Post by sweet_julia on Aug 17th, 2015, 9:27am
from the pss.png, I got dv/dt=48.35G for rising, 48.77G for falling edge
so the jitter=2.34mV/48.35G=48.4 fs for rising,
and =2.2mV/48.77G=45.1 fs for falling edge.
|
The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl Simulators >> Circuit Simulators >> convert noise to jitter https://designers-guide.org/forum/YaBB.pl?num=1224609785 Message started by youchen on Oct 21st, 2008, 10:23am |
|
Title: convert noise to jitter Post by youchen on Oct 21st, 2008, 10:23am I am sorry to re-post it here from Measurement. 1. I had tried to characterize the jitter for driven logic gates (for insance, a simple inverter) due to intrinsic device noise. According to Ken Kundert's paper - An Introduction to Cyclostationary Noise, there are three approaches to do that (on page 38). The first approach needs to determine the instantaneous noise power at the time of threshold crossing time. It is written that "SpectreRF can do this", but I wonder what SpectreRF analysis can do this. 2. On the other hand, I had used 'pnoise' for this purpose, but 'pnoise' gives the time-average of the noise at the output of the circuit in the form of a spectral density versus frequency, according to the reference guide. I was wondering how to convert the resulting noise spectrum to actual time-domain jitter? Thanks. |
|
Title: Re: convert noise to jitter Post by Frank Wiedmann on Oct 22nd, 2008, 12:45am Use pnoise jitter analysis. This is a special case of pnoise timedomain or strobed analysis (also known as tdnoise) where you specify a threshold level for the signal instead of a timepoint. ADE will also calculate some jitter values for pnoise jitter analysis. You can look at http://www.designers-guide.org/Forum/YaBB.pl?num=1092399689 for some further information (please note that the thread spans 3 pages). At the time when this thread was written, pnoise jitter analysis did not yet exist, so pnoise timedomain/strobed/tdnoise was used. |
|
Title: Re: convert noise to jitter Post by youchen on Oct 22nd, 2008, 10:45am Hi Frank, thanks a lot for your help. I will look into the thread to get started. But meanwhile, what is this 'pnoise jitter' analysis? I have IC5141 USR5 (released June 2007), I click on 'pnoise' but do not know how to have 'pnoise jitter' analysis? I really appreciate it. |
|
Title: Re: convert noise to jitter Post by Frank Wiedmann on Oct 23rd, 2008, 12:51am There should be a selection box called "Noise Type" in the setup form for pnoise analysis where one of the choices is "jitter". |
|
Title: Re: convert noise to jitter Post by youchen on Oct 23rd, 2008, 4:20pm thanks again, Frank. I had a simple inverter circuit driven by a clock to generate an inverse clock, and I just want to see what is amount of jitter for the inverse clock due to device noise. I used 'pss' analysis first. I do not know how to set either 'beat frequency' or 'beat period'. It seems by default it is the clock frequency or clock period. After 'pss', I run 'pnoise' and choose 'noise type' as jitter as you suggested. I select the output as the inverse clock voltage output and input source as the 'vpulse' from analogLib. 'Sidebands' is set to 100 and 'reference sideband' is 0 since the inverse clock output has the same frequency as the input clock. One thing I am not sure is the 'sweeptype', what is the difference between absolute and relative? However, in the compute power spectral density plot for the voltage output, the reported 'jittereventtime' (about 4ns) does not seem to be the correct transition time for inverse clock? I thought it should be 5ns for rising transitions based on the transient output. Maybe I either misunderstand something or I set something wrong for my simulation. Also, how do I then convert the PSD to time-domain jitter? Which ADE functions I should use? Thanks very much. |
|
Title: Re: convert noise to jitter Post by Frank Wiedmann on Oct 24th, 2008, 1:04am Beat frequency or beat period is a misnomer for many applications. It only really makes sense for mixer simulation with pss. The "beat period" is the time with which the entire circuit is periodic, the "beat frequency" is its inverse. If there are no frequency dividers in your circuit, "Auto Calculate" usually chooses the correct frequency. For jitter simulation, you should usually set "Sweeptype" to "absolute". The "jittereventtime" refers to the timescale of the pss timedomain result that you get when you select "time" for the "Sweep" parameter in the Direct Plot Form. Depending on your pss simulation setup (for example the "tstab" parameter), this may be different from the timescale in a transient analysis. The simulation result is exactly the same as for the corresponding tdnoise analysis, so you can use the method described in http://www.designers-guide.org/Forum/YaBB.pl?num=1092399689/20#20 to convert it to jitter. Alternatively, you have some jitter measurements available in the Direct Plot Form under "pnoise jitter". For some additional information, see http://sourcelink.cadence.com/docs/files/Application_Notes/2007/JitterAN0306.pdf. |
