What you always wanted to know about TINA-TI but were afraid to ask! (Part 3)


Whether or not you were ever “afraid” to ask about any of the TINA-TI topics we discussed in Part 1 or in Part 2 of this Analog Wire series, I’m hoping that you find my next topic, noise analysis using TINA-TI, useful in your day to day work.

Below are some of the TINA-TI noise simulation features which make it a great analysis and optimization tool:

1. Output RMS noise plot over any noise bandwidth.

  • Integration “lower” and “upper” frequencies are entered when noise analysis is initiated.
  • Use cursor(s) to read RMS noise over any bandwidth.

2. Noise density plot- referred to either input or to the output.

  • Input referred noise density, when compared with signal power, lets you observe SNR directly.
  • Output referred density plot to uncover unexpected peaking which could impact noise.

3. Noise gain frequency dependence is automatically factored in.

The requirements for running noise analysis in TINA-TI are listed below:

1. One (and only one) source designed as input. Can be either voltage or current source!  More than one source situation covered below.

2. At least one output node.

3. Active devices macromodels which include noise behavior.

  • Automatically done in TINA-TI when a part is placed on the schematic.
  • Making sure modelled noise matches datasheet is covered below.

4. Start and stop frequency to be specified

  • These entries define the range of noise density x-axis plots but also determine the output RMS noise integration bandwidth.

Figure 1 below shows the noise analysis panel and where the start and stop integration frequencies are entered.

Figure 1: Noise analysis panel & required frequency entries

 Figure 2 shows the use of cursors to find noise over a narrower band. An example of where this may be useful is to see how much noise can be lowered by filtering unwanted bandwidth.

Figure 2: Total noise over any bandwidth using cursors

If your circuit requires the use of multiple sources, simply follow the instructions in Figure 3.

Figure 3: Multiple source strategy for noise simulation

If you doubt how accurate your device noise model is, use the simulation circuits in Figure 4 to generate the plots (Figure 5) which you can then compare with the datasheet:

Figure 4: Uncovering the modelled noise of a device

Figure 5 shows the plots generated by noise-simulating the Figure 4 circuits. Results confirm good agreement with LMH6629 datasheet plots!

Figure 5: LMH6629 TINA-TI noise model matches well with datasheet

In the course of noise analysis, when curious whether the thermal noise (Johnson noise) of any of your resistors is dominant, replace that resistor with Figure 6 circuit (or its Macro provided in link further below). If you find that, as a result, output noise is reduced, then your circuit noise can be improved by lowering that resistor value (and thereby its thermal noise)! This is viable in many amplifier circuits as circuit operation is not affected if resistor ratios are maintained while the resistor values are lowered for lower noise.

Figure 6: Create a noiseless resistor, that you can place on your schematic, to evaluate thermal noise impact

Click here to get the TINA-TI macro using the Figure 6 technique. You can copy and paste this macro in any of your TINA-TI circuits to test for thermal noise (Right click on Macro, select Enter Macro and change “HCCVS1” from 10k to any resistor value you need, as shown in Figure 7):

Figure 7: Noiseless Resistor Macro (how to edit resistor value to what you need)

I’ll wrap this post up by providing a list of suitable devices for your next low noise design. I have included a column in Table 1 called “Critical Resistance” as the value of source resistance beyond which input noise current dominates over input noise voltage. When your source resistance exceeds this critical resistance, it is likely that you can benefit from changing your device to one with a lower noise current. The good thing is that you have TINA-TI at your disposal, to quickly change your device to another type and to run new simulations to verify lower noise.

Device

Voltage Noise

Current Noise

Critical Resistance

see text above

(nV/RtHz)

(pA/RtHz)

(Ω)

Low Voltage Noise:

LMH6629

0.69

2.6

265

LMH6624

0.92

2.3

400

LMH6626

1

1.8

550

LMH6628

2

2

1k

Low Current Noise:

OPA211

1.1

1.7

650

OPA300

3

0.0015

2M

OPA827

4

0.0022

1.8M

OPA657

4.8

0.0013

3.7M

Table 1: Low noise amplifiers

Until we meet again for the next TINA-TI “afraid” series, post your comments here and I will be happy to respond to them.

TINA TI noiseless resistor macro.TSC
  • Interesting article, thank you.

    However, I am involved in designing low noise discrete circuits where you have the option of paralleling devices to reduce noise as op-amps are not good enough.

    Unfortunately Tina is not helpful as it seems that Rbb defaults to 10 ohms for all bipolars. We all know Rbb can be up to hundreds of ohms so Tina simulation results for noise are usually far too optimistic.

    Of course you can always change Rbb to the correct value but shouldn't this be there in the first place?

    Clive Read.

  • Hi Clive,

    You have raised a good point with regard to simulation and how it is important to always keep in mind that the simulated behavior is only as good as the behavior model built-in (which in many cases can be edited for the user's particular needs).

    I've looked at the range of NPN BJT base resistance (Rbb) default value in TINA-TI and I agree that many are set to 10 ohm and that might be on the low side for noise purposes. But there are other values as well. For example:

    2N2923:   109 ohm

    2N3299:   33 ohm

    etc.

    Most likely these are the typical values (not worst case) in the individual BJT datasheets originally used to generate the models.

    Fortunately it is rather easy to double-click the TINA-TI BJT symbol and then click the "3-dot" symbol next to Type to select the device type and then alter "Base Resistance" to get a more accurate noise predictions.

    Regards,

    Hooman

  • Hello All,

    Here is an E2E post which gets into more detail regarding how TINA-TI computes RMS, how SNR is computed and displayed, and how to relate the output noise plot to the output noise density plot (as additional reference information):

    e2e.ti.com/.../346098.aspx

    Regards,

    Hooman

  • You can also make resistors noiseless by changing their temperature to "absolute" -273.2 °C, no?

  • You can also make resistors noiseless by changing their temperature to "absolute" -300 °C, no?  Then the resistor value is still displayed and you don't have to edit the macro to set it.

  • Hi Jonathan9420,

    Sorry for the late response.

    I tried to do what you suggested (change the operating temperature to -273.2 deg. C in order to get noiseless resistors), but it did not work. In TINA-TI, I went to Analysis, Set Analysis Parameters, Temperature of Environment (deg. C), and the lowest possible temperature is -100 deg. C (you get an error with anything more negative).

    If you have found a way to set the temperature to -273 deg. C, please share.

    Regards,

    Hooman