Trying too different circuits producing noise, I get 0 Volts output running the circuits in LTspice. One circuit obtains noise from a Zener diode, and the other one from the reverse-biased emitter-base junction of a NPN bipolar transistor. Am I doing something wrong, or is LTspice not capable of simulating a noise source as a transient response?

In Ltspice, resistance of a resistor labeled 1m equals 1 Meg Ohm, is that correct?

Thanks,
Pete

 

Hi Pete,
Please post the LTS asc file you are using for testing.
E

In Ltspice, resistance of a resistor labeled 1m equals 1 Meg Ohm, is that correct?

Updated:
1meg =1meg ohm
1m= milli-ohm

 

Here it is as requested-

 

Trying too different circuits producing noise, I get 0 Volts output running the circuits in LTspice. One circuit obtains noise from a Zener diode, and the other one from the reverse-biased emitter-base junction of a NPN bipolar transistor. Am I doing something wrong, or is LTspice not capable of simulating a noise source as a transient response?

In Ltspice, resistance of a resistor labeled 1m equals 1 Meg Ohm, is that correct?

Thanks,
Pete

Is there anything on the ".model" card for the diode that might lead you to believe that the noise behavior of the diode would be availablein an LTspice simulation?

 

Specify a transistor model for Q1. Not "NPN".
Use a Bv source with an equation (maybe white(), or random() function) to inject noise into the collector of Q1.

 

Specify a transistor model for Q1. Not "NPN".
Use a Bv source with an equation (maybe white(), or random() function) to inject noise into the collector of Q1.

Do I need to do one or the other, or both? What is a Bv source? Writing an equation to do what you say would be much more sophisticated than I currently am using LTspice, but thanks for the advice.

 

Do I need to do one or the other, or both? What is a Bv source? Writing an equation to do what you say would be much more sophisticated than I currently am using LTspice, but thanks for the advice.

It is a "Behavioral Voltage Source". Look in the LTspice help for a device that begins with the letter "B".

​

B. Arbitrary Behavioral Voltage or Current Sources ​

Symbol names: BV, BI​

​

Syntax: Bnnn n001 n002 V=<expression> [ic=<value>]​

+ [tripdv=<value>] [tripdt=<value>]​

+ [laplace=<expression> [window=<time>]​

+ [nfft=<number>] [mtol=<number>]]​

​

Bnnn n001 n002 I=<expression> [ic=<value>]​

+ [tripdv=<value>] [tripdt=<value>] [Rpar=<value>]​

+ [laplace=<expression> [window=<time>]​

+ [nfft=<number>] [mtol=<number>]]​

​

The first syntax specifies a behavioral voltage source and the next is a behavioral current source. For the current source, a parallel resistance may be specified with the Rpar instance parameter.​

​

Tripdv and tripdt control step rejection. If the voltage across a source changes by more than tripdv volts in tripdt seconds, that simulation time step is rejected.​

​

Expressions can contain the following:​

​

• Node voltages, e.g., V(n001)​

​

• Node voltage differences, e.g., V(n001, n002)​

​

• Circuit element currents; for example, I(S1), the current through switch S1 or Ib(Q1), the base current of Q1. However, it is assumed that the circuit element current is varying quasi-statically, that is, there is no instantaneous feedback between the current through the referenced device and the behavioral source output. Similarly, any ac component of such a device current is assumed to be zero in a small signal linear .AC analysis.​

​

• The keyword, "time" meaning the current time in the simulation.​

​

• The keyword, "pi" meaning 3.14159265358979323846.​

​

• The following functions:​

​

The list of functions is in the help pages which I'm sure you can find on your own.

 

In spice programs, models of transistors, diodes (zener), and resistors do not include noise in the high-signal mode (Tran mode). Noise modeling is only used in low-signal analysis - Noise.

 

Here's a simple example of the use of a BV source to generate a random voltage :-