Skip to content



The interface program Mesh2XXX has a generic name and it involves both interface tools: Mesh2HOMAT and Mesh2ABAQUS (see Fig. 1). The aim of this interface program, written in C++, is miscellaneous. Four different input file formats are currently available and read by the interface program Mesh2XXX: the standard platform exchange format VTK, the universal format UNV of IDEAS, the Abaqus input format INP 1 and the MICRESS format for which the possibility to read the compressed grain information directly is retained. In the latest case, the user has to provide the compressed grain structure PROBLEM_NAME.korn, the geometry file PROBLEM_NAME.geoF file and, if specified in MICRESS, the ASCII file TabO containing the orientation definition and the phase of each grain. The standard platform exchange format VTK as well as the Abaqus input format present several definition variants. In order to read straightforward these different variants of VTK and INP files, Mesh2XXX requires since its version 5.3 to specify the program which has written the considered VTK or INP geometry file.

Figure 1: Overview of the prediction of effective material properties of a simulated MICRESS microstructure.

On the one hand, this interface program allows the conversion of a structured or unstructured mesh in another data format as the given input format. It works as a mesh translator:

  • Mesh2HOMAT writes a specific geometry file for HOMAT, named PROBLEM_NAME.hgeo and, if desired, also a VTK geometry file which contains always an unstructured mesh of the discretized Representative Volume Element (RVE). Per default, the specific geometry files is zipped in order to reduce its size.

    As the homogenization method requires the automatic generation of interface elements with zero thickness at the boundaries between grains, spherulites or material domains (see Fig. 2), Mesh2HOMAT generates automatically new nodes and the corresponding interface elements. Therefore, Mesh2HOMAT converts always a structured or unstructured mesh of the microstructure in an unstructured mesh with interface elements at the grain or material domain boundaries. Since version 6.0, it is also possible to write an unstructured mesh without generation of interface elements by specifying an additional parameter no_clones. This way, an inp geometry can be converted in a VTK one, it works as a simple inp2vtk converter. Moreover, Mesh2HOMAT evaluates the outward normal to the free surfaces and defines the pair of periodic surfaces in function of the user specifications. Depending on the actual problem, either 1-D, 2-D or, per default, 3-D periodic boundary conditions can be specified on the unit cell. The microstructure solutions of MICRESS and SphaeroSim, available in the initial VTK format, are converted in another VTK file containing the newly generated, unstructured finite element mesh of the RVE. Eventually, Mesh2HOMAT writes a geometry file PROBLEM_NAME.hgeo.gz and a template of the HOMAT command file PROBLEM_NAME.hin.

  • Mesh2ABAQUS writes in his first variant only a ABAQUS input file, named NAME.inp, which contains all nodes, elements and solid sections. But, no specific boundary or loading conditions are specified. No information about the material is given and no additional node and/or element sets are built and, in contrast to Mesh2HOMAT, no interface elements between different materials are generated.

    The second, more relevant variant of Mesh2ABAQUS generates automatically the six (or three in 2D) input files necessary to perform uniaxial virtual tests of the discretized RVE of the considered microstructure within ABAQUS. The program generates the required periodic boundary conditions. Moreover, if the TabO file of Micress is provided, the program reads also the orientation definition by a quaternion of each grain and transforms this quaternion in an Abaqus orientation definition (a local axis system X'Y'Z' specified by the two nodes a and b in Fig. 3). As the phase information is also included in the ASCII TabO file, the redundant definition of material properties per grain/material can be replaced by a material definition per phase of the discretized RVE.

Figure 2: Duplication of the nodes at interfaces between two phases or material domains and definition of the interface element 2-3-7-8.

Figure 3: Abaqus orientation definition of a material or grain by two nodes a and b, specify the plane X'-Y' of the local axis system X'Y'Z'. Note that the center c of the local axis system is here identical with the structural center.

