The option enables transferring Moldex3D orientation data for short and long fiber reinforced composites to solid meshes for further structural analysis.
Several options are available to handle short fiber reinforced composite materials with the LS-DYNA application. The Envyo program supports *MAT_ANISOTROPIC_ELASTIC_PLASTIC (*MAT 157) and output of *ELEMENT_SOLID_ORTHO cards for the use of other arbitrary orthotropic material models within the LS-DYNA application. Support for *MAT_4A_MICROMEC (*MAT 215) is also available.
For more information about the handling of short fiber reinforced materials with *MAT 157, see [11], [16], [15], and [10]. For more details on *MAT 215, see [21].
This section covers the following topics:
| SourceFile = STRING | Define the name and, if needed, the path of the source file. This must be a Moldex3D mesh that is translated into LS-DYNA format. |
| TargetFile = STRING | Define the name and, if needed, the path of the target file. This must be an LS-DYNA mesh. |
| MappingResult = STRING | Define the result file name. The mapping result is written into this newly generated file. |
| OrientationFile = STRING | Moldex3D - o2d files containing the fiber orientation tensor are considered. |
| InitialStressFile = STRING | Moldex3D - so2d files containing resulting stresses from Moldex3D simulation. If this option is active, stresses are also mapped. |
| WeldlineFile = STRING | If weldlines are considered, define the .nwd weldline-file which contains nodes and respective main angles with this option. With the MapWeldline flag, weldline consideration is activated, and a different part is assigned to weldline elements. You can define corresponding material parameters for these parts. |
| TransformedMeshFile = STRING | Specify the file name where the transformed mesh is written. This option is intended solely for postprocessing of the transformation. For additional details, refer to the Transformation Options section below. |
| NumTargetPids = INT |
Define the number of parts in the target mesh which are considered within the mapping. This option must be followed by TargetPid#i definitions. |
| TargetPid#i = INT | Define as many part IDs as given in NumTargetPids. These parts are considered for the mapping. |
| NumSourcePIDs = INT |
Define the number of parts in the source mesh which are considered within the mapping. This option must be followed by SourcePID#i definitions. |
| SourcePID#i = INT | Define as many part IDs as given in NumSourcePIDs. These parts are considered for the mapping. |
Note: The options above specifically narrow down the scope of the mapping procedure to defined-part IDs. Other parts are ignored on both the source and target meshes.
| TRANSFORMATION = YES/NO | Turns the transformation on or off. |
| TransformBack = YES/NO | Activates or deactivates transformation backward transformation. |
| WriteTransformedMesh = YES/NO | Flag to enable output of the transformed mesh for mapping. This enables verifying the success of the transformation. If set to YES, a TransformedMeshFile must be specified (see Input and Output Meshes ). |
There are three available methods for performing mesh transformation:
TRAFO_OPTION is required:
Iterative Closest Point (ICP)
Four-Points-Congruent Sets (4PCS)
TRAFO_OPTION is not required:
User-defined translation and rotation
The 4PCS method must be used with caution, as it is fully automatic and may not accurately transform stress tensors and fiber orientations between different coordinate systems. The ICP algorithm is the recommended approach.
The user-defined translation and rotation options are listed underneath TRAFO_OPTION.
Note: Transformation options are used to transform the source mesh.
