Abaqus/CAE evaluates the expression field at different locations on the model depending on the type of region that you selected when you created the interaction or prescribed condition. Table 1 indicates the locations on the model that Abaqus/CAE uses for evaluation of the expression field. For fluid boundary conditions, Abaqus/CAE averages the evaluated expressions at the element nodes of each element and applies that value to the centroid of the element face.
Table 1. Expression field evaluation locations.
| Region type |
Location of expression field evaluation |
|---|
| Node or vertex |
At the node or vertex |
| Edge |
At the midpoint of the edge of each element |
| Surface or face |
Centroid of each element face contained in the region |
| At the element nodes (fluid boundary conditions) |
| Cell |
Centroid of the element |
Next, Abaqus/CAE multiplies the magnitude that you specify for the spatially varying parameter, such as a pressure magnitude, by the evaluated expression at each element or node to determine the final values that are submitted to the analysis. The expression field is applied to magnitudes in the interaction or prescribed condition, including the real and imaginary parts of complex magnitudes. Beam and shell gradient values, such as gradients in temperature, are not affected by the expression field. During the analysis, Abaqus applies any amplitude that you have specified for the interaction or prescribed condition.