A detailed description of the common commands of both interface program versions Mesh2HOMAT and Mesh2ABAQUS is provided in Sec. Common features and commands of Mesh2XXX. Sec. Specific features and commands of Mesh2HOMAT addresses the specific commands of Mesh2HOMAT, whereas the specific commands of Mesh2ABAQUS are outlined in Sec. Specific features and commands of Mesh2ABAQUS.

Common features and commands of Mesh2XXX

The execution of either Mesh2HOMAT or Mesh2ABAQUS without any argument on the command line or introduced via a small driving file, named classically problem_name.min or PROBLEM_NAME_MIN.txt, provides a quick and short description of the available program parameters.

Both program variants, Mesh2HOMAT and Mesh2ABAQUS, have the following keywords in common:

RVE_name: This first parameter defines the name of the analysed RVE geometry and always has to be specified with its extension. The allowed extensions are at the moment: vtk, unv, inp and korn for a microstructure simulated by MICRESS. Based on the specified extension, a specific routine is called to read the RVE geometry.

Note that, except the RVE_name, all other parameters are optional:

  • -scal SX | SX SY SZ: This optional parameter permits to scale the initial geometry either in an isotropic way by a factor SX (default option) or in an anisotropic way by a specific factor SX, SY and SZ in each direction of the RVE axis system. If anisotropic scaling is adopted, all the three scale factors have to be specified. Note that the default length unit in HOMAT and Abaqus is millimeter.

    Note: The grid spacing of a structured MICRESS mesh is automatically converted from cm to mm by a factor 10. If the user specifies the optional parameter -scal, then the initial mesh is scaled by the factor: 10 SX in the isotropic case and by 10 SX, 10 SY and 10 SZ in the anisotropic case.

  • -output_level n: This optional parameter controls the level of verbosity of the log messages. For example, the number of generated new nodes is printed to standard output which can be redirected in a specific log file of your choice, e.g. PROBLEM_NAME.mout. This output control parameter varies between 0 and 4 and a higher value induces automatically more output. The level 2 is frequently used and recommended. For n =0, the output is strictly limited. Values above n =2 are restricted to debug purpose and are not recommended for practical applications.

  • -rotX: This parameter allows to turn around the common axis X by an angle of 90° the 2-D structured mesh of MICRESS, classically defined in the E_{X}-E_{Z} plane, in the e_{X}-e_{Y} plane of HOMAT or Abaqus (see Fig. 4). As the rotation angle is fixed here to 90° around the common X axis, only the parameter rotX has to be specified by the user for each 2D MICRESS simulation.

    Figure 4: MICRESS 2-D model (E_{X}, E_{Y}, E_{Z} axis system) rotated around the common axis E_{X} = e_{X} in the e_{X}-e_{Y} plane of HOMAT.

  • -cut Xmin Xmax Ymin Ymax Zmin Zmax: This optional keyword permits to reduce the size of the RVE for homogenization or virtual testing analyses. This option is interesting for some particular applications, for example, for the prediction of effective properties of a reactive air brazing microstructure. In fact, MICRESS discretized also the air phase, which, of course, is problematic in thermoelastic homogenization analyses. Therefore, option -cut allows to cut the outer air domain and to define mechanical rigid body motion fixations on filler nodes and not on air nodes 2.

    The parameters Xmin, Xmax, Ymin, Ymax, Zmin and Zmax represent the minimum and maximum coordinates of the reduced RVE in X, Y and Z direction respectively. These coordinates are provided in the specified unit length, per default mm. Mesh2XXX divides these coordinates by the grid spacing in order to evaluate the number of cells to remove before Xmin (or Ymin or Zmin) and after Xmax (or Ymax or Zmax) from the initial RVE.


    • This simple cutting algorithm can only be applied to structured meshes provided by MICRESS, but is not applicable to complex unstructured meshes generated by a finite element mesh generation program.

    • If the parameter -scal is specified, the user has to introduce the boundaries Xmin, ... of the reduced RVE in the scaled geometry definition.

    • If parameter -rotX is specified in the same time as the -cut option for a 2-D model, the rotation around the common axis X is performed first. Then, the cutting algorithm is applied. Therefore, it is mandatory to specify the cutting parameters in the ABAQUS or HOMAT X-Y plane, where the homogenization or virtual test will be performed.

