Within the Ansys fatigue module, the first decision that needs to be made in performing a fatigue analysis is which type of fatigue analysis to perform, Stress-life or Strain-life. Stress-life is based on empirical S-N curves which are modified by a variety of factors. Strain-life is based upon the Strain Life Relation Equation where the Strain-life Parameters are values for a particular material that best fit the equation to measured results. The Strain Life Relation Equation requires a total of 6 parameters to define the strain-life material properties: four strain-life parameter properties and the two cyclic stress-strain parameters. The Strain Life Relation Equation is shown below:

The two cyclic stress-strain parameters are part of the equation below:

Where:

= Total Strain Amplitude

= 2 x the Stress Amplitude

= Modulus of Elasticity

= Number of Cycles to Failure

= Number of Reversals to Failure

And the parameters required for a Strain Life analysis include:

= Fatigue Strength Coefficient

= Fatigue Strength Exponent (Basquin’s Exponent)

= Fatigue Ductility Coefficient

= Fatigue Ductility Exponent

= Cyclic Strength Coefficient

= Cyclic Strain Hardening Exponent

Note in the above equation, total strain (elastic + plastic) is the required input. However, running a finite element analysis to determine the total response can be very expensive and wasteful, especially if the nominal response of the structure is elastic. An accepted approach is to assume a nominally elastic response and then make use of Neuber’s equation to relate local stress/strain to nominal stress/strain at a stress concentration location.

To relate strain to stress we use Neuber's Rule:

Where:

= Local (Total) Strain

= Local Stress

= Elastic Stress Concentration Factor

= Nominal Elastic Strain

= Nominal Elastic Stress

The Fatigue Tool assumes nominal elastic behavior and therefore , and by simultaneously solving Neuber's equation along with cyclic strain equation, we can calculate the local stress/strains (including plastic response) given only elastic stress input. Note that this calculation is nonlinear and is solved using iterative methods. In addition, Ansys fatigue calculations use a value of 1 for the Elastic Stress Concentration Factor (), assuming that the mesh is refined enough to capture any stress concentration effects. in this case is not be confused with the Stress Reduction Factor option which is typically used in a Stress-life analysis to account for factors such as reliability and size effects.