Translating Moldflow Data to Abaqus Input Files

The following procedure summarizes the typical usage of the abaqus moldflow translator:

1. Run a Moldflow simulation.

2. Export the data as follows:

   • For a midplane Moldflow simulation export the finite element mesh data to a file named job-name.pat and the results data (material properties and residual stresses) to a file named job-name.osp.

   • For a three-dimensional solid Moldflow simulation using Moldflow Version MPI 6 run the Visual Basic script mpi2abq.vbs to export the finite element mesh data to a file named job-name_mesh.inp and the results data to .xml files.

3. Run the abaqus moldflow translator to create a partial Abaqus input file from the Moldflow interface files.

4. Edit the Abaqus input file to add appropriate data for the analysis (for example, add boundary conditions and step data).

5. Submit the Abaqus input file for analysis.

The Moldflow interface files contain finite element mesh data, material property data, and residual stress data.

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 1.

For midplane simulations the abaqus 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 moldflow translator converts the triangular elements to an identical mesh of AbaqusS3R shell elements. One-dimensional elements in the Moldflow mesh are not translated.

• The number of layers in the AbaqusS3R shell elements created by the abaqus moldflow translator 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 translator apply to 20 layers through the thickness.

• The Abaqus input data created by the abaqus moldflow translator 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 moldflow translator generates does not contain boundary condition and load data. You must add this information to the input file manually.

For three-dimensional solid simulations the abaqus 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 abaqus moldflow translator converts the tetrahedral elements to an identical mesh of AbaqusC3D4 or C3D10 solid elements (for more information, see the command line options below).

• Orthotropic material constants are in terms of material principal directions.

• Material properties are constant for each element.

• Orientations are defined in job-name_principalDirections.xml by giving vectors defining the local 1- and 2-directions.

• Residual stresses computed by the WARP3D module of Moldflow in job-name_initStresses.xml are transformed from global coordinates to local material directions and used as initial stresses in Abaqus.

• Loads and boundary conditions representing service loads must be added to the input file manually. For simulations using Moldflow Version MPI 6, the Abaqus input file created by the translator contains boundary conditions sufficient to remove rigid body modes from the model so that an analysis can easily solve for the response due to initial stresses.

The abaqus moldflow translator reads the Moldflow interface files and creates the relevant files. The files created depend on which options you include on the command line when executing the translator. For a midplane simulation the abaqus moldflow translator creates a partial Abaqus input file, a neutral file, and an initial stress file.

The abaqus moldflow translator reads the Moldflow interface files and creates the relevant files. The files created depend on which options you include on the command line when executing the translator.

If you are using an unfilled model, the abaqus moldflow translator creates only the partial Abaqus input file described below. For a three-dimensional solid simulation using a filled model, the translator may create additional files, as described below.

Once the abaqus moldflow translator has created the Abaqus input file, you must complete the input file manually before submitting it for analysis (see Abaqus Model Definition for details).