Ensuring matching nodes at the interface regions

You may have dissimilar meshes in regions shared in the model definitions. For Abaqus/Standard to Abaqus/Explicit co-simulation, you can improve solution stability and accuracy in some cases by ensuring that you have matching nodes at the interface (see Dissimilar Mesh-Related Limitations). This section describes the recommended modeling practices for ensuring matching nodes at the interface regions.

Context:

In general, 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.

Detailed instructions are provided in the following procedure.

  1. In the Abaqus/Explicit model:
    1. 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 Skin and stringer reinforcements.
    2. If the part is geometry based, mesh the part.
    3. Create a mesh part (even if you are working with a mesh part).
    4. Delete all of the elements in the newly created mesh part other than those on the skin or stringer. In addition, delete the associated unreferenced nodes using the Edit Mesh toolset.
  2. In the Abaqus/Standard model:
    1. Copy the mesh part containing the skin or stringer from the Abaqus/Explicit model, and create an instance of the newly copied part.
    2. To simplify region selection procedures, create a named set or surface that contains the mesh part.
    3. In the Interaction module, create a tie constraint specifying the copied mesh part (using the named set or surface) as the main region and the interface region on the Abaqus/Standard model as the secondary region.
    4. In the Interaction module, define a Standard-Explicit co-simulation interaction and specify the mesh part (using the named set or surface) as the interface region. For more information, see Specifying the interface region and coupling schemes.
  3. In the Abaqus/Explicit model:
    1. Delete the mesh part that contains the skin or stringer.
    2. Delete the skin or stringer from the part geometry.
    3. If the part is geometry based, remesh the part.
    4. 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.
  4. Continue with the co-simulation procedure as described in Overview of co-simulation.