|
Dear Members,
?
Is there any chance to calculate of real or imaginary part of impedance while doing a simulation?with any AC voltage?
?
Or is it possible to draw?a trace of real part or imaginary part of impedace in LTspice?
?
Thank you in advance,
?
Mahmudul Kabir, Japan
?
[Non-text portions of this message have been removed]
|
--- In LTspice@..., Mahmudul Kabir <nilonjana@...> wrote:
Dear Members,
?
Is there any chance to calculate of real or imaginary part
of impedance while doing a simulation?with any AC voltage?
?
Or is it possible to draw?a trace of real part or imaginary
part of impedace in LTspice?
?
Thank you in advance,
?
Mahmudul Kabir, Japan
Hello Mahmudul Kabir, I assume you use .AC simulation. In this case you can plot in Cartesian format which shows the real part with a solid line and the imaginary part with a dashed line. Best regards, Helmut
|
Dear Helmut, ? Thank you very much for your quick response. Yes, I was doing .AC simulation. ? Sincerely, ? Mahmudul Kabir, Japan? --- In LTspice@..., Mahmudul Kabir <nilonjana@...> wrote:
Dear Members,
?
Is there any chance to calculate of real or imaginary part
of impedance while doing a simulation?with any AC voltage?
?
Or is it possible to draw?a trace of real part or imaginary
part of impedace in LTspice?
?
Thank you in advance,
?
Mahmudul Kabir, Japan
Hello Mahmudul Kabir, I assume you use .AC simulation. In this case you can plot in Cartesian format which shows the real part with a solid line and the imaginary part with a dashed line. Best regards, Helmut [Non-text portions of this message have been removed]
|
What is the purpose of Cartesian plot? I'm sure it makes some things more convenient than a bode plot. What things?
- keantoken
|
--- In LTspice@..., "keantoken" <keantoken@...> wrote:
What is the purpose of Cartesian plot? I'm sure it makes some things more convenient than a bode plot. What things?
- keantoken
Hello Keantoken, If you're doing RF design, on oscillators, for example, it is essential to be able to see both real and imaginary parts clearly and separately without having to do mental arithmetic for each frequency displayed. The Cartesian presentation shows this much better for most people, although a few will claim they can glean everything they need from a polar plot. But then some people are able to write a complete GUI in one line of C. For doing serious RF design, LTspice is not the ideal tool, since it does not have native Smith chart and cannot handle S-parameters, but it is at least possible. Regards, Tony
|
Tony, While LTspice may not be the ideal tool for RF design, it can still be quite useful. You are correct that it does not have native support for producing a Smith chart. However, some clever contributor to this group has provided a means to plot the graticule of a Smth chart and impedance curves with frequency markers (Files > Examples > Apps > SmithLTspice.zip). ? With respect to LTspice handling s-parameters, it certainly can. The .NET command computes network parameters in an AC sweep. The HELP files says in part, ? "This statement is used with a small signal(.AC) analysis to compute the input and output admittance, impedance, Y-parameters, Z-parameters, H-parameters, and S-parameters of a 2-port network. It can also be used to compute the input admittance and impedance of a 1-port network. This must be used with a .AC statement, which determines the frequency sweep of the network analysis." ? There is an entire section in the tutorial section of this groups files devoted to s-parameters in LTspice (Files> Tut> S-Parameter). ? All the best, ? ?? - Philip ________________________________ From: Tony Casey <tony@...> To: LTspice@... Sent: Thu, September 15, 2011 8:55:18 AM Subject: [LTspice] Re: About impedance ? --- In LTspice@..., "keantoken" <keantoken@...> wrote:
What is the purpose of Cartesian plot? I'm sure it makes some things more
convenient than a bode plot. What things?
- keantoken
Hello Keantoken, If you're doing RF design, on oscillators, for example, it is essential to be able to see both real and imaginary parts clearly and separately without having to do mental arithmetic for each frequency displayed. The Cartesian presentation shows this much better for most people, although a few will claim they can glean everything they need from a polar plot. But then some people are able to write a complete GUI in one line of C. For doing serious RF design, LTspice is not the ideal tool, since it does not have native Smith chart and cannot handle S-parameters, but it is at least possible. Regards, Tony [Non-text portions of this message have been removed]
|
--- In LTspice@..., Philip Bellingham <rmhc78a@...> wrote:
Tony,
While LTspice may not be the ideal tool for RF design, it can still be quite
useful.
