N. García-Pedrajas et al. (Eds.): IEA/AIE 2010, Part I, LNAI 6096, pp. 489–498, 2010.
© Springer-Verlag Berlin Heidelberg 2010
Simul-EMI II: An Application to Simulate Electric and
Magnetic Phenomena in PCB Designs
Juan-Jesús Luna-Rodríguez1, Ricardo Martín-Díaz1, Manuel Hernández-Igueño1,
Marta Varo-Martínez2, Vicente Barranco-López3, Pilar Martínez-Jiménez2,
and Antonio Moreno-Muñoz1
1 University of Cordoba, Department of Computer Architecture, Electronic and Electronic
Technology. 'Leonardo da Vinci' building (Campus Rabanales)
14071 Cordoba, Spain
2 University of Cordoba, Department of Applied Physics. 'Einstein' building
14071 Cordoba, Spain
3 University of Cordoba, Department of Electrical Engineering. 'Leonardo da Vinci' building
14071 Cordoba, Spain
firstname.lastname@example.org, email@example.com, firstname.lastname@example.org,
email@example.com, firstname.lastname@example.org, email@example.com,
Abstract. In this work, an application to simulate electric and magnetic phe-
nomena during design of printed circuit boards (PCB) is presented. The com-
mercial schematic simulation software currently uses advanced models of com-
ponents, but not of connections. However, with Simul-EMI II it is possible to
get results very close to physical reality of the electronic circuits, in the same
environment of schematic simulation. The parasitic effects considered are: con-
nection resistance (traces, solder pads and vias), insulation resistance (prepreg,
air, solder mask, etc.), self inductance and capacity (traces, solder pads and
vias) and mutual inductances and capacities. For that, several applications of
data mining, parametric model extraction and knowledge management have
been developed in the MATLAB™ environment. Finally, the results of a PCB
simulation with PSPICE™ before and after Simul-EMI II application, together
with the electronics laboratory validation tests, are shown.
Keywords: EMI simulation, PCB simulation, EDA application, connection
model, model generation, trace coupling, crosstalk, signal reflection.
The Printed Circuit Boards (PCB) are the most important circuit technology in the
electronic industry. The increase of connection density and signal frequency has
been the trend in the last years . In that sense, the separation and routing of
490 J.-J. Luna-Rodríguez et al.
traces1 in connection layers have become one of the most critical design tasks. Cur-
rently, electronic design engineers need new software technologies (e.g. in
simulation) to develop circuits in environments as Computer Aided Design (CAD),
Computer Aided Engineering (CAE) or Electronic Design Automation (EDA). The
main purpose of that is to reduce the cost and time of electronic circuit development,
whereas the reliability and function complexity of the modern circuits are
In practice, the probability of design errors and operation failures during the devel-
opment of a circuit is high and that increases its cost and completion time. This is
mainly due to the fact that modern electronic circuits are very complex hardware
systems. The components are connected by means of hundreds or even thousands of
traces, vias (plated holes that connect several layers) and pad solders, whose behav-
iour differ from ideal connections. 
The electrical simulation is usually done during the schematic circuit design by
means of simulators such as PSPICE™ or Electronic Work Bench™ (EWB), in a
Computer Aided Simulation (CAS) environment. These computer applications use
advanced models of the components but not of the connections, which are considered
as ideal connections. To understand the importance of this fact, Fig. 1 shows an ex-
ample of the difference between an ideal connection (connecting two resistors) in a
schematic circuit and a real connection in the PCB, where there are multiples electri-
cal and magnetic phenomena. 
Fig. 1. Changes of circuit connection model after its implementation on a PCB
Currently there are plenty of commercial solutions to simulate the electromagnetic
interference (EMI) phenomena of printed circuits, e.g. SI Verify by Zuken™ or IE3D
by Zeland Software™, which are based in Finite Element Modeling/Method (FEM).
1 Thin copper sheets, also called tracks, used to connect the pins of components.
Simul-EMI II: An Application to Simulate Electric and Magnetic Phenomena 491
But these are independent of the electric simulation environments, most popular
among electronic designers. In addition, their acquisition and maintenance cost is very
high and they are not easy to use. 
