Dear Ken,

I recently read the paper "Accurate Fourier analysis for circuit simulators". I don't have access to Spectre, therefore I wanted to try out the described Fourier analysis by writing a custom MATLAB script that processes the SPICE output.

I wanted to start on the ua741 example from the paper to have a good reference and than go forward from there. However, when trying to reproduce the 'normal' Fourier analysis results from SPICE, I could not come up with the numbers presented in the paper. These are the numbers SPICE reports (THD is smaller than reported in the paper):

Code:

Fourier analysis for vout:
  No. Harmonics: 10, THD: 2.93336 %, Gridsize: 200, Interpolation Degree: 1

Harmonic Frequency   Magnitude   Phase	 Norm. Mag   Norm. Phase
-------- ---------   ---------   -----	 ---------   -----------
 0	 0	     -0.0027612  0	     0	     0
 1	 1000	  0.94215     0.271005    1	     0
 2	 2000	  0.00485751  -115.89     0.00515577  -116.16
 3	 3000	  0.00667308  136.829     0.00708282  136.558
 4	 4000	  0.00713215  -42.948     0.00757008  -43.219
 5	 5000	  0.000858787 -51.735     0.000911518 -52.006
 6	 6000	  0.0181092   -49.895     0.0192211   -50.166
 7	 7000	  0.00353059  -55.709     0.00374738  -55.98
 8	 8000	  0.0173587   129.745     0.0184246   129.474
 9	 9000	  0.00152307  127.297     0.00161659  127.026
 

I see some possible causes for this and it would be nice if you could comment on them:

1. Different SPICE version: I used spice3f5 while the paper mentions spice2g6.

2. SPICE testbench: this is my SPICE deck:
Code:

*
* uA741 opamp Fourier analysis
*


* Netlist
.include UA741_model.sp

X1 vin vout vdd vss vout UA741


* Bias
Vdd vdd 0 dc 12
Vss 0 vss dc 12


* Input
Vin vin 0 sin(0 1.0 1e3 0 0 0)


* Analysis
.tran 1e-9 10e-3
.four 1e3 vout


* Output
.print tran v(vin) v(vout)



.end
 

3. ua741 model: I used the so called Oregano model:
Code:

.subckt UA741	   1 2 3 4 5
* connections:	  | | | | |
*			   | | | | |
*   non-inverting input | | | |
*	   inverting input | | |
*     positive power supply | |
*	 negative power supply |
*				output
*
*
  c1   11 12 8.661E-12
  c2    6  7 30.00E-12
  dc    5 53 dx
  de   54  5 dx
  dlp  90 91 dx
  dln  92 90 dx
  dp    4  3 dx

*SPICE2:
*  egnd 99  0 poly(2) (3,0) (4,0) 0  .5  .5
*SPICE3:
  Begnd 99 0 V = .5*V(3,0) + .5*V(4,0)

*SPICE2:
*  fb    7 99 poly(5) vb vc ve vlp vln 0 10.61E6 -10E6 10E6 10E6 -10E6
*SPICE3:
  Bfb 7 99 I = 10.61E6*I(vb) + -10E6*I(vc) + 10E6*I(ve) + 10E6*I(vlp) + -10E6*I(vln)
  ga    6  0 11 12 188.5E-6
  gcm   0  6 10 99 5.961E-9
  iee  10  4 dc 15.16E-6
  hlim 90  0 vlim 1K
  q1   11  2 13 qx
  q2   12  1 14 qx
  r2    6  9 100.0E3
  rc1   3 11 5.305E3
  rc2   3 12 5.305E3
  re1  13 10 1.836E3
  re2  14 10 1.836E3
  ree  10 99 13.19E6
  ro1   8  5 50
  ro2   7 99 100
  rp    3  4 18.16E3
  vb    9  0 dc 0
  vc    3 53 dc 1
  ve   54  4 dc 1
  vlim  7  8 dc 0
  vlp  91  0 dc 40
  vln   0 92 dc 40
.model dx D(Is=800.0E-18 Rs=1)
.model qx NPN(Is=800.0E-18 Bf=93.75)
.ends UA741
 

My gut feeling says the model is the culprit...

Kind Regards

Peter

Dear Ken,


thank you for the ua741 Spectre netlist, I think I will be able to convert this to SPICE format. I personally think the difference between the actual device-level netlist and the macro-model will account for much of the difference between the Fourier analysis results.

As I understand your reply correctly, my effort of implementing the proposed Fourier analysis using Matlab does not  make sense.

When I read the paper, I thought I could just take the waveform I'm interested in straight from SPICE and than calculate the sum of integrals as discussed in the paper (these are all just numerical calculations).

As I understand it now (please correct me if I'm wrong), the problem lies in the polynomial fit of the waveform. My approach would be to fit an N-degree polynomial through every (N+1) points from the calculated SPICE solution. I know SPICE already performs such a fit, therefore the only benefit would be to obtain the coefficients of the polynomial.

Of course, it might very well be that the order of the polynomial fit SPICE uses changes during simulation and than my approach would not work well.

Otherwise, I think I can still obtain the coefficients of the polynomial (dubbed 'cm' in the paper) and calculate the sum of integrals.

Regards

Peter

Dear Ken,

ok, I understand your point now.

One more thing though (for my understanding): you state that the presented methodology's benefits are not so apparent on the ua741 example as they are on the PWM example.

I understand why the method is much better for the PWM case (compared to DFT), but in your paper, the Spectre results (implementing this method) are also much better than the SPICE2g6 results (using 'traditional' .four analysis), apart from the RELTOL setting which is equal for both.
So based on those results, I would conclude that the presented method also has *significant* (tens of dB more resolution compared to SPICE2g6) benefits for a ua741 type of circuit, although a DFT would also be able to provide the same accuracy/resolution, given enough FFT points (~simulation time).

Regards

Peter