You are correct that it does not have native support for producing a Smith
chart. However, some clever contributor to this group has provided a means to
plot the graticule of a Smth chart and impedance curves with frequency markers
(Files > Examples > Apps > SmithLTspice.zip).
??
With respect to LTspice handling s-parameters, it certainly can. The .NET
command computes network parameters in an AC sweep. The HELP files says in part,
??
"This statement is used with a small signal(.AC) analysis to compute the input
and output admittance, impedance, Y-parameters, Z-parameters, H-parameters, and
S-parameters of a 2-port network. It can also be used to compute the input
admittance and impedance of a 1-port network. This must be used with a .AC
statement, which determines the frequency sweep of the network analysis."
??
There is an entire section in the tutorial section of this groups files devoted
to s-parameters in LTspice (Files> Tut> S-Parameter).
??
All the best,
??
???? - Philip
Hello Philip, Thanks for the info. I'm aware of the Smith chart add-on, which is why I said native. It's clever as you said, but not slick enough for serious design work; even the author concedes it's crude. I'm also aware that adding the .net directive enables an .ac analysis to generate S-parameters; and indeed, I make a lot of use of this feature. But you cannot use S-parameters as input data. This was my point, although I admit I didn't make that very clear. There are also various utilities that claim to generate SPICE subcircuits from S-parameter files, but this is something of a holy grail, which is why the only commercial product that really claims to have cracked this with multiport demonstrable accuracy over decades of frequency range costs thousands of dollars. Regards, Tony
|
In message <j4t6tu+4c59@...>, dated Thu, 15 Sep 2011, Tony Casey <tony@...> writes: There are also various utilities that claim to generate SPICE subcircuits from S-parameter files, but this is something of a holy grail, which is why the only commercial product that really claims to have cracked this with multiport demonstrable accuracy over decades of frequency range costs thousands of dollars. Naive question. Why would you want to do that? If you have s-parameter files, presumably they came from measurements of a real circuit. So why ask Spice (or anything else) to generate a circuit? To track down parasitics? -- OOO - Own Opinions Only. Try www.jmwa.demon.co.uk and www.isce.org.uk John Woodgate, J M Woodgate and Associates, Rayleigh, Essex UK When I point to a star, please look at the star, not my finger. The star will be more interesting.
|
<snip> However, some clever contributor to this group has provided a means to plot the graticule of a Smth chart and impedance curves with frequency markers
(Files > Examples > Apps > SmithLTspice.zip).
??
With respect to LTspice handling s-parameters, it certainly can. The .NET
command computes network parameters in an AC sweep. The HELP files says in part,
??
"This statement is used with a small signal(.AC) analysis to compute the input
and output admittance, impedance, Y-parameters, Z-parameters, H-parameters, and
S-parameters of a 2-port network. It can also be used to compute the input
admittance and impedance of a 1-port network. This must be used with a .AC
statement, which determines the frequency sweep of the network analysis."
??
There is an entire section in the tutorial section of this groups files devoted
to s-parameters in LTspice (Files> Tut> S-Parameter).
??
All the best,
??
???? - Philip Hello Philip,
Thanks for the info.
I'm aware of the Smith chart add-on, which is why I said native. It's clever as you said, but not slick enough for serious design work; even the author concedes it's crude.
</snip> Other folk might like to be aware that also exist several ways of plotting Smith charts in Excel by using similar kludges. This is one of several: Regards, Tony
|
Naive question. Why would you want to do that? If you have s-parameter
files, presumably they came from measurements of a real circuit. So why
ask Spice (or anything else) to generate a circuit? Often you have s-parameters for a component (a transistor or MMIC), which you get from the component vendor, and you want to use it in a circuit. Andy
|
In message <CALBs-ThF7REAcCQEOUOw2A8J1qBi752gUcHTrqUnBUatD03Scg@...>, dated Thu, 15 Sep 2011, Andy <Andrew.Ingraham@...> writes: Naive question. Why would you want to do that? If you have s-parameter
files, presumably they came from measurements of a real circuit. So why
ask Spice (or anything else) to generate a circuit? Often you have s-parameters for a component (a transistor or MMIC), which you get from the component vendor, and you want to use it in a circuit.