|
TRAFO_OPTION = 4PCS ICP | Flag that enables specification of the desired transformation option. |
| NodalPair#i = INT INT | Define nodal pairs to initialize mesh alignment for the ICP algorithm. You may specify up to ten nodal pairs, with a required minimum of three. In each pair, the first integer represents a node ID in the source mesh, and the second corresponds to a node ID in the target mesh. Input values must be space-separated, with each nodal pair provided on a separate line. |
| MAX_NUM_ITER = INT | Maximum number of iterations to be performed by the 4PCS algorithm. |
| GLOBAL_ERR = DOUBLE | Global error measure to accept transformation as best fit 4PCS algorithm. |
| MATCHING_POINT_DIST = DOUBLE |
Maximum distance between points so that they are accepted as matching (4PCS). |
| PERCENTAGE_OF_MATCHING_POINTS = DOUBLE | Percentage of matching points to accept the transformation (4PCS). |
Additionally, a custom sequence of user-defined transformations can be applied. These transformations are executed in the order in which they are specified and multiple transformations may be defined:
|
RotateSRC = DOUBLE;X DOUBLE;Y DOUBLE;Z DOUBLE; DOUBLE DOUBLE DOUBLE | The source mesh rotates by a specified angle (first value, in degrees) around a defined axis. Predefined axes include X, Y, and Z. Alternatively, a custom axis can be specified by providing three space-separated floating-point values following a semicolon (; x y z). |
| MoveSRC = DOUBLE DOUBLE DOUBLE | The source mesh moves along the user-defined vector (x y z). |
| ScaleSRC = DOUBLE | The source mesh scales around the origin using the defined scale factor. |
In addition to the transformation options, there are options to convert the unit systems:
| ChangeUnitSystem = YES/NO | Activates or deactives unit system conversion. |
|
SourceUnitSystem = kg - m - s ton - mm - s kg - mm - ms g - mm - ms lb - in - s | If the unit system conversion is activated, provide information about the source unit system. |
|
TargetUnitSystem = kg - m - s ton - mm - s kg - mm - ms g - mm - ms lb - in - s | If the unit system conversion is activated, provide information about the target unit system. |
| ALGORITHM = ClosestPoint | The only available option is ClosestPoint. Values are mapped to the nearest node, integration point, or element center. |
|
Search_Radius = SrcEleLen TarEleLen DOUBLE | Specifies the search radius for the mapping algorithm. The default is SrcEleLen, which sets the radius to the average element size of the source mesh. Alternatively, you can use TarEleLen to apply the average element size of the target mesh, or provide a positive DOUBLE value to define a custom radius. |
| Scale_SearchRadius = DOUBLE |
Coefficient to scale search radius. The default value is 1.0. |
| INN = INT |
This flag is similar to the invariant node numbering flag in the LS-DYNA application provided in the *CONTROL_ACCURACY card, see [19]. To properly calculate orientations with respect to the element coordinate system, the program needs information about how the LS-DYNA application calculates the element coordinate system. The default is similar to the LS-DYNA application’s default: Off. |
|
OUTPUT_OPTION = INITIAL STRESS ONLY |
Only *INITIAL_OPTION cards are written to the mapping result file. Nodes and elements are skipped. |
| SORT = BUCKET |
Using bucket sort is strongly recommended, as it provides a substantial performance improvement for the search algorithm. |
| REPEAT = YES | Enable this option to ensure that all elements and integration points receive mapped data. When there is a significant difference in element sizes between the source and target meshes, the default bucket refinement may be insufficient to cover all points, sometimes by design. In such cases, this flag must be set to guarantee complete data coverage. |
|
TENSORIALINT = CENTER IP |
You can define the output of only the values mapped to the central integration points for higher order tetrahedral elements (NIPTETS = 5). The value mapped to this center integration point is distributed to the other integration points in a postprocessing step. |
The following cards are needed to define the output for *ELEMENT_SOLID_ORTHO cards for the LS-DYNA application. The mapped orientations are given by the main axis of the orientation tensor corresponding to the largest eigenvalue. This enables modeling with any arbitrary orthotropic material law available in the LS-DYNA application.
