开云体育

Strange impedance curve

gasoltroll All Messages By This Member #47087 Hi i'm looking at an impedance curve of a non-ideal tantalum capacitor in LTSpice. The test circuit and impedance curve is seen in this screengrab: The spice file is here . So, the imdpedance curve shows the expected impedance minimum, but also an unexpected maximum at about 100MHz, where there is also a polarity switch in phase. This feature does not show up if I do an impedance plot in octave: octave:1> f = [1000:1000:1e9]; octave:2> C = 2e-3C = 0.0020000 octave:3> R = 2e-3R = 0.0020000 octave:4> L = 1e-9L = 1.0000e-09 octave:5> z = R + f.2pijL-1./(f.2pijC) octave:6> loglog(f,abs(z)) octave:7> semilogx(f,atand(imag(z)./real(z))) Which result in these plots The parameters in the octave code are the same as in LTSpice component. Anyone know where this comes from? The phases look pretty different, is there something wrong with the test circuit?
Christian Thomas All Messages By This Member #47096 I used to get strange differences between linear and log scales in earlier version of LTspice, though I haven't had any in the last year or two. They were never explained, but they certainly disappeared. If it's not an early version, have a look at the no of points per octave you are using. If you have too few there can be some very strange plotting as the otherwise seemingly excellent interpolation does its best with the derivatives it's given. A bouncing ball shape is one definite symptom of this. CT On 18 September 2011 20:15, gasoltroll <johan.lans@...> wrote: ** Hi i'm looking at an impedance curve of a non-ideal tantalum capacitor in LTSpice. The test circuit and impedance curve is seen in this screengrab: The spice file is here . So, the imdpedance curve shows the expected impedance minimum, but also an unexpected maximum at about 100MHz, where there is also a polarity switch in phase. This feature does not show up if I do an impedance plot in octave: octave:1> f = [1000:1000:1e9]; octave:2> C = 2e-3C = 0.0020000 octave:3> R = 2e-3R = 0.0020000 octave:4> L = 1e-9L = 1.0000e-09 octave:5> z = R + f.2pijL-1./(f.2pijC) octave:6> loglog(f,abs(z)) octave:7> semilogx(f,atand(imag(z)./real(z))) Which result in these plots The parameters in the octave code are the same as in LTSpice component. Anyone know where this comes from? The phases look pretty different, is there something wrong with the test circuit? [Non-text portions of this message have been removed]
Andy I All Messages By This Member #47100 SPICE (and LTspice is no exception) can have additional shunt elements from every node to ground, added to help convergence. ?I've kind of lost track of exact details, over the years, but there can be a gshunt (conductance) and a cshunt (capacitance) added to every node. I think cshunt is resonating with the tantalum's inductance. I don't know exactly where the value of this capacitance is set (other than an .OPTIONS statement), but I saw in the "Hacks" tab of the Control Panel, there is a setting for "Minimum shunt to main capacitance ratio". ?Changing that number moves the parallel resonance,?so I think it is the cause. ?If you make the "Hacks" value very small, or zero, the curve looks like your Octave plot. Andy
Helmut Sennewald All Messages By This Member #47102 --- In LTspice@..., "gasoltroll" <johan.lans@...> wrote: Hi i'm looking at an impedance curve of a non-ideal tantalum capacitor in LTSpice. The test circuit and impedance curve is seen in this screengrab: The spice file is here . So, the imdpedance curve shows the expected impedance minimum, but also an unexpected maximum at about 100MHz, where there is also a polarity switch in phase. This feature does not show up if I do an impedance plot in octave: octave:1> f = [1000:1000:1e9]; octave:2> C = 2e-3C = 0.0020000 octave:3> R = 2e-3R = 0.0020000 octave:4> L = 1e-9L = 1.0000e-09 octave:5> z = R + f.2pijL-1./(f.2pijC) octave:6> loglog(f,abs(z)) octave:7> semilogx(f,atand(imag(z)./real(z))) Which result in these plots The parameters in the octave code are the same as in LTSpice component. Anyone know where this comes from? The phases look pretty different, is there something wrong with the test circuit? Hello Johann, Please set a value for Cpar when you have set Lser. Right-mouse-click on the capacitor. Then set the following. Equivalent parallel capacitance(Cpar): 0p Best regards, Helmut