|
Title: Re: convert noise to jitter Post by youchen on Oct 27th, 2008, 1:18pm Frank, thanks for your continued help. I have used the method your introduced in that thread for jitter computation. So, set noise type in 'pnoise' to 'timedomain', then complete the simulation. From Direct Plot, I select 'tdnoise', 'integ output noise', 'total noise' and 'magnitude', and was able to get the RMS noise power at the jitter event time. Dividing that by slew rate, I obtained the jitter amount, which seems very reasonable. However, one thing confuses me is the units of measure for 'magnitude' shown in Direct Plot. I thought it should be 'V', not 'V/sqrt(Hz)', because the slew rate is by default 'V/s' so that the division would give 's' for jitter amount. Why is it shown as 'V/sqrt(Hz)'? Then, to confirm my jitter amout, I set noise type in 'pnoise' as 'jitter'. And I suppose that I should get the same jitter amount as before. Afer simulation, in Direct Plot, I select 'pnoise jitter', 'Jee' and it gives the jitter spectral density after clicking Plot. However, it did not give me the 'Jee' amount, as claimed in page 30 of the application note you gave me in last reply. Also I checked 'Jc' or 'Jcc', clicking Plot did not give any value either. What may be the problem? Thanks. |
|
Title: Re: convert noise to jitter Post by Frank Wiedmann on Oct 28th, 2008, 2:29am The unit for the Integrated Noise should indeed be V and not V/sqrt(Hz). This looks like an error in ADE to me. What you get when you select Jee in the Direct Plot Form is the strobed noise divided by the slope of the signal, so the unit Sec/sqrt(Hz) is correct in this case. In order to get Jee, you need to square the result, integrate it, and take the square root. It should then match your other result. The integrated Jee result is displayed as a marker in WaveScan but not in AWD, you can select the Waveform Tool in ADE under Session->Options. |
|
Title: Re: convert noise to jitter Post by youchen on Oct 28th, 2008, 4:00pm Frank, again thanks are due to you. I got the ‘Jee, Jc, Jcc’ as mentioned in my previous reply. Somehow, they show in my AWD plot, but not in WaveScan. Assuming the output of a driven circuit is a periodic clock-like signal. But due to device noise, there will be variations for this periodic signal. ‘Jee’ is edge-to-edge jitter, so it characterizes the jitter amount for a single edge. But the ‘Jee’ could be different for a rising or a falling edge due to different noise injection at those moments or even different slew rates, right? ‘Jc’ is the period jitter and a period is defined as the time duration of two consecutive rising/falling edges. But for the time duration defined by the rising edge following by the closest falling edge, (for example, this time duration is almost X% of the period if the ideal periodic clock-like output signal is designed to have X% duty cycle), how to calculate its jitter in ‘pnoise’? I think I can not simply find the ‘Jee’ for both edges and then take RMS of them, because they are correlated. In fact, I feel that this question is very similar to asking how ‘Jc’ is computed in ‘pnoise’ when there is correlation between two consecutive jittered rising/falling edges? Please correct me when I am wrong. thanks. |
|
Title: Re: convert noise to jitter Post by Frank Wiedmann on Oct 29th, 2008, 3:34am You are right that Jee can be different for different edges that occur during a period (the rising and the falling edge, but also different rising and falling edges if there are several of them during a period). I don't think that it's possible to simulate Jc between different edges in a period with pnoise jitter analysis. The calculator expression for Jc for 3 cycles at a "beat frequency" of 1 GHz for the rising edge at a node named "vout" is: Code:
For a different number of cycles, replace the 3 in the expression with that number. Also replace the number 1e9 with your "beat frequency" and the number 0.5e9 with half that value. I think that the strobed noise spectrum already includes the correlation between consecutive "identical" edges. |
|
