The Designer's Guide Community
Forum
Welcome, Guest. Please Login or Register. Please follow the Forum guidelines.
Mar 28th, 2024, 7:21am
Pages: 1 2 
Send Topic Print
question in sigma-delta ADC (Read 4047 times)
chuzi
Junior Member
**
Offline



Posts: 12
BeiJing China
question in sigma-delta ADC
Dec 20th, 2005, 7:00pm
 
hi,all
i am a beginer in analog ic design and recently in my first project sigma-delta ADC.
my case is: 1 bit, cascade 2-1-1modulator, 64 OSR, in simulink SNR could be 108dB, considering KTC noise/clock jitter/nonideal opamp,SNR could be 97dB, noise level is about -140dB.
then i begin my circuit.
when simulate circuit, it is said noise floor is about -100dB, SNR lower than 80dB, why noise floor is so great? what reason may make this happen?
thanks a lot, bow to all:|

my opamp(5.6pf load):unitfreq 372Mhz,phasemargin 71.6, gain 97dB,slew rate 280V/us, input noise 5nV/sqr(hz).
in simulation, sample rate is 20Mhz, signal i choose 100khz,
simulation software is hspice, and VCS(nanosim)

thanks
Back to top
 
 
View Profile   IP Logged
Paul
Community Fellow
*****
Offline



Posts: 351
Switzerland
Re: question in sigma-delta ADC
Reply #1 - Dec 20th, 2005, 11:19pm
 
Hi Chuzi,

is this a result from FFT after transient analysis? If so, are you sure you sample your output data correctly? You may want to have a look at sheldon's "user's guide" for achieving good FFT measurements:
http://www.designers-guide.org/Forum/?board=ms_design;action=display;num=1118555...

The following posts may also be useful:
http://www.designers-guide.org/Forum/?board=ms_design;action=display;num=1119874...

Paul
Back to top
 
 
View Profile WWW   IP Logged
chuzi
Junior Member
**
Offline



Posts: 12
BeiJing China
Re: question in sigma-delta ADC
Reply #2 - Dec 21st, 2005, 5:15pm
 
dear Paul,
   thanks a lot for the reply, it is my first time to go to forum, and i am very exiting to hear from seniority designer far away, thanks for the guidance:)
   i always think that there must be something wrong in my fft program, because in my opinion the peak of input signal in spectrum should be narrow, but actually in my result it is very wide. i'd better check it, thanks, it is helpful, i usually cannot find useful resources:)
   and i am also wandering how to reduce noise floor in circuits:)what reason will lead noise floor become higher? i mean in the same fft program, result from simulink shows noise floor is lower, but result from hspice shows noise floor is higher, does it means my matlab model is not succesful? where should i change?:)
and what reason lead this differece?:)thanks:)
   should i copy simulink graph on forum, that everyone could find my fault easily? thanks again,Paul:)
                                                     sincerely,chuzi
Back to top
 
 
View Profile   IP Logged
Paul
Community Fellow
*****
Offline



Posts: 351
Switzerland
Re: question in sigma-delta ADC
Reply #3 - Dec 21st, 2005, 11:52pm
 
Chuzi,

try to follow the guidelines described in sheldon's post, as well as in the other post mentioned earlier. It should help to reduce both spectral signal width and noise floor. You should be able to get reasonably close to your Matlab results in Spice simulations.

Paul
Back to top
 
 
View Profile WWW   IP Logged
chuzi
Junior Member
**
Offline



Posts: 12
BeiJing China
Re: question in sigma-delta ADC
Reply #4 - Dec 22nd, 2005, 12:57am
 
i see, thanks a lot,Paul Cheesy
bow~~~
              chuzi Smiley
Back to top
 
 
View Profile   IP Logged
sheldon
Community Fellow
*****
Offline



Posts: 751

Re: question in sigma-delta ADC
Reply #5 - Dec 22nd, 2005, 6:45am
 
chuzi,

  Please be aware that the guidelines in the previous
append were intended for a Nyquist-rate ADC. A Sigma-
Delta ADC has additional requirements. For Nyquist-Rate
ADC, we can force the solution to be "periodic" using the
method outlined in the post. As a result, spectral leakage
is suppressed and the the Rectangular window function
can be used. However, a Sigma-Delta ADC has a
feedback loop which means that it has memory/ its
response is chaotic[non-periodic]/ it has an infinite
impulse response. These are different ways of saying
you can not entirely suppress the spectral leakage.

