Addition of Noise file to input voltage source of Cadence Spetcre

 Hi............,

I wan to do transient analysis by noise signal in cadence spectre(version 5.4). Means I wan to give noise signal as vsource .Then ,how would it can be made a noise source which act as vsource(or vpulse type) for transient simulation . Or is there any other approach to do this noise analysis in transient analysis . Can any1 help me ?

First of all, please write full English words. You are not paying by the character here, so there is no need to abbreviate proper English words to "u" or "ur" or "any1". My natural inclination is to ignore any post written using such "text speak" because it is so difficult to comprehend - and even more so if English is not your first language (which is fair enough) and so I have to compensate for that too.

I merged all the different posts together on this. Asking the same question again (with no more information than the first time) is unlikely to increase your chances of  getting an answer quickly. Given that everyone here is answering these forum questions as a community activity, the more detail and precision you can give, the better.

I already explained how to do this, so I am at a loss to know what the problem is. You did not say what  you'd tried and what exactly did not work.

It's as simple as this:

1. Create a file with two columns - the first is the frequency in Hertz, and the second is the noise PSD in V^2/Hz
2. On the voltage source, specify the noisefile parameter to reference this file. For example, using the "vsource" component from analogLib, or if in the netlist, something like:
       noiseSrc (PLUS MINUS) vsource type=dc noisefile="noise1.txt"
3. In ADE, do a Choose Analysis and set up your transient. Enable the checkboxes to allow transient noise and fill in the noisefmax (maximum frequency that it will include noise contributions from) and quite likely the noisefmin too (the lowest frequency) - otherwise it will only include white noise at the values found at noisefmax. See "spectre -h tran" for more details, or read the manual.

That's it. Not hard. If this doesn't work, please explain precisely (using real words) what you were doing, what happened, what version of the IC environment and what version of spectre you were using, and any error messages that were given.

Regards,

Andrew.

First of all, the Forum Guidelines say that you should not append new questions onto an existing, old post. 

You can do what you want using Verilog-A. This has functions to generate white and flicker noise with coefficients, which should allow you to get the kind of shaping you want.

Andrew.

hi andrew:

how to create a noiseless resistor instance in spectre ac noise analysis?

thanks.

jian

Putting aside the fact that you didn't read the previous entry in the post telling the previous appender not to append an old thread (especially when your question is not about noise files nor is it about transient analysis), as covered in the forum guidelines, you can do this by using the "isnoisy" parameter on a resistor (in analogLib this shows up as "Generate Noise" or something like that).

Alternatively there is (in recent IC versions in conjunction with recent MMSIM versions) a field on the Simulation->Options->Analog form which allows you to specify which devices do or don't include noise.

Regards,

Andrew

Which version of the IC tools and MMSIM tools are you using? Type "virtuoso -W" and "spectre -W" in the UNIX terminal window to find out...

It would be at the bottom of the Main tab on the Simulation Options Analog form, as shown in the picture.

Regards,

Andrew.