PSPice Ftable Parameters 

Hi there.

I'm developing a circuit in PSpice including an Impedance-model, which is simulated within a real and a complex part. Also can be looked like a Resistor and a Capacitor that change values according to varying the frecuency.

So, for example, I have:

@35kHz: R=2000; C=2.27nF or also can be modeled like 0-2000j or |Z|=2000 and Phase=-90º

... 

@39kHz: R=1550; C=2.39nF or also can be modeled like 202.32-1536.7j or |Z|=1550 and Phase=-82.5º 

and so on, until 45kHz (steps can be from 250Hz). 

When I try to insert this behavior into my Schematic, using FTABLE Part, I cannot get the right way to simulate whe whole circuit (the output I get has no-sense).

I know the circuit is well designed because if I put single values of a Resistor and a Capacitor instead of the FTABLE componet, I get a correct output. But that's not a polite solution, because I have many values for these components.

I'm trying to set up the FTABLE like this (Parameters are in Modulus and Phase Expression mode)

row1: 35kHz    2000         -90

row2: 38.5kHz     1650       -86.25

row3: 39kHz     1550       -82.5 

row4: 41.750kHz     2100       -88

row5: 45kHz     1800      -90 

 MAGUNITS=mag

What am I doing wrong? Do I need to change other parameters or settings in the FTABLE setup? Is there other way to do what I'm trying to?

Thank you in advance, any help will be much appreciated.

Regards,

D. 

You may want to try the GTABLE device, that voltage controlled current source, with input to output relationship governed by TABLE.

I think G device may be more appropriate for impedance (transconductance) modeling, F would simply model current gain in it's simplest form. However this would depend upon the circuit configuration.  FTABLE is an E device, which may not be suitable for modeling impedance.

Here is what I tried

G_TABLE1         N00129 0 FREQ {V(N00223)}  DB 
+0Hz         0         0 
+ 10Hz      -3       -30 
+ 20Hz      -6       -90 
+ 30Hz     -10      -120 
+ 40Hz     -15      -150
V_V1         N00122 0 DC 0Vdc AC 1Vac
R_R1         N00122 N00223  1m TC=0,0
R_R2         N00129 0  1 TC=0,0

 And resultant current waveform at o/p of Gdevice (or voltage across R2) follow the gain/phase relation defined in table. I think this can be configured to provide frequency dependent impedance.

online photo storage

Hope this helps.

Hi alokt.

Thanks for the reply.

I've been studing other parameters, such as EFREQ and GFREQ (better this one for modeling Impedance), and according to the manual, seems to be perfect for what I'm trying to do.

The question is, how can I define the values table from the data I have? I had never do it before, could you please tell me how to fill it? or just an example of one sample data.

And the other fact is, how must I connect this kind of Part in my circuit? I mean, it has 2 Inputs and 2 Outputs, and it has to be changing a R and a C in series (only one wire as Input and another one as Output).

Hope you can help me out with this as well.

Best regards,

D. 

Please refer the app note http://www.cadence.com/rl/Resources/application_notes/nonlinear_capacitor_model_appnote.pdf

This has detailed instruction on how to use G device to model non-linear capacitor. It also has example of how to use TABLE based G device, you need to replace this with  frequency dependent G devices. Hope this enables you to move forward. Let us know if you have further questions.

Much appreciated for the note, but I think its not my case.

I have two elements, R and C, and their values changing due to frecuency variation.

What is more, I can combine them to create a Real and Complex Equivalent Impedance, because they are connected in the circuit in series mode.

But, I cannot get the voltage outsite the Capacitor to use that kind of tables.

I dont care about using two tables (one for R and other one for C) or one for both elements, but there must be a quite easy solution for this case, and I cannot find it. 

I just want to avoid making a lot of simulations changing the values of R and C in each step, taking the exact value of the Output-Voltage of my circuit for each frequency, record them into a table in other software, plotting it...

Hope its better understood now, and also anyone could help me out with this.

Thank you in advance.

Regards,

D. 

Hi again. 

Nope, I'm not simulating an impedance network. But I find quite useful your advices in the last post.

Let me explain you what I have and what I need:

I have a little microphone which impedance is specify by manufacturer in two figures:

As you can see, Module and Phase Angle are shown there, varying with the frequency (x-axis).

So, I have filled up value table-data, and have converted them into values: Real Part (Resistor Value) and Complex Part, and from this one I can get the Capacitor value for each frequency.

So, in my circuit, I have to insert a Resistor and a Capacitor, and their values are going to change in each frequency. So, when I'll do an AC Sweep, it must show the output value depending of them.

The hard and heavy way is to simulate, for example, one circuit with each value of Resistor and Capacitor for each kHz. I will obtain the Output for each single value of Frequency, and then just have to join each value to get the whole output figure.

But, I really think PSpice must have a easier way to do that. Just need a table instead of the RC and fill it with the data I have.

Hope its now better understood and you can tell me how to define the data and how to connect the GTABLE (or whatever I need) into my circuit.

Much appreciated for your help.

Regards. 

Hi alokt,

Thank you very much. 

Just to let you know, the values in the impedance curve I've post are |Z| and Phase (Z). And the |Z| axis is expressed in decades (logarithmic). And the degrees values are a bit hard to understand because they are in the same graph.

So, for example, @ 40kHz, the correct values are:

|Z| = 2000Ohm (I've sampled that to 1800Ohm)

Phase =  -36 º

And it results:

R=1456.2 Ohm

C=3.76nF

when I calculate the R and C values.

I'll try your method when I arrive at home.

Thank you so much,

Regards.

Yes, you are right, accidentally I interchanged amplitude/phase curves while reading the values. However concept should still be valid. Since phase is now lagging, you would need to assign appropriate sign for phase in Gtable parameter.