This appendix includes advanced analysis topics for users who want more detailed information on these methods.
Simulated Load Pull functionality supports the AWR multi-dimensional A/B Wave Load Pull file format. Variable sweeps (for example; input power, bias, or frequency) are controlled via the Load Pull Template schematic. For more information see “Load Pull Script”.
Several Load Pull file formats encompassing both swept and non-swept data are supported. You can import all of these file types using the
script. This file supports the following file types:Swept Load Pull formats
*.cst
*.spl
*.lpc
*.mdf
, *.mdif
(“A/B Wave Format”)
Non-swept Load Pull formats
*.sp
*.lp
*.lpd
The NI AWR Design Environment platform supports applying a de-embedding network to the output pin of a load pull file DUT, allowing the data reference plane to be moved to either side of the specified de-embedding network. For example, moving from an external device pin, through a package model, to an internal device pin. The de-embedding is done at the load pull data file level so all measurements applied to that document show the de-embedded result. See “Project Options Dialog Box: Interpolation/Passivity Tab ” for details on configuring the de-embedding network.
Load Pull measurements are often more easily visualized through a marker-defined reference, allowing the coupling of measurements together and quickly parsing through the individual sweeps. For information on setting up a marker-defined reference, see “Using a Marker to Define a Sweep Index”.
Load Pull measurements are differentiated by a naming convention that separates swept and non-swept based measurements. The measurement names are interpreted as follows:
Swept Load Pull measurements are prefixed with "G_", while non-swept measurements have no prefix.
Measurements that align data to a specified value end in “A”.
Measurements that plot a single value contain “_V”.
Measurements that plot a real value contain “_R”.
Measurements that plot a complex value contain “_C”.
The following is a list of commonly used measurements:
For plotting contours
plots contours
plots contours aligned to a specified value (for example: 1 dB compression)
plots the intersection between two contours
For plotting contour interpolated min or max value
plots the contour min value
plots the contour max value
To plot a single contour at a specified value
plots a single contour at a specified value
For plotting all the gamma points in your Load Pull file
plots gamma points for a swept load impedance
For plotting swept data on a rectangular plot (like PAE vs. output power)
plots real data with a derived value chosen for the x and y axis in the measurement setup
For measurement details, click the
button in the Add/Modify Measurement dialog box.When working on convergence problems, you need to change APLAC simulator settings. You can set simulator-specific settings globally (choose Use project defaults to override the global options.)
) or locally for each schematic (right-click a schematic in the Project Browser and choose , and for each option tab you can clearAPLAC settings are controlled on the Circuit Options or Options dialog box APLAC Sim tab as shown in the following figure.
The dialog box splits the simulator settings into Common Simulator Options, and APLAC Simulator Options. Select an option to view additional information about it in the lower window of the dialog box.
Always begin with default settings, as these are most commonly successful. If you copy an existing project as a starting point for a new one, the new project may "inherit" simulator settings that are inappropriate for your new design(s).
DC convergence problems are very rare as various approaches are taken to achieve DC convergence.
A common problem arises when using S-parameters for models that do not have a DC point defined, and the simulator must extrapolate to DC. You can try to change the extrapolation settings. Choose Options > Project Options and click the Interpolation/Passivity tab. You can try Rational function as the interpolation method or switch between Polar and Cartesian coordinate systems.
Harmonic balance can have convergence problems in some cases. If this occurs you can use the following steps to try to help the circuit converge.
Ensure that all nodes of every element are connected.
You can inspect your circuit visually or use the Design_Checker script to check for you.
To access the Design_Checker script choose
and configure the settings as follows.
Change the HB Matrix Solver to Sparse or GMRES (whichever is not currently selected).
The default HB Algorithm setting is Auto select, which analyzes the circuit topology and then uses either Piecewise or Nodal. You can switch to each of these settings specifically to see if it helps.
Use a power sweep. Instead of using power levels that force the circuit into strongly nonlinear modes of operation with a port set to a single power, use a port that sweeps power from a small signal region of operation into the strongly nonlinear region.
Try changing the Maximum Voltage or Current Change
parameter to "1e6
" or decreasing it to
"1e-3
".
Use transient assisted harmonic balance by selecting the Transient Assisted HB check box.
Answer these simple questions to help determine why the simulator is not converging:
Are your models valid at the highest frequency at which harmonic balance needs to simulate, at the highest tone product specified by your number of tones and highest tone order? One way to check is to make a plot of Pharm of a simple circuit (maybe just a resistor) to see the highest frequency the simulator needs.
If you have an APLAC Transient license, use it with enough periods to reach steady state to see if the answers look reasonable in that simulator. If the answers don't look good, it could signal that there is a model problem.
When working on convergence problems, you need to change APLAC simulator settings. You can set simulator-specific settings globally (choose Use project defaults to override the global options.)
) or locally for each schematic (right-click a schematic in the Project Browser and choose , and for each option tab you can clearAPLAC settings are controlled on the Circuit Options or Options dialog box APLAC Sim tab as shown in the following figure.
The dialog box splits the simulator settings into Common Simulator Options, and APLAC Simulator Options. Select an option to view additional information about it in the lower window of the dialog box.
Always begin with default settings, as these are most commonly successful. If you copy an existing project as a starting point for a new one, the new project may "inherit" simulator settings that are inappropriate for your new design(s).
DC convergence problems are very rare as various approaches are taken to achieve DC convergence.
A common problem arises when using S-parameters for models that do not have a DC point defined, and the simulator must extrapolate to DC. You can try to change the extrapolation settings. Choose Options > Project Options and click the Interpolation/Passivity tab. You can try Rational function as the interpolation method or switch between Polar and Cartesian coordinate systems.
Transient analysis can have convergence problems in some cases. If this occurs you can use the following steps to try to help the circuit to converge.
Change the truncation error method by changing the Truncation Error Mode to either Voltage or Charge.
Change the integration method by changing Integration Method to either Euler or Gear.
Try increasing the Maximum Voltage or Current Change
parameter to "10 ... 100
" or decreasing it to
"0.5
".
Change the Step time under Transient Options to smaller or larger time steps.
Use fixed time steps by changing Time Stepping to
Fixed and specifying the fixed step size by typing
"TMIN
" in Free Text under
Miscellaneous Options; otherwise the Step time under
Transient Options is used.
Answer these simple questions to help determine why the simulator isn't converging:
Are there potentially bad component values (for example, unrealistically large capacitors or inductors)? For example, for a DC block, you could use a very large capacitor (such as 1 mF) for harmonic balance and it simulates correctly. For transient analysis, this large capacitor causes problems.
Are there short transmission lines in the circuit that limit the time step? Can you replace these with RLC networks? The lines might be inside models so you may need to check the input netlist.
Are there huge voltages in your design? If so, you may need to increase Maximum Voltage or Current Change.
What does HB say about the circuit? If the answers do not look correct, this could signal a model problem.
Convergence failures, though rare, are usually a consequence of very strongly nonlinear circuit behavior. In such cases, one difficulty encountered by the simulator is a lack of a "good guess" at the solution. Some of the common causes for convergence failure are circuit instabilities, too few frequency components, discontinuities in nonlinear device modeling, and too few simulation iterations.
