Post by thread:[EE] LTSPICE plot variables

I searched the entire documentation and more but couldn't find what I'm looking for. How does one include schematic variables or values in plot calculations? For example, I'm trying to plot reactance via R = 1/2*pi*frequency*C via a small signal AC analysis. I guessed that the plot variable for frequency would be "frequency", but I have no idea how to refer to the value for my capacitor. For example, getting the V or I can be done with V(n001) or I(R1) or something like that

On Wed, Jun 6, 2012 at 4:19 AM, V G <spam_OUTx.solarwind.xTakeThisOuTgmail.com> wrote: > I searched the entire documentation and more but couldn't find what I'm > looking for. > > How does one include schematic variables or values in plot calculations? > For example, I'm trying to plot reactance via R = 1/2*pi*frequency*C via a > small signal AC analysis. I guessed that the plot variable for frequency > would be "frequency", but I have no idea how to refer to the value for my > capacitor. For example, getting the V or I can be done with V(n001) or > I(R1) or something like that. >

On Wed, Jun 6, 2012 at 6:37 AM, Oli Glaser <.....oli.glaserKILLspam@spam@talktalk.net> wrote: > If I understand what you are asking for: > > 1. Run the simulation. > 2. Right click the graph and select "add trace". > 3. In the box add the V/I of the relevant component - e.g. something like > V(n001)/I(C1) > 3. Press OK and it should plot in Ohms - to view real and imaginary parts > left click on the y axis values (cursor changes to a ruler) and select > "cartesian" in the drop down box (default is "bode", or nyquist is the > other option) > > Hope this helps.. > I tried all that, everything I could think of, before posting. This is what LTSPICE is showing me for the calculated impedance graph (red) and I don't really know why. If I punch those numbers (the red graph's equation) into a calculator, I get expected values for the capacitor's impedance. But for some reason, the graph looks really strange with really odd values in LTSPICE. The green and blue graphs look fine though. Screenshot: http://i.imgur.com/hQXwn.pn

Really dumb thought - Bob Pease says that someone he knows (worked with?) said to use 50.1 Ohms instead of just 50 Ohms - somehow, that got rid of weirdness. Might it apply to your situation - I really don't know. But that little tidbit of info got tucked into my brain when I read it and I'm just passing it on. dwayne At 02:49 AM 6/7/2012, V G wrote: > This is what >LTSPICE is showing me for the calculated impedance graph (red) and I don't >really know why. If I punch those numbers (the red graph's equation) into a >calculator, I get expected values for the capacitor's impedance. But for >some reason, the graph looks really strange with really odd values in >LTSPICE. The green and blue graphs look fine though. > >Screenshot: http://i.imgur.com/hQXwn.png -- Dwayne Reid <dwaynerKILLspamplanet.eon.net> Trinity Electronics Systems Ltd Edmonton, AB, CANADA (780) 489-3199 voice (780) 487-6397 fax http://www.trinity-electronics.com Custom Electronics Design and Manufacturing

On Thu, Jun 7, 2012 at 9:49 AM, V G <.....x.solarwind.xKILLspam.....gmail.com> wrote: {Quote hidden}> On Wed, Jun 6, 2012 at 6:37 AM, Oli Glaser <EraseMEoli.glaserspam_OUTTakeThisOuTtalktalk.net> > wrote: > > > If I understand what you are asking for: > > > > 1. Run the simulation. > > 2. Right click the graph and select "add trace". > > 3. In the box add the V/I of the relevant component - e.g. something like > > V(n001)/I(C1) > > 3. Press OK and it should plot in Ohms - to view real and imaginary parts > > left click on the y axis values (cursor changes to a ruler) and select > > "cartesian" in the drop down box (default is "bode", or nyquist is the > > other option) > > > > Hope this helps.. > > > > I tried all that, everything I could think of, before posting. This is what > LTSPICE is showing me for the calculated impedance graph (red) and I don't > really know why. If I punch those numbers (the red graph's equation) into a > calculator, I get expected values for the capacitor's impedance. But for > some reason, the graph looks really strange with really odd values in > LTSPICE. The green and blue graphs look fine though. > > I just tried that circuit and it works fine for me. Only thing I can think of is that you are trying to plot just the real component of C1, which will be 0 if you have not set the ESR of C1 to a realistic value (say 100mOhm or whatever). So this means you probably have "don't plot imaginary component" set. If you left click on the right side axis and press ok you should get the imaginary component plotted (the axis should show e.g. 10KiOhm, 20KiOhm, etc, with the i being for imaginary) which should be what you expect. Let me know how it goes..