2 General Description of Simul-EMI II
The main aim of “Simul-EMI II” project is to provide an affordable alternative
(cheap, easy and fast) to expensive commercial EMI simulation software, with results
very close to the physical reality of the electronic circuits. For this purpose, our appli-
cation includes most electric and magnetic interference phenomena (coupling,
crosstalk, reflections, etc.) that are actually produced in a PCB. In this simulation
environment the all near field EMIs can be simulated, which include the resistance
effects (contact and isolation), inductance (self and mutual) and capacity (self and
mutual) of traces, solder pads and vias . The far field phenomena (electromagnetic
radiation) are not supported in Simul-EMI II, for the time being.
The main premises for the Simul-EMI II development have been: working in the
same electrical simulation environment as in the schematic design (PSPICE in this
case) and using only the normally available information from the PCB design soft-
ware. In Fig. 2, a scheme of the general steps of our simulation environment is shown,
where the typical workflow can be easily understood.
Fig. 2. Steps in the development process of an electronic circuit using Simul-EMI II
Briefly, Simul-EMI II can read the schematic design from EDA software (with
ideal connections) and then the physical design of the corresponding PCB is inter-
preted. Finally, a new schematic circuit (compatible with PSPICE™) is redesigned
492 J.-J. Luna-Rodríguez et al.
automatically, which includes electromagnetic models of the actual connections. In
order to achieve this, a MATLAB™ program is executed with help from the
EXCEL™ spreadsheet. This program performs the following tasks:
1. Data mining:
• Net-list and component-list reading.
• “Gerber” files (geometric data) interpretation.
• Technological information acquisition.
2. Extraction of models:
• Conversion of geometric and technological data to parasite parameters.
• Management of data base of EMI knowledge.
3. Redesign of schematic circuit:
• Equivalent connection models builder.
• Net-list rebuilder.
Consequently, Simul-EMI II can be considered as an “application to design” (in the
EDA context) related to Data Mining in field of the Artificial Intelligence (AI).
3 EMI Phenomena Modelling
In the computer application presented in this paper, a knowledge database on near
field EMIs has been included. The parasitic effects considered in this database are:
connection resistance, insulation resistance, self inductance and capacity and mutual
inductances and capacities . These parasitic elements are the ones that cause the
most disturbing phenomena in the electronic circuits, such as crosstalk and reflec-
tions, especially when high frequency signals are present.
The calculation of connection return resistance may be more complicated when the
same path return is used to finish loops of multiple signals. Considering a distribution
multiple traces of the “microstrip line” type sharing the return signal through the
ground plane, a resistance matrix, as shown in (1), can be defined to establish the
interaction between conductors and their return paths. 
The values showed on the main diagonal (R11, R22, …, Rij) represent the conductor
resistances in free loop, including the resistance of its return path when the others are
conducting zero current. The terms outside the main diagonal represent the mutual
resistance between each conductor. Finally, note that the dielectric losses of insula-
tions, the side etching factor of the conductors and its temperature dependence are
also included in the matrix formulation of resistive parasitic effects. 
Parasitic capacitances are present between any two conductive surfaces at different
voltage. For traces of a PCB, this means that there will be capacities between each
Simul-EMI II: An Application to Simulate Electric and Magnetic Phenomena 493
other and also between them and the reference plane . The relations of self and
mutual capacity on PCB traces can be defined by means of a capacity matrix, similar
to the previous resistance matrix.
2 22 21
1 12 11
The mutual capacitances are out of the diagonal in (2) and represent the charges be-
tween a set of conductors. In the circuit, these charges are considered capacitive cou-
plings and must appear as negative in the matrix. The self capacitance C11, C22, …, Cij
represent the capacitive coupling between conductors with the GND conductor. 
As it was done with the parasitic resistances and parasitic capacitances, an induc-
tance matrix including self and mutual inductances related to each of the PCB traces
can be defined. 
1 12 11
The inductance matrix (3) shows the inductance of each track with his return in the
main diagonal, when currents in the rest of the conductors are zero. The non-diagonal
terms represent the coupling inductance that appears between traces. 
In Fig. 3 the equivalent model of a continuous transmission line, applicable to the
traces on a PCB, is shown. This model divides the transmission line (the trace) in a set
of standard length segments.
Fig. 3. Characteristic impedance of transmission lines from R, L, G and C parameters
The series impedance consists of a resistance R coupled with an inductance L. The
shunt admittance is a conductance G in parallel with a capacitance C. The values of R,
L, C and G represent the cumulative amount of resistance, inductance, capacity and
conductance per unit length, respectively, in the transmission line. 
