SPICE - Frequency dependent resistor model

[[email protected]]

Hi,

I would like to know if there is any way to include a resistor with
frequency dependence in SPICE. Specifically, I am looking for some
spice element that has a voltage current relationship given by

V / I = k * (w ^ 2) where k is a constant and w is the angular
frequency

I'm working on an electroacoustical model of a microphone. For those
who are not familiar with this, electroacoustic circuits are equivalent
analog electical models of acoustic devices. Different acoustic
elements are transformed into equivalent resistances, capacitances,
etc. So please note that the resistance that I refer to is NOT a real
electrical resistance. It is just an equivalent model.

I tried looking into all the user manuals that I could lay my hands on,
but am unable to find anything that I can use. I am an absolute newbie
when it comes to SPICE, so I'm not even sure if this can be done in
SPICE at all. I would be grateful if you could either tell me how to do
this or tell me where I may find this information. Any help would be
greatly appreciated.

Thanks,

Aravind

 

[JeffM]

I would like to know if there is any way

to include a resistor with frequency dependence in SPICE.
Aravind

http://groups.google.com/group/sci....ependent-resistor+ingroup:sci.electronics.cad

 

[qrk]

Hi,

I would like to know if there is any way to include a resistor with
frequency dependence in SPICE. Specifically, I am looking for some
spice element that has a voltage current relationship given by

V / I = k * (w ^ 2) where k is a constant and w is the angular
frequency

I'm working on an electroacoustical model of a microphone. For those
who are not familiar with this, electroacoustic circuits are equivalent
analog electical models of acoustic devices. Different acoustic
elements are transformed into equivalent resistances, capacitances,
etc. So please note that the resistance that I refer to is NOT a real
electrical resistance. It is just an equivalent model.

I tried looking into all the user manuals that I could lay my hands on,
but am unable to find anything that I can use. I am an absolute newbie
when it comes to SPICE, so I'm not even sure if this can be done in
SPICE at all. I would be grateful if you could either tell me how to do
this or tell me where I may find this information. Any help would be
greatly appreciated.

Thanks,

Aravind

You can use Laplace transforms to make frequency dependent resistors
for AC simulations. See
http://www.ecircuitcenter.com/Circuits/vc_resistor1/vc_resistor1.htm
for ideas on making resistors out of voltage and current sources. I
like using current sources to make variable resistors. Some flavors of
Spice (LTspice and PSpice come to mind) allow you to use Laplace
transforms in the E and G devices.

 

[Bob Penoyer]

Hi,

I would like to know if there is any way to include a resistor with
frequency dependence in SPICE. Specifically, I am looking for some
spice element that has a voltage current relationship given by

V / I = k * (w ^ 2) where k is a constant and w is the angular
frequency

I'm working on an electroacoustical model of a microphone. For those
who are not familiar with this, electroacoustic circuits are equivalent
analog electical models of acoustic devices. Different acoustic
elements are transformed into equivalent resistances, capacitances,
etc. So please note that the resistance that I refer to is NOT a real
electrical resistance. It is just an equivalent model.

I tried looking into all the user manuals that I could lay my hands on,
but am unable to find anything that I can use. I am an absolute newbie
when it comes to SPICE, so I'm not even sure if this can be done in
SPICE at all. I would be grateful if you could either tell me how to do
this or tell me where I may find this information. Any help would be
greatly appreciated.

For an explanation from the PSpice folks, go to
http://www.orcad.com/community.pspice.faqs.aspx
and select Item 2. That example deals with frequency dependent
inductors where Z = Ls. Since a resistor is simply Z = R without the
trailing s, follow the example but exclude the trailing s. You will
have to use the abs(s)/6.283185 operator as your frequency dependence
since abs(s)/6.283185 = f. Good luck.

 

[[email protected]]

Thanks everybody for your replies. I guess my searches weren't
comprehensive enough, and I apologise for not having checked out all
the threads before posting a new one.

