Characterization of semiconductor devices in terms

of their technological and geometrical parameters is de-

scribed in this paper. This characterization is generated

by a software tool composed of the SPICE-PAC simula-

tion package and the symbolic simulator SYBILIN. The

paper discusses the general structure of the program,

its principle of operation, some implementation details,

and its computational efficiency. A characterization of

Heterojunction Bipolar Transistor (HBT) for microwave

applications is used as an illustration

Konczykowska, A.

Zuberek, W. M.

Memorial University Research Repository

European Design Automation Conference (EURO-DAC’90); Glasgow, UK, March 12-15, 1990, pp.2.6.1-4.Copyright c© 1990 IEEE (DOI 10.1109/EDAC.1990.136610).TEGESED, a tool for efficient technological and geometricalcharacterization of semiconductor devicesA. Konczykowska W.M. ZuberekCentre National d’Etudes des Telecommunications Department of Computer ScienceLaboratoire de Bagneux Memorial University92220 Bagneux, France St. John’s, NL, Canada A1C-5S7A b s t r a c tCharacterization of semiconductor devices in termsof their technological and geometrical parameters is de-scribed in this paper. This characterization is generatedby a software tool composed of the SPICE-PAC simula-tion package and the symbolic simulator SYBILIN. Thepaper discusses the general structure of the program,its principle of operation, some implementation details,and its computational efficiency. A characterization ofHeterojunction Bipolar Transistor (HBT) for microwaveapplications is used as an illustration.1. INTRODUCTIONA complete, detailed characterization of semiconduc-tor devices is of significant importance not only to cir-cuit designers, but also to all researchers interested inimproved or new technologies and manufacturing pro-cesses. This paper presents a software tool, TEGESED,that provides characterization of semiconductor devicesin terms of their technological and geometrical param-eters. Its basic feature is flexibility which is due to an“open” structure of the simulation package that consti-tutes the “backbone” of this tool.In order to illustrate TEGESED’s properties, one par-ticular example is presented in greater detail. It is acharacterization of transistors in the frequency domain,as required in microwave applications. The programis composed of two computer-aided analysis tools, theSPICE-PAC simulation package [12] which is used fornonlinear and time-domain analyses, and the SYBILINsymbolic simulator [7,8] for (linear) frequency-domainanalyses. SPICE-PAC has been chosen because of itsmodular form and very flexible interfacing capabilities,while SYBILIN because of its efficient implementationof repetitive AC analyses. A brief description of SPICE-PAC and a short discussion of symbolic simulation arepresented in the next sections, and are followed by anoutline of the TEGESED’s structure as well as a practicstudy of Heterojunction Bipolar Transistor characteri-zation.2. SPICE-PACSPICE-PAC is a simulation package that is upwardcompatible with the popular SPICE simulator [3,9,11].It means that SPICE-PAC accepts the same circuit de-scription language as SPICE (with a few minor excep-tions) and provides the same set of circuit analyses, butit also supports a number of new features, not availablein the original SPICE simulators. Examples of theseextensions include:• a uniform hierarchic naming scheme for all levelsof subcircuits; subcircuit elements can be used inparameter lists and output specifications,• dynamic (i.e., at the “simulation-time”) definitionsof analyses, their parameters and outputs,• parameterized subcircuit invocations; subcircuitdefinitions can be modified by parameters passedto the subcircuit expansion phase,• static and dynamic circuit variables; circuit vari-ables are those attributes of circuit elements thatcan be modified during a simulation session; staticcircuit variables must be defined within the cir-cuit description, and these definitions are neededby the package to implement a very efficient accessto static variables, as required in circuit optimiza-tion; dynamic circuit variables do not require anydefinition, so they are very flexible but relativelyslow,• enhanced circuit elements, i.e., circuit elementswith characteristics defined by users in the formof formulas or tables of values, etc.,• enhanced analyses, i.e., circuit analyses which areextended by user-defined operations.However, the most important difference between theSPICE program and the SPICE-PAC package is in theirinternal organizations. SPICE is a program with one,fixed sequence of analyses, indicated by appropriate pa-rameters within the circuit description. The order ofthese analyses as well as the form of results are al-ways the same since they are “built-into” the simulationprogram. SPICE-PAC, on the other hand, is a rather“loose” collection of simulation “blocks” (implementedby different components of the package), which can becombined together in many different ways (similarly tobuilding a variety of structures from a set of LEGO-type elements). Typical examples of such “simulationblocks” include reading a circuit description, performingan analysis, changing values of (some) circuit elements,or redefining analysis parameters. The operations of thepackage are thus performed “on demand”, as requiredTEGESED, a tool for efficient technological and geometrical characterization ... 