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

phase noise in hspice

Status
Not open for further replies.
P

parnia

Newbie level 3
Joined
Nov 14, 2015
Messages
4
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
28
Hi all
I'm master student. i want to simulate phase noise of phase locked loop in HSPICE RF. but when i simulate it, I see this warning:
Warning: HB_WARN.3: HB oscillator convergence failure. Oscillator analysis terminated.
Click to expand...
even this warning be seen for an ideal vco.
My netlist for define ideal vco as follows:

Code: 
*******VCO DEMO****************** 
.option POST
.TRAN .01n 100n
***********************vco_define***************
Evco nco 0 vol='0+1.8*sin(6.28*1e9*V(vctrl)*time)'
Vcontrol vctrl 0 pwl (0  0  100n  .1)
R1 nco 0 10meg
**************** Harmonic Balance Test Bench**** 
.HBOSC tones=150meg nharms=10  PROBENODE=nco,0,0.9
.PHASENOISE v(nco) dec 10 0 300meg
.END

please help me?
thanks.
 
Last edited by a moderator:

The problem is that you are performing an analysis using a voltage source with a frequency near to the standard time step of simulator.
 

dear andre_teprom
thanks for your reply, how I can solve it? what is your end of from ''frequency near to the standard time step of simulator''???
 

You can reduce the time-step size by setting new values for the arguments RMIN and TSTEP with the .TRAN command.
 

I do it, But the problem is not resolved
I set the step_time=1p or 10p or 100p but The result was not changed!!!
also I set the initial point as follow :
.ic nco=.9 vctrl=.9
and the problem is still there.
 

[moved]phase noise in hspice

hi
can you solve your oscillator convergence problem ? can you help me?
I have a same problem.
thank you
 

Re: [moved]phase noise in hspice

Unfortunately, I do not have SPICE installed on my PC, but despite that, as you informed that you are a master student, it's an excellent opportunity to learn by doing. The most important general tips have been already provided, and from now on it's up to you make trial and error attempts in order to obtain the appropriate configuration parameters for YOUR particular case. Furthermore, you did not say what progress obtained by reading the document suggested above.
 

parnia said:
*******VCO DEMO******************
.option POST
.TRAN .01n 100n
***********************vco_define***************
Evco nco 0 vol='0+1.8*sin(6.28*1e9*V(vctrl)*time)'
Vcontrol vctrl 0 pwl (0 0 100n .1)
R1 nco 0 10meg
**************** Harmonic Balance Test Bench****
.HBOSC tones=150meg nharms=10 PROBENODE=nco,0,0.9
.PHASENOISE v(nco) dec 10 0 300meg
.END
Click to expand...
You use behavioral expression which include system variable "time".
Generally HB Analysis can't treat behavioral expression which include system variable "time".
This is true for $abstime in Verilog-A.

Try to use .SNOSC (Autonomous Shooting Newton Analysis) instead of .HBOSC (Autonomous HB Analysis).

And your circuit is no more than driven circuit.
You don't have to invoke autonomous analyses such as ".HBOSC" and ".SNOSC" at all.
Simply use ".SN".

If you use special system task, $cds_set_rf_source_info() in Verolog-A of Cadence Spectre,
you can treat behavioral expression which include $abstime in HB Analysis.

However this is not true for HB Analysis of Synopsys HSPICE.
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top