Some of the most common messages in the Status Window are "Simulation only partially completed" and "Step size for source stepping has decreased below a minimum allowed value". The following figure shows an example warning message for a circuit that has failed convergence.
The following section is a generic procedure for finding convergence problems. These are basic guidelines based on NI AWR experience.
Simulate a DC annotation to test if the circuit is converging at DC, and to provide a check for the proper operating condition of your circuit (for example if you accidentally specified 50 volts for the supply voltage instead of 5 volts). See “Creating a New Annotation” for information about adding an annotation.
Simulate at low input levels (for example, -30 dBm for power, 1mV) to see if you get a solution at low powers.
If the previous step works, try sweeping your input source. Many times a circuit converges better if you sweep from a low input level to a high power rather than just setting a high input level.
Verify whether your Harmonic Balance settings use the project default settings or are set at the schematic level. Right-click the top level schematic in the Project Browser, choose Use project defaults is selected in the Harmonic Balance Options section, the schematic uses the project settings. You can access project settings in the Circuit Options dialog box (choose ).
and then click the appropriate simulator tab in the Options dialog box. IfIn Iteration Settings, increase the Max iterations to 100 or 200 and see if it helps. For strongly nonlinear circuits you may need to set this value higher. Another way of increasing the number of iterations is by increasing the number of sweep steps. For example, a power sweep from -20 db to 20 db in steps of 1 db is more likely to converge than that with steps of 5 db.
Increase the number of harmonics. If the circuit you are analyzing is strongly nonlinear, it is important for both accuracy and convergence to specify a sufficient number of frequencies in the simulation. This is the first step in troubleshooting convergence problems.
Add a small conductance across the nonlinear elements. Choose AWR Sim tab under Convergence Aids verify your results are correct.
and on the Circuit Options dialog boxAlso under Convergence Aids, remove voltage limiting by clearing the Limit step size check box.
Use a predefined set of convergence settings. In many cases selecting some of these predefined convergence settings along with tolerance settings helps the circuit to converge. If the circuit always needs to source step, you can speed up the simulation by selecting Start with source stepping under Configuration Wizard.
Under Advanced HB Options, select any linearization method along with a degree of tolerance to speed up the convergence in Linearization Mode and Linearization Tolerance.
Change the simulation accuracy. The simulation terminates when the absolute current error at each nonlinear element and at each harmonic is below Absolute Tolerance, or when the Relative Tolerance criterion is satisfied. The default value of Absolute Tolerance is "1e-9" and sometimes this number is very low for highly nonlinear circuits. You can increase this number to a value such as "1e-7" while leaving Relative Tolerance as is.
The standard method for checking the stability of an active two-port is to use the stability factors K and B1 or some other measure of stability.
Although these measures are useful for analyzing the stability of a two-port, there are many situations where the satisfaction of the standard criteria for stability (K and B1) do not guarantee that the circuit is stable. Microwave Office or Analog Office programs offer some alternative stability analysis techniques to reduce the likelihood of an unstable design.
CAUTION: Stability analysis methods try to prove a negative-- the absence of instability. No one method, or even collection of methods, can guarantee stability. NI AWR does not claim that the following approaches find all stability issues. You should consider all stability analysis approaches.
Two examples of circuits where K and B1 do not detect instability are described in the article by Platzker and associates. ^{[3]}The article demonstrates how NDF detects the instability of these circuits (NDF finds poles in the right half plane).
The basics of NDF analysis in the Microwave Office program are:
NDF analysis is only available with the APLAC simulator, so all models must function with APLAC.
NDF is a complex measurement vs. frequency at schematic load impedance. It must be measured over a very wide frequency range ("DC to daylight"). At low frequencies and as the frequency approaches infinity, NDF is real. The circuit is unstable if the measurement circles the origin of a polar plot more times clockwise than counter-clockwise; i.e. if the change in the unwrapped phase (AngleU) of the NDF measurement (from near DC to approaching infinity) decreases by more than 360 degrees.
For optimization, use Output Equations to calculate the difference between the initial and final values of AngU(NDF), and set a goal for this value to be less than 360 degrees.
IMPORTANT: Like other measurements, the frequency sweep for NDF is set on the schematic, or in the project options, so it is "fixed", not adaptive. You should set the frequencies to ensure that the measurement is well resolved, and encirclements of the origin can be detected for each simulation, even over parametric sweeps and optimization. The most efficient frequency sweep may involve varying step sizes over different frequency ranges. For this reason, it is usually best to have a separate frequency sweep for the NDF measurement. There are two ways to do this:
Create a new top level schematic with its own frequencies for the NDF measurement, and place the circuit of interest in it as a subcircuit.
Add a FRQSWP block, and set its Values parameter to an equation that concatenates multiple sweeps together. (See the table at “Built-in Functions ”). The frequencies are automatically collated for simulation.
To function properly, NDF needs to identify individual dependent (voltage- or current-controlled) sources in the circuit. Active S-parameter files, or compiled linear models with controlled sources inside them do not allow this and are therefore not included in the measurement calculation.
The schematic on which NDF is measured must include a PORT element. If the schematic is drawn with the (source and) load impedances represented by other elements, you need to place a PORT element anywhere on the schematic, without anything connected to it.
The basics of stability envelope analysis are:
Stability envelope analysis is only available with the APLAC simulator, so all models must function with APLAC.
APLAC computes the envelope of the NDFs corresponding to all possible passive source and load impedances at the ports.
StabEnv is the complex envelope of the NDFs corresponding to all possible passive source and load impedances at the ports. The circuit is stable if, at each frequency, StabEnv does not circle the origin of a polar plot (if the unwrapped phase (AngleU) of the measurement has a range of less than 360 degrees).
For optimization, use Output Equations to calculate the difference between the maximum and minimum values of AngU(StabEnv), and set a goal for this value to be less than 360 degrees.
The number of points used to approximate the impedances is set by choosing APLAC tab and under Stability in StabEnvelopePoints, increase this number to ensure the measurement is well resolved, and encirclements of the origin can be detected for each simulation, even over frequency/parametric sweeps and optimization.
to display the Circuit Options dialog box. Click theFor more information see the following source: T. Narhi and M. Valtonen, “Stability Envelope - New Tool For Generalized Stability Analysis,” IEEE MTT-S International Microwave Symposium Digest, pp. 623–626, June 1997.
The complex loop gain of a feedback network, such as an amplifier, can be used to check for instability. When loop gain is all real (angle=0) and greater than 1, the circuit is unstable. The LoopGain and NLLoopGain measurements calculate small-signal (linear) loop gain under DC bias or large-signal drive conditions, respectively. These measurements work without modifying the design, by accessing the internal controlled source of nonlinear transistor models. Consider the following linearized model for a FET transistor:
Loop gain measurements internally break the feedback loop that includes this transistor by replacing the controlling voltage of the transconductance gm with a test signal, Vin, and measuring the resulting output voltage, Vgs, where the controlling voltage should be:
The loop gain is defined as the voltage gain Vout/Vin. All the other measurements see the unmodified circuit, allowing other measurements to work normally for the same schematic. You are required to point to the place in the circuit where the feedback loop is broken by selecting an internal branch of a nonlinear device as the Measurement Component in the Add/Modify Measurement dialog box. For example, the CURTICE nonlinear FET model has three internal branches: "ds", "gd" and "gs". The drain-source branch "ds" is a good place to break the loop for a FET amplifier. Note that the feedback loop can be formed by internal elements like Cgd in the previous example, by external elements like biasing networks, or both.
