


Power Magnetics Tools
RF Inductor Tools
New! CM Choke Finder
New! LC Filter Designer IC / Inductor Match Tool Application Notes Other Tools Designer's Kits

Implementing Models in Microwave Office 
Important! Even the most current version of Microwave Office may not contain uptodate libraries of our inductor models and Sparameters. Coilcraft provides the most current and accurate versions of our models on our web site. SparametersOur Sparameters are provided in a single compressed "zipped" file. The file must be "unzipped" after downloading to obtain the separate inductor value Sparameter files. You can either link to or import our Sparameter data files. Right click over the "Data Files" folder on the left. Select either "Link To Data File." or "Import Data File." Browse to the folder where the unzipped files are located and select the desired Sparameter file. To place the data file on a schematic: 1. Select the "Elem" tab. 2. Click on the "Subcircuits" folder. 3. Click on the selected data file element. 4. Drag the element onto your schematic. Lumped element (SPICE) modelsTo model our chip inductors, either select the CCIND element from the Lumped Element  Inductor menu or place each individual lumped element for the model onto the schematic. An example chip inductor schematic is shown in Figure 1. Figure 1. Example schematic for a Coilcraft chip inductorTo model our power inductors, each individual lumped element (L_{VAR}, C, R2, R1, R_{VAR1}, R_{VAR2}) for the complete model must be placed into the schematic. An example of a power inductor schematic is shown in Figure 2. Figure 2. Example schematic for a Coilcraft power inductorAfter all the lumped elements are placed into the schematic, change the value for each element to match the value in the model table for the specific inductor. If you plan to model different Coilcraft inductors in the same schematic, be sure to rename the individual lumped elements and variables, then update the values from the model table for each inductor. For a frequencydependent resistance (R_{VAR1}, R_{VAR2})Note: This example uses R_{VAR1} ( = k1 * sqrt(Frequency)). 1. Place an ideal resistor on the schematic. 2. Double click on the resistor to edit the value. 3. Rename it to identify it as a variable resistor (e.g. "Rvar1"). 4. For the resistance value, enter the equation: k1*(_FREQ)^0.5. 5. Replace k1 with the value from the model table. For a frequencydependent inductance (L_{VAR})Note: This element is used in some of our power inductor models. 1.Place an ideal inductor on the schematic. 2. Double click on the inductor to edit the value. 3. Rename it to identify it as a variable inductor (e.g. "Lvar"). Note: The "log" function in the following equation is the natural logarithm, base e, not base 10. 4. For the inductance value, enter the equation: k3(k4*log(k5*_FREQ)) 5. Replace k3, k4, and k5 with the values from the model table. Graphing specific model inductance and Q resultsImportant! Our models represent deembedded measurements in which fixture parasitic reactances have been removed. Fixture (or circuit board) parasitic reactances raise the effective impedance (and the effective inductance), lower the selfresonant frequency (SRF), and shift the Q curve. For the most accurate model of our inductors in your specific circuit environment, you must include your circuit board model in the simulation. InductanceTo view the effective series inductance of the model in a graph: 1. Right click on the graph name. 2. Click on "Add Measurement." 3. In the "Add Measurement" dialog box, select "Linear" as the Meas. Type. and "L_SRL" as the Measurement. 4. Use your model schematic for the Data Source Name. 5. Check the "Sweep Proj. Freqs" box, and select the input port to your model. 6. Click Add." Quality factor (Q)Q values and curves in our data sheets are typically based on measurements using an impedance analyzer in a 50 Ohm environment, giving a 1port (reflection) measurement result. If Q calculations are to be compared with data sheet values and curves, they should be based on a simulation with one port of the inductor model connected to ground (as shown in Figure 2). If you are interested in the Q of the inductor in a 2port series configuration, the additional 50 Ohms impedance of the second port results in a lower simulated Q value than the 1port configuration. This result is logical considering that the additional 50 Ohms applies to the "Re [Z]" in the denominator of the Q calculation equation. Q = Im [Z] / Re [Z] At this time, Microwave Office does not have a Q measurement function. You must enter the equation for Q in the "Output Equations" window. Im [Z] output equation1. Open the "Output Equations" window. 2. Click on the "Output Equation" icon or select it from the "Add" menu. 3. Enter a variable name, such as x", 4. Select "Linear" as the Meas. Type and ZIN" as the Measurement. 5. Select your model schematic for the Data Source Name. 6. Check the "Sweep Proj. Freqs" box. 7. Check "Imag" as the Complex Modifier. 8. Select the input port to your model. 9. Click "Add." Re [Z] output equation1. Open the "Output Equations" window. 2. Click on the "Output Equation" icon, or select it from the "Add" menu. 3. Enter a different variable name than the one used in Im [Z], such as y", 4. Select "Linear" as the Meas. Type and ZIN" as the Measurement. 5. Use your model schematic for the Data Source Name. 6. Check the "Sweep Proj. Freqs" box. 7. Check "Real" as the Complex Modifier. 8. Select the input port to your model. 9. Click "Add." Q equation1. Open the "Output Equations" window. 2. Click on the "Equation" icon or select it from the "Add" menu. 3. Enter a variable name, such as Q1port", 4. Complete the equation using your Im [Z] and Re [Z] variables (for example: Q1port = x / y). To view the Q vs. frequency of the model in a graph1. Right click on the graph name, and click "Add Measurement." 2. In the "Add Measurement" dialog box, select Output Equations" as the Meas. Type, and Eqn" as the Measurement. 3. Use your Q equation variable name for the Data Source Name. 4. Check "Mag" as the Complex Modifier. 5. Check the "Sweep Proj. Freqs" box, and select the input port to your model. 6. Click "Add." 