Learn how easy it is to sync an existing GitHub or Google Code repo to a SourceForge project! See Demo
Close
From: walter <steffe@ti...>  20070311 12:00:55

Hi Using qucs I would like to performe the analysis of a passive spice circuit= =20 (containing L R and G elements) having some ports terminated on the=20 characteristic impedance of a waveguide. It is well known that the characteristic impedance Zc depends on the=20 frequency as given below: Zc_TE =3Dsqrt(mu/epsilon) f / sqrt(f^2fc^2)=20 Zc_TM =3Dsqrt(mu/epsilon) sqrt(f^2fc^2) / f =20 where f=3Dfrequency fc=3Dcutoff frequency for the particular w.g. mode (TE or TM) =46or f>fc (where Zc is real) I would like to have a scattering matrix that= is=20 normalized with respect to Zc (as usual for a waveguide component). May you please give me some hints. Tanks in advance Walter Steff=E8 
From: Stefan Jahn <stefan@gr...>  20070313 12:35:08

Am So, 11.03.2007, 13:01, schrieb walter steffè: > Hi Hello Walter, > Using qucs I would like to performe the analysis of a passive spice > circuit > (containing L R and G elements) having some ports terminated on the > characteristic impedance of a waveguide. > It is well known that the characteristic impedance Zc depends on the > frequency as given below: > > Zc_TE =sqrt(mu/epsilon) f / sqrt(f^2fc^2) > Zc_TM =sqrt(mu/epsilon) sqrt(f^2fc^2) / f > where f=frequency > fc=cutoff frequency for the particular w.g. mode (TE or TM) > > For f>fc (where Zc is real) I would like to have a scattering matrix that > is > normalized with respect to Zc (as usual for a waveguide component). > > May you please give me some hints. Currently such a thing is not possible with Qucs. There are ging to be two possible ways to do it probably in a future version. Way 1: Implementation of a rectangular waveguide as a builtin device. Probably you can supply us with computation formulas for Zl, alpha, etc.? Way 2: In Qucs 0.0.11 (upcoming release, very soon) you will have the possibility of equation variables in component parameters. I could add it on my TODO list to make also "frequency" for AC and SParameter analysis available in these equations. What do you think? Is this necessary? Sorry for the inconvenience, Stefan. 
From: Stefan Jahn <stefan@gr...>  20070313 19:57:31

Am Di, 13.03.2007, 19:49, schrieb walter steffè: > Hello Stefan, Hi Walter, > I think that it should be nice to have implemented both ways. Ok, I see. > The waveguide line is usefull to connect different components which > interface > trough waveguide ports. > > The frequency variable in AC mode can be used to define a frequency > dependent > load such as the characteristic impedance of a waveguide. > > Regarding the computation of the wave guide line parameters there is not a > very big difference with respect to the TEM transmission line. > The difference is really small if you look at the S parameters. > As for the TEM line it holds S11=S22=0 and S12=S21=1. > The phases of S12 and of S21 are equal to beta_wg * length > and beta_wg is given by: > > beta_wg=sqrt(beta^2 kt^2) > > beta is 2PI/lambda in free space (or in the TEM line) Yep, so far for an ideal 50Ohm TEM line... > kt is the eigenvalue of the Hellmoltz equation associated with the > given > mode. It depends on the waveguide section, on the mode type (TE or TM) and > on > the mode order. For the rectangular waveguide there this number can > computed > with a simple formula but I think it would be better to make a generic > waveguide component where kt is a user defined parameter. > Then if you want you can specialize this generic component for the > rectangular > waveguide and in this case the kt of all modes will be computed > automatically. > The user still should be able to define the number of modes. > > I have not spoken about alpha because I have assumed a lossless waveguide. > At the moment I do not remember a formula for the computation of the > attenuation parameter. I think you can find tabulated data (which depend > on > the waveguide/mode/material/surface finishing...) on books like Matthaei > Young, Marcuvitz ... I think that the definition of this parameter can be > left to the user who should know the losses of its waveguide. Have you already looked at the QucsTranscalc tool? There is synthesis and analysis for rectangular waveguide available. It also tells if there occur beside the TEM mode any TE or TM modes. When creating a waveguide component we can probably easily make a good model for the TEM mode. When higher order TE or TM modes occur it gets perhaps difficult because each mode has different Zl and gamma. Michael: What do you know about this topic? (Me is not too familiar with waveguides. :( ) > The only problem I see is that the S parameters I have spoken about are > those > that are normalized versus the characteristic impedance. This can also be > written as: Zc_TE=beta/beta_wg, Zc_TM=beta_wg/beta. > The rules for the computation of the S matrix normalized versus Zc are > similar > to those explained in your paper but you must take care that Zc is a > function > of frequency and that it can be different on the different ports. I don't yet understand it fully... :( But the Sparameter simulation results are normalized to the impedance given in the Sparameter port (e.g. 50 Ohm). When Zl is different you get appropriate reflections, etc., also depending on the frequency. Hope this helps, Stefan. 
From: Stefan Jahn <stefan@gr...>  20070314 17:20:59

