By default, in Abaqus/Standard an element is removed (deleted) once D reaches Dmax at all of the section points at all integration locations in the element. If an element is removed, the output variable STATUS is set to zero for the element, and it offers no resistance to subsequent deformation. However, the element still remains in the Abaqus/Standard model and may be visible during postprocessing. In the Visualization module of Abaqus/CAE, you can suppress the display of elements based on their status (see Selecting the status field output variable).
Alternatively, you can specify that an element should remain in the model even after all of the damage variables reach Dmax. In this case, once all the damage variables reach the maximum value, the stiffness remains constant.
Input File Usage
Use the following option to delete failed elements from the mesh (default):
SECTION CONTROLS, ELEMENT DELETION=YES
Use the following option to keep failed elements in the mesh computations:
SECTION CONTROLS, ELEMENT DELETION=NO
Difficulties associated with element removal in Abaqus/Standard
When elements are removed from the model, their nodes remain in the model even if they are not attached to any active elements. When the solution progresses, these nodes might undergo non-physical displacements in Abaqus/Standard. In addition, applying a point load to a node that is not attached to an active element will cause convergence difficulties since there is no stiffness to resist the load. It is the responsibility of the user to prevent such situations.