output noise. PSpice has built-in commands for calculating output noise density and noise figure. However, the active element or amplifier may not have a complete or accurate noise model to be used by PSpice. Usually, devices designated as “low noise” tend to have fairly accurate noise macro-models but not always.

Also, the flat-band noise model may be fairly accurate but the 1/f region noise may not have been modeled. It is beneficial to have a technique which allows the use of PSpice for numerical analysis of a circuit to simplify noise bandwidth determination and integration even though the amplifier noise model itself may be questionable in terms of full proof accuracy. One such technique is explored below. This technique also allows the user to quickly analyze “what if” scenarios such as replacing an amplifier with one that has different noise, etc.

Figure 1 shows a hypothetical, yet realistic example:


Click to Enlarge Image
Figure 1: This is an example of an amplifier circuit which cannot be analyzed for noise by simple inspection

In the figure, the National Semiconductor LMV772 amplifies the tiny output current of a photo diode for further processing. There are several factors that complicate this circuit beyond simple analysis:

  • 1/f region noise needs to be taken into account. In the 1/f region, a designer has to deal with a noise density that varies with frequency and therefore calculations involve performing a finite integration.
  • The various noise sources operate over differing bandwidths and determining these bandwidths’ requires rigorous calculation.
  • The choice of operational amplifier itself needs contemplation for cost and performance reasons. To determine output noise for more than operational amplifier would require calculations to be repeated many times.
  • Individual transfer function calculations from each source to the output are not trivial and are also frequency dependant.
  • Amplifier parasitic elements, such as input common mode capacitance, affect frequency response and therefore noise bandwidth.

Direct PSpice noise simulation

The equivalent circuit of Figure 2 can be directly imported to a PSpice program along with the macro-model of the active components (in this case that of the LMV772).


Click to Enlarge Image
Figure 2: With Photodiode equivalent circuit inserted, the circuit can be directly imported into PSpice for noise analysis

The LMV772 model accurately represents the input-referred noise voltage of the device, both in the flat-band and in the 1/f region. The determination of RMS noise becomes a simple task as PSpice allows the “Vout” pin to be designated as the output node and automatically generates the spectral noise density [V/SQRT(Hz)] at that node (depicted as “V(onoise)” in PSpice).

The RMS noise is the square root of the integral of this V(onoise) squared, over the entire frequency range. The following expression in PSpice Probe will display this result in Volts: “SQRT(s(V(onoise)^2))”

(The “s” in the expression above refers to the integral of what follows (in this case the squared value of output noise density).

Some PSpice programs do not allow the use of the squaring function (^2). This can be circumvented by using the following expression which simply multiplies the argument by itself to arrive at the squared result: “SQRT(s(V(onoise)*V(onoise)))”

For the circuit of Figure 2, here is a screen-capture of Probe result:


Click to Enlarge Image
Figure 3: Use the cursors on the Probe display to read total RMS noise within a range of frequency

To read the value from the PSpice Probe screen, simply put the probe cursors between the frequencies of interest. The cursors placed between 1Hz and 1MHz (or >1MHz) yield an output noise reading of 4.39mV_RMS as shown above.

Next, let’s consider the option when either the noise macro-models are questionable or it is more important to know the individual contribution of each noise to the overall value.

Indirect PSpice noise simulation

PSpice can be used to simplify some of the tedious calculations involved with predicting noise even if the active components do not have accurate noise models. In this case, the simulation is used for additional calculations to arrive at the output noise and is herein called “indirect simulation.” With this method, PSpice is used to calculate the gain from each noise source to the output, over the frequency range, without necessarily invoking the noise simulation. The PSpice Probe can then be used to show gain frequency response for each noise source. The task of predicting RMS noise is then handled separately, perhaps by employing a spreadsheet, using the results of these PSpice gain simulations.

Here is a step-by-step set of instructions to carry out the indirect PSpice noise predication along with the results obtained when applied to the circuit of Figure 2 shown in Italics :

Step 1: For each noise source, simulate the output voltage with PSpice running “AC” analysis and with that source frequency swept. This involves running one AC analysis simulation for each source. Resistor thermal noise is modeled as a shunt current source across the particular resistor (as shunt elements are slightly easier to add and delete in PSpice than series voltage sources).

Figure 4 is the resulting circuit for RF thermal:


Click to Enlarge Image
Figure 4: For each noise source, construct a circuit to calculate that source’s gain referred to the output

Results for the other sources are not shown here but are procedurally similar to the one already shown. The other sources for the circuit of Figure 2 are: U1 Input noise voltage U1 Inverting input noise current U2 Input noise voltage U2 Inverting input noise current R2 Thermal R3 Thermal RD Thermal

Step 2: Use the PSpice Probe function to display the output voltage divided by the input, in other words, calculate gain for each source.

The result of simulating the circuit of Figure 4 is shown in Figure 5 with PSpice Probe displaying “Vout/ I_RF_thermal” gain (or “V(9)/ I(I_in”), in this case for the particular node names used):


Click to Enlarge Image
Figure 5: Use the Probe cursors to read the gain and the bandwidth of the RF thermal noise response

Step 3: For each simulation, note the peak gain and appropriate –3dB bandwidth (or –3dB roll off frequencies). Use a spreadsheet to organize and manipulate the results obtained.