Title: Re: convert noise to jitter Post by youchen on Oct 29th, 2008, 1:06pm Thanks, Frank. I guess that the calculator expression you gave me last time is for the so called 'K-cycle jitter' (K=3) (defined on page 12 of the application note)? I was also thinking that if the output signal is NOT periodic, then can we apply ‘pss’ and ‘pnoise’? For example, I have a driven circuit which is a 2-input NAND gate and the two inputs are non-periodic, so that the output is not periodic either, can we still apply ‘pss’ and ‘pnoise’ for this circuit? My guess is possibly yes, because I feel the essence of ‘pss’ is not exactly a periodic time-varying operating point, but a finite number of operating points (such as the low-high transition, high-low transition, high state and low state)? Or this case is where ‘qpss’ and ‘qpnoise’ would kick in? Further, if the output signal is non-periodic for a general driven circuit, then I guess only ‘Jee’ would make sense? What do you think? Thanks again. |
|
Title: Re: convert noise to jitter Post by Frank Wiedmann on Oct 30th, 2008, 2:14am Yes, the calculator expression is for k-cycle jitter and corresponds to equation (1-18) of the application note. You cannot do a pss analysis (and hence a pnoise analysis) for a signal that is not periodic. You need to create a periodic input signal that is representative of the non-periodic signal in your application. I don't think that qpss and qpnoise analyses would be suitable here. |
|
Title: Re: convert noise to jitter Post by youchen on Oct 30th, 2008, 3:00pm thanks for your reply, Frank. I think I know how to calculate time jitter due to intrinsic device noise. One more question I have is that how to simulate the time jitter caused by power supply noise and substrate noise? I looked into the user guide and I am under the impression that I need to model these noise as small signal noise and run 'pxf' analysis in SprectreRF? Also, how to measure power supply reject ratio for a general deriven logic circuit? Are there any other noise source causing jitter? thanks for your patience for helping me through this. |
|
Title: Re: convert noise to jitter Post by Frank Wiedmann on Oct 30th, 2008, 3:45pm I have mentioned other causes for jitter in http://www.designers-guide.org/Forum/YaBB.pl?num=1092399689/22#22. For the simulation of jitter due to disturbances on the power supply, see http://www.designers-guide.org/Forum/YaBB.pl?num=1187679312 and http://www.designers-guide.org/Forum/YaBB.pl?num=1178780148/5#5. |
|
Title: Re: convert noise to jitter Post by youchen on Oct 31st, 2008, 1:49pm thank you, Frank. I looked into the thread and can understand the idea. I also found an application note at sourcelink which taught how to measure PSRR, but that 'modulated pxf' is used instead of 'sampled pxf' analysis. So, still 'pss' first and then 'pxf'? what is the sweep type in 'pxf'? I seem to get a plot of the gain transfer function of the output with respect to the each supply voltage source in my driven logic circuit (in Results Browser), but how to transform it to the time-domain jitter? Still use 'pnoise' to do that? Your brief description is highly appreciated. |
|
Title: Re: convert noise to jitter Post by youchen on Oct 31st, 2008, 3:28pm I would suppose also that there should be a field to specify the characteristics of the power noise, such as the amplitude and the frequency spectrum, because these should affect the amount of jitter. But I do not know how to do that. |
|
Title: Re: convert noise to jitter Post by Frank Wiedmann on Nov 1st, 2008, 2:19pm You always have to do a pss analysis first for the periodic small-signal analyses pac, pxf, and pnoise because the pss analysis determines the periodic operating point for these analyses. If you want to simulate jitter, use sampled pxf with an absolute frequency sweep. As mentioned in http://www.designers-guide.org/Forum/YaBB.pl?num=1187679312/1#1, you convert the result to jitter by dividing it by the slope of the signal, in the same way as for tdnoise. As you correctly noted, the result is a transfer function, so there is no need (and no possibility) to specify an input spectrum. |
|
Title: Re: convert noise to jitter Post by youchen on Nov 2nd, 2008, 11:00am Hi Frank, to make sure I do it correctly, can I formulate it as follows? After 'sampled pxf' analysis, I got two tranfer function plot with respect to the Vdd and Vss. So, suppose I know that the power noise or substrate noise is characterized by a sinwave of 1mV and 1MHz, then I find the resulting noise at the output by mulitiplying 1mv with the gain at 1MHz. Finally, I divide the resulting noise by the slope, which gives me the jitter. Is that right? If it is, I was wondering what if the power or substrate noise is not well approximated as a sinwave, but with a certain spectrum, for example 100k to 1MHz, because in reality the power noise is very complicated? Thanks very very much. |
