The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Design Languages >> Verilog-AMS >> (rf_ahdl.va) file
https://designers-guide.org/forum/YaBB.pl?num=1085085916

Message started by vikas on May 20^th, 2004, 1:45pm

Title: (rf_ahdl.va) file
Post by vikas on May 20^th, 2004, 1:45pm

Hello,

I was trying to run a transient analysis for my PLL circuit.
when i use capacitor model which calculates current through it by ,
---
(q=(cgmin+dcg)*V(vp, vn)+vgnorm*dcg*ln(cosh((V(vp, vn)-dvgs)/vgnorm));)
I(vp, vn) <+ ddt(q);

---
it gives me an error (fatal one artithmatic exception).
But when i use it as given below than it works.
---------------------------------------------------------------
module rfCap(vp, vn);
inout vp, vn;
electrical vp, vn;
real c,q;
parameter real cgmin=1;
parameter real dcg=1;
parameter real dvgs=1;
parameter real vgnorm=1;
analog begin
c=cgmin+dcg*(1.0+tanh((V(vp ,vn)-dvgs)/vgnorm));
// q=(cgmin+dcg)*V(vp, vn)+vgnorm*dcg*ln(cosh((V(vp, vn)-dvgs)/vgnorm));
I(vp, vn) <+ ddt(c*V(vp, vn));
// I(vp, vn) <+ ddt(q);
end
endmodule
-------------------------------------------------------------
does anybody know what is the diference between these two, and how these things are connected with my circuit?........I am using TSMC-rf library,but i do'nt know to which RF_cap this ahdl is referring to.....

Thanks,
--Vikas

Title: Re: (rf_ahdl.va) file
Post by Ken Kundert on May 20^th, 2004, 9:27pm

The second version is incorrect (see the article on modeling varactors in www.designers-guide.com/Modeling).

Perhaps if you gave the full model and described the arithmetic exception we could help you debug your model.

-Ken

Title: Re: (rf_ahdl.va) file
Post by vikas on May 21^st, 2004, 1:54pm

Hello Ken,

Thanks for your reply first.
Two varactor capacitor are used in VCO block of PLL circuit. If i simulate my VCO design seperately by either method (i=dq/dt or cdv/dt) simulation works fine and gives the same result (which i think is correct) ,but when i simulate my whole PLL block where VCO forms a close loop with other block i get fatal error -arithmatic exception. It does'nt say what arithmatic exception.

Here i am including the model file part of this varactor and the hdl,( is that what you wanted to see?)

original hdl ********************
module rfCap(vp, vn);
inout vp, vn;
electrical vp, vn;
real c,q;
parameter real cgmin=1;
parameter real dcg=1;
parameter real dvgs=1;
parameter real vgnorm=1;
analog begin
// c=cgmin+dcg*(1.0+tanh((V(vp ,vn)-dvgs)/vgnorm));
q=(cgmin+dcg)*V(vp, vn)+vgnorm*dcg*ln(cosh((V(vp, vn)-dvgs)/vgnorm));
// I(vp, vn) <+ ddt(c*V(vp, vn));
I(vp, vn) <+ ddt(q);
end
endmodule
******************************************
And this is how varactor is described in model file
*************************************
HSPICE LEVEL 49:
//
// ## library files:
//
// The varactor are modeled with sub-circuit 'MOSCap_g3' and 'MOSCap_g6'
//
// Model name L(um) Wf(um) Side Branch Group
// ----------------------------------------------------
// MOSCap_g3 0.5 2 2 50 3
// MOSCap_g6 0.5 2 2 50 6
// ----------------------------------------------------
//
// Following is a poly gate of a varactor which has 3 Groups, 5 Branches.
// There are 2 Sides of Branches in per Group.
//
// --+----+----+--
// -+- -+- -+-
// -+- -+- -+-
// -+- -+- -+- <<___Branch
// -+- -+- -+-
// -+- -+- -+-
// ^
// ^---Group
//
// *************************************
// Varactor's Group number=3 *
// *************************************
subckt moscap_g3 ( Gate Bulk )
parameters dt=temp - 25
+ cgmin=0.95 * (1 + 3.503e-4 * dt + 1.071e-5 * (pow(dt,2))) * 1.0e-12
+ dcg=1.029 * (1 - 6.564e-5 * dt + 1.836e-7 * (pow(dt,2))) * 1.0e-12
+ dvgs= - 0.116 * (1 + 1.814e-3 * dt - 8.909e-6 * (pow(dt,2)))
+ vgnorm=0.456 * (1 + 9.656e-4 * dt - 1.841e-6 * (pow(dt,2)))
lgate ( Gate 3 ) inductor l=36.6e-12
rgate ( 3 4 ) resistor r=0.7947 tc1=5.498e-3 tc2=8.1779e-6
cgate ( 4 5) rfCap cgmin=cgmin dcg=dcg dvgs=dvgs vgnorm=vgnorm
rch ( 5 2 ) resistor r=1.4703 tc1=2.945e-3 tc2=2.9702e-5
cov ( 5 2 ) capacitor c=147.5e-12
csub ( 5 6 ) capacitor c=30.2e-15
rsub ( 6 0 ) resistor r=21.1820 tc1=9.396e-3 tc2=-4.9267e-6
rs ( 2 9 ) resistor r=0.7906 tc1=4.111e-3 tc2=3.9114e-6
ls ( 9 Bulk ) inductor l=19.3e-12
ends moscap_g3
**************************************
Thanks again
--Vikas

Title: Re: (rf_ahdl.va) file
Post by Ken Kundert on May 21^st, 2004, 10:51pm

I don't see anything obviously wrong. Can you post a small netlist that exhibits the problem?

-Ken

Title: Re: (rf_ahdl.va) file
Post by vikas on May 26^th, 2004, 2:14pm

Hello Ken,

Thanks for reply but i did'nt understand what netlist you want to see.

It create netlist with no error. While running, simulator gives fatal error "arithmatic exception at line no. so ...." and that line actually is the charge storage model of varcap which i posted in earlier mail.

Regards,
--Vikas

Title: Re: (rf_ahdl.va) file
Post by Ken Kundert on May 26^th, 2004, 3:58pm

It is often had to determine what is going wrong only from the error messages. If I could run the circuit I could look at the waveforms, etc. It is also difficult to determine what is going wrong from a large complicated netlist. That is why I was asking for a simple netlist that exhibits the problem. I would need both the netlist and the models; everything needed to run Spectre stand-alone. That way I could run the circuit and try to find the problem. It may not be the model itself. It instead may be an interaction between the model and the circuit.

-Ken

Title: Re: (rf_ahdl.va) file
Post by Geoffrey_Coram on Jul 9^th, 2004, 8:49am

Vikas -
Is the arith error during the time=0 solution, or does the simulator indicate that it has progressed into the actual transient?

My guess would be that Newton's method is failing to converge because a very large number is passed to/returned by cosh(). A certain simulator I know would not try homotopy methods if Newton failed due to an arith error; I believe that was fixed in a more recent version.

If this is the problem, you have a couple options (besides upgrading the simulator):
1. Create a nodeset file using the "bad" model (capacitance-based) and tell the simulator to use this as the starting point for the good model. (You could also try just setting a few initial conditions by hand to help convergence.)
2. Re-write cosh(x) as (limexp(x)+limexp(-x))/2, where x=(V(vp,vn)-dvgs)/vgnorm)

If the DC/time=0 solution is obtained, then Ken's right, you'll probably need to investigate the waveforms.

-Geoffrey