I said it was naive! The data are s-parameter values as functions of frequency, I suppose? Synthesising circuits from impedance values in any form is difficult but only very nearly impossible unless the functions of frequency are rather simple. -- OOO - Own Opinions Only. Try www.jmwa.demon.co.uk and www.isce.org.uk John Woodgate, J M Woodgate and Associates, Rayleigh, Essex UK When I point to a star, please look at the star, not my finger. The star will be more interesting.
|
--- In LTspice@..., Andy <Andrew.Ingraham@...> wrote:
Naive question. Why would you want to do that? If you have s-parameter
files, presumably they came from measurements of a real circuit. So why
ask Spice (or anything else) to generate a circuit? Often you have s-parameters for a component (a transistor or MMIC),
which you get from the component vendor, and you want to use it in a
circuit.
Andy
Indeed. And for passive products, such as SAW filters or isolators, S-parameters are the only data you're ever likely to get from vendors. Also for capacitors and inductors, vendors such as Murata and ATC also provide S-parameter data for use at frequencies at which the simple equivalent circuits we're used to in SPICE are hopelessly inadequate to describe the performance. Regards, Tony
|
Tony, All valid points. I agree that creating SPICE models for s-parameter characterized passive parts using only native SPICE passives (C, L, and R) is an art and the native models are often inadequate even with the provision for adding parasitics. The same is true for modeling active components. Therefore, I agree that creating SPICE models that can be used for all types of analysis (TRAN, AC, etc.) is a daunting task when the only data you have is s-parameters. My experience has been that frequency domain characterization and simulation is often sufficient. To that end, the utility, in our group files, that converts an s-parameter file to a set frequency dependent controlled sources in SPICE, creates models that are quite acceptable when performing AC network analysis.?This does limit you to AC analysis, and for active devices you are constrained to the bias conditions present?when the s-parameters were measured. Regards, ?? - Philip ________________________________ From: Tony Casey <tony@...> To: LTspice@... Sent: Thu, September 15, 2011 12:42:09 PM Subject: [LTspice] Re: About impedance ? --- In LTspice@..., Andy <Andrew.Ingraham@...> wrote:
Naive question. Why would you want to do that? If you have s-parameter
files, presumably they came from measurements of a real circuit. So why
ask Spice (or anything else) to generate a circuit? Often you have s-parameters for a component (a transistor or MMIC),
which you get from the component vendor, and you want to use it in a
circuit.
Andy
Indeed. And for passive products, such as SAW filters or isolators, S-parameters are the only data you're ever likely to get from vendors. Also for capacitors and inductors, vendors such as Murata and ATC also provide S-parameter data for use at frequencies at which the simple equivalent circuits we're used to in SPICE are hopelessly inadequate to describe the performance. Regards, Tony [Non-text portions of this message have been removed]
|
--- In LTspice@..., Philip Bellingham <rmhc78a@...> wrote:
Tony,
All valid points. I agree that creating SPICE models for s-parameter
characterized passive parts using only native SPICE passives (C, L, and R) is an
art and the native models are often inadequate even with the provision for
adding parasitics. The same is true for modeling active components. Therefore, I
agree that creating SPICE models that can be used for all types of analysis
(TRAN, AC, etc.) is a daunting task when the only data you have is s-parameters.
My experience has been that frequency domain characterization and simulation is
often sufficient. To that end, the utility, in our group files, that converts an
s-parameter file to a set frequency dependent controlled sources in SPICE,
creates models that are quite acceptable when performing AC network
analysis.??This does limit you to AC analysis, and for active devices you are
constrained to the bias conditions present??when the s-parameters were measured.
Regards,
???? - Philip
All, By definition s-parameters are small signal linear AC parameters, and in most cases the parameters are a function of frequency. Usually, one is interested in only a single frequency or a mall range of frequencies. The work fine for their intended purpose. Rick
|
