Keyboard Shortcuts
ctrl + shift + ? :
Show all keyboard shortcuts
ctrl + g :
Navigate to a group
ctrl + shift + f :
Find
ctrl + / :
Quick actions
esc to dismiss
Likes
- LTspice
- Messages
Search
|
Re: FFT Resolution
John Woodgate
In message
<CALBs-TipQ2tWb71L_jO+d3CysuyxmNHd1cAx+162RVC-OCHd9g@...>, dated Mon, 16 Dec 2013, Andy <Andrew.Ingraham@...> writes: You need at least two time samples at the highest frequency of the FFT.Thanks. I hope that makes it all clear: To get x Hz resolution, you should, in practice, simulate for 2/x seconds. You can simulate for longer to get a clearer spectrum display, say N/x seconds. To get a spectrum up to X Hz, you then need more than 2*N*X/x samples, preferably the next higher power of 2. I do think that, if it's correct, is a bit more lucid than the Help text. -- OOO - Own Opinions Only. With best wishes. See www.jmwa.demon.co.uk Nondum ex silvis sumus John Woodgate, J M Woodgate and Associates, Rayleigh, Essex UK |
|
MMBTH81 transistor model
kalias
I am trying to create a model for the MMBTH81 transistor.? I extracted the following model from the datasheet and put it in a LTspice schematic with a directive. ? .MODEL MMBTH81? PNP(Is=10f Xti=3
+ Eg=1.11 Vaf=100 Bf=133.8 Ise=1.678p + Ne=2.159 Ikf=.1658 Nk=.901 Xtb=1.5 Var=100 Br=1 + Isc=9.519n Nc=3.88 Ikr=5.813 Rc=7.838 Cjc=2.81p + Mjc=.1615 Vjc=.8282 Fc=.5 Cje=2.695p Mje=.3214 Vje=.7026 + Tr=11.32n Tf=97.83p Itf=69.29 Xtf=599u Vtf=10) ? The reason that I have picked this device is that it should provide a better gain bandwidth than a 3906.? However in my simulation I have two identical circuits and it seems as if the performance is the same.? Is there something wrong with this model?
? I compared the model file of this device to that of the 3906 and there appears to be something missing.? There is no Rb = or Re=.? Could this model be flawed or am I doing something incorrect? ?
kalias |
|
Re: FFT Resolution
John Woodgate asked: This is all good stuff, but could you please comment in the OP's You need at least two time samples at the highest frequency of the FFT. 1/90MHz * 0.5 = 5.56 ns Helmut's example simulates for 20 ms, which actually gives you 50 Hz resolution, enough to see the "trough" between alternate components that are 100 Hz apart. ?Given that, you need at least 3600000 for the "Number of data point samples in time" to have time samples no greater than 5.56 ns apart. ?Using Helmut's recommended 4194304 (= 2^22) gives you that. ?That simulation's FFT goes up to (1/2) * 1/(20ms/4194304) = 104.858 MHz, which is what I see when I run it.
Using the bare minimum (3600000) probably stops exactly AT 90 MHz and isn't enough to show you the 90 MHz component. ?So always go higher if there is any doubt.
Andy |
|
Re: FFT Resolution
John Woodgate
In message
<CALBs-TgcwTBCyW1+=wNz4R7Yk09QHzk1sbNYC1ii8HU7SecrFg@...>, dated Mon, 16 Dec 2013, Andy <Andrew.Ingraham@...> writes: Here are some tips.This is all good stuff, but could you please comment in the OP's question about analysing a 10 MHz square wave with a resolution of 100 Hz? Given that 20 ms is long enough to get 100 Hz resolution, how many data points are required to get up to, say, 90 MHz? -- OOO - Own Opinions Only. With best wishes. See www.jmwa.demon.co.uk Nondum ex silvis sumus John Woodgate, J M Woodgate and Associates, Rayleigh, Essex UK |
|
Re: CD74HC4017E.sym missing pins
Steve wrote:
That depends on the component's SPICE model. Some SPICE models do not require power connections because the model itself implicitly includes power. A more complete SPICE model should have power and (floating) ground pins too. ?(By floating, I mean not already connected to GND = Node 0.)
Adding power and ground pins to an LTspice symbol should be easy. ?Just add them, like you added every other pin to the symbol. ?Are you trying to modify an existing symbol, or creating your own from scratch? ?It would help if you explained what the actual difficulty is, rather than just saying you "can't add them", since, of course you can.
Note that if you have a SPICE model in the form of a subcircuit for your component, the symbol must have exactly the same pins on it as the subcircuit has.
Regards,
Andy |
|
Re: FFT Resolution
ronw6wo?wrote:
I think "the value of the window" as used before, refers to the time interval that was simulated and sent to the FFT. ?Not the number of cycles, but the number of seconds of time.
You could take Helmut's example and change V2 from a Sine wave source to a Pulse source.
