I am trying to create a analogique amplification chain between a piezo sensor (10mVPP) and 16 bits ADC in 3V3 range. I try to simulate the chain on LTSpice to get the lower noise density I can get.
@3V3 for 16bits 3.3/2^16 = 50.35 µVRMS for 1 LSB.
When I simulate the noise on a nominalistic chain I quickly go over the ADC LSB only with thermal noise.
I think I misunderstand my result.
In this exemple I just put an OPAMP with gain x400 and two filter HP 1.5 kHz and LP 50 kHz and I already go 523 µVRMS that is 10 times the LSB of the ADC… (This use 4 bits of my ADC just for thermal noise)
Can someone help me to clarify this ?
(I know it's just a simulation and not real life, but I don't understand why I can't go down to 1 LSB on 16 bits on simulation)
Schematic
Noise analysis
Signals
Response
Best Answer
Input voltage noise of the op-amp
Your op-amp has an input noise voltage of typically 1.1 \$\text{nV/}\sqrt{Hz}\$. Your noise bandwidth is 50 kHz x 1.57 (for a simple RC low pass filter). Hence the equivalent noise at your input is: -
$$1.1 \text{nV} \times \sqrt{50,000 \times 1.57} = 308 \text{ nV RMS}$$
Multiply this by the circuit gain (400) and the output noise is 123 μV RMS.
Input current noise of the op-amp
The op-amp also has an input current noise of typically 2.4 \$\text{pA/}\sqrt{Hz}\$. Your input circuit isn't balanced so that produces an equivalent voltage noise source into R2 of 2.4 \$\text{nV/}\sqrt{Hz}\$. Using the same math as above and multiplying by the gain (400) yields an output noise of 268 μV RMS.
Combining the noises
Adding the two noises together (using Pythagoras) means a combined noise of 295 μV RMS.
I haven't tried to calculate thermal noises from resistors nor the low frequency noise of the op-amp because my numbers look close enough to your LTSpice calculation.
Personally, I'd reduce the 400 k and the 1 k feedback resistors to one tenth their value and eradicate the major contributor (the input current noise).
Do you understand now?