    • In the scientific notation the cutting coordinates Xmin, ... have to be specified as 1.4E-04. A definition as 1.4D-04 will be ignored and leads to an input error.

  • -input_format name: This optional keyword allows Mesh2XXX to know directly the origin of the specified VTK or INP file. The mandatory parameter name corresponds then either to mesh2abaqus, digimat or neper-gmsh for an inp input file, or to micress, sphaerosim or homat, in the case of a vtk input file. Note that the new combined name neper-gmsh handles inp files generated either by the polycrystal mesh generator NEPER or directly by the F.E. mesh generator Gmsh. If the parameter homat is specified, Mesh2ABAQUS starts by automatically suppressing the generated interface elements. The parameter digimat specifies here the commercial program Digimat-FE, which can be used in combination with Abaqus to generate and analyse a 3-D finite element model of a synthetic microstructure. The parameter sphaerosim stands for the 3D cellular automaton program SphaeroSim 3 which predicts the microstructure evolution of semi-crystalline thermoplastics.

    In the different inp files formats a lot of additional elsets, nsets and other more specific input data for a problem definition exist. By specifying the .inp format of Abaqus, Mesh2Homat is able to read and treat only the HOMAT relevant information (keywords: nodes, solid section,...). Additional information (keywords: tie, equation,...) are ignored at the moment.

    Remark: If the considered microstructure comes from Micress, directly via grain structure file .korn or via a VTK file, or generated by Neper or Gmsh, than Mesh2XXX searchs for the presence of a grain orientation file, named PROBLEM_NAME.TabO. This orientation file can by either written directly by Micress or generated by a dedicated Python script, named If a TabO file is specified, then Mesh2XXX replaces the redundant definition of material properties per grain by a material definition per phase, which is more concise in the command file PROBLEM_NAME.hin and achieves the grain orientation definition either for Mesh2HOMAT or Mesh2ABAQUS.

  • -mod2D n: For a 2-D microstructure, this optional parameter permits to specify directly the nature of the 2-D homogenization analysis within HOMAT or of the virtual tests within ABAQUS. Since the version 5.3, the user can specify for a 2D microstructure, generated by MICRESS, not only plane strain or plane stress analysis, but also a 2-5D analysis. The 2.5-D analysis is in fact a 3D homogenization analysis or virtual tests on a geometric 3D model having only one hexahedral element in its thickness. Following syntax is adopted here:

    • n = 0: 2-5D analysis within HOMAT or ABAQUS,

    • n = 1: plane strain analysis within HOMAT or ABAQUS,

    • n = 2: plane stress analysis within HOMAT or ABAQUS.


    • If this optional parameter is introduced by the user, its value prevails and overwrites the value, defined initially in the inp file of the microstructure.

    • For already specified 2D plane stress or strain models in an inp input file, only the options n=1 (plane strain) or n=2 (plane stress) are active. In the special case of desired 2-5D analyis, please convert your inp file at first in a VTK one, then you can specify mod2D = 0 and perform a 2-5D analysis.

  • -check_nodes: This option is only active for a VTK file, coming from a previous homogenization analysis with HOMAT. This new option checks the presence of additional nodes, having same coordinates as the original node, and removes them from the model. This way, a geometrical model already used in HOMAT can be reused for nonlinear homogenization via virtual tests in Abaqus.

  • -output: This new parameter allows the user to specify the base name, common to the command and geometry output files, written by Mesh2XXX.

Mesh2XXX has no influence on the desired discretization degree of the finite element model of the RVE. The user has to specify this degree in the adopted mesh generation tool, namely Abaqus CAE, Gmsh, Neper or Digimat. Per default, linear element formulations are adopted. But, since version 6.0, quadratic volume elements with either 10 (tetrahedron), 15 (pentahedron) or 20 nodes (hexahedron) can be specified in these FE microstructure generation tools. In this case, the displacement field and the geometry of each volume element are both quadratic. This way, a more accurate geometrical representation, for example, of cylindrical or spherical inclusions in the RVE, is achieved. Both microstructure evolution tools Micress and SphaeroSim generate in Mesh2XXX structured, voxelized meshes and are not concerned by this new feature. Indeed, for these two programs, Mesh2XXX generates only FE models with linear hexahedrons of the discretized microstructure.

