This mapping option enables the transfer of stresses, strains, and temperatures from solid meshes to LS-DYNA meshes. Therefore, the source file may contain *INITIAL STRESS/ STRAIN SOLID cards and *INITIAL TEMPERATURE NODE.
It is also possible to transform the source file to match the target mesh.
This section covers:
| SourceFile = STRING |
Define the name and, if needed, the path of the source file, usually a *.dynain file. |
| 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 to this newly generated file. |
| TransformedMeshFile = STRING |
Define the file name where the transformed mesh is written. This option is for the transformation's post-processing only. For further information, see Transformation Options below. |
There are some options available for source, target, and result file formats:
| SourceFileFormat =LS − DYNA |
The source file format. LS-DYNA is the preferred format. |
| TargetFileFormat =LS − DYNA |
The target file format. LS-DYNA is the preferred format. |
| ResultFileFormat =LS − DYNA |
The result file format. LS-DYNA is the only accepted format. |
| NumTargetPIDs = INT | Specify the number of parts in the target mesh to be considered for mapping, 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 to be considered for mapping, 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 above options limit the scope of the mapping procedure to defined part IDs. Other parts are ignored on both the source and target side.
|
TRANSFORMATION = YES NO |
Turns the transformation option on or off. |
|
WriteTransformedMesh = YES NO |
Flag to enable the transformed mesh's output for mapping. This option enables you to control 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 4PCS with caution since it is fully automatic and might not transform stress-tensors and fiber orientations properly between the different coordinate systems. The ICP algorithm is recommended.
User-defined translation and rotation options are listed below after TRAFO_OPTION.
Note: Transformation options are used to transform the source mesh.
|
TRAFO_OPTION = 4PCS ICP | Flag for choosing a transformation option. |
| NodalPair#i = INT INT |
Define nodal pairs for initial mesh alignment for the ICP algorithm. Up to ten nodal pairs can be defined, and a minimum of three nodal pairs must be defined. The first integer refers to a node ID in the source mesh. The second integer refers to a node ID in the target mesh. The two IDs must be separated with a space, and each nodal pair must be on separate lines. |
| Additional Transformations = INT | Define the number of additional transformations to be done using the ICP algorithm. |
| AddTrafo#i = INT | Define as many additional transformation IDs as defined for Additional Transformations. INT represents the element set ID to add to the algorithm. |
| AddNodalPair#i = INT INT | Use this option to define 4 nodal pairs for additional mesh alignment for the ICP algorithm. |
| 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). |
|
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). |
Furthermore, you can specify a set of user-defined transformations to be performed. They are executed in the order of input:
|
RotateSRC =DOUBLE;X DOUBLE;Y DOUBLE;Z DOUBLE; DOUBLE DOUBLE DOUBLE | Rotates the source mesh at an angle (first value) in degrees around the defined axis. Predefined axis are X, Y, and Z. To use a user-defined axis, seperate three double values with a space, following a semicolon (;x y z). |
| MoveSRC = DOUBLE DOUBLE DOUBLE |
Moves the source mesh along a user-defined vector (x y z). |
| ScaleSRC = DOUBLE |
Scales the source mesh along the origin using the defined scale factor. |
In addition to the transformation options, you can 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 | Provide information about the source unit system if unit system conversion is activated. |
|
TargetUnitSystem =kg − m − s ton − mm − s kg − mm − ms g − mm − ms lb − in − s | Provide information about the target unit system if unit system conversion is activated. |
ALGORITHM =ClosestPoint
|
MapStress =YES NO | Activates or deactivates the mapping of stress data (every value stored in *INITIAL STRESS OPTION cards on the source side). The default algorithm is the closest point algorithm (or nearest neighbor search). See below for additional option details. |
|
MapStrain = YES NO | Specify if strains have to be transferred or not. |
|
MapTemperature = YES NO | Specify if temperatures are transferred or not. |
|
MapThickness =YES NO | Activates or deactivates thickness transfer. This option requires having *ELEMENT SHELL THICKNESS cards in the dynain file. If TargetThickness is defined, it is ignored. Default option is CP (closest point). Thickness mapping is based on the thicknesses stored on the nodes. Thickness is averaged over all elements attached to a node, regardless of the chosen interpolation option. The listed interpolation options function similarly to those described in MapStress. |
| TargetThickness = DOUBLE | Define the thickness in the target shell mesh. |
If the target mesh lacks details about integration rules like element formulation and through-thickness points, you must define them. The input is as follows:
| NPLANE = INT |
1 - Reduced integrated shell elements. 4 - Fully integrated shell elements. This option is formerly known as NumberOfTARInPlaneIPs. |
| NTHICK = INT |
Define the number of through-thickness integration points (IPs). |
|
IntegrationRule =Gauss Lobatto Autoform Moldflow | Define the through-thickness integration rule for the mapping result. This option directly affects the positions of the through thickness integration points on the target mesh. |
|
Search_Radius =SrcEleLen TarEleLen DOUBLE | Search radius declaration for the mapping algorithm. SrcEleLen is the default, which uses the average source mesh element size as a search radius. Average target mesh element size can be used by defining TarEleLen, or a positive DOUBLE value can be defined. |
| Scale_SearchRadius= DOUBLE | Coefficient to scale search radius. |
| SORT= BUCKET | Always use bucket sort for a significant speed-up of the search algorithm. |
| REPEAT= YES | Turn on this option to ensure that all elements and integration points receive some data. Depending on the size differences of the elements in source and target meshes, bucket refinement may be too small for all points to receive values. In those cases, you must define this flag. |