Abaqus/CAE automatically associates top-down meshes with the underlying geometry. Abaqus/CAE can make this association since the mesh conforms exactly to the geometry. In contrast, a bottom-up mesh does not have to conform to the geometry and, therefore, Abaqus/CAE may not associate parts of the mesh with the geometry. The following rules apply to the association of bottom-up elements:
Abaqus/CAE always associates bottom-up elements with the selected region.
When the underlying geometry is used to define the shape of the mesh, Abaqus/CAE associates the mesh with that geometry.
When portions of the geometry are not used to define the bottom-up mesh, Abaqus/CAE does not associate them, even if the mesh and geometry are in the same location.
You can edit the mesh-geometry association of any bottom-up meshed region.
If you edit a generated mesh so that it matches the geometry, you must still manually associate the mesh with the geometry.
Attributes such as loads and boundary conditions are applied to geometry. Proper mesh-geometry association ensures that these attributes are transferred correctly to the mesh during the analysis.
If you select a geometric face as a source or connecting side, Abaqus reuses the existing mesh entities on that face to create a compatible mesh only if the mesh entities are fully associated with the selected face. Full association means that:
The selected face is associated with element faces
All edges of the face are associated with element edges
All vertices of the face are associated with nodes
Abaqus tries to merge meshes that are associated with the same geometric entities. Unassociated meshes may require you to merge nodes along mesh boundaries using the Edit Mesh toolset.
You should always check that a bottom-up mesh is correctly associated with the geometry. Abaqus/CAE will issue an error in the Job module if you submit a job and attributes are applied to geometry with no associated mesh. However, Abaqus/CAE cannot determine whether the association is correct. For example, if a load is applied to a geometric face that should have several hundred elements but only one element is associated with that face, Abaqus/CAE will attempt to analyze the model with the entire load applied at the single associated element. Incorrect association produces incorrect analysis results.
You can use the mesh-geometry association 
tool in the Mesh module toolbox to view or edit the mesh-geometry associations for a bottom-up mesh. For detailed instructions, see “Viewing and editing mesh-geometry associativity,” Section 17.11.9.