Just wondering whether that's just using familiar speech patterns or did you not realize that Bob Pease died, just about 1 year ago, June 18. http://www.ti.com/ww/en/bobpease/index.html Joe W On 6/7/2012 12:14 PM, Dwayne Reid wrote: {Quote hidden}> Really dumb thought - Bob Pease says that someone he knows (worked > with?) said to use 50.1 Ohms instead of just 50 Ohms - somehow, that > got rid of weirdness. > > Might it apply to your situation - I really don't know. But that > little tidbit of info got tucked into my brain when I read it and I'm > just passing it on. > > dwayne > > > At 02:49 AM 6/7/2012, V G wrote: >> This is what >> LTSPICE is showing me for the calculated impedance graph (red) and I don't >> really know why. If I punch those numbers (the red graph's equation) into a >> calculator, I get expected values for the capacitor's impedance. But for >> some reason, the graph looks really strange with really odd values in >> LTSPICE. The green and blue graphs look fine though. >> >> Screenshot: http://i.imgur.com/hQXwn.png >

At 11:23 AM 6/7/2012, Joe Wronski wrote: >Just wondering whether that's just using familiar speech patterns Yep >or did you not realize that Bob Pease died, just about 1 year ago, June 18.. >http://www.ti.com/ww/en/bobpease/index.html Yeah - he died about a week after we lost one of my other heros - Jim Williams. It was a bad week for the electronics community. Bob Pease *hated* SPICE because, he said, that it always lied to him. But he did recognize that many people do actually get good results from it and he passed on that tip. I have NO idea if it applies to LTspice. dwayne {Quote hidden}>Joe W > > >On 6/7/2012 12:14 PM, Dwayne Reid wrote: > > Really dumb thought - Bob Pease says that someone he knows (worked > > with?) said to use 50.1 Ohms instead of just 50 Ohms - somehow, that > > got rid of weirdness. > > > > Might it apply to your situation - I really don't know. But that > > little tidbit of info got tucked into my brain when I read it and I'm > > just passing it on. > > > > dwayne > > > > > > At 02:49 AM 6/7/2012, V G wrote: > >> This is what > >> LTSPICE is showing me for the calculated impedance graph (red) and I don't > >> really know why. If I punch those numbers (the red graph's > equation) into a > >> calculator, I get expected values for the capacitor's impedance. But for > >> some reason, the graph looks really strange with really odd values in > >> LTSPICE. The green and blue graphs look fine though. > >> > >> Screenshot: http://i.imgur.com/hQXwn.png > > >

On Thu, Jun 7, 2012 at 12:20 PM, Oli Glaser <oli.glaserspam_OUTtalktalk.net> wrote: > I just tried that circuit and it works fine for me. Only thing I can > think > of is that you are trying to plot just the real component of C1, which will > be 0 if you have not set the ESR of C1 to a realistic value (say 100mOhm or > whatever). > So this means you probably have "don't plot imaginary component" set. If > you left click on the right side axis and press ok you should get the > imaginary component plotted (the axis should show e.g. 10KiOhm, 20KiOhm, > etc, with the i being for imaginary) which should be what you expect. > Let me know how it goes... > I'm still getting a strange graph output. Can you please send me your LTspice circuit file and plot settings file? I want to see if there's something I'm missing