The following parameters are specified only in combination with MICRESS results and are not relevant for other HOMAT and ABAQUS analyses.

  • -time sim_time: this keyword defines the simulation time of the transient phase-field simulation which is selected for a homogenization analysis. The value sim_time is expressed in sec. If the parameter sim_time is not specified, Mesh2XXX sets sim_time = 0.0 and extracts the initial microstructure.

    Note: If the specified simulation time does not correspond to a saved time in the PROBLEM_NAME.korn file, Mesh2XXX will then select the time nearest to the specified one.

  • -timestep nbr: This keyword allows an alternative definition of the selected microstructure RVE. Indeed, the user has to introduce the number of the selected time step in the list of the saved grain configurations of MICRESS. For example, in the PROBLEM_NAME.korn file MICRESS saves the current microstructure each 5 sec until 30 sec and then each 2 sec until 50 sec. In this case, the user specifies -time step 9 to select the time step corresponding to the simulation time 36 sec.

Note If neither -time nor -timestep are specified, Mesh2XXX extracts the initial microstructure per default. Therefore, the specification of either -time or -timestep is mandatory for the selection of any other transient microstructure or to select the final configuration state.

Remark: Since version 6.0 Mesh2XXX introduces named place holders instead ‘...' for the name of an unknown material: NAME=material_<Nr> on the keyword /MATERIAL of HOMAT or on the keyword *MATERIAL of Abaqus. In the case of unknown phases, NAME=ph_<Nr> is written then in the keyword /MATERIAL of HOMAT or in keyword *MATERIAL of Abaqus. Note that in both cases <Nr> corresponds to the number of the actual material or phase.

Specific features and commands of Mesh2HOMAT

Mesh2HOMAT detects automatically the interfaces between different material domains as well as the outer free surfaces on which periodic boundary conditions can be defined. Moreover, for each spatial direction, it specifies the linked free surfaces and evaluates the translation distance between the linked surfaces. In order to define the periodic boundary conditions, Mesh2HOMAT needs to know the nature of the microstructure periodicity: either 3D, 2D or 1D. In the case of 2D and 1D periodicity, the notion of periodic directions is also mandatory.

  • The keyword -per type, where type can be either 3D, 2D, 2D_XZ, 2D_YZ, 1D, 1D_Y, 1D_Z allows the definition of the nature of the periodicity boundary conditions:

    • 3D is the default option and implies Mesh2HOMAT to realize a link between the faces X- (smallest X coordinates) and X+ (largest X coordinates), then a link between Y- and Y+ faces and eventually a link between the Z- and Z+ faces of the RVE.

    • 2D specifies a 2-D periodicity in the directions X and Y. If the 2-D periodicity is not defined respective to the X and Y directions, the two other parameters 2D_XZ and 2D_YZ allow the definition of the corresponding periodic B.C.

    • 1D similarly specifies a 1-D periodicity in the X direction, for example of the ferrite-cementite bi-lamella of the pearlite phase (see Ref. 4). Again, variants 1D_Y and 1D_Z allow the definition of 1D periodicity in the Y and Z direction respectively.


    • If the keyword -per is omitted, Mesh2HOMAT defines 3D periodic B.C. on the microstructure per default.

    • Mesh2HOMAT detects the oblique parallel faces of the RVE's of the cooled multilayer plate (see Fig. 5) and evaluates the translation in X direction. But, it is not able to treat any kind of oblique parallel faces in the 3D space. Moreover, the application of Mesh2HOMAT is restricted to microstructures of cubic or parallelipedic shape, hexagonal unit cells, like the unidirectional reinforced composite with staggered fibres (see Fig. 6), are not treated at the moment.

