Previous Up Next




EUROPLEXUS is a computer code being jointly developed since 1999 by CEA (CEN Saclay, DMT) and EC (JRC Ispra, SS&M) under a collaboration contract. It stems from CEA’s CASTEM-PLEXUS (a program belonging to the CASTEM system) and the previous CEA-EC joint product PLEXIS-3C.

The code analyses 1-D, 2-D or 3-D domains composed of solids (continua, shells or beams) and fluids. Fluid-structure interaction is also taken into account.

The program uses an explicit algorithm (central-difference) for the discretization in time and therefore it is best adapted to rapid dynamic phenomena (fast transient dynamics) such as explosions, impacts, crashes etc. Geometric non linearity (large displacements, large rotations, large strains), and the non-linearity of materials (plasticity, viscoplasticity, etc) are fully taken into account.

The spatial discretization is mainly based on the Finite Element or Finite Volume method. Other formulations such as SPH (Smoothed Particle Hydrodynamics), Spectral ELements, Diffuse Elements etc. are also available or under development. Numerous element types and a comprehensive library of material types for solids, fluid and special media (e.g. impedances) are available.

Three main descriptions are available in the code: the Lagrangian description which is well suited for the structural domain, the Eulerian description useful for purely fluid problems, and the Arbitrary Lagrangian Eulerian (ALE) description which is typically used in fluid-structure interaction problems.

EUROPLEXUS is interfaced to various pre- and post-processing programs that enable the meshing of the studied domain (e.g. CEA’s Cast3m) and the visualization of the results (e.g. Cast3m, ParaView or EUROPLEXUS itself).

Different types of licenses are available of EUROPLEXUS. A limited version of the code can be downloaded. For research and education these licenses are mainly for free. Details can be found on the web page of EUROPLEXUS ( This User’s manual is updated daily and can be downloaded from

A large bibliography concerning EUROPLEXUS as well as its ancestors is provided at the end of the present manual (see Section BIB). Many of the cited documents are available to EUROPLEXUS developers in electronic form on the EUROPLEXUS Consortium web site (


1.2  Installation

1.2.1  License types

Different types of licenses are available of EUROPLEXUS. A limited version of the code can be downloaded for free. For research and education a full version can be obtained for free. Details can be found on the web page of EUROPLEXUS ( This User’s manual is updated daily (development version) and can be downloaded from

1.2.2  Installation under Windows

to be written

1.2.3  Installation under Linux

to be written

1.2.4  Manual

The getting started manual is part of the EPX manual containing all information of the code. It is divided in main sections (GROUPS). In general an EPX input file can be created by following all groups and taking the needed commands.

A large bibliography concerning EUROPLEXUS as well as its ancestors is provided at the end of the present manual (see GBIBB). Many of the cited documents are available to EPX developers in electronic form on the EPX Consortium web site (

1.2.5  Benchmarks

to be written


1.3  Data flow

The first step in learning an FE tool is to understand its particular data flow. Figure 1 presents a general description of the procedure how to perform an EPX calculation.

Figure 1: General data flow in EPX

The mesh creation concerns the creation of nodes and elements. The meshes were mainly stored in external files. The next step is to define materials, loadings and calculation parameters in an EPX input file. The calculation of the inputs is done normally via the command line tool. The result files can be then assessed by several post-processing tools. The detailed data flow is shown in 2.

Figure 2: Detailed data flow in EPX

1.3.1  Files in EPX

epxinput fileGBINT_0018
kMesh file: k file format from ls_dynaGBINT_0016
listingListing output 
logLog fileGBH_0020
medMesh file: salomeGBINT_0016
mshMesh file: Cast3mGBINT_0016
pvdParaView time step fileGBG_0070
stdStandard outputs (error messages) 
vtuParaView result fileGBG_0070


1.4  Mesh generation

One of the fundamental steps to perform a FE/FV calculation is to create the meshes. There are several possibilities in EUROPLEXUS to perform that task.

