This option transfers stresses, strains, history variables, and masses from 2D shell meshes onto 3D shell meshes with a user-defined axis for the rotation. Transferring masses creates *ELEMENT MASS cards on the result mesh. Furthermore, there is an option to map the 2D shell mesh thickness to the 3D shell mesh by using the distance between the outer edges of the 2D source mesh as the 3D shell mesh's thickness value. This output creates *ELEMENT SHELL THICKNESS cards.
An offset angle can also be defined, which significantly speeds up the mapping process, but may cause significant inaccuracies of chosen to large.
This section covers:
| 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 application mesh. |
| MappingResult = STRING | Defines the result file name. The mapping result is written into this newly generated file. |
|
OrientationFile = HISV Nodes | To enable the transfer of orientations, define this flag. 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 was 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 section below. |
The following are available source and result file formats:
| SourceFileFormat = LS − DYNA |
The source file format. The only format available 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 above options narrows the scope of the mapping procedure to defined part IDs. Other parts are ignored on both source and target side.
|
TRANSFORMATION = YES NO |
Turns on or off the transformation option. |
WriteTransformedMesh = YES NO |
Flag to enable the output of the transformed mesh used 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
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 specifying a 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 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 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, 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 Interpolation | The default option is ClosestPoint. Values are mapped to the nearest node, integration point, or element center. |
As an alternative, you can select between different scalar interpolation techniques. These techniques are defined using the command SCALARINT (see below). Scalar averaging techniques only affect history variables and the effective plastic strain. Stress and strain tensors are transferred with the ClosestPoint method.
|
SCALARINT = AVG SHEPARD NO1 SHEPARDNO2 SHEPARDNO3 SHEPARDNO4 FE FE_NODAL_AVG |
The AVG method calculates the standard average values from the number of found points, without including distances or directions. No interpolation is performed. SHEPARD NO1 includes a simple distance weighting function to the standard averaging technique. SHEPARD NO2 is similar to SHEPARD NO1, but differentiates a minimum of four points and a maximum of ten points found within a specific search radius. |
Depending on the distance between the source and target points, a little difference is made between the weighting functions. SHEPARD NO3 now includes the direction of the points from a target points perspective and SHEPARD NO4 also determines the slope between the interpolated points. The basic theory for this implementation is provided by [22] and is extended to 3D for usage within Envyo.
The standard FE interpolation method makes use of the FE shape functions. In this case after rotating the source mesh towards the target integration point, the Envyo application determines the position of the target integration point within the source element in local coordinats ξ and η. The integration point values are extrapolated to the nodes, and from there interpolated onto the target integration point.
The enhanced FE NODAL AVG also calculates the local coordinates ξ and η after rotating the source mesh onto the target integration point. In addition to the extrapolation onto the nodes of the source mesh, values of connected elements are also extrapolated to these nodes. The nodal average is calculated and then, interpolation onto the target integration point is performed. Both FE interpolation methods are for now only active for scalar values, namely the equivalent plastic strain and history variables.
|
Search_Radius = SrcEleLen TarEleLen DOUBLE | Declares search radius for mapping algorithm. SrcEleLen is default, which uses average source mesh element size as the search radius. You can use average target mesh element size by defining TarEleLen, or a positive DOUBLE value. |
| Scale_SearchRadius= DOUBLE |
Coefficient to scale search radius. The default value is 1.0. |
| Search_Radius Mass = DOUBLE | Double value which defines a specific search radius for mass mapping. All mass elements found within this specific range are mapped. |
| Shepard Exponent = DOUBLE | Double value which defines the exponent for the Shepard’s distance weighted functions as used for the scalar interpolation methods SHEPARD NO1 through SHEPARD NO4. |
| NTHICK = INT | Number of through-thickness integration points in the target mesh. |
| NPLANE = INT |
1 - Reduced integrated thick shell elements. 4 - Fully integrated thick shell elements. |
|
IntegrationRule = GAUSS LOBATTO AUTOFORM MOLDFLOW | You can choose between different predefined through-thickness integration rules. Further integration schemes can be added upon request. |
|
MapStress = YES NO | Activates or deactivates stress mapping. |
|
MapStrain = YES NO | Activates or deactivates strain mapping. |
|
MapThickness = YES NO | Activates or deactivates thickness mapping. |
| TargetThickness = DOUBLE | If thickness is not defined or mapped, you can define a target thickness with this option. |
|
MapMass = YES NO | Activates or deactivates mass mapping, and creates *ELEMENT MASS cards. |
| Shell_Option = BETA
COMPOSITE COMPOSITE LONG | Defines shell output. Defining shell output is optional. |
|
OUTPUT_OPTION = INITIAL STRESS ONLY |
Only *INITIAL OPTION cards are written to the mapping result file. Nodes and elements are skipped. |
|
RotationAxis = X Y Z x y z | For this option, you must define a rotation axis for the source mesh. The rotation axis may correspond with any global coordinate system axis (X Y Z), or a custom orientation axis with vector coordinates seperated by spaces. Per default, this vector is attached to the point of origin (0 0 0). |
| ORIGIN = x y z | You can define an additional origin point for the rotational symmetry axis. The default is (0 0 0). |
| ANGLEOFFSET = DOUBLE | Defining ANGLEOFFSET speeds up the mapping process. Based on the offset angle, different meshes are created and mapping is performed for a specific number of elements or integration points. If the offset angle is too large, information is lost. There is no reccomended value, because the default is already a compromise between accuracy and speed, which is dependent on source and target mesh size. |
| 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. |