part 1 1256 bytes content-type:text/plain; charset="iso-8859-1" (decoded quoted-printable) On Mon, Jun 11, 2012 at 2:05 AM, V G <@spam@x.solarwind.xKILLspamgmail.com> wrote: {Quote hidden}> On Thu, Jun 7, 2012 at 12:20 PM, Oli Glaser <KILLspamoli.glaserKILLspamtalktalk.net> > wrote: > > > I just tried that circuit and it works fine for me. Only thing I can > > think > > of is that you are trying to plot just the real component of C1, which > will > > be 0 if you have not set the ESR of C1 to a realistic value (say 100mOhm > or > > whatever). > > So this means you probably have "don't plot imaginary component" set. If > > you left click on the right side axis and press ok you should get the > > imaginary component plotted (the axis should show e.g. 10KiOhm, 20KiOhm, > > etc, with the i being for imaginary) which should be what you expect. > > Let me know how it goes... > > > > >I'm still getting a strange graph output. Can you please send me your > >LTspice circuit file and plot settings file? I want to see if there's > >something I'm missing. > > Okay, here's the files. I started the sweep from 1kHz to make the imaginary (dotted) curve more obvious. The 1mOhm real part is just the cap ESR. part 2 678 bytes content-type:text/plain; name="VG.asc" (decoded base64) Version 4 SHEET 1 880 680 WIRE -448 96 -496 96 WIRE -144 96 -384 96 WIRE -496 176 -496 96 WIRE -144 176 -144 96 WIRE -496 320 -496 256 WIRE -144 320 -144 256 WIRE -144 320 -496 320 FLAG -144 320 0 FLAG -144 96 Vout SYMBOL voltage -496 160 R0 WINDOW 123 24 124 Left 2 WINDOW 39 -147 33 Left 2 SYMATTR Value2 AC 1 SYMATTR SpiceLine Rser=0 SYMATTR InstName V1 SYMATTR Value 5 SYMBOL res -160 160 R0 SYMATTR InstName R1 SYMATTR Value 50 SYMBOL cap -384 80 R90 WINDOW 0 0 32 VBottom 2 WINDOW 3 32 32 VTop 2 SYMATTR InstName C1 SYMATTR Value 1�F SYMATTR SpiceLine Rser=1m TEXT -856 32 Left 2 !.ac lin 100000 1000 100e3 part 3 401 bytes content-type:application/octet-stream; name="VG.log" (decode) part 4 224 bytes content-type:application/octet-stream; name="VG.net" (decode) part 5 354 bytes content-type:application/octet-stream; name="VG.plt" (decode) part 6 181 bytes content-type:text/plain; name="ATT00001.txt" (decode)

On Sat, Jun 16, 2012 at 10:22 AM, V G <spamBeGonex.solarwind.xspamBeGonegmail.com> wrote: > On Mon, Jun 11, 2012 at 12:58 AM, Oli Glaser <TakeThisOuToli.glaserEraseMEspam_OUTtalktalk.net>wrote: > >> Okay, here's the files. I started the sweep from 1kHz to make the >> imaginary >> (dotted) curve more obvious. The 1mOhm real part is just the cap ESR. >> > > Thanks a lot! That worked! I don't understand where the imaginary part is > coming from though (what law/equation, etc...). > Oh I think I can guess... Is it because of the two solutions to the equation involving a square root (for calculation of the RMS voltage at the two nodes)

On Sat, Jun 16, 2012 at 4:31 PM, V G <RemoveMEx.solarwind.xTakeThisOuTgmail.com> wrote: > On Sat, Jun 16, 2012 at 10:22 AM, V G <x.solarwind.xEraseME.....gmail.com> wrote: > > > On Mon, Jun 11, 2012 at 12:58 AM, Oli Glaser <EraseMEoli.glasertalktalk.net > >wrote: > > > >> Okay, here's the files. I started the sweep from 1kHz to make the > >> imaginary > >> (dotted) curve more obvious. The 1mOhm real part is just the cap ESR. > >> > > > > Thanks a lot! That worked! I don't understand where the imaginary part is > > coming from though (what law/equation, etc...). > > > > Oh I think I can guess... Is it because of the two solutions to the > equation involving a square root (for calculation of the RMS voltage at the > two nodes)? > > I think you are on the right track. The imaginary part is simply 1/2pi * F * C. To work out the overall impedance you take the square root of the (squared) imaginary and real impedances. So if you have 50 ohms imaginary and 50 ohms real you have a total impedance of sqrt(50^2 + 50^2) = 70.7 ohms. You can check this in the simulation if you plot V(n001)/I(C1) and look at the bode and cartesian displays. 1uF is 50 ohms around 3.18 kHz. At this frequency on the bode you should read 70.7 ohms on the plot, if you change to the cartesian you should see both real and imaginary at 50 ohms