How to generate Gausian pulse in cadence spectre

A quick bit of googling to find out what you meant by gaussian pulse, I then wrote a short piece of VerilogA to do what you want. If it's not exactly what you want, you can adapt it to suit your needs:

`include "constants.vams"
`include "disciplines.vams"
module gaussianPulse (plus,minus);
inout plus,minus;
electrical plus,minus;
parameter real sigma=1u;
parameter real tcentre=100u;
parameter real amplitude=1;

analog begin
    //V(plus,minus) <+ exp(-pow(($abstime-tcentre)/sigma,2)/2)/sqrt(`M_TWO_PI*sigma*sigma);
    V(plus,minus) <+ amplitude*exp(-pow(($abstime-tcentre)/sigma,2)/2);
end

endmodule

Regards,

Andrew.

Thank you Andrew Beckett

However, I have no experience on Verilog A, and  I want to generate Gaussian pulse in Cadence Virtuoso Analog Design Environment.

I mean by adding components from build-in libraries to the Schematic file, to run transient simulation.

Do you know how to build a component that functions as the code you given ?

Best regards

In the CIW, File->New->CellView, and set the view name to "veriloga".

In the editor that gets launched, paste the code I posted - if you didn't call the call "gaussianPulse" then change the module name in the code to match what you called it.

Save and exit the editor (if you don't like the editor, you can type in the CIW first editor="nedit" or whatever you prefer, before opening the view in the first place). 

It should then prompt you to create a symbol.

Having created a symbol, you can place an instance in your schematic, and change the sigma, tcentre, amplitude parameters as you see fit.

Regards,

Andrew.

Andrew Beckett, thanks you for your kind support. It is really helpful for me.