Figure 5: Inclined RVE of cooled multilayer plate composed a thermal barrier coating, a bondcoat and a superalloy substrate.

Figure 6: The hexagonal unit cell of unidirectional reinforced composite.

  • -all_free_surfaces: This new option permits to write not only the periodic surfaces on the RVE but also all other outer surfaces. Their nomenclature is the same as for the coupled periodic surfaces, namely X+, X-, Y-, Y+, Z+, Z-. This way, in the near future, other types of boundary conditions (Dirichlet, Neumann, inlet or outlet pressure, ..) can by specified on the RVE and use in specific problems, mainly in Stokes flow problems.

  • -write_vtk [ no_clones ]: If this keyword is introduced on the command line or in a small driving file for Mesh2HOMAT, the program writes the unstructured mesh of the microstructure geometry in VTK format. Per default, by omitting the optional parameter no_clones, it contains the newly generated nodes at the interfaces and the corresponding additional interface elements. Compared to the smaller initial structured mesh of MICRESS(korn or VTK format), this unstructured mesh has the advantage to show accurately the material discontinuities at the domains, phase or grain boundaries, but its size is larger. Therefore, per default (keyword data_type not specified), a binary VTK file is written. This way, its size is reduced.

    Since version 6.0, the additional parameter no_clones permits to write a vtk file of the unstructured mesh, but without the newly generated nodes at the material interfaces and without the corresponding additional interface elements. This way, a simple Abaqus2Vtk mesh converter has been achieved.

  • -data_type ascii | binary: This additional keyword takes only effect in combination with the keyword write_vtk and specifies the overall VTK data format: binary or ascii. As already mentioned the binary format is adopted for the VTK file per default. Note that the ascii variant is mainly helpful in debugging mode and is not recommended for the user.

  • -discre options: In order to discretize quasi-incompressible materials in the thermo-elastic or in the Stokes flow homogenizations, several mixed linear finite element formulations have been implemented in HOMAT version 6.0. The optional parameter -discre can be used to specify a specific element type per recognized material. That can be e.g. an element set from an Abaqus input file, grains from a MICRESS result file, or phases if the according orientation file with phase information (TabO) is given. Following nomenclature is introduced:

    • C: classical linear displacement field per volume element. This element version is used mainly to discretize compressible materials and domains in thermo-elasticity and solid domains in Stokes flow homogenization.

    • E: equal order volume elements of tetra-, penta- or hexahedral type. These elements are discretized by a bilinear displacement/velocity field and by a linear pressure field. These elements are not stabilized. Therefore, their use is restricted to academic benchmark tests and not recommended for practical applications.

    • L: equal order volume elements, with bilinear displacement/velocity and pressure fields. According to the formalism of Li & He 5, the pressure field is stabilized via a double Gauß point integration.

    • M: the bilinear displacement/velocity field is enhanced via a volume bubble mode; whereas the pressure field remains linear. Arnold et al. 6 have demonstrated that the corresponding tetrahedral element, named Mini element, is always stable; whereas the corresponding penta- and hexahedral versions are not stable. Therefore, only the tetrahedral mini element is recommended for use in applications.

    • B: element variants dotted with an enhanced bilinear displacement/velocity field and a linear pressure, which is stabilized by double Gauss point integration. Benchmark tests for quasi-incompressible materials in mechanics and for Stokes flow outline their accuracy and robustness. Therefore, this mixed stabilized element formulation is recommended to model the quasi-incompressibility of materials or fluids.


    To specify the desired element type per grain and domain following nomenclature is used

    -discre "C = 1-21, 35, 45-60 ; B = 22-34 ; L = 36-44"

    The use of quotation marks " " allows the user to define different element options separated by blanks. The different specified element types are separated always by a semi-colon (;). In the present example, the classical element version C is adopted for domains/grains ranging from 1 to 21, for domain 25 and for the grains/domains in the range 45 to 60; whereas the enhanced stabilized version B is adopted for grains, numbered from 22 up to 34, and the stabilized equal order version L for grains numbered from 36 to 44.