1.4.1  k-file (LS-DYNA)

The format of the input is described in the LS-DYNA manuals. It is very simple and can therefore also be written by scripts.

The following not exhaustive list of tools can create k-files:

1.4.2  med (SALOME)

SALOME is an open-source software that provides a generic platform for Pre- and Post-Processing for numerical simulation. It is based on an open and flexible architecture made of reusable components. The software can be downloaded on the webpage:

1.4.3  CAST3M

The CAST3M .msh-file format is the mesh file format with the widest support in EUROPLEXUS. Nevertheless, the mesh creation can only be done with the FE software tool CAST3M. This tool is quite powerful since the mesh generation can easily be parametrised and automatized. But it needs additional effort to be learned. For an introduction in the CAST3m methodology it is referred to the CST3M webpage (


1.5  EUROPLEXUS Inputs

1.5.1  First input sample

Let’s start with an very easy EUROPLEXUS example. It is recommend to start with such a very easy calculation in order to test the installation.

1     impact0                                 !title of the problem
2     ECHO                                    !Output on the console
3     KFIL                                    !mesh file definition
4     TRID LAGR                               !3d structural calculation
5     GEOM Q4GS PART 1 TERM                   !element definition
6     COMP EPAI 2 LECT PART 1 TERM            !Thickness
8     MATE LINE RO 7800 YOUN 2.E11 NU 0.3     !Material definition: linear
9               LECT PART 1 TERM              !for part 1
10    LINK COUP                               !Links (coupled)
11         BLOQ 123 LECT NSET 1 NSET 2 TERM   !Boundaries
12    INIT VITE 3 -110 LECT PART 1 TERM       !Initial conditions
13    ECRI FICH PVTK TFRE 1.0E-3              !Output as ParaView
14                   VARI DEPL                !Output variable displacement
15    OPTI NOTE LOG 1                         !Log file written each step
16         CSTA 0.5                           !Stability step
17    CALC TINI 0.0 TFIN 100.E-3              !Start and end time of calculation
18    FIN
  1. The first line contains the title of the calculation. It is important to give that title. Otherwise, the first input line will be taken as the title.
  2. ECHO indicated that the output will be written on the command line and not only to the listing.
  3. KFIL identifies that a k-file in LS-DYNA format will be read. The name of the file can be added after the command included in ’ ’. If the name is not given, the default will be chosen as the name of the epx input file with the extension .k.
  4. TRID identifies a three-dimensional calculation and LAGR a purely structural one.
  5. The elements that were read via the mesh file must be attached to element types. That is done with the command GEOM. A list of all element types is given in GBINT_0080. Some general elements are listed in xxx. The structure of the element type allocation is that first, the element type is given and second the elements are chosen. Here, the PART 1 from the k-file is taken. The keywords depend on the mesh file type used. Here a shell element of type Q4GS is chosen. The command must be closed with TERM as soon as all elements are defined.
  6. Depending on the element type several additional definitions can be given with COMP. All available commands in this section are described in GBC_0010. Here, the thickness of 2 is set to all elements of PART 1 with the command EPAI. The classical structure of reading elements or nodes is to use LECT xxx TERM. This procedure is described more in detail in GBINT_0050.
  7. This line contains the material definition. The complete list of all materials is collected on page GBC_0100. A linear material is defined.
  8. Selection of the elements for the given material
  9. The links (e.g. boundary conditions) are defined here with LINK (GBD_0010). A coupled approach (Lagrange Multiplier) is chosen (COUP).
  10. Boundary conditions are given here with BLOQ (blockages). The number afterwards identifies that all three directions are blocked. The nodes concerned are again taken with LECT. Here two NSETs were chosen.
  11. Initial conditions were given in that line as an initial velocity for PART 1. Initial conditions were described more in detail on page GBE_0040.
  12. The outputs were defined with ECRI (see GBG_0010). FICH indicates that the outputs were written in a separate file and not in the listing. PVTK means the ParaView output files. As default these files were binary. ASCII files can be written by adding FORM. With TFRE, the frequency of the output steps is given (see GBINT_0057).
  13. With VARI (in case of PVTK) the output fields can be defined (here displacement - DEPL).
  14. Some options can be given with OPTI (GBH_0010). LOG 1 indicates that the log file is written per step. This should not be done in case of MPI calculations. NOTE DFEINS the output of the energy check.
  15. CSTA the stability step. A value of 0.5 indicates that the calculated stability step will be multiplied by 0.5 for safety.
  16. The calculation is started with CALC (GBI_0020). TINI (initial time) and TFIN (end time) must be given.
  17. The input file must be closed with FIN.