To add a loop gain measurement, begin by selecting the appropriate top level schematic as the Data Source Name. To identify the internal branch of a nonlinear transistor model as a Measurement Component, click the browse button ("...") as shown in the following figure:
See “Measurement Location Selection” for information on using the window that opens to navigate hierarchy and open the subcircuit schematic (or netlist) containing the desired transistor. Next, select the appropriate branch of that transistor as the Testpoint. For example, select the collector-emitter branch of the BJT model in a subcircuit netlist, as shown in the following figure.
The LoopGain measurement is only possible if the selected transistor exposes its internal branches, so that the transconductance branch can be selected. Some transistors do not expose these branches so therefore cannot be used for a LoopGain measurement.
The linear LoopGain measurement works as described in “Loop Gain”. As with any linear measurement on a nonlinear circuit, an initial DC bias analysis is performed to determine the operating point of all nonlinear devices. This allows the nonlinear transistors to be linearized (represented by an equivalent linear network like the one shown previously), so that the LoopGain measurement can be made using a linear small-signal analysis. For more information see “Loop Gain: LoopGain”.
NLLoopGain is a nonlinear extension to LoopGain that takes into account the large-signal drive of the circuit. First, the nonlinear steady-state solution of the circuit is determined with Harmonic Balance. The circuit is linearized at this operating point and the feedback loop is broken at a user-specified point. Next, a linear small-signal analysis is performed to compute the loop gain. The NLLoopGain measurement requires that an NLSTABILITY control element is placed in the schematic, and it can only be used with the APLAC HB simulator. For more information see “Nonlinear Loop Gain: NLLoopGain”.
Another example of the K and B1 requirements not ensuring stability is that of a two-stage amplifier. K and B1 may indicate the amplifier is stable, but it is still possible for the amplifier to be unstable due to oscillation conditions that may exist between the two amplifier stages. This "internal" instability in the interstage of the amplifier may not be detectable by a simple measure of K and B1 of the entire amplifier.
One approach to solving this problem is to make each device unconditionally stable before adding the matching. This is usually accomplished by adding lossy matching or feedback to the potentially unstable device. Although this may work, there are a drawbacks to this approach.
The first drawback is that it does not guarantee that the amplifier remains stable if there is any amount of feedback between the two stages. Although there is usually not any intentional feedback between the stages, there is often unintentional feedback that arises from the bias circuitry that may be connected together with less than ideal isolation. A thorough stability analysis should attempt to include the bias network as part of the analysis. The standard K and B1 stability factors do not detect instabilities caused by this type of feedback.
The second drawback is that the addition of the lossy matching (or feedback) usually reduces the performance of the device significantly. If a more thorough technique is used to analyze the stability of the interstage circuitry, then it is usually possible to get much better performance from the same devices with an acceptable margin for stability. One such method for predicting internal stability is presented in an S-probe article.^{[4]}. This method requires the measurement of internal reflection coefficients within the circuit, and it also requires the ability to analyze the circuit with arbitrary termination impedances.
Microwave Office and Analog Office programs have several unique features that greatly simplify the analysis of the internal stability:
An element for sampling the internal reflection coefficients at internal nodes in a circuit.
The ability to terminate any port with an arbitrary reflection coefficient (not restricted to two ports).
Built-in measurements that compute the stability without needing to use output equations.
Some background information on internal stability is useful for understanding the analysis method. The following figure shows two networks connected together. The network on the left has S-parameters [S] and the network on the right has S-parameters [S']. The lower part of the figure shows a portion of the signal flow graph that includes the interface between the two networks. The use of a signal flow graph allows the stability to be analyzed using the same techniques as those used for analyzing the stability in control systems.^{[5]}
You can determine the stability of the previous system by viewing the loop in the signal flow graph as a feedback loop. This allows the Nyquist stability criteria to be applied to the open loop frequency domain response given by
G=-Γ_{1}Γ_{2} | (A.1) |
The Nyquist stability criteria states that if the open loop function G, when plotted on the complex plane, encircles the -1 point in the clockwise direction, then the closed loop system will be unstable. The following polar plot of G shows an unstable system (G encircles the -1 point in a clockwise sense).
The Microwave Office STABN_GP2 measurement allows the function G to be plotted on a polar graph for inspection of the stability. When plotting STABN_GP2, the frequency should be swept over the entire range where instability could occur.
An approximate simplification of the Nyquist stability criteria allows the computation of a single stability index that can be plotted as a single real number over frequency. The use of a real stability index makes it easier to include internal stability as an optimization goal.
The meaning of the stability index is shown in the following figure.
The stability index is taken to be the negative of the component of G along the real axis. A value of the stability index greater than 1 is then used to indicate possible instability. The term "possible" is used because it is possible for the stability index to be greater than 1 without an encirclement of the -1 point, as shown in the following figure.
Although the stability index may indicate instability when the device is actually stable, it is still a very useful measure in practice since it does not predict that the circuit is stable when the Nyquist criteria indicates that the circuit is not stable (it is a conservative measure). Usually if the stability index predicts that a stable circuit is not stable, then margin of stability for the circuit is not very high (minor changes in the response could cause instability). Also, if the stability index predicts an instability, then the more rigorous Nyquist criteria can be used to verify the instability. The stability index indicated here is the same as the stability index presented in an S-probe article.^{[4]}. You can use the Microwave Office STAB_GP2 measurement to plot this stability index (STAB_GP2 <1 indicates stability). For more information see “(Obsolete) Stability Index Measured with Gamma-Probe: STAB_GP”.
The following schematic shows the GPROBE element inserted into the schematic at an internal node where the stability is to be analyzed.
The GPROBE element is used to measure the internal reflection coefficients at the reference plane indicated. The stability measurements STAB_GP2 and STABN_GP2 and the internal gamma measurements made with GAM_GP2 require that you select a specific GPROBE2 to identify the reference plane.
One of the drawbacks of the proposed method used to analyze the stability is that it is only valid when the circuit is terminated with the same termination impedances that are used during the analysis. The termination impedances that make the circuit the "most unstable" are generally the impedances with a reflection coefficient of magnitude one, so you should test the stability when the circuit is terminated with impedances that lie on the edge of the Smith Chart.
The port element PORTG allows the termination impedance of the port to be specified as a magnitude and angle of the reflection coefficient. In practice, it is not possible to compute the response of the circuit with perfect magnitude one reflection coefficient on the ports, so a value close to one (0.99 for example) is used instead. You can change a normal port to a PORTG port by editing the port element and selecting the Specify Source Gamma check box on the Port tab of the Port properties dialog box. You can also add the PORTG element through the Element Browser.