    • If the parameter discre is omitted, all grains/domains are discretized by classical linear elements.

    • By default, the element version C is adopted for the solid grains and domains; whereas the enhanced mixed element version B is set, per default, for a melt region (i.e. material 0 for MICRESS default liquid phase 0). Taking these default settings into account, following element discretization definition is equivalent to the precedent one:

      -discre "B = 22-34 ; L = 36-44"

      Using phases, e.g. melt/liquid (phase 0) and austenite/FCC (phase 1):

      -discre "B = 0 ; L = 1"
    • Please check that the grain/domain number used in this discretization definition corresponds to the solid section number in the command .hin file.

  • -problem type this new optional parameter permits the user to specify already in Mesh2HOMAT the kind of homogenization or localization analysis he desires to perform in HOMAT. The list of the possible analysis types is outlined in Tab. 1. This way, not only the parameter TYPE of the general keyword /PROBLEM (see HOMAT manual) but also, per solid section, the analysis type is set and a preselection of the written microscopic result fields is done (see keyword /OUTPUT of the HOMAT manual for more details). Per analysis type, following predefinitions are realized:

Table 1: Predefinition per adopted homogenization or localization analysis of the desired analyses for each solid section of the RVE. Moreover, per analysis type, a preselection of the microscopic result fields is given.

type Solid Section Output
THELAS TEMP=NO, MECH=HOM, FLUID=NO U, (P, for mixed elements)
MECHAN TEMP=NO, MECH=HOM, FLUID=NO U, (P, for mixed elements)
THERMEC TEMP=HOM, MECH=HOM, FLUID=NO T, U, (P, for mixed elements)

Specific features and commands of Mesh2ABAQUS


As already mentioned in the introduction, this program has two variants. The first one allows the transformation of a finite difference or finite element discretization of the microstructure provided either in a VTK, UNV or MICRESS format in a suitable format for ABAQUS. The corresponding ABAQUS input file, named NAME.inp, contains all nodes, elements and solid sections of the microstructure RVE; but no specific element and/or node sets, boundary or loading conditions.

The second more relevant aim of Mesh2ABAQUS is to generate the six (or three in 2D) input files necessary to perform uniaxial virtual tests of the selected microstructure RVE within ABAQUS. The program generates also the required periodic boundary conditions. To achieve this task, Mesh2ABAQUS distinguishes between corners, inner edges and inner face nodes. Specific multi-point constraints are expressed for each node category. A detailed theoretical description of the formalism can be found in Ref. 7. As the mesh can be different on corresponding RVE faces, for example in an extracted unit cell of a material with a random microstructure, a special procedure has been developed here: a copy of the selected surface is translated to the opposite surface and a constraint equation is defined between the surface and its own copy. Afterwards, the copy is tied to the opposite surface. Since program version 5.3, for 2-D structured meshes coming from MICRESS, this fastidious general procedure is skipped and the multi-point constraints are directly written for the linked surfaces and wedges.

As Mesh2ABAQUS transforms and/or manipulates only meshes, no information about the considered material laws is avalable. The user has to supply this information afterwards by adding explicitly specific material files to the ABAQUS input file. Moreover, if a known temperature distribution on the RVE is required by the analysis, the user has to supply them via the *INITIAL CONDITIONS keyword of ABAQUS. In order to reduce the size of the six or three input files, a first file containing all geometric information (nodes, elements, solid sections, node sets formed of corner, inner edge and inner face nodes,...) is written with the name PROBLEM_NAME.geom. This file is common to the six or three (2-D case) generated ABAQUS input files and is included in each of them. The generated input files have the naming convention PROBLEM_NAME_ij.inp, where ij takes the values xx, yy, zz, xy, xz, yz in 3-D and xx, yy and xy in 2-D. Mesh2ABAQUS is able to distinguish automatically between 3-D (default case) and 2-D RVEs of MICRESS type or other. As the 2D MICRESS simulation is performed in the X-Z plane, the use of keyword -rotX is mandatory to rotate this plane around the common axis X to the classical X-Y plane of Abaqus. Moreover, in 2-D case some empty node and surface sets are automatically removed and the corresponding multi-point constraints are omitted.

