This option enables the transfer of stresses and strains from stacked solid meshes to shell meshes.
This section covers the following topics:
| SourceFile = STRING |
Defines the name and, if needed, the path of the source file (usually a *.dynain file). |
| TargetFile = STRING |
Defines the name and, if needed, the path of the target file. The target file must be an LS-DYNA mesh. |
| MappingResult = STRING |
Defines the result file name. The mapping result is written into this newly generated file. |
|
OrientationFile = HISV Nodes |
Define this flag to enable the transfer of orientations. It informs the program that the orientation data is stored within the history variables (HISV). Alternatively, orientations can be derived from the element nodes. This method may yield accurate results if the mesh is well-aligned initially. |
| TransformedMeshFile = STRING |
Specifies 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 below. |
The following are available for source, target, and result file formats:
|
SourceFileFormat = LS − DYNA ESI − PC Nastran HDF5 ESI − HDF5 GCODE ABAQUS STEP CSV | The source file format. The preferred format is LS-DYNA. |
| TargetFileFormat = LS − DYNA | The target file format. The only format available is LS-DYNA. |
| ResultFileFormat = LS − DYNA |
The result file format. The only format available is LS-DYNA. |
| NumTargetPIDs = INT | Defines 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 | Defines as many part IDs as given in NumTargetPIDs. These parts are considered for the mapping. |
| NumSourcePIDs = INT | Defines 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 | Defines 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 source and target meshes.
| TRANSFORMATION = YES/NO |
Turns on or off the transformation option. |
| WriteTransformedMesh = YES/NO |
Flag to enable output of the transformed mesh used for mapping. This enables verifying the success of the transformation. If set to YES, you must define a TransformedMeshFile (see Input and Output Meshes). |
Mesh transformation is possible with three options:
TRAFO_OPTION is required:
Iterative Closest Point (ICP)
Four-Points-Congruent Sets (4PCS)
TRAFO_OPTION is not required:
User-defined translation and rotation
Use the 4PCS method with caution, since it is fully automatic and may not accurately transform stress tensors and fiber orientations between the different coordinate systems. As a result, 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 | Defines nodal pairs to initialize mesh alignment for the ICP algorithm. You may specify up to ten nodal pairs, with a minimum of three required. 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 messure 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 axis 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, you can convert the unit systems:
| ChangeUnitSystem = YES/NO | Activates or deactivates 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, provides 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, provides 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. By default, SrcEleLen is used, 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. |
| MapStress = YES/NO | Activates or deactivates stress mapping. |
| MapStrain = YES/NO | Activates or deactivates strain mapping. |
| MapThickness = YES/NO | Defines if the thicknesses mapping transfers between meshes. This option requires *ELEMENT SHELL THICKNESS cards in the dynain file, and overrides TargetThickness. |
| TargetThickness = DOUBLE | Defines the thickness in the target shell mesh. |
| NPLANE = INT |
1 - Reduced integrated shell elements 4 - Fully integrated shell elements This option is formerly known as NumberOfTARInPlaneIPs. |
| NTHICK = INT | Defines the number of through-thickness integration points (IPs). This option is formerly known as NumberOfTARThroughThicknessIPs. |
|
IntegrationRule = Gauss Lobatto Autoform Moldflow | Defines the through thickness integration rule of the mapping result. This option directly effects the positions of the through thickness integration points on the target mesh. |
| 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. |