Transferring Mesh to Mechanical Solvers
If using Workbench and transferring to a downstream Mechanical solver, the software will transfer geometry and mesh data as follows:
Meshed bodies that have been suppressed for physics will not be transferred to the downstream systems.
Note: For models with multiple bodies in a single component, when transferring the mesh to Mechanical solvers, one or more bodies may lose material assignments when the geometry is updated and transferred again. For example, if a previously suppressed body is activated for physics and the mesh is transferred to the downstream Mechanical solver, the body may lose its material assignment. You can identify such tree objects by filtering the tree with the Scoping option set to Partial.If a part has not been meshed, it will transfer to Mechanical as an unmeshed body.
- In Mechanical, the Transfer Properties: Source will display as SpaceClaim.
- In Mechanical, any unmeshed body will have its state set as unmeshed. Such bodies will follow the typical Mechanical meshing workflows wherein if you generate a mesh, only unmeshed bodies will be meshed.
If a part has been meshed, the block topology (bodies, faces, edges, vertices) will be transferred to Mechanical as geometry. The associated mesh is also transferred.
The body icon in the structure tree will indicate the geometry is suppressed
.- Block materials are used to define the bodies in Mechanical.
- Quadratic element mid-side nodes are added to the mesh in the transfer to Mechanical, if applicable.
- In Mechanical, the Transfer Properties: Source will display as SpaceClaim Meshing.
- In Mechanical, any meshed body will have its state set as meshed.
To generate the body mesh, right-click Blocking in the Structure tree and select Body Mesh. You can also write the mesh data to a file using the Save option and selecting the appropriate format. The Fluent export options can be set in the SpaceClaim Options window.
You cannot use SpaceClaim as an external CAD system for Ansys Workbench, with Meshing enabled. If you want to use SpaceClaim with Meshing enabled, disable Use SpaceClaim Direct Modeler as an External CAD in Workbench options.
Any Match controls defined in SpaceClaim and used for meshing will be transferred to Mechanical as Cyclic Symmetry.
Named selections/groups created in SpaceClaim will be transferred. See Using Named Selections in Ansys for details on creating Named Selections in SpaceClaim.
If using groups to transfer important groups/named selections of edges, faces or bodies, consider the following:
Groups can be applied to edges, faces or bodies of the geometry and/or the blocking. If applied to the geometry topology, the associated block topology should inherit the group information. That said, the transfer of the groups to named selections in Mechanical are done using the block topology, so if named selections do not come in properly to Mechanical it indicates a problem with the association. This can happen when there are thin features, etc. and the mapping of the geometry to blocking is unclear. To avoid problems, it is often easiest to just apply the groups directly to the block topology.
Splitting blocks and other operations that change the block topology IDs can change the contents of groups. For this reason, you should apply groups after the block topology is mostly complete.
When doing design studies where the topology IDs need to persist from one design point to the next design point you should use one of the following approaches:
Use group parameters to drive parameter changes where blocking topology has groups/named selections assigned in a persistent way.
Define groups/named selection at the end of a block recording in a persistent way.
Define groups/named selection at the end of a script in a persistent way.
If you have components of bodies in SpaceClaim, note that shared topology creates multi-body parts. In this instance, the Mechanical application groups multi-body parts together regardless of the assembly structure in SpaceClaim, even if the Assembly Hierarchy option is set to Yes in Mechanical. You can use the View Assembly Structure tool in SpaceClaim to see how the SpaceClaim assembly structure is affected by Shared Topology in Mechanical.
If trying to bring mesh data from SpaceClaim Meshing to Mechanical, the recommended path is to use the Workbench transfer mechanism in the Workbench tab. See Ansys Transfer for details.
You can also write *.cdb/*.inp files that can be read in through External Model.
For large models, there are some benefits to using a two stage attach (writing the *.inp/*.cdb file separately and then reading this in through External Model).
If trying to bring mesh data from SpaceClaim Meshing to Mechanical APDL, save the mesh in Ansys (*.inp/*.cdb) format and read it into the Mechanical APDL system.
You cannot transfer the SpaceClaim Meshing mesh data to a downstream Mechanical APDL system directly in Workbench.
SpaceClaim Meshing mesh data can also be passed to an LS-DYNA system in Workbench using the direct transfer mechanism. Alternatively, a mesh can be saved in LS-DYNA (*.k) format and read it into LS-Pre/Post or LS-DYNA solver, or into Workbench via External Model.
For SpaceClaim assemblies (external documents where parts are saved as different files) when you save in LS-DYNA (*.k) format, the external documents will be written as separate part.k files using the same names as the external SpaceClaim documents. The assembly.k file will contain *include cards to maintain the assembly structure.
Note:Nested assemblies (assembly of assemblies) are not supported.
While saving, if you want all data to be written to a single *.k file, disable the Improve data on export option in the SpaceClaim Options window ().