2by a particular application. In the case of interactivesimulation, it is the user who - during a simulation ses-sion - selects the order, type and all other parametersof analyses. This means that this type of circuit sim-ulation provides the user with a “feedback” which isunavailable in traditional “batch-oriented” simulators;within one interactive simulation session, the results ofone analysis can be used to determine the new valuesof (some) circuit elements as well as the next analysisand its parameters. In cases of integrated applications,when the simulation package is used as a “generator”of circuit responses (e.g., circuit optimization in whichit evaluates the objective function and - possibly - theconstraint functions), the sequence of package’s oper-ations, their types and parameters are determined byother software tools.This flexible structure of the package makes it pos-sible to combine the same set of “standard” analyseswith several input processors accepting different forms ofcircuit specification (e.g., the SPICE input language, afunctional-type circuit description, an output of a circuitextractor, etc.), to represent the results in different ways(graphical for the user, binary for further processing byother tools, textual for storing in a file). Furthermore,it is possible to replace some of the “standard” modulesby dedicated, user-defined methods specialized to par-ticular applications. The integration with the symbolicsimulator is an example of such an enhancement.3. SYMBOLIC SIMULATOR SYBILINThe principle of symbolic simulation (see for exam-ple the list of references in [1,10]) is to derive analytic(or symbolic) network functions from a representationof a network. This means that all (or some of) cir-cuit parameters are represented by symbols in the de-rived functions, and then the circuit responses can beobtained very efficiently by evaluations of the derivedanalytic formulas.Symbolic simulators may use different circuit repre-sentations and different algorithms to derive networkfunctions. The algorithm implemented in SYBILIN issketched in Fig.1.Fig.1. General organization of SYBILIN.SYBILIN uses the Coates flowgraph representation[2]. Variables corresponding to graph nodes are the sameas those used in the known Modified Nodal Admittance(MNA) method [6]. The characteristic functions are inthe form of rational functions, in which the numeratorand the denominator are the determinant and some sub-determinant of the Coates flowgraph. The formula forthe determinant of the Coates flowgraph G is as follows:det(G) = (−1)n∑t∈Tsgn(t)∏1≤i≤nval(ti)wheren is a number of flowgraph nodes,t = (t1, t2, ..., tn) is a 0-connection of a graph G,T is a set of all 0-connections (0-connections are specificsubgraphs),sgn(t) - is a sign of a 0-connection t,val(ti) - is the weight of an element ti(the last three elements are described in greater detailin [1,2,10]).Symbolic formulas generated by such a simulator maybe used in several different ways. They can be ana-lyzed (in the mathematical sense) to provide a qualita-tive evaluation of circuits under design. They can besubjected to “post-processing” in order to perform (ap-proximate or exact) sensitivity analysis, or statisticalanalysis. They can be very useful in circuit optimiza-tion as they can replace many time-consuming circuitsimulations with relatively simple evaluations of (sym-bolic) functions.The network functions generated by symbolic simula-tors can also be represented in a form that is “computerexecutable”, i.e., a form that can be included into circuitsimulations without any further processing. One of suchpossibilities is to generate a “machine code”, as was thecase in some versions of SPICE (for CDC computers);obviously, such a solution is very “machine-dependent”because of the many differences between low-level ma-chine instructions of different computers. A more gen-eral solution that is only slightly less efficient is to useinterpretive techniques, i.e., to generate the symbolicfunctions in an intermediate representation (for exam-ple, the reverse Polish or the postfix notation) that isquite efficient to evaluate, but still preserves machineindependence. Yet another solution (which is used inTEGESED) represents the symbolic functions by equiv-alent segments in a high-level programming language (inthis case, Fortran); this generated code is then compiled,and linked with the simulation environment (using ap-propriate interfacing conventions to pass all the neededvalues of circuit parameters).4. ORGANIZATION OF TEGESEDThe TEGESED program has been obtained by com-bining the SPICE-PAC simulation package with theTEGESED, a tool for efficient technological and geometrical characterization ... 