Intusoft Newsletter Issue #56, June 1999
Copyright ©2002 Intusoft, All Rights Reserved

In This Issue
1	Why You Need ICAP/4: Managing Simulation Results	5	Modeling Op-amps Pspice©; Parts™ vs Intusoft
2	Using SPICE More Effectively: Impedance Measurements	6	Modeling Motors and Motion Control Systems
3	Download ICAP/4Rx	7	New Magnetics Designer Released
4	SPICE Model Web Links

Managing Simulation

With the release of version 8.x.6, the feature set of our ICAP/4 product line was substantially increased (www.intusoft.com/ver8x6.htm). Virtually all of the new features are unique innova-tions. In fact, they are unlikely to ever be present in other SPICE programs for the following reason. Other SPICE simulators have never adopted a scripting methodolgy that can extract data from their simulator. Oddly enough, scripting is a standard Berkeley Spice 3 feature. The ability to run SPICE and process the results using a scripting language is extremely powerful and allows you to better manage the simulation results.

Other SPICE packages, such as OrCAD©; PSpice©;, require the user to manage simulation results apart from the software. The results must be transferred somewhere (for example, to a spreadsheet) and the user is responsible for managing the schematic/output file/waveform relationships. During the design process, hundreds of “what-if” cases are run in order to perfect circuit performance. These cases will be run using many different circuit, analysis and stimulus configurations, thereby causing an insurmountable bookkeeping problem. OrCAD PSpice has essentially abandoned its users in this regard. As the circuit topology and parameter values are tuned, the previous simulation results can’t be easily updated. In fact, it is so difficult using PSpice to do this, it is unlikely to get done at all.

Intusoft is leading the way with Configurable Schematics and “Simulation Templates”, enabling technologies for true worst case analysis. Note that although the entire process described here is script driven, the user DOES NOT have to write any scripts. All of the operations are graphically setup.

In ICAP/4, the user may capture as many circuit variations as desired (Figure 1). By using schematic layers, it is simple to make and store schematic variations. These variations could be completely different circuits, or a single circuit with different modifications (i.e. component values, tolerances, loads, start-up transients, stimuli, etc.). The variations are all stored in the same schematic database. You can assign measurements to each circuit configuration (Figure 2). The measurement type and circuit quantity (node voltage, current, or power dissipation) are chosen from a dialog. There are no limits to the number of nodes or types of measurements which you can assign. For example, finding the peak-peak or maximum value of every node in the circuit is a trivial matter (Figure 3).

Limits can easily be assigned to each measurement in order to form a baseline for design performance. What-if changes of any circuit variable can then be assessed against the baseline values (Figure 4). Limits can be set directly or through simulation, Monte Carlo analysis, or worst case analysis. Each circuit variation, along with its assigned measurements and limits, are stored along with the schematic and are conveniently viewable, printable and transferable to other tools (i.e. MS Excel, Word, etc.) The example in Figure 1 shows two different circuit variations, each with different simuli. Any configuration can be selected and simulated at any time. Figure 2 shows the measurements assigned to each configuration. Performing the 50+ measurements over the 6 circuit configurations with any other SPICE program would be tedious at best. Each waveform would have to be displayed in a post processor, cursors would have to be moved, and measurements would have to be stored in a separate program. With ICAP/4, simply select the circuit configuration(s) to simulate, and the entire set of measurements are automatically recorded. The results, displayed against the baseline, are shown in the Results dialog, Figure 4. A meter bar quickly shows which measurements are out of tolerance. The ability to store the state of a “golden” or baseline design protects against unanticipated changes that could be detrimental.

In the next issue of the newsletter, we will explore how you can set Stress Alarms on any of the measurements. Try to perform the previous global circuit measurements with your SPICE program!

Why is this feature important? ICAP/4 runs an entire suite of tests automatically and creates a report that summarizes the results and pass-fail grades. This powerful capability extends SPICE well beyond its current single simulation oriented boundaries.

References
[1] “New Techniques for Failure Analysis and Test Program Design”, C.E. Hymowitz, Intusoft, http://www.intusoft.com/tech.htm
[2] “New Techniques for Failure Analysis and Test Program Design”, L.G. Meares, Evaluation Engineering Magazine, April/May issues 1998

BACK TO THE TOP

One of the more common measurements you may want to make is that of a network’s impedance. With impedance equal to voltage divided by current the tendency is to drive the circuit with a voltage source. Then, when the simulation is complete, you could display the voltage and current waveforms in the IntuScope post processor and divide the waveforms to get the impedance curve. Although this is possible, it’s not the most efficient method.

A more simple approach is to replace the voltage source carrying the AC stimulus (AC 1) with a current source. In the post processor, the displayed nodal waveforms are voltages. However, since the input from the current source has a magnitude of 1 (AC=1) and impedance = Vout/Iin, then the voltage waveform (magnitude) corresponds to the impedance versus frequency without any additional manipulations. The circuit in Figure 5 illustrates the impedance curve of a capacitor which has parasitics. The impedance of a more complex high voltage booster amplifier is shown in Figure 6.

The .TF Transfer function analysis returns the small signal DC input and output impedance at any point in the circuit, plus the DC gain from any source to any node. It’s a convenient way of finding DC impedance and gain. The results are reported in the IsSpice4 text output file (Figure 6). To perform the analysis, you must specifiy an input source and an output node. The source can be an independent voltage or current source.

