Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

Is the resistor model in analogLib of Cadence noise-free?

Status
Not open for further replies.
M

maldiniz

Junior Member level 1
Junior Member level 1
Joined
Dec 12, 2009
Messages
15
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,379
Is the resistor model in analogLib of Cadence noise-free for trans or ac, dc simulation?
 

I don't know Cadence, but in Spice, the only time noise comes into anything is in a noise analysis. In my simulator there are specific noise sources you can use in a transient analysis but it isn't standard Spice and still doesn't make a resistor 'noisy'.

Keith
 

    M

    maldiniz

    Points: 2
    Helpful Answer Positive Rating
Hi, Keith! Thanks a lot. May I know what's your simulator?
 

I use SIMetrix - a UK based simulator. It is based on Spice as most are. All that varies is the 'wrapping' around the Spice core.

Keith

Added after 4 minutes:

By the way, it should be an easy thing to check - run a transient analysis with simply a resistor in it and plot the voltage. I think you will get a straight line.

The pseudo noise source is handy for checking the performance of circuits with noisy signals.

Keith
 

    M

    maldiniz

    Points: 2
    Helpful Answer Positive Rating
Ya. That's what I've done just now. And it's been proven that transient analysis doesn't include noise.

Really thank you a lot!

Added after 1 minutes:

But for the noise source you mentioned, em... do you have any idea how i can modeling the thermal noise of a resistor?
 

It is worthwhile checking your manuals in case you have a noise voltage source for transient analysis in Cadence - there could be one. Then you just put it in series with the resistor. There may be another way but I need to be at my computer to check.

Keith

Added after 32 minutes:

I believe Cadence can do transient noise analysis. As I don't use Cadence you will have to wait for a Cadence expert to chip in, or do a search for 'Cadence transient noise analysis'.

Keith
 

Re: Is the resistor model in analogLib of Cadence noise-free

keith1200rs said:
I believe Cadence can do transient noise analysis.
Click to expand...
Right. In the ADE (Analog Design Environment) menu, select Analyses -> Choose... In the Choosing Analyses menu, if you select the (default) tran analysis, you may also select Transient Noise, which extends the menu for special noise options:

You can also choose a special noise analysis, which by default sweeps the frequency (like an ac analysis), but can be swept on any other variable:

Moreover, this menu contains still more noise analysis options: periodic, quasi-periodic and harmonic balance noise.

The analogLib res resistor owns a Generate noise? option. By default it doesn't produce noise, but the checkBox may be set to yes:


HTH! erikl
 

    M

    maldiniz

    Points: 2
    Helpful Answer Positive Rating
Thanks for putting me straight, erikl. I wasn't sure about what was available in Cadence and whether transient noise was only part of the RF simulation.

Keith
 

Re: Is the resistor model in analogLib of Cadence noise-free

Danke schön!

You guys are amazing!!!

Added after 2 minutes:

"The analogLib res resistor owns a Generate noise? option. By default it doesn't produce noise, but the checkBox may be set to yes: "

I've tried this one, but even if I put "yes", the output is still zero.
What I'm doing is simply putting a resistor, one end grounded, plot the output from the other end.

Added after 4 minutes:

And I tried the transient noise simulation. That one is really nice! At least for the 1st time, i saw a noise-like signal from the output. However, when I tried to do fourier transform by dft function, the output is not a flat spectrum.

Since there's no supply, the only noise from the resistor should be the thermal noise, isn't it? Any idea why the spectrum is not flat?

Added after 1 minutes:

This is the configuration i'm using.
 

Re: Is the resistor model in analogLib of Cadence noise-free

Well, i think i've got the meaning of the "Generate noise" option. If I put "no", the transient noise simulation will give zero as a result.

Added after 1 hours 2 minutes:

Well. Here's how i did this simulation. Maybe anyone can check for me whether i've done it correctly?
 

Is the dft result considered to be approx. flat?
 

I have checked and SIMetrix also supports real time noise. I can get a flat spectrum but I can also get one that has pronounced dips at certain frequencies. You need to be careful about the settings of the time interval for the noise sources compared to the frequent of interest. The attached two simulations show the difference between two different noise time intervals. All other settings, including the FFT ones, are identical. You also need to watch of for the maximum time step as well.

Keith.



Added after 3 minutes:

Looking at the screenshots erikl posted it looks like you need to adjust the transient noise fmin/fmax etc (in SIMetrix it is done by a time interval). Try some extreme values to find the effect.

Keith.
 

Do you think the noise analysis and transient noise using the same algorithm to calculate noise? If so, i think i can use noise analysis to get the frequency information directly.
 

They will use the same noise 'resistance' value. The AC/noise analysis can use that directly. The transient analysis needs to turn it into a pseudo-random Gaussian distribution which depends on your bandwidth of interest. They should give the same 'answer'.

Normally you would only use the transient noise for something where the noise will affect something which is time varying. A normal opamp for example wouldn't benefit from a transient noise analysis. You might do it with a comparator to see how it affects jitter or pulse width accuracy. You might use it on a PLL to determine phase noise. It all depends on what you are designing.

Keith
 

    M

    maldiniz

    Points: 2
    Helpful Answer Positive Rating
Thank you so much!

Well, in fact, I'm trying to make use of thermal noise to build a random number generator.

Added after 1 minutes:

amplify thermal noise and pass through ADC to get random bits

Added after 2 minutes:

However, noise is hard to modeling. And if over-estimate the input noise level, the amplifier can work properly in simulation , but its gain may not be sufficient for real case.
 

In which case you will need to use transient noise to simulate it. AC noise will help you get roughly enough gain, but then you will need transient noise.

However, will it work? The distribution of noise voltage is not uniform - it is Gaussian. I would have expected a system to be based on measuring the time between crossing a fixed threshold or something like that, although it is not something I have ever done.

Also, look for a good noise source. I seem to remember diodes are often used (reverse biased?). Also zener breakdown.

Keith
 

Yes. You are right. In fact, to measure the gain and BW of the amplifier, I think simple ac analysis will do. The reason why i need transient noise is that I need to show the results are indeed random bits, i.e. '1' or '0'.

As the input noise source, it was specified to be thermal noise of resistor... sign... it's really troublesome...
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top