For midplane simulations, you must use Moldflow to create two interface files: job-name.pat and job-name.osp. Both files must use the same units.
For three-dimensional solid simulations using Moldflow Version MPI 6, the mesh and results files for filled and unfilled models are listed in Table 2–1.
Table 2–1 Interface files generated using the Visual Basic script for Moldflow Version MPI 6.
| Data type | Filled model | Unfilled model |
|---|---|---|
| Finite element mesh data | job-name_mesh.inp | job-name_mesh.inp |
| Results data | job-name_v12.xml | job-name_PoissonRatios.xml |
| job-name_v13.xml | ||
| job-name_v23.xml | ||
| job-name_g12.xml | job-name_ShearModuli.xml | |
| job-name_g13.xml | ||
| job-name_g23.xml | ||
| job-name_ltec_1.xml | job-name_Ltecs.xml | |
| job-name_ltec_2.xml | ||
| job-name_ltec_3.xml | ||
| job-name_e11.xml | job-name_Moduli.xml | |
| job-name_e22.xml | ||
| job-name_e33.xml | ||
| job-name_initStresses.xml | job-name_initStresses.xml | |
| job-name_principalDirections.xml |
The Moldflow interface files contain the following information:
Finite element mesh data:
For midplane simulations the mesh data are in a Patran neutral file containing nodal coordinates, element topology, and element properties.
For three-dimensional solid simulations the mesh data are in an Abaqus input file containing nodal coordinates, element topology, element properties, and boundary conditions sufficient to eliminate the structure's rigid body modes. Solid elements in the mesh files are always 4-node tetrahedra. The translator has an option to convert these to 10-node tetrahedra.
Material property data:
Elastic and thermal expansion coefficients for each element. For midplane simulations, these properties may be isotropic or orthotropic. For three-dimensional solid simulations of filled models, these properties are orthotropic. For three-dimensional solid simulations of unfilled models, the data files contain orthotropic data adjusted to represent physically isotropic materials.
Residual stress data:
The Moldflow simulation calculates residual stresses in the plastic part after it has cooled in the mold. These residual stresses can be translated to initial stresses for the Abaqus structural analysis.
For midplane simulations, a plane stress initial stress state is defined in the same directions as the material properties. The stress state in the material coordinates is defined in terms of the principal stresses (the shear stress is zero).
For three-dimensional solid simulations, residual stresses for each element in job-name_initStresses.xml are in global coordinates. The translator transforms these coordinates to the same directions as the material properties.