In Figure 5, note that the cursors are placed at 70.7% (-3dB) of the peak response in order to read the lower and the upper –3dB frequencies (“f1” and “f2” in Table 1 below). This information is tabulated below in Table 1 for all significant sources identified in Step 1. RF thermal noise entries (labeled as Noise “source # 5” row) are highlighted for emphasis.


Click to Enlarge Image
Table 1: Enter individual gain and the lower (f1) and upper (f2) frequencies in a table for easy manipulation and tracking

Step 4: Multiply the gain from Step 3 by the noise-source magnitude and the square root of the noise bandwidth, to arrive at the contribution of that particular source to the overall output noise. Multiply single-pole response results by a 1.25 factor [SQRT (pi/2)] to compensate for the non-brick-wall behavior. For more accuracy, Application Note OA-12 (www.national.com/OA/)A-12.pdf) explains more accurate correction factors for band-pass response for various peaking values. For the purposes of this article, the 1.25 factor stated above is used throughout, as this simplifies the task of explaining the procedure.

For resistor thermal noise magnitude, here is the rough equivalent shunt noise current at room temperature: i_R_thermal 4pA/RtHz / sqrt [ R(Kohm)] So, for example, a 100 kO resistor would have a 0.4pA/rt-Hz noise source across it.

Table 2 shows the results with columns G, H, and I added to Table 1:


Click to Enlarge Image
Table 2: Here is the tabulation of individual noise contributions with “source magnitude” and “noise out” added

Note that the entry made for “U1 noise voltage” in Table 2 (15nV/RtHz in row 1, column G) is a “visual average” of the LMV772 noise voltage (Figure 6 ) for the range from 12Hz (f1) to 78KHz (f2).


Click to Enlarge Image
Figure 5: Estimate the LMV772 input noise voltage within a band by “eye-balling” this chart

By nature, this sort of approximation is very rough and it should be noted that the analysis outlined above is to get “ball-park” values and cannot be very exact.

If the individual gain frequency responses are more complicated than, for example the band-pass response of Figure 5, one could make other “visual average” estimates of its value and the upper and lower effective frequency and enter them into the spreadsheet. The value of this form of indirect analysis is mostly in how it makes the individual source’s contributions stand out relative to the total, and this sort of 1st order approximation is certainly acceptable, at least as a first-cut type of analysis.

Again, the tabulation for RF_thermal is highlighted in Table 2 (labeled as Noise “source # 5” row). Here is the RF_thermal calculation in detail for reference:

Column G:

Column I:

Step 5: Use the spreadsheet to square the individual source noises and add them all up before taking the square root to arrive at the overall RMS noise from all sources.

Here is the final tabulated result:


Click to Enlarge Image
Table 3: This is the final spreadsheet showing individual noise contributions and the total

The final answer is shown at the bottom right-hand side with a value of “4.99mV_RMS” for all six noise sources combined together. Compared to the value found with direct PSpice noise simulation earlier (4.39mV_RMS), there is a difference of about 14% which would be reasonable for such an approximate indirect analysis.

Here is how the final answer was calculated:


Click to Enlarge Image

Note that the steps outlined above only use PSpice for noise contribution gain calculations and do not rely on accurate active component noise macro-models. However, having reliable noise data is necessary to have even when the indirect PSpice method is used. Further, once the spreadsheet is complete, there is no ambiguity as to which noise sources are dominant and to what extent.

This is in contrast with the direct-simulation technique, where the result does not indicate the dominance of any of the contributing factors. For example, it is clear here that RF_thermal is the most dominant noise contributor.

Another advantage of this indirect PSpice method is that now, with the spreadsheet completed, it is easy to investigate “what if” scenarios. For example, if the LMV771 with its extremely low-input noise current (0.001pA/RtHz) is replaced with a bipolar input device, such as the LMV721, which has an input noise current value of 0.3pA/RtHz, the spreadsheet can be used to immediately predict the new output noise:

With LMV721 instead of the LMV772, the “U1 noise current” component of output noise (row 2, column I in Table 3) would be:

For a new total output noise of:


Click to Enlarge Image

So, the output noise would increase to 12.4mV_RMS and U1 input noise current becomes the most dominant noise source replacing RF_thermal.

Conclusion
This article explored some ways to utilize the advantage of PSpice in simulating noise behavior even in the absence of accurate or complete noise macro models. The direct and indirect PSpice noise simulations introduced will expand the user’s arsenal of analytical tools to tackle noise estimation problems. The indirect simulation method was explained in detail to familiarize the user with it as a useful tool in identifying and isolating the dominant noise sources in a system. This will allow easy cost-benefit analysis and will allow the user to make more informed decisions.

About the Author
Hooman Hashemi is in Applications Engineering at National Semiconductor Corp, Amplifiers Group, www.national.com. He can be contacted at hooman.hashemi@nsc.com

0 comments on “Use PSpice models to estimate amplifier noise

Leave a Reply

This site uses Akismet to reduce spam. Learn how your comment data is processed.