Jeff : Although I had already seen the post on modeling skin effect in
resistors, I found the following relevant post when I searched in
Google groups as you suggested. It refers to modeling the resistance as
a function of frequency using the .PARAM command
http://groups.google.com/group/sci....:sci.electronics.cad&rnum=21#2cfa9b9e98770382

qrk (Mark) : That was a great link that you posted. I found many useful
ideas for simulating a resistor using controlled current and voltage
sources. I will try incorporating
Laplace transforms to model frequency dependence as you suggested.

Bob : This looks like a possible solution to the problem of
incorporating frequency dependence. I think it can be combined along
with Mark's idea above to do the job.

I will try out the various possibilities and post the results. Thanks
again for all your help. It's been a great learning experience.

Aravind.

 

[Jim Thompson]

Thanks everybody for your replies. I guess my searches weren't
comprehensive enough, and I apologise for not having checked out all
the threads before posting a new one.

Jeff : Although I had already seen the post on modeling skin effect in
resistors, I found the following relevant post when I searched in
Google groups as you suggested. It refers to modeling the resistance as
a function of frequency using the .PARAM command
http://groups.google.com/group/sci....:sci.electronics.cad&rnum=21#2cfa9b9e98770382

I think that only works for one specific value of "hertz", or stepping
thru a .AC; certainly not for .TRAN

qrk (Mark) : That was a great link that you posted. I found many useful
ideas for simulating a resistor using controlled current and voltage
sources. I will try incorporating
Laplace transforms to model frequency dependence as you suggested.

Bob : This looks like a possible solution to the problem of
incorporating frequency dependence. I think it can be combined along
with Mark's idea above to do the job.

I will try out the various possibilities and post the results. Thanks
again for all your help. It's been a great learning experience.

Aravind.

...Jim Thompson

 

[[email protected]]

I tried the .PARAM option without much sucess. I keep getting the error
"illegal parameter value: hertz". I substituted HERTZ with other
variants, like FREQ, but got the same error. Finally I tried OMEGA and
got an error message saying that OMEGA is a state variable and cannot
be used in a parameter expression.

The other solution of using voltage controlled current sources works
beautifully. I used a GLAPLACE device and was successfully able to use
it to replace the capacitor in an RC circuit. I guess it should work
for any other element whose transfer function is known beforehand. My
problem is solved !

Thanks again for all your help.

 

[Bob Penoyer]

On 2 Mar 2006 17:04:53 -0800, [email protected] wrote:

Jim,

Regarding my earlier post in this thread: The technique for which I
provided a link works fine for frequency domain simulations. No
surprise there. But I haven't been able to use the same
frequency-dependent resistor model in time domain simulations. Are you
aware of how to use such a frequency-dependent resistor model in both
the frequency and time domains?

 

[Jim Thompson]

Jim,

Regarding my earlier post in this thread: The technique for which I
provided a link works fine for frequency domain simulations. No
surprise there. But I haven't been able to use the same
frequency-dependent resistor model in time domain simulations. Are you
aware of how to use such a frequency-dependent resistor model in both
the frequency and time domains?

As [email protected] discovered, it has to be a "GLAPLACE" or an
"ELAPLACE" device. I know that this works in PSpice, but I don't know
about the others.

...Jim Thompson

 

[Joseph2k]

As [email protected] discovered, it has to be a "GLAPLACE" or an
"ELAPLACE" device. I know that this works in PSpice, but I don't know
about the others.

...Jim Thompson

ELAPLACE and GLAPLACE do not seem to be part of Berkeley Spice, but perhaps
some may find a "B" non-linear dependant source source will do the job for
them.

 

[Fred Bartoli]

ELAPLACE and GLAPLACE do not seem to be part of Berkeley Spice, but perhaps
some may find a "B" non-linear dependant source source will do the job for
them.

No that's not possible. Going from frequency domain to time domain requires
a convolution and this is not supported by the Berkeley spice engine.
This could be added with the XSPICE interface and would indeed be a nice
add-on.

Maybe someone, someday...