Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. Join them; it only takes a minute:

Sign up
Here's how it works:
  1. Anybody can ask a question
  2. Anybody can answer
  3. The best answers are voted up and rise to the top

Is there a way to setup a voltage supply with voltage jitter/noise? I want to experiment with filtering out noise on various voltages etc. but not sure how to configure LTSpice to create a noisy voltage supply.

share|improve this question
up vote 28 down vote accepted

Yes, you can inject noise using the arbitrary voltage (or current) source, then use things like the random or white function to create some noise.

Here is an example circuit (I separated the noise from the signal just to make things clearer - obviously you can combine them together in one function if you wish):

Noise Circuit


Noise Circuit Simulation

All the functions are detailed in the help under circuit elements -> arbitrary behavioral voltage or current sources.

Noise simulation mode

Also, just in case you were not aware, SPICE has a noise simulation mode, to quote from the help files:

.NOISE -- Perform a Noise Analysis
This is a frequency domain analysis that computes the noise due to
Johnson, shot and flicker noise. The output data is noise spectral 
density per unit square root bandwidth.

Syntax: .noise V(<out>[,<ref>]) <src> <oct, dec, lin> <Nsteps> <StartFreq> <EndFreq>

Basic example:

Noise mode


Noise mode sim

The above is rather boring as it only models the resistor noise (I stepped the resistor through various values to show how the Johnson noise increases with resistance). But it can be very useful with more complex circuits containing diodes/transistors/opamps/etc.

share|improve this answer

(Not enough rep. yet to create a comment on Oli's post, so this goes in a post of it own).

Oli's post above is very useful, but for the LTSpice beginner, it is perhaps worth explaining how to actually create of one of those "arbitrary behavioral voltage source" : I was naively expecting to be able to modify the value of a normal voltage source to enter the white(...) formula, but of course, it does not work.

Instead, you have to press the "component" button in the toolbar, and in the window that opens, pick a component of type "bv".

share|improve this answer

SPICE ( I can't tell you if LTSPice is a subset of normal SPICE or not) normally has the ability to model the noise that each device generates. I think your question is more about how to you measure how effective your filtering is and how much an external interfering signal may affect each node.

To do that what you need to do that is .AC analysis of the circuit.

To do a noise analysis you need to use both .ac and .noise. So noise analysis is a subset of ac analysis.

share|improve this answer
Just checked. LTSpice does have a noise analsysis available. But I can't find a noise source in the parts catalog --- hopefully someone can come along and say where to find it. – The Photon Jan 16 '13 at 17:08
@ThePhoton all devices in spice SHOULD be noisy, i.e. not ideal - noise less. So that should already be in the models. I suspect LTSpice should also have that. – placeholder Jan 16 '13 at 17:26
Per the Help file, "This is a frequency domain analysis that computes the noise due to Johnson, shot and flicker noise." So if you have a schematic of your circuit, you're good. But if, for example, you're creating an op-amp model based on datasheet parameters and/or measurements, you often use idealized components like controlled sources, and you want to have a noise source element to fix up the noise characteristics. – The Photon Jan 16 '13 at 18:02
@ThePhoton It's called honesty, I don't have LTSPICE running and I'm not about to presume things. You feeding back info on your instance is ideal. Me showing results from my full blown EDA tools may or may not be useful. Every SPICE variant does things slightly differently. – placeholder Jan 16 '13 at 19:35
@Photon and rawbrawb - since the models for various SPICEs are generally compatible with each other, it would suggest that the issue would lie with the models rather than the SPICE variant. As far as I am aware, the basic models do not include noise modelling for e.g. a transient sim, but will all work with the dedicated noise simulation. For instance if you try the last simulation in my answer as a transient with no input voltage, you will get 0V out (as opposed to the 20-44nV predicted) – Oli Glaser Jan 16 '13 at 21:27

As you want to inject noise from the power supply, I think easiest is to put a small amplitude AC voltage source in series with the DC voltage source you already have and sweep its frequency through the range you are interested in.

share|improve this answer
.ac does that for you automatically – placeholder Jan 16 '13 at 17:36
I guess I have to polish up my SPICE knowledge. – jippie Jan 16 '13 at 17:37

Your Answer


By posting your answer, you agree to the privacy policy and terms of service.

Not the answer you're looking for? Browse other questions tagged or ask your own question.