BACK

# Implementing Models in PSpice

Note:  The models were created and verified in a modern high-frequency simulation program (AWR Microwave Office 2002). The results of identical models in the student version of PSPICE in some cases gave different results (up to 3% different Z and L, and up to a 3° phase angle difference). The differences were not due to rounding of the model table values or number of simulation frequency points. Since the compared models were identical, we must conclude that the differences reside in the simulation software implementation. Since the differences appear to be in the software, they cannot be explained by Coilcraft at this time. Caution is advised.

The models are based only on steady-state AC measurements and analysis. No DC bias or transient analyses were verified.

The GLaplace element is used in PSPICE to describe a frequency-dependent 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 double-clicking 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 frequency-dependent resistance (e.g. RVAR1, RVAR2)

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 frequency-dependent resistance will be in Ohms units.

1/Z(S) = XFORM = 1/(k1*sqrt(S/(2*3.14159265)))

### For a frequency-dependent inductance (e.g. LVAR)

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*LVAR = k3-(k4*LOG(k5*Frequency)), where Frequency is in degrees
The "LOG" function used here is the natural logarithm (base e, not base 10).

Since S is the frequency in radians, Frequency must be converted to degrees.

Since the inductance is given in uH units, the LVAR expression is converted as shown below.

1/Z = XFORM = 1/(S*1e-6*( k3-(k4*LOG(k5*(S/(2*3.14159265))))))

### Other circuit elements

Place 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 netlist

In the case where two GLaplace elements are in series, a large-valued resistance to ground (Rsim) was added to prevent a floating node error. The large-valued 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) } {
+ 1/(k2*sqrt(S/(2*3.14159265))) }
R_R1      \$N_0004 0 16000
G_Lvar    \$N_0003 0 LAPLACE { V(\$N_0003, 0) } {
+ 1/(S*1e-6*(k3-(k4*LOG(k5*(S/(2*3.14159265)))))) }
G_Rvar1  \$N_0001 \$N_0003 LAPLACE { V(\$N_0001, \$N_0003) } {
+ 1/(k1*sqrt(S/(2*3.14159265))) }
C_C         \$N_0001 \$N_0004 .64pF

### To view the specific effective simulation results

Include 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))))

BACK