


Power Magnetics Tools
RF Inductor Tools
CM Choke \ Ferrite Beads
LC Filter Designer IC / Inductor Match Tool Application Notes Other Resources
Designer's Kits

Implementing Models in PSpice 
Note The models are based only on steadystate lowsignal AC measurements and analysis. No DC bias or transient analyses were verified. The GLaplace element is used in PSPICE to describe a frequencydependent impedance. The impedance is given by the inverse of the XFORM, or XFORM = 1/Z(S). First, place a GLaplace element (part) into the model circuit schematic and connect as shown in the schematic below. Next, edit the GLaplace element by doubleclicking on the part in your schematic. Click on the "XFORM =1/S" line and edit the value in the "value" box, as follows: For a frequencydependent resistance (e.g. R_{VAR1}, R_{VAR2})Note: This example uses RVAR1 ( = k1 * sqrt(Frequency)). In your circuit, substitute the numerical value of k1 given in the model table for the specific model value you are using, into the XFORM statement. Z(S) = RVAR1 = k1*sqrt(Frequency), where Frequency is in degrees Since S is the frequency in radians, Frequency must be converted to degrees. The resulting frequencydependent resistance will be in Ohms units. 1/Z(S) = XFORM = 1/k1/(−S*S/4/3.14159^2)^0.25 For a frequencydependent inductance (e.g. L_{VAR})Note: In your circuit, substitute the numerical values of k3, k4, and k5 given in the model table for the specific model value you are using, into the XFORM statement. Z = S*L_{VAR}
= k3(k4*LOG(k5*Frequency)), where Frequency is in degrees Since S is the frequency in radians, Frequency must be converted to degrees. Since the inductance is given in uH units, the L_{VAR} expression is converted as shown below. 1/Z = XFORM = 1/(S*1e6*( k3(k4*LOG(k5*(S/(2*3.14159265)))))) Other circuit elementsPlace and wire the other parts of the model in the schematic. If the specific model inductance element is a fixed value inductor, use the IND part instead of the GLaplace part. Edit the part values to match those of the model table values for the specific inductor you are simulating. See the example schematic and netlist shown below. Example PSpice schematic and netlistIn the case where two GLaplace elements are in series, a largevalued resistance to ground (Rsim) was added to prevent a floating node error. The largevalued resistance (R3) was added to measure voltage across the entire model. Note: Make sure to substitute the specific model table values for each element (part) of the inductor model into the schematic. * Example Schematics Netlist * R_R2 $N_0002 $N_0001 0.001 V_V3 $N_0002 0 DC 0V AC 1v R_R3 $N_0002 0 10meg R_Rsim 0 $N_0003 10meg G_Rvar2 $N_0001 0 LAPLACE { V($N_0001, 0) } { R_R1 $N_0004 0 16000 G_Lvar $N_0003 0 LAPLACE { V($N_0003, 0) } { G_Rvar1 $N_0001 $N_0003 LAPLACE { V($N_0001, $N_0003) } { C_C $N_0001 $N_0004 .64pF To view the specific effective simulation resultsInclude the following Macros in your Probe trace analysis to see frequency vs. inductance, impedance, phase angle (in degrees), and Q factor: PI = 3.14159265 L=(IMG(V(R3:1)/I(R2))/(2*pi*FREQUENCY) Z = V(R3:1)/I(R2) ANG = (180/PI)*ARCTAN((IMG(V(R3:1)/I(R2)))/(R(V(R3:1)/I(R2)))) QFACT = ABS((IMG(V(R3:1)/I(R2)))/(R(V(R3:1)/I(R2)))) 
Home  Design Tools  Samples  Kits  Price + Stock  Sales  Support  Jobs  Index  
Your comments and suggestions are welcome. Contact [email protected] Copyright © 2020, Coilcraft, Inc. Privacy policy Updated: April 16, 2018 
