# Surface Damage

Since fatigue is a surface phenomenon, it is a common practice to assess damage only at the surface of a structure.

Damage is assessed on the surface of a structure modeled with solid elements. Two options are available to assess surface damage of a structure. The surface damage calculation is automatically turned on when multiaxial fatigue analysis is carried out.

## Using Membrane Stress

When requested in FATPARM, OptiStruct automatically creates membrane elements on the surface of the structure to assess surface damage. Unlike skin elements manually created by user, the automatically created membrane elements in OptiStruct does not add any stiffness to the structure. The membrane elements are only used when calculating membrane stress caused by displacement of nodes on the surface.

The normal direction (z-axis) of the internally created membrane elements is inward, which means the normal direction is toward the interior of the structure. The local x-axis of the membrane elements is determined by Material Coordinate System with 0.0 rotation angle by default. With PARAM,OMID,NO, the local x-axis of the membrane elements is determined by Elemental Coordinate System.

In uniaxial EN fatigue analysis, strain tensor component in local z-direction on local z-plane is calculated using Hook’s Law. In multiaxial EN fatigue, a plasticity model in the multiaxial fatigue takes care of the strain component.

If more than 2 free faces are found for a solid element all the free faces are evaluated. The worst damage value out of damages of all the free faces is assigned to the solid element for a reported damage value of the solid element.

Since the membrane elements are not included in the stiffness matrix of user-defined solution sequences, it is not valid to use the option in fatigue analysis with nonlinear analysis when nonlinear material is present. OptiStruct will error out in this case. Therefore, fatigue analysis with nonlinear analysis is supported with membrane stress only if material is linear.

The membrane fatigue method is available in fatigue analysis with linear static analysis, nonlinear static analysis (linear material only), linear transient analysis, random response analysis, and frequency response analysis. It is supported for SN and EN fatigue.

## Using Grid Point Stress

When requested in FATPARM, OptiStruct uses grid point stress to calculate damage on the surface of the structure. The grid point stress is projected onto an imaginary plane to obtain plane stress. The plane stress is used in damage calculation. Normal direction of the imaginary plane is an averaged normal direction of free faces that are attached to the grid. The normal direction is local z-axis of the imaginary plane. Local x-axis is a cross product of z-axis in basic coord. system and the local z-axis. If the z-axis in basic coord. system is parallel to the local z-axis, the local x-axis will be the x-axis in basic coord. system. Local y-axis is a cross product of the local z-axis and the local x-axis.

- Material with the least UTS.
- Material with the least SRI1 (SN) or S'f (EN) before SN / EN curve adjustment.
- Material with the least Young’s modulus.
- Material with the highest MATFAT ID.

Grid-point stress fatigue method is available in fatigue analysis with linear static analysis and nonlinear static analysis. It is supported for SN, EN, and FOS. Pseudo damage is not supported with grid point stress-based damage. Grid-point stress based Fatigue is not supported for Weld Fatigue, Solder Fatigue, Vibration/Dynamic fatigue, Transient Fatigue, or Pseudo Damage analysis.

## Input

The `SURFSTS` field can be set to MBRN (membrane
stress) or GP (grid point stress) for surface stress after
sub-keyword `STRESS` in FATPARM Bulk Data.
Membrane stress is calculated in multiaxial fatigue analysis by default unless grid
point stress is chosen.

## Output

No additional output request is required. Damage/Life/FOS output of an element set will automatically output surface damage. If membrane stress is chosen, the worst damage caused by the membrane stress will assigned to the original solid element. If grid point stress is chosen, damage of surface nodes will be output.