Hi ALL,

I am trying to find the open loop pole-zeros of Boost converter (which operates in Boundary condition mode [BCM]) using PSS and PAC analysis.
The Boost converter is made to work in BCM by turning the MOSFET on whenever the inductor current goes to zero and turning off the MOSFET whenever the inductor current reaches some peak current. This inductor peak current is determined by an external current source. The control circuit has been implemented using VerilogA block.
There are two transfer functions, one from input voltage(Vi) to output voltage(Vo) and another one from control input (which is the external current source[I_ext]) to output voltage, you can refer the circuit attached.

I was able to run the transient analysis and the result were satisfactory. I used the frequeny of MOSFET control signal obtained from transient analysis as the beat frequency for PSS and PAC analysis.

// VerilogA for verilog_a, Comparators1, veriloga

`include "constants.vams"
`include "disciplines.vams"

module Comparators1(vp,vn,r,s,iin,iout);

input vp,vn,iin;
output r,s,iout;

electrical vp,vn,r,s,iin,iout;
parameter real vdc = 0.995;
real vs,vr;

analog begin

@(initial_step)
begin
  V(r) <+ 1;
  V(s) <+ 0;
end;

@(cross(V(vp) - V(vn),0));
@(cross(V(vn) - vdc,0));

// set logic
if(V(vp) - V(vn) < 100n)
  vs = 5;
else      
  vs = 0;

// reset logic
if(V(vp) - V(vn) > I(iin,iout))
  vr = 5;
else      
  vr = 0;

// set and reset signals
V(r) <+ transition(vr,0,1n);
V(s) <+ transition(vs,0,1n);

end

endmodule

After running the PSS and PAC analysis, I was able to plot the magnitude and phase for Vo/Vi but not for Vo/I_ext.

1. Could anyone please tell what am I doing wrong in this analysis and why I am not getting the magnitude and phase plot for Vo/I_ext ?
2. Does PAC analysis work for veriloga block?

Please let me know if any further information is needed.

Below lines give the simulation details:

Global user options:
            reltol = 0.0001
           vabstol = 1e-06
           iabstol = 1e-12          
          homotopy = 7
             limit = delta
            scalem = 1
             scale = 1
        compatible = spice2
              gmin = 1e-12
            rforce = 1
          maxnotes = 5
          maxwarns = 5
            digits = 5
              cols = 80
            pivrel = 0.001
          sensfile = ../psf/sens.output
    checklimitdest = psf
              save = allpub
              tnom = 27
            scalem = 1
             scale = 1

Circuit inventory:
             nodes 13
           bsim3v3 8    
      Comparators1 1    
         capacitor 1    
          inductor 1    
           isource 1    
  my_working_diode 1    
             relay 1    
          resistor 3    
           vsource 2    

Notice from spectre during initial setup.
   Fast APS Enabled ( cktpreset=sampled ).

*******************************************************
Periodic Steady-State Analysis `pss': fund = 210.25 kHz
*******************************************************
   Bad pivoting is found during DC analysis. Option dc_pivot_check=yes is recommended for possible improvement of convergence.
   L0: Initial condition computed for node L0:1 is in error by 1 nA.
       Decrease `rforce' to reduce error in computed initial conditions.  However, setting rforce too small may result in convergence difficulties or in the matrix becoming singular.

DC simulation time: CPU = 2 ms, elapsed = 2.50387 ms.

=================================
`pss': time = (0 s -> 250.005 ms)
=================================

Important parameter values in tstab integration:
   start = 0 s
   outputstart = 0 s
   stop = 250.005 ms
   period = 4.75624 us
   maxperiods = 50
   step = 250.005 us
   maxstep = 190.25 ns
   ic = all
   useprevic = no
   skipdc = no
   reltol = 100e-06
   abstol(V) = 1 uV
   abstol(I) = 1 pA
   temp = 27 C
   tnom = 27 C
   tempeffects = all
   method = gear2only
   lteratio = 3.5
   relref = sigglobal
   cmin = 1 fF
   gmin = 1 pS
   rabsshort = 1 mOhm

Important parameter values in pss iteration:
   start = 2.59215 ms
   outputstart = 0 s
   stop = 2.59691 ms
   period = 4.75624 us
   maxperiods = 50
   steadyratio = 10e-03
   step = 250.005 us
   maxstep = 23.7812 ns
   ic = all
   useprevic = no
   skipdc = no
   reltol = 100e-06
   abstol(V) = 1 uV
   abstol(I) = 1 pA
   temp = 27 C
   tnom = 27 C
   tempeffects = all
   errpreset = conservative
   method = gear2only
   lteratio = 3.5
   relref = alllocal
   cmin = 1 fF
   gmin = 1 pS
   rabsshort = 1 mOhm

pss: The steady-state solution was achieved in 8 iterations.

MultiThread info: 3 new work threads created

****************************************************
Periodic AC Analysis `pac': freq = (1 mHz -> 20 MHz)
****************************************************

Warning from spectre during PAC analysis `pac'.
   WARNING (SPCRTRF-15029): The following results might not be accurate due to undersampling of the actual frequencies above 21.025 MHz:
       Upper side band of 5th harmonic for stimulus frequencies above 19.9738 MHz.
       Upper side band of 6th harmonic for stimulus frequencies above 19.7635 MHz.
       Upper side band of 7th harmonic for stimulus frequencies above 19.5533 MHz.
       
spectre completes with 0 errors, 2 warnings, and 4 notices.

First a few nits. You should place models and simulator output in a code block on the forum so the formatting is preserved. Also, there is no 'circuit attached'.

If you are trying to pass a small signal through the comparator, it will never work because the transition is abrupt and it controlled by a large signal (the small signal is no present when determining when the transition occurs). You need to use a comparator model with a gradual rather than abrupt transition.

