How to Model Initial Strain
To analyze a prestressed system (a material that has already been loaded and stressed before
you load it again, such as an interferencefit 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
realworld 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:
 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, :
 Solving this equation for the temperature difference yields:
The calculated temperature difference must be applied to the model in order to simulate a
prestressed condition based on the known strain and the material properties. You can do so by
using the following procedure:
 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. 
 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. 
 On the "MultiPhysics" 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 "MultiPhysics" 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.