1.5.2  Elements

Several elements are available for EUROPLEXUS. Its full list is given on GBINT_0080. It is very important to know the history behind the elements. These were created in the past either by JRC or CEA and its formulation in the back can be totally different. This means also that not all elements are available for all materials. A table with all possible material-element combinations is given in (GBC_0100) In this general introduction, the main elements for structural and fluid calculations were presented. Details about further elements (like SPH or diffuse elements) can be taken from the list.

The following structural elements are recommended. They vary depending their mechanical assumptions. Further details are given in the description of the elements.

  1. Solid elements: CUBE/CUB8, PRIS, TETR. CUBE is a cubic element with reduced integration while
  2. Beams: POUT for beams. The cross section information can be given with EPAI.
  3. Triangular shells:T3GS, DST3, DKT3
  4. Quadrilateral shells: Q4G4, Q4GS, Q4GR
  5. Loading surface elements: CL3T, CL3D
  6. Material points: PMAT, DEBR

Fluid calculations can be done by using finite elements or finite volumes. The accuracy of finite elements is not very high. Therefore, only finite volumes are recommended to use for fluid or fluid structure interaction calculations. The following finite volumes can be taken: CUVF, PRVF, TEVF, PYVF. Further information about fluid calculations by using finite volumes are given here:

1.5.3  Sandwich Elements

The code also allows to use layered elements for beams and in particular for shell elements. This means that the materials of the integration points through the thickness could be different. More information are given in GBINT_0110. As an example, the benchmark bm_str_lsgl01 could be used.

1.5.4  Materials

Several material laws are implemented in EUROPLEXUS. The full list of materials can be found on GBC_0100. Not all elements accept all material types. GBC_0100 shows also the possible material-element combinations.

The table below presents some materials that have a general use.

numbernamereflaw of behaviour
21CLVF7.9.33Boundary conditions for finite volumes
109DADC7.7.16Dynamic Anisotropic Damage Concrete
111DPDC7.7.17dynamic plastic damage concrete
87DPSF7.7.42Drucker Prager with softening and viscoplastic regularization
83DRPR7.7.51Drucker Prager Ispra model
19DYNA7.7.7dynamic Von Mises isotropic rate-dependent
17FANT7.7.30phantom: ignore the associated elements
9GAZP7.8.4perfect gas
118GGAS7.8.1generic ideal gas material
116GLIN7.7.3generic linear material
117GPLA7.7.4generic plastic material
48GVDW7.8.28Van Der Waals gas
40GZPV7.8.24perfect gas for Van Leer
95HYPE7.7.54hyperelastic material (Model of Mooney-Rivlin, Hart-Smith and Ogden)
4ISOT7.7.7isotropic Von Mises
108JCLM7.7.65Johnson-Cook with Damage Lemaitre-Chaboche for SPHC
50JWL7.8.21explosion (Jones-Wilkins-Lee model)
66JWLS7.8.29Explosion (Jones-Wilkins-Lee for solids)
72LEM17.7.9Von Mises isotropic coupled with damage (type Lemaitre)
1LINE7.7.1linear elasticity
23LIQU7.8.14incompressible (or quasi-) fluid
70LMC27.7.11Von Mises isotropic coupled with damage (Lemaitre) with strain-rate sensitivity
26MASS7.7.29mass of a material point
85MAZA7.7.15Mazars-linear elastic law with damage
2PARF7.7.7perfectly plastic Von Mises
125RIGI7.7.67Rigid material (for rigid bodies)
35VM237.7.38Von Mises elasto-plastic radial return
2/4/5/19VMIS7.7.7Von Mises materials
84VMSF7.7.41Von Mises with softening and viscoplastic regularization
120VPJC7.7.66visco-plastic Johnson-Cook
67ZALM7.7.10Zerilli-Armstrong with damage Lemaitre-Chaboche

