For midplane simulations the Abaqus Interface for Moldflow translator makes a number of assumptions regarding the topology and properties of the data. These assumptions, listed below, ensure compatibility with the options available in the current release of Abaqus.
The Moldflow mesh can consist of 3-node, planar, triangular elements as well as 2-node, one-dimensional elements that represent components such as runners and ribs. The Abaqus Interface for Moldflow translates the triangular elements to an identical mesh of Abaqus S3R shell elements. One-dimensional elements in the Moldflow mesh are not translated.
The number of layers in the Abaqus S3R shell elements created by the Abaqus Interface for Moldflow is equal to the number of layers passed by Moldflow, which is 20. As a result, the mechanical properties and stress data passed to the Abaqus Interface for Moldflow apply to 20 layers through the thickness.
The Abaqus input data created by the Abaqus Interface for Moldflow depend on the kind of material defined in the interface (.osp) file as follows:
For unfilled isotropic materials Abaqus assumes the following:
A homogeneous shell formulation.
Isotropic material constants.
Abaqus section point initial stresses are interpolated from the values at the Moldflow through-thickness integration points.
For unfilled transversely isotropic materials Abaqus assumes the following:
A homogeneous shell formulation.
Transversely isotropic material constants defined for the section in terms of material principal directions plus the orientation with respect to the local Abaqus coordinate system.
Abaqus section point initial stresses are interpolated from the values at the Moldflow through-thickness integration points.
For fiber-filled materials Abaqus assumes the following:
A composite shell formulation.
Lamina material constants defined for each layer in terms of material principal directions plus the orientation with respect to the local Abaqus coordinate system for each layer.
Moldflow through-thickness integration points are taken as the midpoint of each Abaqus layer.
Material properties are constant for each layer.
Abaqus section point initial stresses are the same as the values at the Moldflow through-thickness integration points and constant through each layer.
The Abaqus input file that the Abaqus Interface for Moldflow generates does not contain boundary condition and load data. You must add this information to the input file manually.