One method for testing the stability for a wide range of port terminations takes advantage of the yield analysis feature. If all the terminal ports use PORTG elements, and the magnitudes of the reflection coefficients are set to something close to 1 (0.99 for example) then the angle parameter can be set to 180 degrees, and the statistical properties can be set so the angle has a uniform distribution with a tolerance of 180 degrees. When the yield analysis is run, the angle takes on random values from 0 to 360 degrees which covers all points on the outer radius of the Smith Chart. The stability index can be plotted during the yield analysis and any trace that exceeds a value of one indicates that the circuit can become unstable.
Linear internal stability analysis can be generalized to nonlinear circuits. First, a large-signal solution is computed using the APLAC HB simulator. Next, the circuit is linearized at the found HB solution and the internal reflection coefficients are solved at each small-signal frequency. If there are sweeps in the simulation setup, the large-signal solution and the following internal stability analysis are performed at each sweep point. This allows analyzing the stability of the circuit as a function of some swept quantity, for example input power.
The NLGAM_GP2, NLSTABN_GP2, and NLSTAB_GP2 measurements are straightforward nonlinear generalizations of their linear counterparts. They can only be used with the APLAC HB simulator. Analyzing nonlinear stability requires that control element NLSTABILITY is placed in the schematic. The Fstart, Fend, and Fsteps parameters define the range of small-signal frequencies to sweep over. Note that these are absolute frequency values, not offsets to the large-signal fundamental frequency. SwpType defines the type of small-signal frequency sweep (linear or log).
By default, the Microwave Office program places a perfect electric conductor (PEC) on the top and bottom of the enclosure. Since the side-walls are always PEC, the default configuration is completely enclosed by the perfect conductor and no radiation is possible. To allow radiation into an infinite region, you must model the top of the enclosure as an open boundary.
If the top of the enclosure is made to have a boundary condition that approximates the
boundary condition of an open box, then you can use the tangential electric field at the
top of the enclosure (the tangential field at the absorbing boundary) to compute the
far-field radiation pattern. A detailed description of the method used for determining
the radiation pattern from the tangential electric field is included in Chapter 12 of
Antenna Theory Analysis and Design
.^{[6]} This process involves two steps:
The first step is the computation of the tangential electric field. This is performed using an approximation to the aperture boundary condition at the top (and/or bottom) of the enclosure (currently there are two different types of boundaries you can use). Using these boundary conditions, the currents on the internal conductors are determined for a given excitation using standard EMSight methods. After these currents are known, the tangential E-fields are determined on the top surface of the enclosure. These fields are used in step two of the process.
The second step in the process involves re-radiating the equivalent currents of these tangential electric fields into the upper hemisphere, assuming that these equivalent currents are present upon a perfectly conducting half plane. Using the equivalence theorem and the image theorem, you can represent the radiation problem as a sheet of magnetic current that is infinitely close to a perfectly conducting half plane. From this sheet of magnetic currents, you can obtain a far-field radiation pattern.
Note that the problem used to find the sheet of equivalent currents is not exactly the problem used to compute the radiation. As a result, errors in the problem solution can result from these differences. You can minimize these errors by properly selecting the enclosure size and the location of the free space boundary or boundaries.
The first type of boundary is a resistive boundary. You can use a resistive material of 377 ohms per square to provide an approximation to the free-space boundary. The 377 ohms is an approximation because the boundary would only have an impedance of 377 ohms at normal incidence and without the presence of the side-walls. A problem that can arise when using this type of boundary condition involves the absorption of power from the near fields of the antenna. This occurs when the resistive boundary is located too close to the radiating structure, artificially absorbing the stored energy of the structure. Nevertheless, the use of the 377 ohm boundary condition seems to give reasonable results when it located an appropriate distance from the radiating conductors. To test that this boundary is not absorbing stored energy, you should conduct two simulations with the boundary located at slightly different (for example λ/10) distances from the radiating structure. If no significant impact is seen in the S-parameters of the structure, then you can assume that the boundary is not absorbing substantial amounts of stored energy.
The second type of boundary is the boundary condition that you would see if the side-walls extended to infinity. This boundary condition is equivalent to the boundary seen looking into an infinitely long waveguide.
What is important for getting an accurate radiation pattern is that the computed tangential E-field at the top of the enclosure looks as much like the E field of an equivalent problem radiating into free-space. The infinite waveguide termination provides a reasonable approximation for the tangential E-field as long as the boundary is not too far from the radiation element. The tangential E-field far from the radiating element always tends to the field pattern of the dominant waveguide modes as the distance between the enclosure top and the radiator increases. When the radiator is far enough away, you always obtain the radiation pattern of an open-ended rectangular waveguide when using the infinite waveguide termination.
Since the EM simulator solves for the fields inside a conductive box, several assumptions are made that allow for the computation of the radiation pattern. One of these assumptions is that the side-walls of the enclosure are far enough away that they do not have a significant effect on the electric field on the top boundary of the enclosure. You should always view the electric field on the top of the boundary when working with antennas. This allows a quick check on the validity of this assumption. If the electric field has a very low magnitude near the edges of the enclosure, then the assumption is valid. If the electric field is relatively high near the edges, then the fields are interacting with the side-walls and the assumption is not valid.
The second part of the solution involves the determination of the radiation pattern from the tangential E-field present on the top surface of the enclosure. Using the equivalence theorem and the image theorem, you can represent the radiation problem as a sheet of magnetic current that is infinitely close to a perfectly conducting half plane. From this sheet of magnetic currents, you can obtain a far field radiation pattern. Again, note that the problem used to find the sheet of magnetic currents is not exactly equivalent to the problem used to compute the radiation. As a result, difficulties arise in forcing conservation of power, so the far-field radiation patterns are normalized to an average radiated power which is determined via an integration of all of the power radiated in the upper hemisphere. The normalization does not account for mismatch or resistive losses and thus results in a polarization sensitive directivity for the antenna.
Unfortunately, while the S-parameters of the structure reveal the mismatch losses of the antenna, the resistive losses associated with the antenna cannot be determined due to the previously mentioned lack of conservation of power due to the imposed boundary condition. For antennas constructed with perfect conductors, the radiated power equals the power into the structure (easily computed from the S-parameters). If you want to compute the ohmic or dielectric loss of an antenna, two problems should be solved. One of the problems should use a PEC radiator (and no dielectric loss) and the other should use the lossy conductor and/or lossy dielectric that the true antenna uses. You can use the difference between the radiated power in the two cases to estimate the ohmic or dielectric losses in the antenna.
Two coordinate systems are used in an EM antenna simulation, one for drawing the structure and another for the radiation patterns. The second coordinate system is conforms to the standard coordinate system used in antenna analysis.
The coordinate system for the antenna measurements is shown in Figure A.1, “3D View of Coordinate System Used For Antenna Measurements”. This system is a right-hand coordinate system with the origin located at the center of the top of the enclosure. When viewing a two-dimensional image, the y-axis of the antenna coordinate system extends upward, the x-axis extends to the right, and the z-axis extends out of the image toward the viewer.
