Translating Moldflow Data to Abaqus Input Files

The Moldflow interface files contain 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.

The Moldflow interface material property data file contains 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.

The abaqus moldflow translator 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.

The partial Abaqus input file contains model data consisting of nodal coordinates, element topology, and section definitions. It also contains a STATIC step with default output requests. If you are working with isotropic materials, the input file contains material property data. Each input file begins with a series of comments that summarize the data provided by the Moldflow interface files and how the data are translated to the Abaqus input file. Additional data, such as boundary conditions and loads, and nondefault output requests must be added to this file manually.

Material data are translated into an appropriately formatted ASCII neutral file. This file contains lamina material property data for each layer of each element. The AbaqusELASTIC, TYPE=SHORT FIBER and EXPANSION, TYPE=SHORT FIBER options in the Abaqus input file direct Abaqus/Standard to read material data from this file during the initialization step.

Data lines in the neutral file:

1. First line:

2. Number of elements in the .shf file.

3. Number of layers in each shell section.

1. Subsequent lines:

2. Element label.

3. Layer identifier.

4. $E_1$ .

5. $E_2$ .

6. ${\nu }_{12}$ .

7. $G_{12}$ .

8. $G_{13}$ .

9. $G_{23}$ .

10. ${\alpha }_1$ .

11. ${\alpha }_2$ .

12. Fiber orientation angle (in degrees), measured relative to the default element orientation.

This data line is repeated as often as necessary to define the above parameters for different layers of a shell section within different elements.

Residual stress data from the Moldflow analysis are translated into an appropriately formatted ASCII neutral file. These data are defined in terms of the local Abaqus coordinate system at each section point. The AbaqusINITIAL CONDITIONS, TYPE=STRESS, SECTION POINTS option in the Abaqus input file directs Abaqus/Standard to read initial stress data from this file during the initialization step.

The partial Abaqus input file contains model data consisting of nodal coordinates, element topology, and section definitions. Additional data, such as service loads and boundary conditions, and nondefault output requests must be added to this file manually.

Boundary condition data sufficient to remove rigid body modes are also included.

Material data from the Moldflow analysis are collected and placed in a binary file. The data written to the file are in the same form as the information provided for the AbaqusELASTIC, TYPE=ENGINEERING CONSTANTS option. These are defined in terms of the local Abaqus coordinate system of each element.

Orientations defining the directions for material properties and initial stresses are computed and placed in this binary file.

The orthotropic thermal expansion data from the Moldflow analysis are collected and placed in a binary file. These are defined in terms of the local Abaqus coordinate system of each element.

A shrinkage and warpage analysis calculates the deformation caused by the residual stresses in the model after it is removed from the mold. Usually only rigid body modes must be removed.

In this case you must ensure that residual stresses have been translated. For three-dimensional solid Moldflow simulations boundary conditions sufficient to restrain rigid body modes are automatically translated to the input file. In other cases you are required to add appropriate boundary conditions to remove the rigid body modes of the model.

In certain cases problems with convergence can occur when you must account for geometric nonlinearity and large initial stresses are present. You can overcome these problems by using two analysis steps:

• In the first step, constrain all displacement degrees of freedom.

• In the second step, use the OP=NEW parameter to apply boundary conditions that remove the rigid body modes.

A service loading analysis (with appropriate boundary conditions) assesses the performance of the model. You can perform this analysis with or without initial stresses. You must specify the appropriate boundary conditions and loads as history data in the Abaqus input file.

Any Abaqus/Standard analysis procedure can be performed with the translated model provided that you specify the correct boundary conditions and loading in the Abaqus input file. In addition, certain analysis types may require you to specify additional material constants, model data, and/or solution controls in the input file.