1.5.5  Element erosion

Element erosion means that elements are deleted from the table of elements and were not treated any more. This is a particular procedure in explicit codes since the general energy balance is violated by eroding elements. There are several reasons why element erosion could be indicated:

  1. The material has reached a failure mode (damage or other criteria)
  2. The element became so distorted that it cannot be treated any more (CROI)
  3. The time step size of the element is too small (CALC TFAI)
  4. Parts of the model should be removed at a certain time (e.g. certain elements have to become “fantom”, i.e. have to be eroded, at a chosen time GBH_0100), or due to further criteria (e.g. displacement-driven erosion GBC_0067).
  5. The user decides to erode some elements interactively at the current time reached by the calculation GBO_0010.

The objective in most of the cases is that the calculation is not stopped due to critical behaviour of material or elements.

In all cases, the keyword EROS (see GBA_0030) must be added in the beginning (before DIME and GEOM). This keyword is followed by CROI as soon as element erosion for distorted elements is needed. Erosion due to too small time steps sizes can be activated in the CALC PART by adding TFAI (see GBI_0020).

In case of failure erosion, the ratio between failed and total gauss point in an element can be given. This parameter must be written immediately after EROS. The global value for the material failure element erosion can be overwritten for parts of the elements by COMP EROS (see GBC_0069).

1.5.6  Fluid calculations


EUROPLEXUS offers a rich variety of models for Fluid-Structure Interactions (FSI). The following is a short introduction to FSI and a tentative classification of the models available in the code, in order to guide the user in the choice of the most appropriate FSI models for the applications of interest. For a more detailed overview of the available FSI models see e.g. [303].

Fluid-structure interaction (FSI) phenomena play an important role in many areas, ranging from aeronautical and space applications, to civil and marine/offshore engineering and to the transport industry, to name just a few. The EUROPLEXUS development team has been involved for many years in the development of numerical methods for FSI modeling applied to safety studies—initially for the nuclear industry and more recently for conventional power plants (electrical machinery)—to civil engineering (vulnerability of buildings and other critical infrastructures to terrorist attacks) and to land mass transports (blast effects in railway stations, metro lines, rolling stock).

All these studies are characterized by the violent blast loading, resulting either from an accident or from an intentional attack, and by the very short time scale (fast transient dynamics). Strong pressure waves propagate in the fluid and load the surrounding structures, which typically undergo large deformations and in some cases reach complete failure and fragmentation.

For this class of problems, an explicit time marching algorithm is usually adopted, where the fluid is modelled as compressible and inviscid (Euler equations). An Arbitrary Lagrangian Eulerian (ALE) formulation is adopted for the fluid sub-domain, while the structure is Lagrangian.

Three different discretization approaches are available in the code for the fluid sub-domain: finite elements (FE), node-centred finite volumes (NCFV) and cell-centred finite volumes (CCFV):

The coupling between the fluid (ALE) and the structure (Lagrangian) is realized by suitable FSI algorithms. Two broad classes of algorithms are available in the code. The first class uses a strong approach, based on constraints imposed on the (velocity of) fluid and structure nodes at the F-S interface. The second class uses a weak approach, based on direct application of fluid pressure forces to the structure. This terminology (strong/weak) is tentatively adopted here in an attempt to characterize the different nature of the two approaches, but it should not be confused with other uses of the same terms in the literature, in particular with weak (i.e. integral) forms in continuum mechanics. Traditionally, strong FSI algorithms are mainly used in FE, while weak FSI algorithms are mainly used in FV.