The antenna coordinate system is in contrast to the coordinate system used to draw structures in the Microwave Office program. The drawing coordinate system is a Left Hand Coordinate system with its origin located in the upper left-hand corner of the Microwave Office enclosure as viewed in a two-dimensional view of an EM simulation. Figure A.2, “2D View of Structure Showing Antenna and Drawing Coordinates ” contrasts these two coordinate system in a two-dimensional view.
Physically, an antenna radiates energy at all frequencies in all directions simultaneously. To visualize the radiation, measurements that fix all but one of the independent parameters (Freq, θ and φ) must be implemented to allow a two-dimensional plot. Further, the phase and magnitude of the radiation is affected by the polarization of antenna used to measure the antenna under test. For this reason, you can make three basic types of antenna measurements that fix all but one of the independent axes. Further, each of these measurements can be performed for five common polarizations.
The following are the antenna measurements types:
Principal Plane Cut (PPC): Also known as a Theta or an Elevation Cut, this antenna measurement type fixes the values of Frequency and φ to user-specified values. Theta is then swept to cover an entire sweep of the upper hemisphere (-90 to 90 degs or -π/2 to π/2 rads) if there is an infinite ground plane below the antenna, or to cover an entire sweep of the lower hemisphere (90 to 270 degs or π/2 to 3π/2 rads) if there is an infinite ground plane above the antenna, or from -180 to 180 (-π to π radians) if there is not an infinite ground plane. An example of a Principal Plane Cut is shown in Figure A.3, “Example of a Principal Plane Cut”.
Conic Cut (CON): Also known as a Phi or Azimuth Cut, this antenna measurement type fixes the values of Frequency and θ to user-specified values. Phi is then swept to cover an entire sweep of the upper hemisphere (-180 to 180 degs or -π to π rads). An example of a Conic Cut is shown in Figure A.4, “Example of a Conic Cut”.
Swept Frequency (SF): This antenna measurement type fixes the values of φ and θ to user-specified values. Frequency is then swept over a user-defined range.
The following are the antenna measurement polarizations:
E-Phi (E_{φ}): This represents signals received or transmitted by the test antenna if it is linearly polarized with its E-field aligned with the unit vector dφ in the previously mentioned antenna coordinate system. Importantly, the positive direction of dφ is in the increasing direction of φ. You should notice the dependence of dφ on the current value of φ and θ.
E-Theta (E_{θ}): This represents signals received or transmitted by the test antenna if it is linearly polarized with its E-field aligned with the unit vector dθ in the previously mentioned antenna coordinate system. Importantly, the positive direction of dθ is in the increasing direction of θ. You should notice the dependence of dθ on the current value of φ and θ.
Right-Hand Circular Polarization (RHCP): This polarization is a linear combination of E_{θ} and E_{φ}; it is defined as: RHCP=(E_{θ}+jE_{φ})/√2
Left-Hand Circular Polarization (LHCP): This polarization is a linear combination of E_{θ} and E_{φ}; it is defined as: LHCP=(E_{θ}-jE_{φ})/√2
Total Power (TPwr): Although this is not strictly a polarization, it is a very useful measure. TPwr represents the total power available regardless of polarization, and is obtained by summing the powers available from E_{θ} and E_{φ}. This measurement is purely real and does not have a phase associated with it.
Actually, antenna measurements represent the square root of the partial directivity in the specified direction that retain the phase of the corresponding electric field component (barring total power measurements that represent the square root of total directivity in the specified direction).
Two options are available for radiation pattern analysis:
Setting the top boundary of the enclosure to the impedance boundary condition (Approximate Open)
Setting the top boundary of the enclosure to an Infinite Waveguide termination.
Since the EM simulator solves for the fields inside a conducting box, several assumptions are made that allow for the computation of the radiation pattern. One of these assumptions is that the side-walls of the enclosure are far enough away that they do not have a significant affect on the electric field on the top boundary of the enclosure. It is best to view the electric field on the top boundary after solving when working with antennas. This allows a quick check of the validity of this assumption. If the electric field has a very low magnitude near the edges of the enclosure, the assumption is valid. If the electric field is relatively high near the edges, then the fields are interacting with the side-walls and the assumption is not valid.
If an impedance boundary condition (such as an approximate open) is used to terminate the enclosure above an antenna, it is possible for the boundary to be close enough to interact with the near field (read: stored energy) of the antenna, thus resistively loading the antenna and causing significant undesired changes. This undesired effect occurs when the top of the enclosure is too close to the antenna surface.
Moving the top of the enclosure away from the antenna reduces the resistive loading, but exposes more of the metallic side-walls for reflections. Although the input impedance of the antenna has stabilized, you are now sampling the field for re-radiation much further from the antenna. In this region, the interactions with the side-walls is converting the radiated fields into the modes of the waveguide.
Elevation of the enclosure top above the upper layer of dielectric stack may be crucial for obtaining correct results. You should select this height equal to approximately one quarter of the wavelength at the central frequency of operation. Control of the electric field on the top boundary may help to validate your choice. If the enclosure top is too close to radiating elements, distribution of the electric field displays dips just above the radiator locations. If the enclosure top is too far, distribution of the electric field develops pronounced oscillations from the center to the edges; whereas a reasonable selection of enclosure height provides distribution with a smooth slope towards all edges.
A better approach is to sample the fields very close to the antenna surface without resistively loading the structure with an impedance boundary condition. You can do so by replacing the surface impedance boundary condition with an infinite waveguide termination. This type of boundary condition does not resistively load the near field of the antenna. Since you are sampling the electric fields very close to the antenna, they have minimal corruption due to side-wall locations.
Unfortunately, antennas that direct significant amounts of energy toward the horizon still have significant degradation of the sampled electric field due to side-wall reflections.
The following sections include information on calculating antenna far-field radiation patterns, directivity, and gain.
Conic Cut or Phi Sweep (2D plot with
specified constant value of θ and φ swept from -180 to 180
degrees): Use Con_EPhi or Con_ETheta to plot the normalized
radiation pattern of Eφ or Eθ components of the E-field in the far
zone correspondingly.
Principal Plane
Cut or Theta Sweep (2D plot with specified constant value of
φ and θ swept from -90 to 90 if there is an infinite ground plane
below the antenna, or from 90 to 180 if there is an infinite ground plane
above the antenna, or from -180 to 180 if there is not an infinite ground
plane): Use PPC_EPhi
or PPC_ETheta to plot the normalized radiation pattern of Eφ
or Eθ components of the E-field in the far zone
correspondingly.
Directivity: Use SF_TPwr to
calculate the antenna directivity in a given direction (defined by specified
values of θ and φ).
Partial
directivity of an antenna for a given polarization: Use
SF_EPhi or
SF_ETheta
correspondingly for Eφ or Eθ to calculate the partial antenna
directivity in a given direction (defined by specified values of θ and
φ).
NOTE: The
Include Resistive Losses and Include
Reflection/Coupling Losses options are not selected.
Use SF_TPwr to calculate the antenna gain in a given direction (defined by specified values of θ and φ). Ensure that you select the Include Resistive Losses option.