|
Title: Re: convert noise to jitter Post by Frank Wiedmann on Nov 3rd, 2008, 1:09am Yes, this is right. By the way, for the division by the slope, you can take the last part of the calculator expression in reply #9 as a reference. In most cases, you will not know excatly in advance what the disturbances on the power supply will look like. The transfer functions should help you to identify and fix possible weaknesses in your design which might only exist in certain frequency ranges. If you know the disturbances on the power supply exactly, the easiest way to simulate the resulting jitter is probably to model them with time-domain sources, do a transient analysis, and evaluate the result with the help of the eyeDiagram calculator function. |
|
Title: Re: convert noise to jitter Post by youchen on Nov 3rd, 2008, 8:49am Hi Frank, thanks. You also mentioned about jitter caused by intersymbol interference in other threads, what does that exactly mean? Finally, if we want to consider the total jitter, do we simply add the individual jitter caused by device noise, power supply noise, and intersymbol interference (if we consider only the three sources)? I think it is reasonable since they should be independent from each other, at least between device noise and power supply noise. |
|
Title: Re: convert noise to jitter Post by youchen on Nov 3rd, 2008, 11:05am Hi Frank. I have one more question. Is there a way to simulate jitter caused by both device noise and power supply noise in 'pnoise' analysis? thanks. |
|
Title: Re: convert noise to jitter Post by Frank Wiedmann on Nov 3rd, 2008, 1:25pm Regarding intersymbol interference, see for example http://en.wikipedia.org/wiki/Intersymbol_interference (which is the first result of a Google search for this term, by the way). Yes, you should add the jitter due to these three sources (because two of them represent deterministic jitter). You could try to model the disturbances on the power supply with ideal noise sources connected to the supply. However, I am not sure if this would be a very realistic model of these disturbances; usually they do not really look like noise, in spite of often being called "power supply noise". |
|
Title: Re: convert noise to jitter Post by youchen on Nov 3rd, 2008, 4:03pm Hi Frank, I guess I have to bother you with one more question. I get the transfer function plot from 'sampled pxf' analysis, but there seems to be a transfer function for each harmonic (from harmonic=-10 to harmonic=+10)? I guess I only need to look at the one for harmonic=0, right? I wonder the 21 transfer functions (including harmonic=0) are obtained because of 'maximum sideband' set to 10? In 'pnoise', the 'maximum sideband' should be reasonably large in order to account for enough noise folding. What about the 'maximum sideband' in 'pxf' analysis, also be set very large? In 'pss' analysis, a parameter is 'number of harmonics' (default set to 9 for shooting and 10 for harmonic balance). What does this parameter do in 'pss'? I feel that it is not important for a driven circuit, but useful for an autonomous circuit. |
|
Title: Re: convert noise to jitter Post by Frank Wiedmann on Nov 4th, 2008, 1:10am For sampled pxf analysis, you can set "Maximum sideband" to 0 in the pxf setup form. This will eliminate the other harmonics which do not provide any additional information (they give the same result, possibly shifted in frequency and mirrored, depending on the freqaxis parameter). The "Number of harmonics" in the pss setup form does not have any influence on the result (if you use the "Shooting" Engine, which you should do for jitter analysis). It is only used to set the number of harmonics available for display when you want to look at the result of the pss analysis in the frequency domain. |
|
Title: Re: convert noise to jitter Post by Frank Wiedmann on Nov 5th, 2008, 12:43am Another point that I should probably add is that the random jitter due to device noise has a Gaussian distribution and the simulated jitter value is the standard deviation or rms (root mean square) value of this distribution. The "maximum random jitter" depends on the percentage of events in which this value may be exceeded (often defined as bit error rate) and is usually some multiple of the standard deviation. For example, if you look at the figure in http://en.wikipedia.org/wiki/Jitter, you can see that in 0.3% of the cases, the jitter will exceed ±3 times the standard deviation. For lower values of the bit error rate (BER), see for example the table in http://www.sigcon.com/Pubs/edn/RandomJitter.htm. |