This section covers:
| SOLID_OPTION = ORTHO |
Activates the output of *ELEMENT_SOLID_ORTHO cards. |
| MapStress = NO |
Define if *INITIAL_STRESS_SOLID cards are written. For the *ELEMENT_SOLID_ORTHO option, set this flag equal to NO. |
| MapMainDir = YES |
Activates the mapping of the main directions onto *ELEMENT_SOLID_ORTHO cards. |
| ETYP = INT |
1 - Reduced integrated solid elements. 2 - Fully integrated solid elements. This accounts for hexahedral elements as well as for tetrahedral elements. ETYP = 1 activates the mapping to reduced integrated tetrahedral elements (LS-DYNA application ETYP 10 or 13), while ETYP = 2 activates the mapping to fully (4-point) integrated tetrahedral elements (LS-DYNA application ETYP 4, 16 or 17). The number of integration points for tetrahedral elements can also be changed with NIPTETS (see option below). |
| NIPTETS = 1 |
1 - Activates mapping to 1-point tetrahedral elements(LSDYNA ETYP 10 or 13). 4 - Activates mapping to 4-point tetrahedral elements (LS-DYNA application ETYP 4, 16, or 17). 5 - Activates mapping to 5-point tetrahedral elements (LS-DYNA application ETYP 4, 16, or 17). For the *ELEMENT_SOLID_ORTHO option, set this option equal to 1. |
|
MapWeldline = YES NO |
Define if weldlines are considered within the mapping. You must provide the respective Moldex3D *.nwd file. If MapWeldline = YES, define the following two cards: WeldlinePID and WeldlineRADIUS. |
| WeldlinePID = INT | Define the part ID that is assigned to weldline elements. |
| WeldlineRADIUS = DOUBLE | Define the radius for the weldline elements. This option enables adjusting the weldline radius so that the number of elements within the weldline zone can be distinguished and assigned weldline PIDs. If this option is not defined, Search_Radius and Scale_SearchRadius options are used to determine weldline zone. |
This section describes the available options for mapping of material properties for *MAT_ANISOTROPIC_ELASTIC PLASTIC (*MAT 157). The initial input is the same as the previous section, but with minor changes on the target options, and additional cards that are specifically for initializing material properties for (*MAT 157) with the *INITIAL_STRESS_SOLID card.
This section covers:
| TargetMaterialModel = 157 |
Specify the target material model corresponding to the LS-DYNA application’s material model manual [20]. The only available option here is 157. |
| MapStress = YES |
Define whether *INITIAL_STRESS_SOLID cards are written. If data should be made available for the *MAT 215 material model via *INITIAL_STRESS_SOLID cards, this option must be YES. |
| MapMainDir = NO |
Activate mapping of the main directions to *ELEMENT_SOLID_ORTHO cards. For usage with *MAT_215, this option is NO. |
| ETYP = INT |
1 - Reduced integrated solid elements. 2 - Fully integrated solid elements. This accounts for hexahedral elements as well as for tetrahedral elements. ETYP = 1 activates the mapping to reduced integrated tetrahedral elements (LS-DYNA application ETYP 10 or 13), while ETYP = 2 activates the mapping to fully (4-point) integrated tetrahedral elements (LS-DYNA application ETYP 4, 16 or 17). The number of integration points for tetrahedral elements can also be changed with NIPTETS (see option below). |
| NIPTETS = INT |
1 - Activates mapping to 1-point tetrahedral elements (LS-DYNA application ETYP 10 or 13). 4 - Activates mapping to 4-point tetrahedral elements (LS-DYNA application ETYP 4, 16, or 17). 5 - Activates mapping to 5-point tetrahedral elements (LS-DYNA application ETYP 4, 16, or 17). |
|
MapWeldline = YES NO |
Define if weldlines are considered within the mapping. You must provide the respective Moldex3D *.nwd file. If MapWeldline = YES, define the following two cards: WeldlinePID and WeldlineRADIUS. |
| WeldlinePID = INT | Define the part ID that is assigned to weldline elements. |
| WeldlineRADIUS = DOUBLE | Define the radius for the weldline elements. This option enables adjusting the weldline radius so that the number of elements within the weldline zone can be distinguished and assigned weldline PIDs. If this option is not defined, Search Radius and Scale SearchRadius options are used to determine weldline zone. |
| IHIS = INT |
Flag that defines the material parameter written to *INITIAL_STRESS_SOLID cards for *MAT_157, according to [20]. The following values are supported: |
|
IHIS = 1 - q-values are written to the first six history variables. | |
|
IHIS = 3 - q-values are written to the first six history variables, tensor components Cij are written on history variables #7 - #27. | |
