This section describes the recommended modeling practices for ensuring mesh compatibility. Abaqus/Standard and Abaqus/Explicit require that the meshes used for the co-simulation interface regions be topologically similar. The models must have a matching face or edge to define the interface region. Because of differences in mesh densities, element topology, element order, etc., this compatibility may be difficult to achieve.
For example, suppose that you use hexahedral elements to mesh the interface region in the Abaqus/Explicit model and you use tetrahedral elements to mesh the interface region in the Abaqus/Standard model. You will not have compatible meshes at the interface region.
In general, to control the mesh compatibility at the interface region, you will create a skin or a stringer (depending on whether the interface region is a face or an edge) on the part that contains the interface region in the Abaqus/Explicit model, perform a variety of modeling techniques, and obtain a part instance to use to define a tie constraint in the Abaqus/Standard model. In addition, the mesh on the interface region in the Abaqus/Explicit model must be coarser than the mesh on the interface region in the Abaqus/Standard model.
Detailed instructions are provided in the following procedure.
To ensure compatible meshes on interface regions:
In the Abaqus/Explicit model:
In the Property module display the part that contains the interface region. If the interface region is a face, create a skin on the face. If the interface region is an edge, create a stringer on the edge. For more information, see Chapter 33, “Skin and stringer reinforcements.”
If the part is geometry based, mesh the part.
Create an orphan mesh part (even if you are working with an orphan mesh part).
Delete all of the elements in the newly created orphan mesh part other than those on the skin or stringer. In addition, delete the associated unreferenced nodes using the Edit Mesh toolset.
In the Abaqus/Standard model:
Copy the orphan mesh part containing the skin or stringer from the Abaqus/Explicit model, and create an instance of the newly copied part.
To simplify region selection procedures, create a named set or surface that contains the orphan mesh part.
In the Interaction module, create a tie constraint specifying the copied orphan mesh part (using the named set or surface) as the master region and the interface region on the Abaqus/Standard model as the slave region.
In the Interaction module, define a Standard-Explicit co-simulation interaction and specify the orphan mesh part (using the named set or surface) as the interface region. For more information, see “Specifying the interface region and coupling schemes,” Section 25.5.
In the Abaqus/Explicit model:
Delete the orphan mesh part that contains the skin or stringer.
Delete the skin or stringer from the part geometry.
If the part is geometry based, remesh the part.
In the Interaction module, define a Standard-Explicit co-simulation interaction and specify the interface region in the original Abaqus/Explicit part as the interface region.
Continue with the co-simulation procedure as described in “Overview of co-simulations,” Section 25.1.