|
Title: Re: convert noise to jitter Post by youchen on Nov 5th, 2008, 12:54pm Frank, thanks for your notes. I guess in realistic circuits, the jitter caused by power supply noise seems to be much larger than that by device noise. In other threads, you noted that the extracted jitter from transient simulation matches well that from 'sampled pxf' analysis considering only power supply noise. For device noise only, have you ever compared the extracted jitter from transient noise simulation to that from 'pnoise' analysis? I am just curious. I noticed that transient noise is much slower than 'pnoise'. |
|
Title: Re: convert noise to jitter Post by Frank Wiedmann on Nov 6th, 2008, 2:05am I have also seen pretty good matching with transient noise (if all the settings are correct there). The advantage of pnoise over transient noise is not only that it is often faster but also that you can see where the noise comes from in the Noise Summary. |
|
Title: Re: convert noise to jitter Post by youchen on Nov 6th, 2008, 3:56pm Hi Frank. How to start Noise Summay? I tried to find the important noise sources by looking into the noise from each transistor in Results Browser. Talking about noise sources, is there a way to instruct 'pnoise' to analyze only part of the circuit (the rest assumed noise-free)? Is it possible to do this in transient noise too? |
|
Title: Re: convert noise to jitter Post by Frank Wiedmann on Nov 7th, 2008, 12:36am In Virtuoso Analog Design Environment, select Results->Print->Noise Summary. I don't know of a general way to set the noise of a part of the circuit to zero. However, some components may have parameters that permit setting their noise to zero. |
|
Title: Re: convert noise to jitter Post by youchen on Nov 8th, 2008, 10:38am Frank, thanks for your kind and patient help. |
|
Title: Re: convert noise to jitter Post by youchen on Nov 12th, 2008, 10:58am Hi Frank. I notice that the transient analysis gives different timing delays over time for the same driven logic circuit. However, since transient analysis does not consider device noise (no other noise is injected either), why the timing delay is not constant over many cycles? I understand the initial transient effect may cause that, but I am supposing that the delay should approach constant as time goes on. I do not seem to see that. |
|
Title: Re: convert noise to jitter Post by Frank Wiedmann on Nov 12th, 2008, 11:37pm If you are not using Transient Noise, the reason is probably limited numerical accuracy of the simulation. Have you tried setting Accuracy Defaults to conservative in the tran setup form? |
|
Title: Re: convert noise to jitter Post by hiSkill_11 on Apr 24th, 2012, 12:47am Hi, Frank, I am doing sampled pxf for measuring the tf from power supply to jitter( 40MHz crystal oscillator), but I can't setup the pxf analysis form because I don't know what should be typed into the probe field though I can select the output clk net into the voltage field. I don't known exact meaning of the probe signal and it's purpose as well. Could you help me on that? Also I want to know the meaning and the effect of the maximum samples and sample delay on the result. Thanks in advance. Frank Wiedmann wrote on Nov 1st, 2008, 2:19pm:
|
|
Title: Re: convert noise to jitter Post by Frank Wiedmann on Apr 24th, 2012, 2:50am I have answered your questions at http://www.designers-guide.org/Forum/YaBB.pl?num=1335172697. |
|
Title: Re: convert noise to jitter Post by sweet_julia on Aug 16th, 2015, 8:19am Hi Frank, I have read many threads from you about how to simulate the random jitter from device using PSS+Pnoise. Unfortunately, I didn't got consistent results from tdnoise and pnoise jitter. I would like to describe my question here. The circuit I am simulating now consists of one input 16GHz buffer, divider, 4GHz buffer, CML MUX, 4GHz buffer, and one CML phase interpolator. I set the noise type to "jitter". In the tdnoise, I could get the integrated output noise N. From the PSS, I could get the dv/dt at both rising edge and the falling edge. By using the equation in chapter 9, I could get the Jee ~200fs. However, if I use the pnoise jitter directly, the integrated jee I got is around 400fs. Do you have idea what causes this discrepancy? You help is highly appreciated. Regards, Julia |
|