This section illustrates the methods you can use to perform noise and nonlinear simulations when the operating temperature needs to be accounted for, and discusses how to create projects that use temperature as a variable in Microwave Office simulations, including:
A brief discussion of how the built-in variables _TEMP and _TEMPK are used
A description of how component models use temperature for simulation
Temperature controls the noise generation processes and the static operating point of nonlinear components and their dynamic behavior. With the necessary models for these components, it is possible to calculate the DC operating point, noise figure, and both AC small and large signal properties of components as a function of temperature.
The NI AWR Design Environment software uses two built-in variables _TEMP and _TEMPK, and functions such as ctok(x) and ktoc(x) to assist designers in projects to perform temperature sensitive simulations. _TEMP is a built-in variable in the NI AWR Design Environment suite intended for models that have a specific temperature parameter. _TEMP uses the units specified as global units (choose Options > Project Options and click the Global Units tab to select degree Kelvin, degree Celsius, or degree Fahrenheit as the global units. You can overwrite the default value of this variable using an equation; for example the equation "_TEMP = 30" sets this global variable to 30 degrees Celsius if these are the set units. _TEMPK is in degrees Kelvin and retains these units regardless of the global units setting. This variable is used to adjust the temperature for models without a temperature parameter. This variable only affects noise simulation of linear elements.
You can use both _TEMP and _TEMPK in equations to define the operating temperature of components. You can use equations to tie both linear and nonlinear temperature to the same value, and to assign one temperature value to all elements through hierarchy. Also, you can assign different temperatures to passive circuits, small signal amplifiers, Power Amplifier drivers and Power Amplifiers, with a global temperature used to define the base-plate or housing temperature, and equations added to define the unique temperatures of the high temperature components using dissipation and thermal resistance calculations.
You can view the current value of any variable with the
"variable:"
notation. To return or expose the value of _TEMP,
create the following equation in the Global Definitions window or any schematic
window: "_TEMP:" and then simulate. The variable _TEMP is set to 25 and interpreted
as 25 degrees Celsius. Now change the global units for temperature to degree Kelvin
and resimulate. _TEMP is set to 298.1 degrees Kelvin. As previously explained, you
can define the value of _TEMP by using the equation "_TEMP = 30". To see the default
value, overwrite this value with a user-specified value, and confirm the new value,
create the following equations:
_TEMP:
_TEMP=30
_TEMP:
and simulate. The value of _TEMPK always returns the current value in degrees Kelvin. If no value is explicitly set, the value is 290 degrees Kelvin.
How these components use the built-in variables for temperature and derived temperatures depends upon the origin of the model parameters for the component. There are four different situations when setting temperature in simulation:
passive elements
nonlinear elements without _TEMP assigned
nonlinear elements with _TEMP assigned
netlists.
The NI AWR Design Environment suite supports both implicit and explicit methods when using temperature in simulations. The implicit method uses the built-in variable _TEMPK; the use of this approach is illustrated in the following figure. The schematic consists of an attenuator whose shunt and series elements are designed using the standard equations for a PI attenuator. This particular building block is chosen for this example because the NF equals the insertion loss when the physical temperature of a matched attenuator is set to the reference temperature. Here you can see that the resistors responsible for loss and noise generation do not have an explicit temperature defined. The built-in global variable _TEMPK controls the temperature of all such elements that possess loss, and therefore can generate noise.
The simulation uses a local copy of the built-in variable _TEMPK which is controlled by the Swept Variable (SWPVAR) element. The temperature is swept between 0 and 400 degrees K. The X axis of the graph is set to use the sweep variable, _TEMPK. See “Swept Variable Control: SWPVAR” for more information about SWPVAR.
When a specific temperature of an element needs to be defined other than that
defined by the built-in global variable _TEMPK, you can create local variables and
use elements with an explicit temperature parameter. In the following schematic the
REST element is used in place of the RES element. The REST element has a parameter
for the temperature of the resistor. The localTemp
variable is used
to control the temperature of the element and uses the global units setting, which
in this example is in degrees Celsius. Since the sweep is still in degrees Kelvin, a
conversion is used for the temperature setting for each resistor,
T=ktoc(localTemp)
. The ktoc
function converts
from Kelvin to Celsius. Note that you can use the built-in _TEMP variable, or
alternatively, you can not use the ktoc conversion and sweep the
localTemp
variable in degrees Celsius instead of degrees
Kelvin. In every other respect, this design is identical to the previous design. The
simulation results for these schematics are identical.
For passive devices defined by port parameter data files, like S-parameters, use the NPORT_F or NPORT_F_MDIF element, which has a secondary parameter for setting its temperature. SUBCKT blocks that refer to passive port parameter data files use the global _TEMPK setting, which you can change in the Global Definitions document. (Note that the Default Linear simulator overrides the global setting if the schematic in which the SUBCKT block is placed has an equation that sets _TEMPK;. The APLAC Linear simulator only uses the global setting.)
EM structures have schematics in which their individual _TEMPK can be specified using an equation, as previously described.
The principle of defining the temperature of circuit elements can be extended to active devices. The following is a schematic for a bipolar amplifier used later in the system noise figure calculations. The device is modeled using the nonlinear model and several elements to define the package parasitics. The schematic that defines the device model is shown following the test schematic. The top level schematic has _TEMP defined as a variable, and then the swept variable block is used to sweep the temperature from -270 to 100 degrees C in steps of 10 degrees C. The variable is set to be passed down through hierarchy designated by the solid red line surrounding the variable. (You can toggle this setting by using the Tune Tool and holding down the Shift key).
The following schematic defines the transistor parasitic elements.
The following is the transistor model. The _TEMP variable replaces the default value of the device temperature (TEMP = _TEMP).
The assignment of the temperature displays (it is hidden by default) by changing the display options of the parameter on the Display tab of the Element Options dialog box. You can change the default (hidden) by clearing the Default column check box as shown in the following figure.
Many of the device models for Monolithic Microwave Integrated Circuit (MMIC), RFIC and hybrid circuit design use this form when defining temperature. The model variable TEMP is the universal variable used by models within SPICE and other EDA simulations.
The NI AWR Design Environment suite supports the simulation of linearized noise figure, whereby the temperature and bias point dependent operating point is calculated before the small signal noise properties are calculated. The following graph shows the noise and gain for the previous transistor circuit.
In this example, the Gummel-Poon model is used from the NI AWR Design Environment Element Browser under Nonlinear > BJT category. The appropriate model parameters are entered to model this part and _TEMP is assigned to the TEMP parameter. In the PDKs available for NI AWR, the temperature parameter is set to _TEMP by default.
In this example you can set the temperature to any variable name. NI AWR recommends that you use the _TEMP variable to maintain consistency between designs. If you want to assign different temperatures to different elements in the design, you should set a different variable name, however.
Often the device model is found from a component manufacturer's web site in the form of a SPICE compliant netlist. The following netlist was imported into the NI AWR Design Environment suite. Note that on import, the syntax of the file is modified to conform to the NI AWR Design Environment netlist standard. The netlist contains both a circuit description of the transistor and an inline device model section with the normal BJT parameters. In SPICE syntax, the units are always assumed to be in base units (Farads, Amps, Henrys, etc). The base unit for temperature in SPICE is Celsius. The units for each type of variable are shown as follows.