|
IHIS = 11 - q-values are written to the first six history variables, tensor components Cij are written to history variables #7 - #27, table IDs for strain rate dependent plasticity are defined in history variable #28. | |
|
For IHIS = 1, no further input is required. | |
|
If IHIS > 1, define the following variables: | |
|
HomogenizationMethod = Halpin − Tsai Tandon − Weng Voigt Kukuri Mori − Tanaka_1 Mori − Tanaka_2 Mori − Tanaka_3 | Define the homogenization method used to calculate the unidirectional stiffness matrix. For further information about these methods, see [10] or [16]. |
|
ClosureApproximation = Linear Quadratic HybridA HybridB ORF ORS |
Define the closure approximation method used to calculate the 4th-order orientation tensor from the 2nd-order orientation tensor given by Moldflow. For further information about these methods, see [10] or [16]. ORF calls the orthotropic fitted closure approximation proposed by [12], distinguishing between different fiber interaction coefficients based on the equation provided in [7]. ORS refers to the orthotropic smooth closure approximation. |
The following elastic constants must be defined:
| E11F = DOUBLE | Fiber Young’s modulus in main direction. |
| E22F = DOUBLE | Fiber Young’s modulus in thickness direction. |
| RHOF = DOUBLE |
Fiber density. |
| PRBAF = DOUBLE |
Fiber in-plane Poisson’s ratio. |
| PRCBF = DOUBLE |
Fiber out-of-plane Poisson’s ratio. |
| G12F = DOUBLE |
Fiber shear modulus. |
| EM = DOUBLE |
Matrix Young’s modulus. |
| RHOM = DOUBLE |
Matrix density. |
| PRM = DOUBLE |
Matrix Poisson’s ratio. |
| AspectRatio = DOUBLE |
Fiber aspect ratio (length/thickness). |
| FiberVolumeFraction = DOUBLE |
Fiber volume fraction in percent. |
| InclusionShape =
Ellipsoidal Spherical Needle Disc |
Shape of the inclusions. |
If IHIS > 3, you must define several direction-dependent curve files, representing different strain rates, so that the strain-rate and direction-dependent plasticity can be defined. The following input can be given:
| NumberOfCurveFiles = INT |
Define the number of curve files to be read. |
| CurveFileName#i = STRING |
Define the name and, if needed, path of the curve files. This card must be written NumberOfCurveFiles times. |
| NumberOfDirections = INT | Define the number of directions to which the curve files belong. The recommended value for short fiber reinforced plastic materials should be 3 |
| Direction#i = DOUBLE | Define angles, relative to the direction of flow, used to generate the plasticity curves. Typical angles are 0◦, 45◦, and 90◦. This card must be written NumberOfDirections times. |
| NumberOfStrainRates = INT | Define the number of strain rates to which the curve files belong. |
| StrainRate#i = DOUBLE | Define the strain rates that are considered by the defined curves. This card must be written NumberOfStrainRates times. |
| StrainRate#iDirection#j = INT | Define the curve IDs that belong to the respective strain-rate/direction combination. This card must be written NumberOfDirections x NumberOfStrainRates times. |
This section describes the available options for mapping of material properties for *MAT_4A_MICROMEC (*MAT 215). The initial input is the same as above, with minor changes on the target options and additional cards that are specifically for initializing material properties for (*MAT 215) with the *INITIAL_STRESS_SOLID card.
This section covers:
| TargetMaterialModel = 215 | Define the ID of the target material model corresponding to [20]. It must be 215. |
| MapStress = YES | Define if *INITIAL_STRESS_SOLID cards are written. If the data is available for the *MAT 215 material model via *INITIAL_STRESS_SOLID cards, this option must be set to YES. |
| MapMainDir = NO |
Activates the mapping of the main directions onto *ELEMENT SOLID ORTHO cards. For the usage with *MAT 215, this option is set to NO. |
| ETYP = INT | 1 - Reduced integrated solid elements. 2 - Fully integrated solid elements. |
|
MapWeldline = YES NO |
Define if weldlines are considered within the mapping. You must provide the respective Moldex3D *.nwd file. If MapWeldline= YES, define the following two cards: WeldlinePID and WeldlineRADIUS. |
| WeldlinePID = INT | Define the part ID that is assigned to weldline elements. |
| WeldlineRADIUS = DOUBLE | Define the radius for the weldline elements. This is a scale factor based on the average element size of the component, which enables adjusting the number of elements that are considered within the weldline zone. |