In order to reduce the computational time of ABAQUS, the 8 node linear hexahedron element C3D8R with reduced integration is specified per default for 3D and 2.5-D virtual tests, specified via mod2D=0. To avoid possible hourglass modes a specific section control keyword is written, per default, by Mesh2Abaqus. It specifies automatically an enhanced hourglass control of the global stiffness within ABAQUS/STANDARD. Moreover, this element choice is more suitable for ABAQUS simulations based on MICRESS results, as the unique Gauss point of hexahedral element coincidences with the cell centre of the MICRESS structured mesh. Thus, no additional interpolation is needed and no accuracy is lost by the transfer of cell results like the dislocation density to the Gauss points of the mechanical ABAQUS model.

In order to fix the rigid body motion of the RVE, the node Point_1 is completely fixed. Depending on the considered uniaxial test case, additional prescribed nodal displacements are applied automatically in Point_2, Point_4 and Point_5 in 3D (see Fig. 7, left); whereas only Point_2 is fixed in the Y direction for 2D analysis (see Fig. 7, right).

Remark: The input mesh can be generated by any mesh generation program and, of course, by ABAQUS CAE. Therefore, the inp format is also considered as possible input format for the virtual test variant of Mesh2ABAQUS. This input file can be produced also by the first program version of pure mesh format transformation.

Figure 7: Parallelepiped RVE with faces parallel to the structural axis and its corner nodes numbering.

Program limitations:

  • Only parallelepiped RVE's with outer faces parallel to the structural axes are treated by Mesh2Abaqus. Neither oblique parallel faces, accepted in Mesh2Homat, nor hexagonal RVE's are analysed at the moment.

Specific commands

Running the program without any argument is possible and provides a small concise help menu of the required arguments. Depending on the adopted program version, the user specifies following command line.

a) Variant 1: mesh format transformation

Mesh2ABAQUS PROBLEM_NAME.(vtk|unv|inp) -vtest 0

or for MICRESS files

Mesh2ABAQUS PROBLEM_NAME.korn -vtest 0 -time 30.0

or, alternatively,

Mesh2ABAQUS PROBLEM_NAME.korn -vtest 0 -timestep 6

The name and type of the mesh are mandatory. The parameter -vtest has to be specified to 0 if the generation of inp files for virtual testing is not desired. Especially after a multi-phase field analysis with MICRESS, the user has also to define either the simulation time or the number of the selected time step. Per default, the initial microstructure is considered.

b) Variant 2: virtual uniaxial testing

Mesh2ABAQUS PROBLEM_NAME.(vtk|unv|inp|korn) -vtest P -deltaL eps -step L -maxincsize Inc -time sim_time

or alternatively

Mesh2ABAQUS PROBLEM_NAME.(vtk|unv|inp|korn) -vtest P -deltaL eps -step L -maxincsize Inc -timestep nbr
  • -vtest P: the parameter P of the keyword -vtest specifies the nature of the considered virtual tests:

    • P = 1: (default value) all six (or three in 2D) inp files are written in order to perform with ABAQUS the uniaxial tensile, compression and shear tests for the same total elongation;

    • P = 2: only the three (or two in 2D) extension tests are defined for the same total elongation;

    • P = 3: only the three (or the unique in 2D) shear tests are defined. This way, it is possible to specify directly a different elongation for the shear tests as for the tensile or compression ones.

  • -deltaL eps: The real value eps attached to keyword -deltaL specifies the desired total elongation strain of the unit cell in each structural direction respectively. It is expressed in %. For an RVE with different X, Y and Z sizes, a specific total displacement is calculated in each direction in function of the specified total elongation strain. Per default, a strain of 1% is adopted.