Yet another classification of FSI algorithms concerns the degree of deformation/damage that the structure can undergo (and thus the type of application). One class of basic algorithms is suitable for large motion and large deformation of structures, but only provided these do not fail. Another class of algorithms can go up to complete failure, and fragmentation, of the loaded structures. Finally, FSI algorithms can be classified in three types according to spatial discretization: (nodally) conforming, non-conforming, and embedded (or immersed). The first two types are mostly used in applications without structural failure (but there are exceptions), while embedded algorithms are the only ones capable of dealing with extreme loading cases where the structure fails and breaks up in pieces.

The following Table summarizes the architecture of a typical FSI model, consisting of a detection module and of an enforcement module. The various types of approaches (basic / embedded or strong / weak) are briefly summarized.

Table 1: A classification of FSI algorithms
  BasicNo structural failure,
 FSI moderate rotations.
 DetectionEmbeddedStructure can fail,
FSI  arbitrary rotations.
Algorithm  Constraints on F and S velocities
  Strongare imposed, e.g. by Lagrange
 FSI multipliers (implicit).
 Enforcement Pressure forces are transmitted
  Weakfrom the fluid to the structure;
   structure motion provides weak feedback
   on fluid (S= master / F= slave).

The following Table completes the classification of the available FSI models, by showing the type of spatial discretization (conforming, non-conforming or embedded), the name of the input directive (when applicable/needed), and the associated fluid discretization(s).

Table 2: The available FSI algorithms
 DetectionSpatialEnforcementName /Use
  Conforming  NCFV
 BasicF-S meshesWeakMergeCCFV
 (no  F-S nodes 
FSIstructural StrongFSAFE,
Algorithmfailure)Non-  NCFV
  conforming Declare 
  F-S meshesWeaknon-matchingCCFV
 EmbeddedS-mesh isStrongFLSRFE,
 (structureimmersed  NCFV
 can fail)in the F-meshWeakFLSWCCFV

1.5.8  Restart


1.5.9  Index of important commands

This is is an non exhaustive list of important commands that may be useful to understand the basic working of EUROPLEXUS. Additional lists are given for the materials GBC_0100 and elements GBINT_0080.

commandmain groupdescriptionref
BLOQLINKBoundary conditionsGBD_0030
CALC Calculation definitionsGBI_0020
COMP Geometric complementsGBC_0010
COUPLINKTreatment of the links as coupled (Langrange multipliers)GBD_0010
CSTAOPTITime step safety coefficientGBH_0020
DECOLINKTreatment of the links as decoupledGBD_0010
ECHO—-Output on the consoleGBA_0020
ECRI Output of the resultsGBG_0010
EPAICOMPThickness (e.g. of shell elements)GBC_0040
GEOM Mesh and grid motionGBB_0010
KFIL—-mesh file definition (k-file)GBA_0030
INIT Initial conditionsGBE_0040
LAGR—-Structural calculationGBA_0030
LINK LinksGBD_0010
LOGOPTILog file .log is createdGBH_0020
MATE Material definitionGBC_0100
NOTEOPTINo energy check printed per each stepGBH_0020
OPTI Definition of optionsGBH_0010
PVTKECRIOutput as ParaViewGBG_0070
TFINCALCEnd time of calculationGBI_0020
TINICALCStart time of calculationGBI_0020
TRID—-3D calculationGBA_0030

  1. INT.70


1.6  Outputs/Post processing

  1. Writing outputs in EPX in files
  2. Internal postpro
  3. Interactive work
  4. ParaView

Previous Up Next