Perform an analysis on a structure that has already encountered some damage.
Damage tolerance is the ability of a structure to retain required structural strength or stiffness after it has sustained damaged. When a composite part is damaged, there are numerous failure modes that can exist. These failure modes are constituent-level defects (i.e. fiber and matrix level defects), so it is appropriate to model damage at this level. Helius PFA is well-suited for modeling damage tolerance because it allows you to specify constituent-level damage in elements at the start of the analysis. For example, if a plate was impacted by a mass and diffuse matrix damage occurred in the impacted region, you can create an element set that represents the damaged region and assign matrix failure to that region prior to the start of the analysis. At the start of the analysis, this region will have an SDV1 value of 2 (matrix failure) and as the simulation progresses, the region can undergo fiber failure which will result in an SDV1 value of 3. In other words, the initial value of SDV1 that is assigned to the element set is not fixed and can change if either the matrix or fiber failure criterion is satisfied.
*INITIAL CONDITIONS, TYPE=SOLUTION DAMAGED_ELEMENTS, 3
In the above statement, DAMAGED_ELEMENTS is the name of the element set that represents the failed region and 3 indicates that this region will have fiber and matrix damage at the start of the analysis (SDV1 = 3).
Analyses with Helius PFA materials that have more than 7 state variables (specified by the *DEPVAR keyword) require a keyword statement that includes one or more blank lines. These blank lines are required because Abaqus expects to read values for the maximum numbers of state variables for all materials. Refer to the Abaqus Keywords Reference Manual for complete details on the proper usage of the *INITIAL CONDITIONS keyword. For example, if a model contains a Helius PFA unidirectional material with 7 state variables and a Helius PFA cohesive material with 9 state variables, a keyword statement with 3 lines would be required as shown below:
********** *INITIAL CONDITIONS, TYPE=SOLUTION DAMAGED_ELEMENTS, 3, ********
What if you had another case where you wanted to specify both fiber failure (SDV1 = 3) and matrix failure (SDV1 = 2) on different areas of the model? Lets assume we are using a material with 17 state variables (*DEPVAR). As a result we would need two blank lines after each element set listing.
********** *INITIAL CONDITIONS, TYPE=SOLUTION MATRIX_DAMAGE, 2, FIBER_DAMAGE, 3, ********