Andy |
|
Re: FFT Resolution
ronw6wo?wrote, " Here are some tips. (1) ?To get finer frequency resolution in the FFT results, you need to use longer simulation times. ?The two are directly related. For 100 Hz frequency resolution, the total time interval of the waveform data that is sent to the FFT must be 1/100Hz = 0.01 seconds = 10 ms. ?But to examine discrete components that are 100 Hz apart, you might want the frequency resolution to be at least twice as good as that (if not more) ... so simulate for 20 ms if not 40 ms or more. ?Then you can see the dips between the components too. ?Otherwise it tends to look like a big blob and it's hard to tell one component from the next.
(2) ?The "Number of data point samples in time" and the total time interval determine the upper frequency limit of the FFT. ?If the FFT doesn't go up high enough in frequency to show the components you want to see, repeat the FFT with more data point samples in time. ?Hopefully you have simulated with fine enough time steps so that the FFT isn't using fake data (see later, about "Tstep" and "plotwinsize").
An FFT works best when the number of data point samples is a power of 2 (hence LTspice starts with a default of 262144 data points), but I believe LTspice's algorithm does not require a power of 2. ?Just the same, I'd go with the power of 2 in case it impairs accuracy not to use it.
When in doubt, click "Reset to Default Values" at the bottom of the FFT dialog window, then use the up/down arrows to try other powers-of-two.
(3) ?LTspice's FFT display has a truly annoying characteristic when you zoom in to see the individual components of the FFT: ?Each component looks like an arch. ?I think that happens because LTspice does a linear interpolation between the points, BEFORE it computes a logarithm to turn it into Decibels for display. ?Hence you end up with those deceptive arch-like bumps. ?(Note: LTspice's developer says this is actually intentional. ?Not a bug. ?Could've fooled me.)
The apparent "width" of those bumps means nothing and does not imply a width of the components present! ?The tip of each bump is the ONLY thing that matters. ?The sides of the bumps are meaningless.
You can highlight the individual FFT components (right-click in the FFT window, then "Mark Data Points"), and then LTspice draws little dots at the actual FFT components. ?The curves between the dots are interpolations, not real data, and should be ignored. ?Be aware that turning on the display of those data point dots can make LTspice VERY slow and unresponsive when there are a very large number of data points on your screen. ?But this is the only way to see what's really there when your FFT's resolution is 100 Hz and you need to see frequency components every 100 Hz.
(4) ?Many things affect the apparent accuracy of the FFT results, i.e., the "noise floor" of the FFT plot, the appearance of extraneous signal components, etc. Most important is to simulate (and send to the FFT) an integral number of cycles. ?If you have multiple known components present, use an integral number of cycles of ALL of them, if you can. ?In Helmut's example, the time interval (20 ms) is a multiple of both 10.0000 MHz and 10.0001 MHz.
Here's why. The time-domain simulation generates a bunch of data points running from t=0 to t=Tstop = Stop Time. ?Think of turning that into a continuous waveform, by repeating that interval indefinitely. ?This is effectively what the output of the FFT represents. ?When you "splice" the waveform at t=0 to the waveform at t=Tstop, is it continuous, or is there a "glitch" at the splice? ?If there's a glitch, the waveform effectively has a modulation applied to it, which shows up in the spectrum as unwanted sidebands around everything and an increased noise floor.
In the FFT dialog box, the "Time range to include" controls the amount of waveform sent to the FFT. ?Normally one would "Use Extent of Simulation Data". ?A case where you might not do that, is when the simulation includes a start-up transient, and you want to include only the steady-state waveform after that transient has died. ?Make sure the time range you include, has the integral number of cycles, even if the total simulation time does not.
Simulating over many cycles seems to work better than simulating fewer cycles. ?I think it allows mathematical errors to average out better, and this reduces the FFT's noise floor and spurious components in the display.
When it is impossible to simulate for an integral number of cycles of all components, that's when one of the Windowing functions is used. ?My understanding is that they force the pre-FFT, time-domain data to fall somewhat gracefully to zero at t=0 and at t=Tstop. ?Thus, a nasty glitch is avoided when you "splice" the ends together. ?Instead, a gentler modulation is applied to your signal, so it still causes sidebands to appear in the output spectrum.
(5) ?It helps to turn off waveform compression in the time-domain data:
.options plotwinsize=0
Also, make Tstep (Maximum Timestep) as small as practical. ?The less interpolation between data points that the FFT needs to do, the better. (6) ?Enabling double precision may also help: .options numdgt=15 Regards,
Andy |
|
Re: LTspice Install problem under linux
"Business Kid" wrote, "Is this a 'known issue?' (m$ speak for A BUG)? Where should I report it?"
The way to report bugs (if it continues to be one) is via email to: "LTspice @ " (remove the spaces).
For you other LTspice users: from within LTspice, click on
? Help > About LTspiceIV and it shows you the email address for bug reports and suggestions.