The advantage of the connection equivalent model based on transmission lines
with infinite blocks in series (Fig. 3) is that adding a new block does not change the
input impedance of the whole structure. 
494 J.-J. Luna-Rodríguez et al.
4 Data Mining and Automatic Generation of Parametric Models
To calculate the actual connection models, the geometric data of PCB design are
required, as well as some technological information (e.g. layer stack, materials, etc.).
Geometrical information of the traces, solder pads and vias are contained in the de-
sign software database, but these are not usually accessible from another computer
However, this information can be extracted by applying data mining to GERBER2
files (all EDA software can generate them), which are typically used to send drawings
of the different layers to the manufacturer . Then, as the GERBER format contains
only graphic information, it has been necessary to implement an “interpreter” to trans-
form the drawing into dimensions. 
The numerical extraction phase of coordinates from a GERBER file has been
automated with MATLAB™, working with Microsoft EXCEL™ , since it is
possible to separate and classify the numerical data and ASCII characters in the
spreadsheet in a simple and effective way.
Fig. 4. A simple layout of top connections and its corresponding extended GERBER file
In order to simplify and systematize the final parameterization algorithm, each
trace is divided into segments. For example, track 3 of the layout shown in Fig. 4 will
be processed as 5 traces, corresponding to its 5 segments.
In order to calculate the “length” of each trace, it has only been necessary to draw
each segment step by step, while a program counter updates that parameter. The in-
ference of the parameter “separation” has been somewhat more complicated, because
our MATLAB™ program must check the parallelism of each trace segment with
others traces, and how much of its length they are facing. 
A study about the influence of distance on the parasitic capacitance between two
traces is shown in Fig. 5. This study has allowed to identify a threshold value
(~10mm) from which the coupling effects between two traces are discarded.
2 The extended GERBER is the currently used format for obtaining the manufacturing artworks
by photoplotter, and it is specified in the RS-274X standard by Barco Graphics.
Simul-EMI II: An Application to Simulate Electric and Magnetic Phenomena 495
Fig. 5. Study of mutual capacity depending on the distance between traces
The calculated geometrical parameters, together with some data entered via user
interface, are now used for the model extraction. For this, a database of knowledge
about the parasitic effects described in section 3 (EMI Phenomena Modelling) has
been implemented with the available formulas in the current literature.   
5 Reconstruction of the PCB Equivalent Schematic Circuit
The description of schematic circuits in file form has been traditionally done by the
“net-list” format. This file contains all the information related to the circuit compo-
nents and the connections between them. A file containing this information can
be obtained directly from the CADSTAR™ through a tool called “report genera-
tor”, which is only a processor of scripts with access to the PCB design software
In addition to the data of components and connections (obtained from the net-list
file) it is necessary to relate each net with the component pins and their exact posi-
tions on the PCB. Below, the simple program that extracts this information from the
database of CADSTAR™ is showed.
Text "Component Value Position X Position Y"
For Each Component (Component, Testpoint)
If Component.Comp Side = All on Top Side
For Each Pin
Text " "
496 J.-J. Luna-Rodríguez et al.
To simulate the printed circuit in the same environment of the schematic circuit
(PSPICE™), including models of the actual connections, the original net-list is modi-
fied by inserting new nodes . Fig. 6 shows an example of the reconstruction of the
original net-list to include EMI phenomena of the PCB.
Fig. 6. A net-list example of a simple circuit and its reconstruction using SIMULEMI II
The final result of this process, automated by using programming functions in
MATLAB™ code, is a net-list file compatible with PSPICE™ to simulate an actual
PCB electronic circuit like a schematic circuit  .
6 Tests and Validation
To validate the Simul-EMI II application, a simple passive voltage divisor circuit has
been designed. As shown in Fig. 7, the traces routing (layout) on the PCB is pretty
bad (it has been done on purpose) in order to highlight the EMI phenomena.
The practical net-list (with actual connections) of this circuit after the application of
Simul-EMI II includes more than 70 lines. Each of these lines corresponds to a parasitic
effect, which is not considered in the theoretical net-list based on ideal connections.
