Email

* Required Fields

Recipients email * (separate multiple addresses with commas)

Your name *

Your email *

Message *

Contact Us

* Required Fields
First Name *

Last Name *

Email *

Company / Institution *

Comments: *

 PSPice Ftable Parameters 

Last post Wed, Feb 27 2013 5:06 AM by alokt. 9 replies.
Started by Daniel P 12 Feb 2013 05:31 AM. Topic has 9 replies and 2428 views
Page 1 of 1 (10 items)
Sort Posts:
  • Tue, Feb 12 2013 5:31 AM

    • Daniel P
    • Not Ranked
    • Joined on Tue, Feb 12 2013
    • Posts 6
    • Points 105
    PSPice Ftable Parameters Reply

    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. 

     

    • Post Points: 20
  • Tue, Feb 12 2013 10:40 PM

    • alokt
    • Top 25 Contributor
    • Joined on Fri, Aug 22 2008
    • Noida, Uttar Pradesh
    • Posts 241
    • Points 3,470
    Re: PSPice Ftable Parameters Reply

    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.

    • Post Points: 20
  • Wed, Feb 13 2013 3:42 AM

    • Daniel P
    • Not Ranked
    • Joined on Tue, Feb 12 2013
    • Posts 6
    • Points 105
    Re: PSPice Ftable Parameters Reply

    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. 

    • Post Points: 20
  • Wed, Feb 13 2013 9:29 PM

    • alokt
    • Top 25 Contributor
    • Joined on Fri, Aug 22 2008
    • Noida, Uttar Pradesh
    • Posts 241
    • Points 3,470
    Re: PSPice Ftable Parameters Reply

    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.

    • Post Points: 20
  • Thu, Feb 14 2013 8:39 AM

    • Daniel P
    • Not Ranked
    • Joined on Tue, Feb 12 2013
    • Posts 6
    • Points 105
    Re: PSPice Ftable Parameters Reply

    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. 

    • Post Points: 20
  • Thu, Feb 14 2013 8:43 PM

    • alokt
    • Top 25 Contributor
    • Joined on Fri, Aug 22 2008
    • Noida, Uttar Pradesh
    • Posts 241
    • Points 3,470
    Re: PSPice Ftable Parameters Reply

    I believe you are trying to simulate a frequency depended impedance network. This network can be represented by series RC circuit. You have this network characterized in form of gain/phase table.
    Something like given below
    Frequency GAIN(DB) PHASE
    0Hz 0 0
    30KHz -72 40
    35KHz -69 45
    36KHz -67.96 46.74
    39KHz -67.25 47.76
    Now I can use the following circuit to simulate a frequency dependent impedance
    G_GTABLE1 LOAD 0 FREQ {V(SENSE)} DB
    +0Hz 0 0
    + 30KHz -72 40
    + 35KHz -69 45
    + 36KHz -67.96 46.74
    + 39KHz -67.25 47.76
    V_V1 N00122 0 DC 0Vdc AC 1Vac
    R_R1 N00122 SENSE 1m TC=0,0
    V_V2 LOAD 0 DC 0Vdc AC 1Vac
    Here variable impedance is modeled by GTABLE1, and it connected across voltage source V2. Source V1 is dummy in nature and used only to sense frequency. If I simulate above circuit and compare result with following circuit at 35KHz
    C_C1 N03035 0 2.27n TC=0,0
    V_V3 N03025 0 DC 0Vdc AC 1Vac
    R_R3 N03025 N03035 2000 TC=0,0
    Current drawn from source in these circuits, V3 & V2, matches, thus confirm the equivalent impedance seen by both sources.I hope you would find this helpful.

    • Post Points: 20
  • Tue, Feb 19 2013 5:14 AM

    • Daniel P
    • Not Ranked
    • Joined on Tue, Feb 12 2013
    • Posts 6
    • Points 105
    Re: PSPice Ftable Parameters Reply

    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:

    Impedance_Phase

    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. 

     

     

     

    • Post Points: 20
  • Wed, Feb 27 2013 4:27 AM

    • alokt
    • Top 25 Contributor
    • Joined on Fri, Aug 22 2008
    • Noida, Uttar Pradesh
    • Posts 241
    • Points 3,470
    Re: PSPice Ftable Parameters Reply



    Refer the attached design. In this design GTABLE device is used to simulate microphone. The value shown in table does not represent the actual microphone characteristics for complete frequency range. These value are indicative in nature. I have calculated and put in value for only one frequency, that is 40KHz to explain the concept. Here load (microphone) is modeled using G table and this is connected to source V2. Source V1 is dummy in nature. In this specific circuit configuration, microphone is supposed to be connected between V2 and ground.

    In simulation results, at 40KHz frequency, you would see that overall impedance seen by source(V2) is ~400 Ohms. This is in line with value shown in impedance curve (shown in your append). Similarly you can see phase value is ~6 degree at 40KHz. This is also in line with value shown in microphone curve. Based on microphone impedance curve, it should behave largely as resistive element (since phase is ~0 degree), and hence major contribution to impedance would be largely due to resistive component (~400 ohms). I have tried to show the same by separate RC circuit in same design. At 40KHz, chosen RC (397.8 Ohms, 96n) value seems to offer similar impedance characteristics.


    Calculating the GTable parameters:

    Phase value can be directly obtained from microphone impedance curve.

    Since magnitude need to be defined in DB, it should be calculated using impedance value (400Ohms @40KHz), input voltage source magnitude (1V). G device is voltage controlled current source: which is current at output terminal for a given voltage at input terminal, thus I/V is my transfer function (gain or attenuation). If you plot the Gain/phase plot for RC circuit, you would see the similar (used in GTABLE device) value for gain/phase as seen by source V3.

    If you simulate and plot impedance seen by V2 and phase of current flown from V2, you should see plot similar to one shown in microphone impedance curve. Since this is plotted using only 4 data point this seems bit erratic, however it follows similar variations. This waveform can be further smoothen up using more data points in table.


    I hope this make sense, explains use of GTABLE device to simulate impedance and you find this relavent for your case.

    • Post Points: 20
  • Wed, Feb 27 2013 4:57 AM

    • Daniel P
    • Not Ranked
    • Joined on Tue, Feb 12 2013
    • Posts 6
    • Points 105
    Re: PSPice Ftable Parameters Reply

    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.

     

     

     

    • Post Points: 20
  • Wed, Feb 27 2013 5:06 AM

    • alokt
    • Top 25 Contributor
    • Joined on Fri, Aug 22 2008
    • Noida, Uttar Pradesh
    • Posts 241
    • Points 3,470
    Re: PSPice Ftable Parameters Reply

    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.

    • Post Points: 5
Page 1 of 1 (10 items)
Sort Posts:
Started by Daniel P at 12 Feb 2013 05:31 AM. Topic has 9 replies.