Hi Champs,
I was calculating and simulating the total noise of the following opamp configuration. Apparently the results do not match.
I was wondering why there is so much noise collected at frequencies way beyond the corner frequency (150kHz)? Could somebody explain this? The calculated noise is much lower at around 138uV.
Hey Simon,
After doing hand calculations and simulating the circuit (both of which I’ve attached), it appears that the macromodel is incorrect. Many factors are affecting the AC response that causes the closed loop gain to have problems. Luckily, this was a recently discovered problem and we are already working to correct it.
If you look at the AC response of this circuit you will find a strange zero-pole pair effect after 3MHz—which is shown below.
Ideally, an op amp’s AC response is supposed to roll off constantly at -20dB/decade until the second pole in the frequency response is hit. This “bulging” effect will accrue more area in the noise calculation than the simple brick wall correction factor (KN) used in the hand calculations. This is why you see more noise than expected.
In the attached TINA file, we have added a low pass filter with a cutoff of 2 MHz at the output of the OPA314 in an attempt to counteract this high frequency bump. The response is closer to the calculated values but still not exact. If you download the file, you will be able to see the changes.
Please feel free to go over my hand calculations and see where they differ. I calculated around 143µVrms while you calculated 138µVrms which is agreeable.
I’m sure you’ve already seen it, but just in case you haven’t: TI Precision Labs has an excellent series on noise and how to calculate it. You can find a link to the video here.
I’d also like to mention that you are simulating the OPA314 outside of its recommended voltage range (±2.75V Max). While this won’t affect the noise simulations it will affect performance of other metrics.
Hope this helps,
-Cole
OPA314_Hand Calculations of Noise.docx
OPA314 Voltage Noise Test G.TSC
