How to Model Initial Strain

To analyze a pre-stressed system (a material that has already been loaded and stressed before you load it again, such as an interference-fit system), you must model the initial strain.

The easiest way to model an initial strain in a part is to induce a thermal stress that will produce the desired strain. (Even if the strain in the real-world system was actually created by some circumstance other than thermal stress, the FEA modeling technique remains the same.) If you know the amount of existing strain and the properties of the material, then you can calculate the necessary temperature difference as follows:

1. The basic equation for thermal stress states that the strain, , is equal to the product of the coefficient of thermal expansion, , and the temperature difference, :
2. Solving this equation for the temperature difference yields:

The calculated temperature difference must be applied to the model in order to simulate a pre-stressed condition based on the known strain and the material properties. You can do so by using the following procedure:

1. For each part that you want to set to a specified temperature, on the "Element Definition" screen (for all element types except plate), make sure that the "Stress Free Reference Temperature" field is set to the default value of 0 (see Figure 1).

With plate elements, you must specify the "Mean Temperature Difference" and "delta T thru thickness" values on the "Element Definition" screen. To calculate the "Mean Temperature Difference", take the average temperature through the thickness (i.e., the average of the temperature of the top of the plate and the temperature of the bottom of the plate) and subtract the stress free reference temperature. To calculate the "delta T thru thickness", take the temperature difference through the thickness (i.e., the difference between the temperature of the top of the plate and the temperature of the bottom of the plate) and divide it by the thickness of the plate.

Figure 1: Specifying the "Stress Free Reference Temperature" value on the "Element Definition" screen.

2. On the "Multipliers" tab of the "Analysis Parameters" screen, type a value of 1 in the "Thermal" column (see Figure 2).

Figure 2: Specifying the "Thermal" multiplier on the "Analysis Parameters" screen.

3. On the "Multi-Physics" tab (for all element types except plate elements), enter the calculated temperature difference value in the "Default nodal temperature" field (see Figure 3).

Figure 3: Specifying the "Default nodal temperature" value on the "Multi-Physics" tab of the "Analysis Parameters" screen.

The thermal stress is created due to the difference between the nodal temperatures and the stress free reference temperature (except for plate elements, which use the "Mean Temperature Difference" and "delta T thru thickness" values).

For more information about specifying an initial strain by inducing a thermal stress, see the ALGOR User's Guide.