OPA1637: noise simulation using PSpice for TI

Hello, 

General Resources:

• For general analysis to compute the contribution of each noise source to the overall, you may be able to apply the technique shown in this Planet Analog article:
  • Use PSpice models to estimate amplifier noise

• Texas Instruments Precision Labs (TIPL) Video Training Noise Analysis Series can be found here
  • Op Amp Series with Noise Section that includes basics of noise sims
  • FDA Series With Noise Section

• Tina Ti Free Download
  • TINA-TI

• Analog Engineers Calculator
  • Calculator Download Link

I used Tina Ti to compare. Tina Ti is a free download from Texas Instruments. I have attached my simulation below as well. You can see my curve below is below 10nV/rtHz. It still isn't perfect but much closer. 

I made the resistors noiseless resistors. In TINA-TI, a noiseless resistor can be simulated by disabling the noise contribution of a standard resistor. This is achieved by setting the temperature of the resistor to absolute zero (-273.15°C), which effectively eliminates thermal noise. TINA-TI allows for noise analysis, and by manipulating component attributes, individual noise contributions can be isolated and evaluated

1.  Standard Resistor Noise Model:

   
   

   In TINA-TI, resistors are modeled as ideal noiseless resistors in parallel with a thermal noise current source. This noise source is a white noise, meaning it has a uniform distribution across all frequencies. 
2. Disabling Resistor Noise:

   
   

   To simulate a noiseless resistor, you need to effectively turn off the thermal noise generated by the resistor. This is done by setting the temperature of the resistor to absolute zero (-273.15°C). This can be achieved by modifying the component's properties within the simulation environment. Double click the resistors and make the settings as shown below:

   
3. Noise analysis in TINA-TI:

   
   

   TINA-TI offers a dedicated noise analysis feature (Analysis > Noise Analysis). This analysis allows you to examine the noise contributions of individual components, including resistors, within a circuit. 
4. Isolating Noise Contribution:

   To isolate the noise contribution of a specific resistor, you can disable the noise of all other resistors in the circuit by setting their temperatures to absolute zero. This allows you to focus solely on the noise generated by the resistor of interest. 

Here is a noiseless resistor macro:

• Noisless Macro

Using the Analog Engineers Calculator we can calculate the noise contribution of the 2k ohm resistors. I believe if you set your resistors to noisless resistors to isolate the noise to the amplifier you will get much closer results like I did. 

OPA1637.TSC

Best Regards, 
Chris Featherstone

Hello Chris,

Thank you for helpful reply. I can understand that need sqrt(s(v(onoise)*v(onoise))) to convert V/sqrt(Hz) to Vrms. And will check TINA-TI later.

Unfortunatelly I can't find use 'noiseless' resister for PSpice. Is there more information? 

Best,

Yasunori Okutsu

Hello Chris,

Added option:

@PSPICE:
.OPTIONS PRINT_NOISE_CONTRIBUTORS=10

seems work well. Thank you.

But adding "NOISELESS=YES" to the resistors properties, seems to be ignored. The result is:

**** Top Contributors To Output Noise [DeviceName = TotalDeviceNoise (Contribution percentage)] ***
X_U1.X_U1.D1 = 6.390E-15 (49.26 %)
  R_R1 = 3.315E-17 ( 0.26 %) 
  R_R3 = 3.315E-17 ( 0.26 %)
  R_R2 = 3.315E-17 ( 0.26 %)
  R_R4 = 3.315E-17 ( 0.26 %)
X_U1.X_U1.R4 = 2.497E-17 ( 0.19 %)
X_U1.X_U39.D1 = 2.389E-18 ( 0.02 %)
X_U1.X_U40.D1 = 2.389E-18 ( 0.02 %)
X_U1.X_U39.R4 = 2.404E-19 ( 0.00 %)
X_U1.X_U40.R4 = 2.404E-19 ( 0.00 %)

In stead, I added "R_NOISELESS " before the value:

The result is same as your's TINA-TI.

Best regards,

Yasunori Okutsu