So you will have to

1) Use a window function for the FFT, I use the Hanning
   window function. It suppress leakage and does not
   "smear" the fundamental too much.

2) You may need to run the simulation for two cycles
    of the fundamental. This improves the resolution
    bandwidth of the FFT, lowering the noise floor. In
    addition over two cycles relative effect of the spectral
    leakage is suppressed. Twice as much signal for
    the same amount of leakage. Of course more cycles
    is better, at the cost of extremely long simulation
    times.

3) You will also need to control the accuracy of the
   simulator carefully.  These designs can have very
   low noise floors and the simulator accuracy controls
   need to be set appropriately.

Again, the issue is that even simple Sigma-Delta ADC
can have very low noise floors. Look at Brian Brandt's
papers on Sigma-Delta design from the early 90's, for
a second-order ADC, the noise floor is -150dB.  

                                                     Best Regards,

                                                        Sheldon
Back to top
 
 
View Profile   IP Logged
chuzi
Junior Member
**
Offline



Posts: 12
BeiJing China
Re: question in sigma-delta ADC
Reply #6 - Dec 22nd, 2005, 10:38pm
 
great thanks! sheldon, under your guidance, my noise floor is reduced about 10dB~20dB, and previous append help me understand simulation tools. thanks a lot!thanks!~~
       bow~~
                    chuzi
Back to top
 
 
View Profile   IP Logged
chuzi
Junior Member
**
Offline



Posts: 12
BeiJing China
Re: question in sigma-delta ADC
Reply #7 - Dec 28th, 2005, 4:43pm
 
Sheldon and Paul,
 First,thanks for earlier helps.Under your guidance, I could get SNR to be 92.4dB.
 My case is: 2-1-1 cascade 1-bit sigma-delta mudolator, 64 oversample ratio.
 In simulation:
   1)11/1024=107.421875KHz sine wave as input, 20MHz sample clock;
   2)1024 points fft, 2x simulation time;
   3)hanning window is chosen to suppress the spectral leakage;
   4)the disadvantage is I used VCS(nanosim) which one has higher speed and lower accuracy.
 I am going to use hspice which one has higher accuracy but lower speed. Because it will take maybe 2 weeks, I turn to you for some now problem I am not quite sure:)
   1)My goal is to simulate the sigma-delta modulator, I just use hspice to simulate the   circuits and get the output of the 3 stages, then import it into matlab to finish the   error cancellation and decimation.
     Will this way bring some more error? doing fft in simulation tools could be more   accurate or same? I think use more accurate hspice to simulate digital circuit is a   waste of time, when I combine analog and digital part, how could I simulate it?
    2)I get 2048 points output data and do 1024 points fft, so I chose latter 1024   points, am I right? Did it do some effort to suppress the spectral leakage?
    3)Since the noise floor become flater, circuit noise become the major noise. Could you give me same advice on how to suppress the circuit noise? I mean should I make switches to be smaller? How small should I take it? In faster simulation I can hardly tell the diffrence. And how could I change the capacitance?
    Great thanks and best regards!
                                                               chuzi  
Back to top
 
« Last Edit: Dec 29th, 2005, 12:58am by chuzi »  
View Profile   IP Logged
chuzi
Junior Member
**
Offline



Posts: 12
BeiJing China
Re: question in sigma-delta ADC
Reply #8 - Dec 29th, 2005, 1:02am
 
Dear Sheldon,
   there is another question which bother me. In my fft output figure, distance between the peak of spectrum and the noise floor is over 120dB, but the peak of spectrum is above 120dB and noise floor is about 0dB. Since the input signal should below 0dB, could you be patient to tell me how to get fft figure under 0dB?
   my .m file is:



N=2048;    %NP=2048


for mm=1:N
   OSR64Out(mm)=output64(mm+50);   %50 is settle time
end
figure;

w=hann(N);
OSR64Outinv=OSR64Out(1:N)';
Osr64outPtot=((abs(fft((OSR64Outinv(1:N).*w)'))).^2/N);
Osr64outPtotdB=10*log10(Osr64outPtot);

for mm=1:N
   Pyy(mm)=Osr64outPtot(mm);
   dbpyy(mm)=Osr64outPtotdB(mm);
end

CenP=17;              %17 is for exclude dc peak
maxP=-100;            % find peak
for i=10:N/2
   if dbpyy(i)>maxP
       maxP=dbpyy(i);
       CenP=i;
   end
end

f=1:N/2;
plot(f,dbpyy(1:N/2));