Regards,
Andy |
|
Re: LTspice Install problem under linux
Hello, I also had a problem to update LTspice on two WIN7 PCs the last week. When I clicked on Sync Release, it simply did nothing. It behaved like when another LTspice is open. I rebooted the PCs and then the update worked. Please try immediately after reboot. Best regards, Helmut ? |
|
LTspice Install problem under linux
Business Kid
I can't install the latest update in linux. It certainly doesn't go in painlessly like the last one did, and may need shoehorning in. That's a pity, because I uninstalled the older version. Is this a 'known issue?' (m$ speak for A BUG)? Where should I report it? |
|
Re: FFT Resolution
John Woodgate
In message <ENcQOfEjUjrSFwah@...>, dated Sun, 15 Dec 2013, John Woodgate <jmw@...> writes:
I'm sorry: I got a bit confused myself in trying to explain this and I inadvertently sent it before I'd fixed the text. Please disregard. -- OOO - Own Opinions Only. With best wishes. See www.jmwa.demon.co.uk Nondum ex silvis sumus John Woodgate, J M Woodgate and Associates, Rayleigh, Essex UK |
|
Re: My collection of models and examples for LTspice.
Hi.
My file 100MEG LTspiceDoc contained different files with instructions on using LTspice. These files I found on the internet. Files including in Russian. Links to some of them are in this group. These files can be useful for beginners. To reboot I have technical difficulties (very slow internet). Bordodynov. |
|
Re: Questions about phase in .AC LTspice Analysis
hoa van nguyen
Hello Andy, Thank for sharing your thoughts with me. I discover something that I do not understand. Maybe you or other people can answer my questions. All 2stages_2CascodeDiff_ACsim_test1_orig.asc, Readme,Cmosedu_models.txt, 2stages_2CascodeDiff_ACsim_test1_orig.jpg (graph) are under Files > temp > GainPhase_inAC (folder). 1) from the graph 2stages_2CascodeDiff_ACsim_test1_orig.jpg: the difference of first stage outputs (Vodp - Vodm) = 2dB, but the Difference of second stage outputs (Vod - Vom) = 0.6dB. Q: Why the Vod & Vom are nearly equal now? (Improved) 2) At f=30MHz the Vodp-phase goes up to positive, but the the gain is below 0dB. Q: How does the diff. Amplifier behave in real life at this frequency? Best Regards Hnguyen On Tuesday, December 10, 2013 4:01 PM, Andy
wrote:
?
Hnguyen wrote: "Q1: Why |Vop| and |Vom| are nearly equal??why not equal?"
A1: ?Ideally they are equal. ?Real circuits are not ideal. ?If there is any common-mode component present in the output signal, the two output pins would not be precisely complementary and then their amplitudes might not be equal.
"
A2: ?When exactly complementary, if you look at their AC components (and ignore the DC offset), V(vom) = -V(vop).
V(vop,vom) = V(vop)-V(vom) = V(vop)-(-V(vop)) = 2*V(vop).
So, in an AC simulation, the amplitudes of vop and vom should be equal, and the amplitude of V(vop,vom) should be 6 dB higher.
Andy |
|
Re: FFT Resolution
Hello Ron,
If you want 100Hz resolution, you have to simulate at least 1/100s=10ms. I have uploaded an example "fft10meg.asc" to the Temp-folder folder. I simulated 20ms. http://groups.yahoo.com/neo/groups/LTspice/files/%20Temp/ Run the simulation. Then in the FFT dialog window choose 4194304 samples. Please be aware that the FFT/DFT only looks so perfect because my second source has 100Hz offset which exactly fits to the FFT's frequency resolution. If this is not the case, one would try with a window function to get a good resolution. Best regards, Helmut |
|
Re: A Noisy Question
I guess my question with respect to noise and LTspice is how the time step between noise samples is established? And, how is it then interpreted - as a PWL source, for example??All I see is .noise - I don't see how to create a time-domaine noise signal is LTspice. To do an FFT on the noise, doesn't it have to be in the time domain? I see rand() but that appears to be uniform, not gaussian.?
toggle quoted message
Show quoted text
The time between noise samples must set the upper frequency of the noise spectrum (maybe at 1/2T, where T is the sample interval ??). Where and how is T set in LTspice?? And, if the noise samples are taken as points in a PWL, then that says how the system treats that source between the sample points. Or, is there no "between the sample points"? I see random() which says it is smoothed between samples, but still nothing about the time interval between samples. I hope these questions make sense, because I am not totally certain what I am asking about :) [If I were certain, I probably would not have to ask!!] Thanks Jim Wagner On Dec 15, 2013, at 1:40 PM, David Hawkins wrote:
|
|
Re: FFT Resolution
John Woodgate
In message <l8l5j2+4h2m77@...>, dated Sun, 15 Dec 2013,
ronw6wo@... writes: It isn't very clear. No. It's the 'width' in frequency of one window. Working backwards through that last bit in the Help, to get 100 Hz resolution, the window width is 1/100 s = 10 milliseconds. You need to consider at least harmonics up to the ninth, 90 MHz, so the number of samples has to be at least 90 MHz/100 Hz = 90000. LTspice supports much larger numbers. But the necessary simulation time may be archaeological. Your spectrum analyser works in the analogue domain, so the only time constraint is the settling time of the 100 Hz filter, which might be as long as 100 ms. So you do need to sweep the frequency slowly enough. -- OOO - Own Opinions Only. With best wishes. See www.jmwa.demon.co.uk Nondum ex silvis sumus John Woodgate, J M Woodgate and Associates, Rayleigh, Essex UK |
to navigate to use esc to dismiss