BACK TO THE TOP

The Intusoft website offers links to manufacturer’s web sites where SPICE models can be found. You can find the most current list at: www.intusoft.com/slinks.htm. ICAP/4 Windows Deluxe, ICAP/4 Professional and Test Designer users, or those who have our vendor supplied IC/op-amp models option should note that all of the models posted on vendor’s web sites are already in your system. As new models are posted on each vendor’s sites, Intusoft performs the integration work for you. Intusoft tracks the models, makes sure that they are compatible with the simulator, tests them, makes the schematic symbols, and posts the updated model library files on the Intusoft technical support web pages.

BACK TO THE TOP

SPICE does not have a generalized built-in op-amp model. Given the variations of the internal topologies of op-amp circuits, it’s no wonder. Op-amps are modeled using subcircuits (collections of elements) which can better account for the design variations. Op-amp topologies typically don’t emulate all characteristics; only a subset is supported. Op-amp vendors use different internal circuit topoliges and usually don’t provide much documentation. This makes it difficult to evaluate model performance.

One of the more common topolgies used by many op-amp vendors is the Boyle model. The first op-amp subcircuit is credited to G. Boyle [1] (Figure7). Boyle eliminated all but two transistors that formed the input differential stage. The rest of the op-amp is modeled using behavioral and passive elements. Though the Boyle topology achieves significant gains in simulation performance over transistor level topologies, it has many deficiencies. As shown in table 1, it has only 2 poles and its internal node voltages are referenced to ground. Therefore, simulation of many power supply topologies is impossible. The output current flows from a controlled source connected to ground rather than the power supplies. It does not model noise or temperature effects accurately, and its output impedance is not accurately represented. This is essentially the model topology which is used by the OrCAD©; PSpice©; Parts modeling tool. Several op-amp vendors also use this topology or a somewhat improved version.

The generic Intusoft op-amp model (Figure 8) is much more sophisticated and represents an excellent compromise between simulation performance and the op-amp characteristics which it emulates. See Sidebar.

References
G Boyle, B. Cohn, D. Pederson, Macromodeling of integrated circuits operational amplifiers, IEEE Journal of solid State Circuits, Vol. SC-9, No. 6 pp. 343-363, 12/74

Side Bar: Obtaining open loop gain and phase characteristics using a closed loop test. Making a stable bias for a circuit under test without designing a special bias network is a recurring problem. This problem was solved a number of years ago for power supplies, by a number of researchers including Dr. Middlebrook. A signal was inserted via a current probe, and vector {real, imaginary} measurements were made on each side of the probe. The loop gain and phase was then computed as follows: Vout(s)/Vin(s) = (ReVout + jImVout)/ (ReVin + jImVin) By converting to gain in dB and phase in Degrees, the respective quantities can simply be subtracted in order to obtain the desired result. This technique is naturally suited to Spice simulations via the use of a voltage source in place of the current probe. The results of this process are shown below (Figure 10). The phase goes through 360 degrees from DC to infinity, exposing the low frequency, primary stabilization pole and the less desirable high frequency effects.

BACK TO THE TOP

By Johan Scolliers, VTT Automation

Motion control systems consist of subsystems from different disciplines such as electrical, hydraulic, and mechanical. The extensive behavioral modeling capabilities, along with the ability to model each part at different levels of complexity, make IsSpice4 perfect for simulation of such Mechatronic systems.

The following example describes a cascade current-velocity-position control system (Figure 11). The desired position, j, is compared with the (sampled) feedback signal jS from an encoder, and sent through a limiting PI-controller (LPIC). The output is the desired voltage, which is compared with the return signal wS from a tachometer, and sent to a second LPIC, which calculates the desired motor current iD. The current signal is sent through a limiter (LIM), compared with the signal iS of a current sensor (CSEN), and sent through a third LPIC. The output, iA, of this LPIC is the control signal for the current controlled power amplifier. The power amplifier consists of a 1-phase full bridge diode rectifier which converts the AC net voltage to a DC voltage, and of a full bridge switch-mode converter, built from 4 MOSFETs. The algorithm which is used to control the MOSFET gates is hysteretic current control. The motor is a permanent magnet DC-motor. A flexible coupling with backlash connects the motor to the rotational load, which consists of inertia, damping and friction. Figure 12 shows the ICAP/4 schematic. Figure 13 shows parameter values used for key variables, along with the netlist for the DC motor model. The (current controlled) power amplifier is modeled on a behavioral level, i.e. as a first order system, with a limiter on the output voltage. For the idealized tachometer and encoder models, no mechanical parts have been used. The parameters of the PI-controllers have been optimized using classical control techniques. To determine the system control parameters, the system was linearized by making the friction in the motor zero, and by removing the backlash element.

Figure 14 shows the IntuScope simulation results for the load position and the load and motor velocity, for a step change input of the desired position. The oscillations in the load velocity are due to the flexibility between the motor and the load. Figure 16 shows the motor current and the motor voltage.

At the start of the simulation, the desired output motor current is very high. Due to the inductance of the motor, the current cannot immediately reach the desired value, and the output of the voltage is as high as allowed. As the motor current is increases rapidly, the input current ia for the amplifier decreases rapidly. After about 6 ms the (scaled) current ia becomes smaller than the actual motor current is. Since ia increases rather rapidly, the motor current cannot follow the desired current, and the motor voltage is as negative as possible. After 7 ms both currents are again approximately equal to each other, and a (temporary) equilibrium condition is achieved. In order to analyze the motor control more exactly, the behavioral model of the power amplifier can be replaced by an electric model of the amplifier.

[1] Johan Scholliers, Timo Yli-Pietila, The Modeling of Motion Control Systems With An Analog Circuit Simulator, 16th Intl. PCIM, 1995

BACK TO THE TOP

BACK TO THE TOP

Copyright ©2002 Intusoft, All Rights Reserved