%%%count SNR
%%%NOISE Power
PNNoDnoise=0;TTP=0;SP=0;THDP=0;PNDnoise=0;
for i=20: (N/2)
   TTP=TTP+Pyy(i);
end


%%%signal power
for i=1:25             %25 is because peak is not narrow enough
   SP=SP+Pyy(CenP-i+1)+Pyy(CenP+i);
end

%%%noise
PNnoise=TTP-SP;

SNR=10*log10(SP/PNnoise)




Great thanks and best regards!
  chuzi
Back to top
 
 
View Profile   IP Logged
hzheng
Guest




Re: question in sigma-delta ADC
Reply #9 - Dec 29th, 2005, 1:18am
 
hi chuzi:
i have a question about 2-1 sigma-delta modulator behavial model simulation,i use matlab simulink simulation too,but i have bad result PSD,why?can you gave me some advice about it.thank you.
Back to top
 
 
  IP Logged
chuzi
Junior Member
**
Offline



Posts: 12
BeiJing China
Re: question in sigma-delta ADC
Reply #10 - Dec 29th, 2005, 4:58pm
 
hi Zheng,
   I do the same thing as you do, but I don't know where problem is because I can't see your detail.
   If your modulator is just 2-1 cascade 1-bit, I recommand a reffrence book to you:
   Shahriar Rabii, Bruce A.Wooley,"The Design of Low-Voltage, Low-Power Sigma-Delta Modulators" Kluwer Academic Publishers.
   It maybe what you need.
     Hope it helps.
       Best regards.
      chuzi
Back to top
 
 
View Profile   IP Logged
c.h.zheng
New Member
*
Offline



Posts: 6

Re: question in sigma-delta ADC
Reply #11 - Dec 30th, 2005, 1:29am
 
hi chuzi:
thanks for your advice.but i can't find the book that you said,could you gave me the copy of that book  to study?thanks !my emial add:wwwhzhenghao@163.com
Back to top
 
 
View Profile   IP Logged
chuzi
Junior Member
**
Offline



Posts: 12
BeiJing China
Re: question in sigma-delta ADC
Reply #12 - Dec 30th, 2005, 5:18pm
 
hi zhenghao,
   Your email address is invalid, my deliver failured. My book is borrow from library, and maybe you could find it in your library, it is very useful.
   In my simulink program, I mainly focus on integrator‘s
output, when modifying the scaling factors, first make sure integrator's output not to overload.
   Hope it helps.
   Best regards!
                             chuzi
Back to top
 
 
View Profile   IP Logged
sheldon
Community Fellow
*****
Offline



Posts: 751

Re: question in sigma-delta ADC
Reply #13 - Dec 30th, 2005, 6:54pm
 
Chuzi,

  There is a good description of the factors you might
want to explore, at this link

http://www.imse.cnm.es/esd-msd/WORKSHOPS/MIXMODEST/PRESENTATIONS/medeiro1.pdf

Medeiro has done a good job of breaking down the
factors that effect performance.

  Next, you might want to spend some more time
thinking about your overall methodology/strategy
for performing this design, in particular, look at the
stuff that Ken has written about top-down design. My
experience is that using just system level, Simulink,
and transistor level simulation is not going to get
you the result you want in the time you want.
You really need to think about using mixed-level
simulation. You will always need to run that final
simulation. You just want to run minimize the number
of times you run that two week long simulation.

                                              Best Regards,

                                                Sheldon
Back to top
 
 
View Profile   IP Logged
c.h.zheng
New Member
*
Offline



Posts: 6

Re: question in sigma-delta ADC
Reply #14 - Jan 1st, 2006, 8:14am
 
hi chuzi:
thanks for your advice,my email add:wwwzhenghao@163.com.could you try again,where are you?i'm  from chengdu,in china.could you tell me where that book can buy?thanks very much.
Back to top
 
 
View Profile   IP Logged
Pages: 1 2 
Send Topic Print
Copyright 2002-2024 Designer’s Guide Consulting, Inc. Designer’s Guide® is a registered trademark of Designer’s Guide Consulting, Inc. All rights reserved. Send comments or questions to editor@designers-guide.org. Consider submitting a paper or model.