Fig. 7. Passive voltage divisor in a printed circuit board designed (badly) in CADSTAR
Simul-EMI II: An Application to Simulate Electric and Magnetic Phenomena 497
Subsequently, this circuit has been manufactured and there have been several tests
in the laboratory, using a wave generator Tektronix AFG 3022B Dual Channel –
Arbitrary / Function Generator (250MS/s – 25MHz) and an oscilloscope Tektronix
TDS2002B Two Channel Digital Storage Oscilloscope (1GS/s – 60MHz). In Fig. 8,
the results of simulation with PSPICE™ before and after Simul-EMI II application,
together with the electronics laboratory tests, are shown.
Fig. 8. Simulation with sinusoidal excitation signal of 10MHz frequency and 5Vpp range
As shown, the simulation results with Simul-EMI II are very similar to the tests
conducted in the laboratory. However this does not happen in the simulations without
Simul-EMI II. Laboratory tests with frequencies below 1 MHz showed no parasitic
effects, and consequently they have not been included in this paper.
The schematic simulation software currently uses advanced component models, but
connection models are simple (ideal). However, with the application presented in this
work is possible to get results very close to the physical reality of the electronic cir-
cuits, in the same environment of schematic simulation. Simul-EMI II can read the
schematic design from EDA software (with ideal connections) and then the physical
design of the corresponding PCB is interpreted. Finally, a new schematic circuit
(compatible with PSPICE™) is redesigned automatically, which includes electromag-
netic models of the actual connections.
Given the results of the validation tests, we can conclude that the parasitic effects
of the connections are irrelevant below 1MHz. However, above 3MHz these effects
can modify substantially the expected (ideal) behaviour of the circuit.
Moreover, comparative analysis of simulations carried out with Simul-EMI II and
the measurements performed in the laboratory confirm the validity of this computer
application as a useful tool for electronic design.
1. Jonson, H., Graham, M.: High Speed Signal Propagation - Advanced Black Magic. Pren-
tice Hall, Upper Saddle River (2003)
2. Abhari, R., Eleftheriades, G.V., Deventer-Perkins, E.: Physics-Based CAD Models for the
Analysis of Vias in Parallel-Plate Environments. IEEE Transactions on Microwave Theory
and Techniques 49(10), 1697–1707 (2001)
498 J.-J. Luna-Rodríguez et al. Download full-text
3. Thierauf, S.C.: High-Speed Circuit Board Signal Integrity. Artech House, Norwood (2004)
4. Luna-Rodríguez, J.J.: Diseño de Circuitos Impresos: un Manual Teórico-Práctico con
CadStar. Universidad de Córdoba, Córdoba (2008)
5. Klee, H.: Simulation of Dynamic Systems with MATLAB and Simulink. CRC Press, Boca
6. Braithwaite, N., Weaver, G.: Electronic Materials inside Electronic Devices. The Open
University, London (1990)
7. Scarlatti, A., Holloway, C.L.: An equivalent transmission-line model containing dispersion
for high-speed digital lines with an FDTD implementation. IEEE Transactions on Electro-
magnetic Compatibility 43(4), 504–514 (2001)
8. Kusiak, A., Kurasek, C.: Data Mining of Printed-Circuit Board Defects. IEEE Transactions
on Robotics and Automation 17(2) (2001)
9. Choudhary, A.K., Harding, J.A., Tiwari, M.K.: Data mining in manufacturing: a review
based on the kind of knowledge. J. Intell. Manuf. 20, 501–521 (2009)
10. Barco Graphis, N.V.: Gerber RS-274X Format. User’s Guide. Gent. (2001)
11. Artwork Conversion Software, Inc.,
12. Downey, A.B.: Physical Modeling in MATLAB. Green Tea Press, Needham (2008)
13. Abhari, R., Eleftheriades, G.V., Deventer-Perkins, E.: Analysis of Differential Vias in a
Multilayer Parallel Plate Environment Using a Physics-Based CAD Model. In: IEEE Inter-
national Microwave Symposium, Phoenix, pp. THIF-09-4 (2001)
14. Chen, H., Li, Q., Tsang, L., Huang, C.C., Jandhyala, V.: Analysis of a Large Number of
Vias and Differential Signaling in Multilayered Structures. IEEE Transactions on Micro-
wave Theory and Techniques 51(3), 818–829 (2003)
15. Kouzaev, G.A., Nikolova, N.K., Deen, M.J.: Circular-Pad Via Model Based on Cavity
Field Analysis. IEEE Microwave and Wireless Components Letters 13(11), 481–483
16. Quintáns, C.: Simulación de Circuitos Electrónicos con OrCAD® 16 Demo. Marcombo,