-Ken

You do not really need a filter at all. What you need is a range of input voltages for which the gain from input to output is nonzero. Specifically, rather than using:
Code:

if (V(in) > 0)
    vr = 5;
else
    vr = 0; 

You should have something like:
Code:

if (V(in) > delta)
  vr = 5;
else if (V(in) < -delta)
  vr = 0;
else
  vr = 2.5*(1 + V(in)/delta); 

(Sorry for changing the model, but I found the idea of comparing a voltage to a current confusing).

This issue has been discussed before on this forum. You might want to look around a bit.

-Ken

Did you try using pxf instead of PAC? It should pick up the
transfer functions from all the sources to the output.

Hi ALL,

I tried implementing the comparator block as per Ken´s suggestion. But I think I am making some mistake again and simulation is not completing.
Below is the code for comparator:

Code:

// VerilogA for verilog_a, Comparators1, veriloga

`include "constants.vams"
`include "disciplines.vams"

module Comparators2(vp,vn,r,s,iin,iout);
input vp,vn,iin;
output r,s,iout;

electrical vp,vn,r,s,iin,iout;

branch (vp,vn) vres;

real vs,vr;

analog begin

	@(above(V(vres)-200n,0));
	@(above(V(vres)-100n,0));
	@(above(V(vres)-I(iin,iout)-100n,0));
	@(above(V(vres)-I(iin,iout)+100n,0));

	// set logic
	if(V(vres) > 200n)
		V(s) <+ 0;
	else if(V(vres) < 100n)
		V(s) <+ 5;
	else
		V(s) <+ 2.5*(1 - (V(vres)-150n)/50n);

	// reset logic
	if((V(vres)-I(iin,iout)) > 100n)
		V(r) <+ 5;
	else if((V(vres)-I(iin,iout)) < -100n)
		V(r) <+ 0;
	else
		V(r) <+ 2.5*(1+V(vres)/100n);


end

endmodule 

Code:

*************************************************
Transient Analysis `tran': time = (0 s -> 150 ms)
*************************************************

Notice from spectre during IC analysis, during transient analysis `tran'.
    GminDC = 1 pS is large enough to noticeably affect the DC solution.
        dV(I33.MP1.m1:int_s) = -593.122 mV
        Use the `gmin_check' option to eliminate or expand this report.
    L0: Initial condition computed for node L0:1 is in error by 2 nA.
        Decrease `rforce' to reduce error in computed initial conditions.  However, setting rforce too small may result in convergence difficulties or in the matrix becoming singular.

DC simulation time: CPU = 2.999 ms, elapsed = 2.50697 ms.
Important parameter values:
    start = 0 s
    outputstart = 0 s
    stop = 150 ms
    step = 150 us
    maxstep = 1.5 ms
    ic = all
    useprevic = no
    skipdc = no
    reltol = 10e-06
    abstol(V) = 1 uV
    abstol(I) = 1 pA
    temp = 27 C
    tnom = 27 C
    tempeffects = all
    errpreset = conservative
    method = gear2only
    lteratio = 10
    relref = alllocal
    cmin = 1 fF
    gmin = 1 pS


Output and IC/nodeset summary:
                 save   4       (current)
                 save   12      (voltage)


Warning from spectre at time = 1.70218 us during transient analysis `tran'.
    WARNING (SPECTRE-16266): Error requirements were not satisfied because of convergence difficulties.
Warning from spectre at time = 257.998 us during transient analysis `tran'.
    WARNING (SPECTRE-16266): Error requirements were not satisfied because of convergence difficulties.
Warning from spectre at time = 260.058 us during transient analysis `tran'.
    WARNING (SPECTRE-16780): LTE tolerance was temporarily relaxed to step over a discontinuity in the signal: s.
    WARNING (SPECTRE-16881): Detected possible convergence difficulties which might be related to Verilog-A models. Use the command-line option '-ahdllint=warn' to check the Verilog-A modeling issues.

Error found by spectre at time = 629.057 us during transient analysis `tran'.
    ERROR (SPECTRE-16927): Transient simulation reaches maximum allowed number of convergence failures below minstep within 5% of stop time.
        Change option `max_minstep_nonconv' to adjust the allowed maximum number of convergence failures below minstep.
Last acceptable solution computed at 629.057 us.

The values for those nodes that did not converge on the last Newton iteration are given below.  The manner in which the convergence criteria were not satisfied is also given.
            Failed test: | Value | > RelTol*Ref + AbsTol

 Top 10 Solution too large Convergence failure:
    I(V0:p) = 78.3997 kA, previously -74.5598 uA.
        update too large:  | 1.76542 kA | > 783.997 mA + 1 pA
    I(I38:r_flow) = -209.857 kA, previously 12.3957 nA.
        update too large:  | -4.28769 kA | > 2.09857 A + 1 pA
    V(I32.MN1.m1:int_s) = 14.8515 V, previously 17.2562 uV.
        update too large:  | 297.03 mV | > 148.531 uV + 1 uV
    V(I32.MN1.m1:int_d) = 14.8669 V, previously 14.9482 mV.
        update too large:  | 297.039 mV | > 198.754 uV + 1 uV 

Can anyone please tell me why the simulation is not completing?
Is it because of discontnuity warning? But I do not see any discontinuity in the code. Please give some suggestions.

@Ken,

Thank you for your reply.

It seems like the error message is pretty clear. What is confusing you?

-Ken

Quote:


You only need pacmag. By adding the frequency, you are converting them to be large signal sources. The frequency of a small signal source is controlled by the analysis (just like with AC and noise), so you should not not specify freq on the small signal source itself.

-Ken