  • -step L: As no information about the involved nonlinear material laws is available in the program, the total strain defined via keyword -deltaL is subdivided simply in L equal displacement increments. Per default, L = 1: only one step is specified.

  • -maxincsize Inc: This new parameter allows the user to adapt the maximal allowed increment size per step to the nonlinearity of the adopted material laws of the RVE model. Per default, Inc = 0.05, leading to 20 increments for the defined step.

  • -mod2D n: Mesh2ABAQUS specifies automatically in the case of a 2D plane strain analysis (=-mod2D=1) elements of CPE4R type, if linear shape functions are specified in the initial geometrical model, or elements of type CPE8R for a quadratic displacement field discretization. Note that both adopted element types are under-integrated element versions and hourglass control is achieved by adding automatically the section control keyword with enhanced hourglass control in the ABAQUS model file PROBLEM_NAME.geom. On the other side, if -mod2D=2 (plane stress analysis) is set, Mesh2ABAQUS writes, depending on the element discretization degree, automatically elements of type CPS4R or CPS8R in the model file PROBLEM_NAME.geom. The written element type came from the element degree of the initial model.

    Remark: The new option -mod2D=0 of 2-5D analysis allows to derive effective flow curves under a more realistic stress/strain state than both extreme situations: either a 2-D section of an infinitively thick polycrystal (plane strain assumption with \varepsilon_{zz} = 0.) or a 2-D thin film of polycrystal (plane stress assumption with \sigma_{zz} = 0). In reality, neither \varepsilon_{zz} = 0 nor \sigma_{zz} = 0., so that both extreme 2-D situations define an upper (plane strain case) and lower bound (plane stress case) of the unknown effective flow curve respectively. Of course, such a 2-5D investigation requires more CPU time and space as 3D hexahedral elements are used in the virtual uniaxial tests.

Remark: The parameter -time 0 has to be specified for a Mesh2ABAQUS run without coupling to MICRESS, in the case if you want to specify the orientation of each grain of the RVE via a TabO file generated by the Python script This Python script generates uniformly distributed random grain orientations of quaternion type, by applying the Halton sequence procedure 8.

  1. Dassault Systèmes Simulia Corp. Abaqus Finite Element Analysis, User manual. Providence, RI, USA, 2019. 

  2. Markus Apel, Gottfried Laschet, Bernd Böttger, and Ralf Berger. Phase Field Modeling of Microstructure Formation, DSC Curves, and Thermal Expansion for AgCu Brazing Fillers Under Reactive Air Brazing Conditions. Advanced Engineering Materials, 1612:1468–1474, 2014. _eprint: doi:10.1002/adem.201400101

  3. Gottfried Laschet, Hamed Nokhostin, Simon Koch, Marc Meunier, and Christian Hopmann. Prediction of effective elastic properties of a polypropylene component by an enhanced multiscale simulation of the injection molding process. Mechanics of Materials, 140:103225, January 2020. doi:10.1016/j.mechmat.2019.103225

  4. G. Laschet, P. Fayek, T. Henke, H. Quade, and U. Prahl. Derivation of anisotropic flow curves of ferrite–pearlite pipeline steel via a two-level homogenisation scheme. Materials Science and Engineering: A, 566:143–156, March 2013. doi:10.1016/j.msea.2012.12.064

  5. Jian Li and Yinnian He. A stabilized finite element method based on two local Gauss integrations for the Stokes equations. Journal of Computational and Applied Mathematics, 2141:58–65, April 2008. doi:10.1016/

  6. D. N. Arnold, F. Brezzi, and M. Fortin. A stable finite element for the stokes equations. CALCOLO, 214:337–344, December 1984. doi:10.1007/BF02576171

  7. Ghayath Al Kassem and Dieter Weichert. Micromechanical Material Models for Polymer Composites through Advanced Numerical Simulation Techniques. PhD thesis, Publikationsserver der RWTH Aachen University, Aachen, 2010. 

  8. J. H. Halton. On the efficiency of certain quasi-random sequences of points in evaluating muti-dimensional integrals. Num. Math., 2:84–90, 1960.