3symbolic simulator SYBILIN. Only a brief outline ofthis program is given (a more detailed description willbe presented in the final version of this paper).TEGESED is composed of three basic parts:A) input data processor and a generator of parametervalues,B) circuit analyzer,C) generator of output results.The circuit analyzer performs:B1) calculation of electrical parameters for the currentset of technological and geometrical data,B2) analyses based on calculated electrical parameters,B3) extraction of characteristic information.This organization is presented in Fig.2.Fig.2, General organization of TEGESED.Part A reads the input data and creates internalstructures used by other modules. It also determinesthe changes of technological and geometrical parame-ters and organizes systematic generation of parametercombinations, as required by subsequent analyses.Part B is the central part of TEGESED. It uses manymodules from the SPICE-PAC package for changes ofdevice parameters as well as for performing circuit anal-yses. It also contains an interface to the evaluationof symbolic functions generated by SYBILIN, that re-place the original SPICE analyses in case of repeti-tive frequency-domain analyses of circuits with the sametopologies.Section B1 handles device models and evaluation ofelectrical model parameters on the basis of technolog-ical and geometrical data determined in the part A.SPICE-PAC provides simple mechanisms for manipu-lating parameters of the original SPICE models; it isthus straightforward to use any SPICE model with itselectrical parameters related to technological and geo-metrical ones. Furthermore, it is possible to build mod-els from SPICE primitive elements (resistors, capaci-tors, sources), and due to SPICE-PAC enhanced ele-ments, the functions of such elements can be specifiedrather arbitrarily as table-driven elements or analyticfunctions implemented as user-defined routines linkedwith the package.Section B2 is the proper simulation “engine”. Alltypes of analyses provided by SPICE, i.e., DC, AC, time-domain, noise, distortion, and Fourier analysis, can eas-ily be performed using equivalent SPICE-PAC modules.Due to well-defined and standardized SPICE-PAC in-terfaces, it is possible to add new implementations ofanalyses to speed up the computations as well as to in-troduce new analyses. The symbolic simulation in thefrequency domain is used at this level.Section B3 is application-dependent since it extractssome characteristic values from the results of analysesperformed in the step B2. Examples of such charac-teristic values include the delay time for time-domainanalysis or the cut-off frequency and maximum oscilla-tion frequency for frequency domain analysis. The set ofimplemented characteristic values is “open”, so it is pos-sible to add new definitions of many other parametersthat can be extracted from the results of simulations.An interface with evaluation module based on expertsystem techniques are currently under investigation (seesections 5. and 6.).Finally, part C is responsible for numerical and graph-ical representation of results. This part is not reallysophisticated because the intention is to use a generalpostprocessor for final processing and presentation of re-sults; in the future part C will be actually reduced to apostprocessor’s interface.5. CHARACTERIZATION OF HBT FOR MI-CROWAVE APPLICATIONSThe TEGESED software has been used for anevaluation of performances (in the microwave range)of the Heterojunction Bipolar Transistor (HBT) inGaAlAs/GaAs technology developed at CNET - Bag-neux [5]. Such parameterized characterization usuallymeans an exhaustive simulation in the frequency domainfor different combinations of technological and geomet-rical parameters.The HBT was represented by the modified Ebers-Mollmodel [4]. Some 30 technological and geometrical pa-rameters were used to describe the device; examplesof these parameters include doping density in the base,emitter and collector as technological ones and numberTEGESED, a tool for efficient technological and geometrical characterization ... 4of emitter stripes, length and width of the emitter, baseand collector stripe, or emitter-base distance as geomet-rical parameters.Each analysis step (B2 in section 4) executes theoperating point analysis and then determines the fre-quency characteristic by repeatedly evaluating the sym-bolic functions generated earlier by SYBILIN. The oper-ating point information is passed to the symbolic simu-lation where it substitutes some parameters in the sym-bolic formulas. The values of the cut-off frequency andthe maximum oscillation frequency are extracted fromthe frequency characteristics. Fig.3 shows an exampleof maximum oscillation frequency as a function of theemitter stripe length and the collector doping density.It should be noted that Fig.3 requires some 150 to 200plotted points, i.e., 150 to 200 frequency characteristics(not frequency domain analyses) which correspond todifferent values of the selected parameters. To calculateeach point, a complete set of analyses has to be per-formed, i.e., the operating point analysis and about 100to 200 frequency