.subckt qNE52418_v161 c b e s *---- Intrinsic NPN Model --------------------------------- q1 c b e s qmod .model qmod npn + level= 3 afn= 3.2 + ajc= -0.5 aje= -0.5 + ajs= -0.5 avc1= 3 + avc2= 200 bfn= 1 + cbco= 5.46E-15 cbeo= 8.34E-15 + cjc= 4.62E-15 cjcp= 2.64E-14 + cje= 3.78E-14 cjep= 1.04E-14 + cth= 3.26E-10 ea= 1.133 + eaic= 1.133 eaie= 1.133 + eais= 1.133 eanc= 1.133 + eane= 1.133 eans= 1.133 + fc= 0.95 gamm= 1.50E-11 + hrcf= 1 ibci= 8.22E-20 + ibcip= 0 ibcn= 7.37E-15 + ibcnp= 0 ibei= 1.77E-19 + ibeip= 2.49E-18 iben= 1.10E-15 + ibenp= 0 ikf= 2.51E-02 + ikp= 9.96E-02 ikr= 5.90E-03 + is= 2.87E-17 isp= 1.99E-19 + itf= 6.59E-02 kfn= 1.96E-09 + mc= 0.18 me= 0.2 + ms= 0.47 nci= 1.002 + ncip= 1.005 ncn= 1.5 + ncnp= 1.9 nei= 1.02 + nen= 1.9 nf= 1.015 + nfp= 1 nr= 1.01 + pc= 0.86 pe= 0.92 + ps= 0.55 qco= 1.47E-16 + qtf= 0 rbi= 3.4088 + rbp= 1 rbx= 13.111 + rci= 316.11 rcx= 0 + re= 0.68275 rs= 50 + rth= 644.03 tavc= 8.50E-04 + td= 9.17E-13 tf= 1.17E-12 + tnf= 5.00E-05 tr= 2.50E-11 + tref= 25 vef= 90 + ver= 2.25 vo= 100 + vtf= 0.3 wbe= 1 + wsp= 1 xii= 3 + xin= 2.2 xis= 1.9 + xrb= 0 xrc= 0 + xre= 0 xrs= 0 + xtf= 10 xvo= 0 .ends qNE52418_v161
Typically, the model does not explicitly define the temperature of the device. The
SPICE standard temperature variable is dtemp
. You must add this to
the netlist to simulate at temperatures other than the default. Also, to enable this
variable to pass into the netlist from the parent schematic that owns the netlist,
you must add an additional equation to the line that specifies the element node
numbers.
.subckt qNE52418_v161 c b e s DeviceTemp=1 *---- Intrinsic NPN Model --------------------------------- q1 c b e s qmod dtemp=DeviceTemp .model qmod npn + level= 3 afn= 3.2 + ajc= -0.5 aje= -0.5 + ajs= -0.5 avc1= 3 + avc2= 200 bfn= 1 + cbco= 5.46E-15 cbeo= 8.34E-15 + cjc= 4.62E-15 cjcp= 2.64E-14 + cje= 3.78E-14 cjep= 1.04E-14 + cth= 3.26E-10 ea= 1.133 + eaic= 1.133 eaie= 1.133 + eais= 1.133 eanc= 1.133 + eane= 1.133 eans= 1.133 + fc= 0.95 gamm= 1.50E-11 + hrcf= 1 ibci= 8.22E-20 + ibcip= 0 ibcn= 7.37E-15 + ibcnp= 0 ibei= 1.77E-19 + ibeip= 2.49E-18 iben= 1.10E-15 + ibenp= 0 ikf= 2.51E-02 + ikp= 9.96E-02 ikr= 5.90E-03 + is= 2.87E-17 isp= 1.99E-19 + itf= 6.59E-02 kfn= 1.96E-09 + mc= 0.18 me= 0.2 + ms= 0.47 nci= 1.002 + ncip= 1.005 ncn= 1.5 + ncnp= 1.9 nei= 1.02 + nen= 1.9 nf= 1.015 + nfp= 1 nr= 1.01 + pc= 0.86 pe= 0.92 + ps= 0.55 qco= 1.47E-16 + qtf= 0 rbi= 3.4088 + rbp= 1 rbx= 13.111 + rci= 316.11 rcx= 0 + re= 0.68275 rs= 50 + rth= 644.03 tavc= 8.50E-04 + td= 9.17E-13 tf= 1.17E-12 + tnf= 5.00E-05 tr= 2.50E-11 + tref= 25 vef= 90 + ver= 2.25 vo= 100 + vtf= 0.3 wbe= 1 + wsp= 1 xii= 3 + xin= 2.2 xis= 1.9 + xrb= 0 xrc= 0 + xre= 0 xrs= 0 + xtf= 10 xvo= 0 .ends qNE52418_v161
The transistor is defined by a subcircuit (a netlist in this example) and the deviceTemp variable has in turn been equated to a _TEMP variable.
The following graph shows the results of the gain and NF simulations.
In this case, the project units for temperature are degrees C so assigning _TEMP to the deviceTemp parameter set the correct temperature in the netlist. If the project units for temperature are other than degrees C, the temperature passed to the netlist must be converted to Celsius. For example, the same results can be achieved when the global unit for temperature is set to degrees K with the schematic as follows. This schematic is shown in the following figure.
The differences to note are that the swept values are now from 73 to 313 in steps
of 20 since the units are degrees K. The deviceTemp value passed to the netlist is
now converted to degrees C using the ktoc function. So deviceTemp =
ktoc(_TEMP)
converts _TEMP from Kelvin to Celsius before the value is
passed to the netlist.
Again, you can use any variable value to pass temperature, however you should use _TEMP to maintain consistency between designs.
In IC design, the temperature of each component is normally set to the same value. In this situation, each nonlinear model typically has its explicit temperature set to _TEMP in the PDK model set. The best approach is to assign the temperature at the top level schematic and pass the values down through the hierarchy. Assign _TEMP and _TEMPK to use the same swept values. Because _TEMP uses the temperature units set for the project and _TEMPK is always in Kelvin, built-in equations are used to make the two temperatures the same.
In this example, the unit for temperature is set to degrees Celsius. In the top level schematic, the value for _TEMP is set to sweep its value and pass down its value using the SWPVAR block _TEMP variable. Again, the global temperature unit is Celsius so the swept values are in Celsius. _TEMPK is assigned to follow the _TEMP value, but you must use the "_TEMPK = ctok(_TEMP)" equation to convert it from degrees Celsius to degrees Kelvin. Note that the temperature conversion depends on the global unit setting for temperature.
The following schematic shows the lower level in the hierarchy where a resistor is added at the input to show the effects of _TEMPK.
The following graph shows the swept Noise Figure versus temperature.
Note that different results are achieved if the different temperature settings are not passed down through the hierarchy. When neither _TEMP nor _TEMPK are passed down, the result is shown on the following graph.