gasoltroll All Messages By This Member #47109 A collegue suggested that I put the parasitics of the kapacitor in discrete components in series, and that fixed the problem. Bug? /Johan toggle quoted message Show quoted text --- In LTspice@..., Christian Thomas <ct.waveform@...> wrote: I used to get strange differences between linear and log scales in earlier version of LTspice, though I haven't had any in the last year or two. They were never explained, but they certainly disappeared. If it's not an early version, have a look at the no of points per octave you are using. If you have too few there can be some very strange plotting as the otherwise seemingly excellent interpolation does its best with the derivatives it's given. A bouncing ball shape is one definite symptom of this. CT On 18 September 2011 20:15, gasoltroll <johan.lans@...> wrote: ** Hi i'm looking at an impedance curve of a non-ideal tantalum capacitor in LTSpice. The test circuit and impedance curve is seen in this screengrab: The spice file is here . So, the imdpedance curve shows the expected impedance minimum, but also an unexpected maximum at about 100MHz, where there is also a polarity switch in phase. This feature does not show up if I do an impedance plot in octave: octave:1> f = [1000:1000:1e9]; octave:2> C = 2e-3C = 0.0020000 octave:3> R = 2e-3R = 0.0020000 octave:4> L = 1e-9L = 1.0000e-09 octave:5> z = R + f.2pijL-1./(f.2pijC) octave:6> loglog(f,abs(z)) octave:7> semilogx(f,atand(imag(z)./real(z))) Which result in these plots The parameters in the octave code are the same as in LTSpice component. Anyone know where this comes from? The phases look pretty different, is there something wrong with the test circuit? [Non-text portions of this message have been removed]
Andy I All Messages By This Member #47118 Helmut wrote: Equivalent parallel capacitance(Cpar): 0p Interesting. This is one of those cases where the default value is not zero, but the Help doesn't tell you this. Judging by the Help, I would have thought that the default would be zero. Someone needs to make the Help more helpful! Andy
Andy I All Messages By This Member #47120 gasoltroll wrote: A collegue suggested that I put the parasitics of the kapacitor in discrete components in series, and that fixed the problem. Bug? What that probably did was move the series inductance so it is no longer in parallel with the (unspecified but non-zero by default) parallel capacitance, Cpar. Andy
gasoltroll All Messages By This Member #47126 Ok, that was a good thing to learn... Thanks everyone! /Johan toggle quoted message Show quoted text --- In LTspice@..., "Helmut" <helmutsennewald@...> wrote: --- In LTspice@..., "gasoltroll" <johan.lans@> wrote: Hi i'm looking at an impedance curve of a non-ideal tantalum capacitor in LTSpice. The test circuit and impedance curve is seen in this screengrab: The spice file is here . So, the imdpedance curve shows the expected impedance minimum, but also an unexpected maximum at about 100MHz, where there is also a polarity switch in phase. This feature does not show up if I do an impedance plot in octave: octave:1> f = [1000:1000:1e9]; octave:2> C = 2e-3C = 0.0020000 octave:3> R = 2e-3R = 0.0020000 octave:4> L = 1e-9L = 1.0000e-09 octave:5> z = R + f.2pijL-1./(f.2pijC) octave:6> loglog(f,abs(z)) octave:7> semilogx(f,atand(imag(z)./real(z))) Which result in these plots The parameters in the octave code are the same as in LTSpice component. Anyone know where this comes from? The phases look pretty different, is there something wrong with the test circuit? Hello Johann, Please set a value for Cpar when you have set Lser. Right-mouse-click on the capacitor. Then set the following. Equivalent parallel capacitance(Cpar): 0p Best regards, Helmut

Previous Topic Next Topic