I am trying to build a trans-impedance amplifier circuit using LTC6269-10 opamp. I need to simulate noise density vs frequency for different values of the feedback resistor. Is it possible to simulate using LTSpice? How do I get a similar graph which I have attached?

 

I think so. Here is the help page

.NOISE -- Perform a Noise Analysis

This is a frequency domain analysis that computes the noise due to Johnson, shot and flicker noise. The output data is noise spectral density per unit square root bandwidth.
Syntax: .noise V(<out>[,<ref>]) <src> <oct, dec, lin> <Nsteps> <StartFreq> <EndFreq>
.noise V(<out>[,<ref>]) <src> list <FirstFreq>[ <NextFreq> [<NextFreq> ...]]
V(<out>[,<ref>]) is the node at which the total output noise is calculated. It can be expressed as V(n1, n2) to represent the voltage between two nodes. <src> is the name of an independent source to which input noise is referred. <src> is the noiseless input signal. The parameters <oct, dec, lin>, <Nsteps>, <StartFreq>, and <EndFreq> define the frequency range of interest and resolution in the manner used in the .ac directive.
Output data trace V(onoise) is the noise spectral voltage density referenced to the node(s) specified as the output in the above syntax. If the input signal is given as a voltage source, then data trace V(inoise) is the input-referred noise voltage density. If the input is specified as a current source, then the data trace inoise is the noise referred to the input current source signal. The noise contribution of each component can be plotted. These contributions are referenced to the output. You can reference them to the input by dividing by the data trace "gain".
The waveform viewer can integrate noise over a bandwidth by <Ctrl-Key> + left mouse button clicking on the corresponding data trace label.
The syntax ".noise V(<out>[,<ref>]) <src> list <Freq>" with a single analysis frequency is useful in combination with .step. It allows you to plot noise densities as a function of a stepped parameter as shown in this example.

 

The link which you have sent is showing error.

 

The link which you have sent is showing error.

It came from the LTspice help page.. let me get that for you.

.STEP -- Parameter Sweeps

This command causes an analysis to be repeatedly performed while stepping the temperature, a model parameter, a global parameter, or an independent source. Steps may be linear, logarithmic, or specified as a list of values. The first .step dimension is sorted to be in increasing order so as not to confuse the waveform viewer.
Example: .step oct v1 1 20 5
Step independent voltage source V1 from 1 to 20 logarithmically with 5 points per octave.
Example: .step I1 10u 100u 10u
Step independent current source I1 from 10u to 100u in step increments of 10u.
Example: .step param RLOAD LIST 5 10 15
Perform the simulation three times with global parameter Rload being 5, 10 and 15.
Example: .step NPN 2N2222(VAF) 50 100 25
Step NPN model parameter VAF from 50 to 100 in steps of 25.
Example: .step temp -55 125 10
Step the temperature from -55°C to 125°C in 10°C steps. Step sweeps may be nested up to three levels deep.

The other link is a spice simulation file for download. If you have LTspice you can download it from the help pages. If you don't have it won't do you much good.

 

Hers is the example

 

See

 

What are the steps for simulating pA/root of Hz vs frequency? for the circuit which i have attached?

 

@Bordodynov My hat is off to you. (Tip of the hat). You have a unique and truly amazing skill set.

Спасибо

 

What are the steps for simulating pA/root of Hz vs frequency? for the circuit which i have attached?

This article shows a trick using the "NOISELESS" attribute available in LTSpice to make a noiseless resistor. Add a noiseless resistor to turn the noise current into a noise voltage which can be measured.

https://www.allaboutcircuits.com/technical-articles/using-ltspice-for-amplifier-noise-measurement/

 

Common opinion of noise the lesser the better. Noise is equally unpopular among radio astronomers biomedical
Engineers there are many useful applications for noise like acoustic measurements, instrument calibration antenna tuning, signal jamming, data encryption. But noise is an undesired electronic or electromagnetic signal having frequency components within the frequency range of interest which tends to interfere with reception or detection of a desired signal.

 

Common opinion of noise the lesser the better. Noise is equally unpopular among radio astronomers biomedical
Engineers there are many useful applications for noise like acoustic measurements, instrument calibration antenna tuning, signal jamming, data encryption. But noise is an undesired electronic or electromagnetic signal having frequency components within the frequency range of interest which tends to interfere with reception or detection of a desired signal.

Wasn't that was the whole purpose of the TS's original post?

 

Unfortunately, not only the amplifier but also the photodiode is making noise. The photodiode equivalent in the form of a capacitor is not making noise. Below is an example of the photodiode+amplifier complex. I made the model of the avalanche photodiode myself. This model takes into account noises which depend on the applied voltage to the photodiode.
In my collection of models there is another avalanche photodiode - S8890-05. Also there is a universal photodiode with parameters. In these models there is a third, not a real pin. It needs to be supplied with voltage equal to the power of light.