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 (http://www-epx.cea.fr/).
This User’s manual is updated daily and can be downloaded from
http://europlexus.jrc.ec.europa.eu/.
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 (https://europlexus.jrc.ec.europa.eu/).
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 (http://www-epx.cea.fr/).
This User’s manual is updated daily (development version) and can be downloaded from
http://europlexus.jrc.ec.europa.eu/.
to be written
to be written
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 (https://europlexus.jrc.ec.europa.eu/).
to be written
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.
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.
extension description ref epx input file GBINT_0018 k Mesh file: k file format from ls_dyna GBINT_0016 listing Listing output log Log file GBH_0020 med Mesh file: salome GBINT_0016 msh Mesh file: Cast3m GBINT_0016 pvd ParaView time step file GBG_0070 std Standard outputs (error messages) vtu ParaView result file GBG_0070
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.
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:
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: http://www.salome-platform.org/.
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 (http://www-cast3m.cea.fr/)
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
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.
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:
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.
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.
number name ref law of behaviour 74 ABSE 21 CLVF ?? Boundary conditions for finite volumes 109 DADC ?? Dynamic Anisotropic Damage Concrete 111 DPDC ?? dynamic plastic damage concrete 87 DPSF ?? Drucker Prager with softening and viscoplastic regularization 83 DRPR ?? Drucker Prager Ispra model 12 DRUC ?? Drucker-Prager 19 DYNA ?? dynamic Von Mises isotropic rate-dependent 17 FANT ?? phantom: ignore the associated elements 9 GAZP ?? perfect gas 118 GGAS ?? generic ideal gas material 116 GLIN ?? generic linear material 117 GPLA ?? generic plastic material 48 GVDW ?? Van Der Waals gas 40 GZPV ?? perfect gas for Van Leer 95 HYPE ?? hyperelastic material (Model of Mooney-Rivlin, Hart-Smith and Ogden) 4 ISOT ?? isotropic Von Mises 108 JCLM ?? Johnson-Cook with Damage Lemaitre-Chaboche for SPHC 50 JWL ?? explosion (Jones-Wilkins-Lee model) 66 JWLS ?? Explosion (Jones-Wilkins-Lee for solids) 72 LEM1 ?? Von Mises isotropic coupled with damage (type Lemaitre) 1 LINE ?? linear elasticity 23 LIQU ?? incompressible (or quasi-) fluid 70 LMC2 ?? Von Mises isotropic coupled with damage (Lemaitre) with strain-rate sensitivity 26 MASS ?? mass of a material point 85 MAZA ?? Mazars-linear elastic law with damage 2 PARF ?? perfectly plastic Von Mises 125 RIGI ?? Rigid material (for rigid bodies) 99 SLZA ?? Steinberg-Lund-Zerilli-Armstrong 35 VM23 ?? Von Mises elasto-plastic radial return 2/4/5/19 VMIS ?? Von Mises materials 76 VMJC ?? Johnson-Cook 78 VMLP ?? Ludwig-Prandtl 79 VMLU ?? Ludwik 84 VMSF ?? Von Mises with softening and viscoplastic regularization 77 VMZA ?? Zerilli-Armstrong 120 VPJC ?? visco-plastic Johnson-Cook 67 ZALM ?? Zerilli-Armstrong with damage Lemaitre-Chaboche
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:
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).
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. [].
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.
Basic No structural failure, FSI moderate rotations. Detection Embedded Structure can fail, FSI arbitrary rotations. Algorithm Constraints on F and S velocities Strong are imposed, e.g. by Lagrange FSI multipliers (implicit). Enforcement Pressure forces are transmitted Weak from 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).
Detection Spatial Enforcement Name / Use Strategy Discretization Strategy Command with Strong FSA FE, Conforming NCFV Basic F-S meshes Weak Merge CCFV (no F-S nodes FSI structural Strong FSA FE, Algorithm failure) Non- NCFV conforming Declare F-S meshes Weak non-matching CCFV F-nodes Embedded S-mesh is Strong FLSR FE, (structure immersed NCFV can fail) in the F-mesh Weak FLSW CCFV
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.
command main group description ref BLOQ LINK Boundary conditions GBD_0030 CALC Calculation definitions GBI_0020 COMP Geometric complements GBC_0010 COUP LINK Treatment of the links as coupled (Langrange multipliers) GBD_0010 CSTA OPTI Time step safety coefficient GBH_0020 DECO LINK Treatment of the links as decoupled GBD_0010 ECHO —- Output on the console GBA_0020 ECRI Output of the results GBG_0010 EPAI COMP Thickness (e.g. of shell elements) GBC_0040 GEOM Mesh and grid motion GBB_0010 KFIL —- mesh file definition (k-file) GBA_0030 INIT Initial conditions GBE_0040 LAGR —- Structural calculation GBA_0030 LINK Links GBD_0010 LOG OPTI Log file .log is created GBH_0020 MATE Material definition GBC_0100 NOTE OPTI No energy check printed per each step GBH_0020 OPTI Definition of options GBH_0010 PVTK ECRI Output as ParaView GBG_0070 TFIN CALC End time of calculation GBI_0020 TINI CALC Start time of calculation GBI_0020 TRID —- 3D calculation GBA_0030