how to write a behaviour level voltage source in spectre ?

[zhonghan]

i just know the corresponding hspice syntax, like EXXX V+ V_ VOL=" EXPRESSION"
how to use this device in spectre?

Regards!

 

[JoannesPaulus]

zhonghan,
the syntax is:
E2 3 4 VOLT = "15+2*V(1,2)+0.75 *V(1,2)2"
where 3 and 4 are the controlled nodes and 1 and 2 are the controlling nodes.

Good luck!

 

[zhonghan]

Re: how to write a behaviour level voltage source in spectr

I have tried it as you advised , but it doesn't work , not the spectre statement format

 

[JoannesPaulus]

zhonghan,
sorry, I understood you needed the hspice format, for spectre the format is different:

E0 (n1 n2 n3 n4) pvcvs gain=1.0 coeffs=[c0 c1 c2 c3 c4]

n1 and n2 are the controlled nets and n3 and n4 are the controlling nets; c0-c4 are the polynomial coefficients.

 

[zhonghan]

Re: how to write a behaviour level voltage source in spectr

Thank you!
I want to express my more clrealy. Does pvcvs represent polynomial VCVS ?
If i want a time related sinusoidal wave which can be writtn as
EXXX nodea nodeb volt="sin(2*3.14159*Fosc*TIME+ sin(2*3.14159*Fjitter*TIME))" in HSPICE
Can i get the similar source in spectre?

 

[JoannesPaulus]

zhonghan,
I do not know if there is a voltage source that can do that. I would use a verilog-A module in your spectre netlist (verilog-A is native in spectre).

module vsin_jitter(p,n);
output p,n;
electrical p,n;
parameter real fosc = 1.0, fjitter = 0.0, ampl = 1.0 ;
analog
begin
V(p,n) <+ ampl * sin(2.0 * ‘M_PI * fosc * $abstime + sin(2.0 * ‘M_PI * fjitter * $abstime)) ;
$bound_step(0.02/fosc) ; // Max time step = 1/50 period
end
endmodule

I hope this works!