|
The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl Modeling >> Transmission Lines and Other Distributed Devices >> a problem with mtline,HELP! thanks! https://designers-guide.org/forum/YaBB.pl?num=1261540239 Message started by kennycs on Dec 22nd, 2009, 7:50pm |
|
Title: a problem with mtline,HELP! thanks! Post by kennycs on Dec 22nd, 2009, 7:50pm When I use mtline to model a differential transmission line, I specify the S-paramter S4p file,but why I have to specify the length ? Does not the s4p file describe the lines well? |
|
Title: Re: a problem with mtline,HELP! thanks! Post by pancho_hideboo on Dec 24th, 2009, 1:11am I don't know what simulator you use. But "length" parameter exists in W-element of HSPICE which is absolutely industrial standard transmission line model. Generally Nport is not converted to RLGC model. See http://www.designers-guide.org/Forum/YaBB.pl?num=1237187544 Length information is used for generating RLGC model efficiently from S-parameter in W-element of HSPICE. [S Model form of W-element] Wxxx in1 <in2 <...inx>> refin out1 <out2 <...outx>> + refout <Smodel=modelname> N=val L=val [Parameter Description] Wxxx : Lossy (W-element) transmission line element name. inx : Signal input node for xth transmission line (in1 is required). refin : Ground reference for input signal outx : Signal output node for the xth transmission line (each input port must have a corresponding output port). refout : Ground reference for output signal. Smodel : S Model name reference, which contains the S-parameters of the transmission lines. N : Number of conductors (excluding the reference conductor). L : Physical length of the transmission line, in units of meters. |
|
Title: Re: a problem with mtline,HELP! thanks! Post by sheldon on Dec 24th, 2009, 3:28am Kenny, If you have s-parameter data and want to use it in a simulation, just use the n-port [assuming that you are using a relatively recent version of Spectre]. The manual describes why the length is required when you use the mtline. Best Regards, Sheldon |
|
Title: Re: a problem with mtline,HELP! thanks! Post by kennycs on Dec 29th, 2009, 1:29am sheldon wrote on Dec 24th, 2009, 3:28am:
hi Sheldon ： Thank you very much! the tool I used is spectre. Now I think Nport is much better. In my s4p file , the minimum frequency point is 30Mhz, is it too big to caculate the DC response? Best Regards kenny |
|
Title: Re: a problem with mtline,HELP! thanks! Post by kennycs on Dec 29th, 2009, 1:49am pancho_hideboo wrote on Dec 24th, 2009, 1:11am:
Hi! I use spectre.Now I have changed to Nport with s4p file,but unfortunately I met problems. In my s4p file , the minimun frequency point is 30MHz ,is it enough for Nport extrapolates the time response especially DC ? Thank you very much ! |
|
Title: Re: a problem with mtline,HELP! thanks! Post by sheldon on Dec 29th, 2009, 8:16am Kenny, A couple of comments: 1) Before using a component you might want to review the manual. It appears that the version of MMSIM you are using supports dc extrapolation, it is listed in the instance parameters. You might want to try the dc extrapolation --> unwrap. 2) If you concerned about dc extrapolation, then you might want to try MMSIM72. An additional algorithm for dc extrapolation has been provided along with some other new features. Best Regards, Sheldon |
|
Title: Re: a problem with mtline,HELP! thanks! Post by pancho_hideboo on Dec 29th, 2009, 8:48am kennycs wrote on Dec 29th, 2009, 1:49am:
If you have other simulators, compare results. You had better set on for "Check Passivity". In Agilent Simulator, "Check Passivity" has been implemented since very very long ago. Agilent Simulator also have a function of "Enforce Passivity". Default setting for "Max order impulse response" is "2000000" in current Cadence Spectre ? It is extraordinally large. It seems that still there is no parameter for coping with noncausal issues even in current Cadence Spectre. |
|
Title: Re: a problem with mtline,HELP! thanks! Post by kennycs on Dec 29th, 2009, 9:09pm sheldon wrote on Dec 29th, 2009, 8:16am:
Hi ! Thank you so much! I have read the manual and try unwrap ,but it makes no sense. When I use ADS to simulate the transmission line with my s4p file ,the result is right , but in spectre not . The difference between in spectre and ADS is the common voltage of output, it is lower in spectre .Is it problem of spectre? |
|
Title: Re: a problem with mtline,HELP! thanks! Post by kennycs on Dec 29th, 2009, 9:22pm pancho_hideboo wrote on Dec 29th, 2009, 8:48am:
Hi! I'm sorry , "2000000" for "Max order impulse response" is my set. I have compared spectre with ADS. The result in ADS seems good.it seems the output common vlotage in spectre is much lower. |
|
Title: Re: a problem with mtline,HELP! thanks! Post by sheldon on Dec 30th, 2009, 9:51am Kenny, As previously mentioned, you should review the manual, in particular, with regard to passivity checking (see item #1 below). 1) The check passivity function includes an option to enforce passivity. I believe that passivity enforcement has always been supported by the simulator. 2) As previously mentioned, there is an additional option for dc extrapolation. This option has worked for me when I have had common-mode level issues. 3) Please note that casuality enforcement is supported for the nport from MMSIM72 Best Regards, Sheldon |
|
Title: Re: a problem with mtline,HELP! thanks! Post by pancho_hideboo on Dec 30th, 2009, 10:26am Implementation of NPORT in Cadence Spectre can reach to enoughy practical level ? Is there any one who use NPORT of Cadence Spectre in actual design ? These are still very doubtful. EMSS in VPCD was also never practical use level. http://www.designers-guide.org/Forum/YaBB.pl?num=1244552575/10#10 |
|
Title: Re: a problem with mtline,HELP! thanks! Post by sheldon on Dec 30th, 2009, 10:56pm Kenny, You need to do a quick check, spectre -h nport | grep unwrap. For your case, you probably need to use the dcextrap=hpunwrap option. Just checked my version IC61 and it is not a supported instance parameter so you will need to manually edit the netlist and run the simulation from the command line. This should address your dc level issue. If it does not you should inform your Cadence support person. Best Regards, Sheldon |
|
Title: Re: a problem with mtline,HELP! thanks! Post by Andrew Beckett on Jan 5th, 2010, 2:36am pancho_hideboo wrote on Dec 30th, 2009, 10:26am:
What has EMSS got to do with anything? Nobody even mentioned it. It was EOL'd before the tool had matured - it was still very new (all tools take time to mature). Yet another example of your constant negative and unhelpful comments. Much of the time you give very helpful and useful advice - but unfortunately the negative comments really detract from that. And yes, there are customers using nport in real design. Agreed, it has been problematic (in some cases) in the past but there has been a big focus on it over the last year, to try to address some of the long-standing problems which have caused pain. We are seeing many fewer issues as a result of this focused effort. Andrew. |
|
Title: Re: a problem with mtline,HELP! thanks! Post by RFICDUDE on Jan 6th, 2010, 9:54am I used NPORTs in a commercial design. There was a balun that I didn't have time to optimize an accurate broadband lumped element model from the Momentum results. The Momentum dataset seemed to match the Cadence NPORT results, and the large signal SpectreRF results matched the AC/s-parameter results. I have also used NPORTS to incorporate vendor s-parameter models of SMT inductors for matching networks. The biggest problem area seemed to be multiport models of packages. The multiport models are only needed if coupling is a big issue (and it can be for some specs). So, I would only try to use these for isolation simulations and extracting lumped element equivalents for simplier models which don't capture the coupling effects. |
|
The Designer's Guide Community Forum » Powered by YaBB 2.2.2! YaBB © 2000-2008. All Rights Reserved. |