Title: Re: convert noise to jitter Post by Frank Wiedmann on Aug 17th, 2015, 4:20am If you specified the timepoint for the tdnoise analysis correctly, the reason for the discrepancy can only be an error in your formulas or a misunderstanding about how Jee is calculated. The tdnoise and pmjitter analyses are practically identical, the only difference is how the timepoints for the analysis are specified. When you plot the results from the results browser, you should get identical results from the pnoise_td and the pnoise_pmjitter folders. |
|
Title: Re: convert noise to jitter Post by sweet_julia on Aug 17th, 2015, 8:31am Hi Frank, I just know that the jee contains DSB noise, is it possible that the integrated output noise contains only SSB noise? |
|
Title: Re: convert noise to jitter Post by Frank Wiedmann on Aug 17th, 2015, 8:48am The pnoise timedomain and pmjitter analyses simulate sampled noise. I am not sure if talking about DSB and SSB noise is very meaningful in this context. |
|
Title: Re: convert noise to jitter Post by sweet_julia on Aug 17th, 2015, 9:17am Hi Frank, I am sorry I dont know how to attach three pics in one thread... I set the noise type to "jitter", and then plot the integrated output noise shown below |
|
Title: Re: convert noise to jitter Post by sweet_julia on Aug 17th, 2015, 9:27am from the pss.png, I got dv/dt=48.35G for rising, 48.77G for falling edge so the jitter=2.34mV/48.35G=48.4 fs for rising, and =2.2mV/48.77G=45.1 fs for falling edge. |
|
Title: Re: convert noise to jitter Post by sweet_julia on Aug 17th, 2015, 9:30am However, the jee I got is twice of what I got from the calculation. I am kind of desperate here...really dont know where the problem is... BTW, I am simulating a 16GHz buffer, and I integrate from 1Hz to 8GHz. Frank, your help is really really appreciated. Thanks, Julia |
|
Title: Re: convert noise to jitter Post by Frank Wiedmann on Aug 18th, 2015, 1:13am There are rather few points in your pss results, which might make the calculation of the derivative inaccurate. Try to increase the number of points by increasing the value of the maxacfreq parameter (in the pss form press the Options button and select the Accuracy tab). |
|
Title: Re: convert noise to jitter Post by sweet_julia on Aug 18th, 2015, 10:59am Hi Frank, I can not thank you more for your kind help. Finally I got the problem solved and got the consistent results! I like analog IC very much despite I could be frustrated by it sometimes LOL. Frank, thank you;-) Best Regards, Julia |
|
Title: Re: convert noise to jitter Post by foxbeibei on Dec 27th, 2015, 10:10pm Hi Frank, for the following case, the 1mV is the amplitude of the sinewave or is the peak-to-peak values? i tried to use the sampled pxf method you suggested but found that the jitter values calculated this way is half of the transient aboslute jitter. can you please answer this question? thanks, foxbeibei youchen wrote on Nov 2nd, 2008, 11:00am:
|
|
Title: Re: convert noise to jitter Post by Frank Wiedmann on Jan 18th, 2016, 4:28am If you are looking at peak-to-peak jitter, the 1mV should be the peak-to-peak value of the sinewave. |
|
Title: Re: convert noise to jitter Post by Frank Wiedmann on Jan 18th, 2016, 4:45am Frank Wiedmann wrote on Nov 7th, 2008, 12:36am:
This is now possible by using the noiseoff_inst option (see http://community.cadence.com/cadence_technology_forums/f/33/t/32451). |
|
Title: Re: convert noise to jitter Post by federico.butti on Nov 16th, 2016, 5:31am Hi, I have a question for the experts here! I am doing a SUBsampled PXF analysis (and a sampled PAC analysis) for a driven circuit (cml2cmos converter + inverters) to simulate supply noise. The thing that confuses me is the following: 1) fclk = 100 MHz 2) supply noise BW = 1k-300 MHz Therefore I set PSS fundamental as 100 MHz. In my understanding, sampled PXF output is the contribution of each input sideband to the output frequency sweep chosen, which in this case should be Nyquist BW (50 MHz). Therefore, in the plot I see the first input sidebands which combined reaches 300 MHz (supply noise BW). Is this a correct way of seeing this thing? I suppose that if one wants to have the actual spectrum of the output sample sequence, one should sum up in the Nyquist BW all the input sidebands with the related folding, i.e. BW 0 between 0-50 MHz, sideband -1 between 50 and 100 MHz and so on, due to the subsampling. In case noise BW would be smaller than 50 MHz, no subsampling would occur and therefore result would be correct without summing and folding, simply by taking sideband 0. Am I right? |
|
The Designer's Guide Community Forum » Powered by YaBB 2.2.2! YaBB © 2000-2008. All Rights Reserved. |