domain analyses. As values of char-acteristic frequencies for different parameters can varyfrom tens of MHz to hundreds of GHz, the range of ex-ploration is not known a priori. Therefore, first a globalevaluation is carried out, and then the region for detailedexploration is determined. Since all these analyses areperformed for the same circuit topology, the symbolicfunctions for all these analyses are invariant.The extraction of characteristic information is some-times quite difficult as unexpected situations may hap-pen which are not covered by the definitions. Thesesituations are easily identified and classified by quali-fied users, but may be quite troublesome for automaticprocessing. Therefore, some criteria on the quality of ex-tracted information have been introduced. Three typesof situations are identified: regular extraction, extrac-tion with anomalies, and no-extraction (or impossibleextraction). Each device characterization is accompa-nied by an anomaly report, which indicates all thosecases which need user assistance in extraction of char-acteristic information. The set of built-in criteria maybe tuned to fit better the characterized device.6. CONCLUDING REMARKSTEGESED performs characterization of semiconduc-tor devices especially efficiently in the frequency domain,which is due to the symbolic approach; it allows to un-dertake device characterizations in cases when the clas-sical simulators are rather useless because of prohibitivecomputation times. For example, the HBT characteri-zation presented in the section 5 was carried out on aDEC VAX-11/750 computer running VMS, and it re-quired about 120 hours of the CPU time (distributedover the period of about 1 month). An estimation ofthe speed-up factor due to symbolic simulation (withrespect to the all-SPICE simulations) is between 15 and20 (depending on the number of points on the frequencycharacteristic). This means that the same characteriza-tion without the TEGESED tool would require 1800 to2400 hours of the VAX-11/750 CPU time.As was mentioned earlier, automated extraction ofcharacteristic information requires a flexible set of re-sults evaluation criteria. Generally, these criteria aremodified during the study as new information is ac-quired. Recent developments in expert systems providetechniques which could handle such unexpected situa-tions much easier that the traditional algorithmic meth-ods. A possibility of coupling TEGESED with an “ex-pert” evaluation module is investigated. Some detailsabout this approach might be included in the final ver-sion of the paper.Another interesting area of further modifications ofTEGESED is in full integration of SPICE-PAC andSYBILIN. It means that the same internal structureswould be used by both tools, and this would simplifyinterchange of (internal) information. Also, the use ofsymbolic simulation in speeding-up nonlinear analysesis under investigation.R e f e r e n c e s[1] W.K. Chen, “Applied Graph Theory - Graphs andElectrical Networks”; North Holland, 1976.[2] C.L. Coates, “Flow graph solutions of linear alge-braic equations”; IRE Trans. on Circuit Theory,vol.CT-6, pp.170-187, 1959.[3] E. Cohen, “Program reference for SPICE 2”; Memo-randum UCB/ERL M592, University of California,Berkeley, CA 94720, 1976.[4] J. Dangla et al., “A CAD Model for HeterojunctionBipolar Transistor’; Proc. ESSDERC, Bologna,Italy, 1987.[5] C. Gerard, “Analysis and optimization of frequencyperformances of the Heterojunction Bipolar Tran-sistor GaAlAs/GaAs” (in French); PhD Thesis,Universite Paris VI, 1987.[6] C.W. Ho, A.E. Ruehli, P.A. Brennan, “The modifiednodal approach to network analysis”; IEEE Trans.on Circuits and Systems, vol.22, pp.504-509, 1975.[7] A. Konczykowska, V. Morin, J. Godin, M. Bon,“Symbolic analysis for CAD of microwave circuits”,Coll. Computer Aided Design of Microwave Cir-cuits, London, 1985.[8] V. Morin, “SYBILIN - a program for symbolic de-sign of microwave integrated circuits” (in French);PhD Thesis, Universite de Bretagne Occidentale,Brest, 1988.[9] D.O. Pederson, “A historical review of circuit simu-lation”; IEEE Trans. Circuits and Systems, vol.31,no.1, pp.103-111, 1984.[10] J.A. Starzyk, A. Konczykowska, “Flowgraph anal-ysis of large electronic networks”; IEEE Trans. onCircuits and Systems, vol. CAS-33, pp.302-315,1986.[11] A. Vladimirescu, K. Zhang, A.R. Newton, D.O.Pederson, A.L. Sangiovanni-Vincentelli, “SPICEVersion 2G - User’s Guide (10 Aug. 1981)”; Depart-ment of Electrical Engineering and Computer Sci-ences, University of California, Berkeley, CA 94720,1981.[12] W.M. Zuberek, “SPICE-PAC, a package of sub-routines for interactive simulation and circuit opti-mization”; Proc. IEEE Int. Conf. on ComputerDesign (ICCD-84), Port Chester, NY, pp.492-496,1984.

TEGESED, a tool for efficient technological and geometrical

characterization of semiconductor devices

https://research.library.mun.ca/14772/1/EDAC-90.pdf

TEGESED, a tool for efficient technological and geometrical characterization of semiconductor devices

Abstract

Similar works

Full text

Available Versions

Memorial University Research Repository