Am Mi, 14.03.2007, 08:34, schrieb walter steffè: > Hello Stefan Hi Walter, >> Have you already looked at the QucsTranscalc tool? There is synthesis >> and analysis for rectangular waveguide available. It also tells if >> there >> occur beside the TEM mode any TE or TM modes. > > Not yet. I will look at it Ok, good luck. >> When creating a waveguide component we can probably easily make a good >> model for the TEM mode. When higher order TE or TM modes occur it gets >> perhaps difficult because each mode has different Zl and gamma. > >> > The only problem I see is that the S parameters I have spoken about >> are >> > those >> > that are normalized versus the characteristic impedance. This can also >> be >> > written as: Zc_TE=beta/beta_wg, Zc_TM=beta_wg/beta. >> > The rules for the computation of the S matrix normalized versus Zc are >> > similar >> > to those explained in your paper but you must take care that Zc is a >> > function >> > of frequency and that it can be different on the different ports. >> >> I don't yet understand it fully... :( >> >> But the Sparameter simulation results are normalized to the impedance >> given in the Sparameter port (e.g. 50 Ohm). When Zl is different you >> get appropriate reflections, etc., also depending on the frequency. > > To better clarify what I am asking for look on the annexed schematic. > It is a very simple two port circuit. > First thing I am not able to specify the impedance (Zp=50 ohm or anything > else) associated with the ports. I think there is the need of an > additional > type of port (waveguide port) which gives this possibility. The Sparameter port is different from what you used (you used a succircuit port). You need the "power source" from components/sources. In the properties there is a Z to define. When you press F2 (simulate) then you will get the Sparameters of the circuit normalized to the ones which you specified. BTW: When you press in your schematic F2, then the simulator complains about a missing "Pac" which is the power source I mentioned. > When this is > done > a way to proceed is the following: > > 1) Compute the admittance Y (which is a 2x2 matrix) of the 2 port circuit. When you have the simulated Sparameters, then you can add an equation on the schematic: Y=stoy(S) resimulate and then you have the admittance parameters. > 2) Renormalize Y with respect to the ports characteristic impedance Zp > > y = sqrt(Zp) Y sqrt(Zp) > > here Zp and sqrt(Zp) are diagonal matrices > the diag entries of sqrt(Zp) are the square root of Zp entries. > NB the y matrix is dimensionless You don't need to renormalize, since Sparameter simulation can do it one its own. If, whyever you just use e.g. the default 50 Ohm S parameters, you can renormalize then using an equation: S_new=stos(S,100,50) which renormalizes from 50 to 100 Ohms. > 3) Compute the scattering matrix S as > S = (Iy)/(I+y) I is the identical 2x2 matrix This won't be necessary... Hope this helps, Stefan. 
From: Stefan Jahn <stefan@gr...>  20070314 20:18:21

Am Mi, 14.03.2007, 21:04, schrieb walter steffè: > Hi Stefan Hello Walter, >> The Sparameter port is different from what you used (you used a >> succircuit >> port). You need the "power source" from components/sources. In the >> properties there is a Z to define. > > Ok now I have used the power source > >> >> When you press F2 (simulate) then you will get the Sparameters of >> the circuit normalized to the ones which you specified. >> >> BTW: When you press in your schematic F2, then the simulator complains >> about a missing "Pac" which is the power source I mentioned. >> > > And finally I got the S parameter plot. > > But there are some things I would like to change. > > 1) First of all the S parameter is a complex number and I should be able > to > select between its amplitude and phase while it seems that qucs plots only > the amplitude. > > 2) Usually the amplitudes of S parameters are plotted in dB > (S_dB=20 log10(S). > The plot properties let me to specify a logaritmic scale which is not > exactly > the same as a dB scale and it seems that it does'nt work. Add equations: dB_S21=dB(mag(S[2,1])) ph_S21=phase(S[2,1]) Then you can plot dB_S21 and ph_S21... >> You don't need to renormalize, since Sparameter simulation can do >> it one its own. > > Great . Then the only thing I would like to have are two additional > parameters > in the power source. These parameter are the cut off frequency fc and a > flag that selects between TE and TM modes. The port impedance (used in > the > normalization) has to be redefined as: > > Zc(f) = Zinf f / sqrt(f^2fc^2) for TE ports > Zc(f) = Zinf sqrt(f^2fc^2) / f for TM ports > > You can easely see that Zinf is the limit of both expression when the freq > f > goes to the infinite. > > If you put fc=0 you can see that both expressions reduce to Zc(f)=Zinf > =cost > and this condition corresponds with the TEM case. Hm. Ok for this we would need 'frequency' in equations. I put it on the TODO list. With the new release you will be able to write: freq=1e9 fc=2e8 Zinf=75 Zc=Zinf * freq / sqrt(abs(freq^2  fc^2)) Then you can put Zc into the "Z" property of the power source. Also you will be able to define a subcircuit with freq, fc and Zinf as parameters... Cheers, Stefan. 