The noise figure is flat because the swept temperature is not passed, and so the default values of 25 degrees C for _TEMP and 290 degrees for _TEMPK are used in simulation.
When just _TEMP is passed through hierarchy, the result is shown on the following graph.
When just _TEMPK is passed through hierarchy, the result is shown on the following graph.
When sharing designs between different designers or different projects in the NI AWR Design Environment suite, units can be an issue. If you do not use any variables in a design, there are no issues. However, variables do not use unit scaling and so it is possible for designs to be passed between NI AWR projects that are not identical. The following are some techniques to address this issue:
Set up a common set of global units to use in all projects.
Agree to use base units for all projects.
Agree to select the Dependent parameters use base units check box on the Schematics/Diagrams tab of the Project Options dialog box prior to doing any design.
The following example demonstrates. Assume a designer uses capacitance units of nF and a variable assigned to a capacitance of 0.01. If this schematic is exported and then imported to a project with units of pF, the software does not know how to scale the value of a variable (variables can be combination of equations, etc. so this cannot be done in a general sense). When this schematic is imported the variable still has a value of 0.01. However, now that units are pF, the value is off by three orders of magnitude. Using base units for dependent parameters (Farads) in this example allows for easy design sharing.
You can set Dependent parameters use base units globally by
choosing and clicking the
Schematics/Diagrams tab, or you can set it locally for each
schematic. This option is not set by default
. This setting sets
any parameter using a variable value to base units. Base units are any unit type
without a modifier, such as Farads, Henrys, and Amps, instead of the specified units
in the global units setting. When designers share designs, the software does not
know what the global units setting are in the original design. Always using base
units for any parameter using a variable ensures that values are set appropriately
any time a design is shared.
If you use the Dependent parameters use base units setting, the units for temperature display as degrees Kelvin, and you should sweep temperature values in Kelvin. If using a hierarchical design, you should make this setting for the entire project, if not you need to make the setting for any schematic in the hierarchy with a temperature setting. If using this setting in this example, _TEMP is always in degrees Kelvin and should use those values to sweep. This setting also keeps _TEMP and _TEMPK in the same units and no conversion is necessary.
To demonstrate the Dependent parameters use base units option, the linear simulation is repeated with the explicit temperature model. However, now this option is set locally (right-click on the schematic in the Project Browser, (choose and click the Schematic tab), overriding the default setting. Now the temperature units display in base units and the equation to convert from Celsius to Kelvin is not required. Again, the simulation results are identical.
By default, the Microwave Office program assumes that you design in a 50 ohm system. Microwave Office software is not limited to 50 ohm systems, however, and changing the characteristic impedance of your design is easy. The following sections discuss how to operate in a non 50 ohm system.
When working in a schematic in the NI AWR Design Environment suite, the impedance specified on the ports determines the characteristic impedance of that system. To change the impedance parameter you can either double-click the Z parameter or right-click the port and choose Properties, then change the Z parameter in the Element Options dialog box.
You can generate output files in various formats. See “Working with Output Files ” for more information about generating output files. When creating these files, you must set the reference impedance to match the system impedance of the structure that it represents. If the reference impedance is not set correctly, there are unexpected results. See “Generate Touchstone, MDIF, or MATLAB File: NPORTF” for details on setting up this output file, particularly the Ref. Impedance setting.
The Ref. impedance sets the characteristic impedance of the circuit and overrides the impedance set by the ports in the structure that is simulated. For example, if the ports in the schematic are set to 75 ohms, but the reference impedance is set to 50 ohms, the results are based on a 50 ohm characteristic impedance, not 75 ohms. This is equivalent to changing the port impedance in your schematic to 50 ohms rather than 75.
In the Microwave Office program, you can plot Port Parameters measurements directly from data files if the impedance specified in the file is normalized to the default characteristic impedance, 50 ohms. If the data file is normalized to a different impedance, you must place it in a schematic as a subcircuit, where the ports are set to the corresponding impedance of the data file. See “Adding Subcircuits to a Schematic or System Diagram ” for information on using a data file as a subcircuit in a schematic. When plotting directly from a data file, the characteristic impedance is always 50 ohms.
For example, if you have an S-parameter file normalized to 75 ohms for use in a 75 ohm system, plotting a measurement directly from this file is equivalent to placing it in a schematic with a 50 ohm characteristic impedance (50 ohm ports) and making the measurement. To achieve the desired measurements, you must place the data file in a schematic with 75 ohm ports and make the measurements from this schematic, not the data file directly.
If EM analysis is required in your design and the characteristic impedance of the EM structure is not 50 ohms, plotting Port Parameters measurements directly from the EM structure yields seemingly incorrect behavior. Plotting directly from an EM structure, like plotting directly from a data file, sets the characteristic impedance to 50 ohms. Although you can set the termination impedance for each port in the EM structure, these are not used when calculating the port parameters, but are instead used for computing the currents in the structure. See “Setting the Port Excitation or Termination” for more information.
To set the characteristic impedance for an EM structure to something other than 50 ohms for Port Parameters measurements, you can place the EM structure as a subcircuit in a schematic and change the impedance of the ports to the desired impedance.
Load pull analysis in Microwave Office software is simple when using the NI AWR Load Pull Script. See “Load Pull Script” for more information on using this script to perform a load pull analysis. Performing load pull on a non 50 ohm system only requires a few extra steps.
Set the system impedance for the schematic by changing the impedance of all the ports used in the schematic to the new characteristic impedance. See “Setting the Characteristic Impedance of a Schematic” for information on how to make these changes.
Set the System Impedance parameter (Z0) on the load pull tuner you are using (for example, LTUNER, LPTUNER, or HBTUNER). To change the system impedance parameter you can either double-click the Z0 parameter or right-click the tuner, choose Properties, and change the Z0 parameter in the Element Options Dialog Box.
Generally, when you view port parameters on a Smith Chart they are normalized to a specific impedance. You can, however, view the un-normalized impedances directly on the Smith Chart. To change this option, right-click on the graph and choose Properties to display the Smith Chart Properties dialog box. Click the Markers tab and change the Z or Y display from Normalized to Denormalized to. By default, the normalization impedance is set to 50 ohms. For the impedances to be correct, it is important to change this to the characteristic impedance of your system.
^{[3] }A. Platzker, W. Struble, and K. Hetzler, “Instabilities Diagnosis and the Role of K in the Microwave Circuits,” IEEE MTT-S International Microwave Symposium Digest, pp. 1185–1188, 1993.
^{[4] }Wang, K., Jones, M., Nelson, S., "The S-Probe. A New, Cost-Effective, 4-Gamma Method for Evaluating Multi-Stage Amplifier Stability", IEEE MTT-Symposium Digest,1992, p. 829-832.
^{[5] }Truxal, J. "Introductory Systems Engineering", McGraw Hill, 1972.
^{[6] }C. A. Balanis, Antenna Theory Analysis and Design (2nd Edition), John Wiley & Sons, Inc.,1997.
Please send email to awr.support@ni.com if you would like to provide feedback on this article. Please make sure to include the article link in the email.