Post Go back to editing

Spice MODEL for ADA4941

Category: Datasheet/Specs
Product Number: ADA4941-1

Hello,

When performing a noise simulation in LTSpice, the results showed a noise level of 2.0 mV/√Hz at 100 mHz, decreasing toward 0.0 mV/√Hz as the frequency approached 1 kHz. Could you please provide your perspective on this? Specifically, is the simulation correct, is this a characteristic of the device itself, or is there an issue with the model data?



Circuit diagram created by the customer
ADA4941_sim.asc


The customer is creating the circuit schematic in accordance with AN-1495. The specific details are being handled by the customer.

How to create model data for the ADA4941.
1. Download the .cir file from the "ADA4941 SPICE Macro MODEL" section under "Tools & Simulations" on the ADA4941 webpage.
2. Open the LTspice .asc file provided by the customer; then, go to File > Open and select the corresponding .cir file—which should be located in the same folder as the .asc file—by choosing "Netlists (*.cir, *.net, *.sp)" as the file type.
3. Place the cursor on a line in the netlist that begins with ".SUBCKT," then select "Create Symbol" from the right-click context menu.
4. Import the generated .assy data and start the simulation.
5. The curve in the upper left shows the result obtained by applying a probe to OutP.

The customer comment 
I downloaded the ADA4941 SPICE Macro Model from the webpage, built the circuit according to the APPLICATION NOTE (AN-1495), and performed a simulation using LTspice.
After performing a transient analysis and confirming that the differential converter was functioning correctly, a noise analysis revealed noise levels higher than expected.
(Noise is occurring in the mV range.)
Given that this noise level deviates significantly from the device's performance, I suspect there may be a problem with the SPICE Macro Model.
I have attached the circuit diagram (.asc file). Please verify that there are no errors in the low-frequency noise (1/f noise, etc.) settings within the model.

As the customer suggests, could this be due to device performance, or is there a possibility of an error in the simulation methodology or the circuit configuration?

Parents
  • Hi  

    Thanks for the schematic. The circuit and simulation method is correct. The issue is the model itself.

    I reproduced your 2 mV/√Hz result, then tried a simple gain-of-2 circuit using only the model, with ideal sources and nothing else attached. The noise was still far higher than the datasheet. So the model's noise is too high regardless of the surrounding circuit.

    The cause is in how the model's internal noise sources are set up: they aren't given a proper bias, so LTspice ends up producing far more low-frequency noise than the real part has. That's why you only see 1/f noise falling across the whole sweep, with no flat region.

    On your OUT+ question: yes. Feedback should be taken from OUT+.

    For now, please use the datasheet noise specs rather than the model for noise budgeting. I'll bring this to our LTspice model team for review.

    Best Regards,
    Ian

  • Hi Ianguied-san,

    Thank you for your reply.

    I got the issue is the model itself.
    Could please let me know once an improved model has been released.

    Thank you so match.

    Best regards,

Reply Children
No Data

Before You Switch


Switching languages will make ADI Explorer unavailable. Resume your session by switching back to English and reopening ADI Explorer.