3.2.41 Translating Moldflow data to Abaqus input files
Product: Abaqus/Standard
References
Overview
Moldflow Plastics Insight (referred to as Moldflow in this section) from Autodesk, Inc. models the plastics injection mold-filling process. The results of a Moldflow simulation include calculations of material properties and residual stresses in the plastic part.
The abaqus moldflow translator transforms finite element model information from a Moldflow analysis into a partial Abaqus input file. The translator requires the Moldflow interface files that are created by the Moldflow analysis. (See “The Moldflow interface files” for more information.)
For midplane simulations the abaqus moldflow translator reads the interface (.pat and .osp) files created by abaqus moldflow translator Version MPI 3 or later.
For three-dimensional solid simulations using Moldflow Version MPI 6 the translator reads the interface (.inp and .xml) files created using the Visual Basic script mpi2abq.vbs. This script is part of an Abaqus installation and is typically found in the moldflow_install_dir/Plastic Insight 6.0/data/commands directory.
Using the translator
The following procedure summarizes the typical usage of the abaqus moldflow translator:
Run a Moldflow simulation.
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.
Run the abaqus moldflow translator to create a partial Abaqus input file from the Moldflow interface files.
Edit the Abaqus input file to add appropriate data for the analysis (for example, add boundary conditions and step data).
Submit the Abaqus input file for analysis.
The Moldflow interface files
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 3.2.41–1.
Table 3.2.41–1 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 |
Finite element mesh data
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.
Material property data
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.
Residual stress data
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.
Assumptions used to translate the Moldflow data for midplane simulations
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 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 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.
Assumptions used to translate the Moldflow data for three-dimensional solid simulations
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 Abaqus C3D4 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.
Files created for a midplane simulation
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.
Partial Abaqus input (.inp) file
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.
Neutral (.shf) file containing material data for layered, spatially varying material properties
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 Abaqus *ELASTIC, 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:
Number of elements in the .shf file.
Number of layers in each shell section.
First line:
Element label.
Layer identifier.
.
.
.
.
.
.
.
.Fiber orientation angle (in degrees), measured relative to the default element orientation.
Subsequent lines:
This data line is repeated as often as necessary to define the above parameters for different layers of a shell section within different elements.
Initial stress (.str) file
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 Abaqus *INITIAL 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.
Files created for a three-dimensional solid simulation
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.
Partial Abaqus input file
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 (.mpt) file containing orthotropic material properties data
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 Abaqus *ELASTIC, TYPE=ENGINEERING CONSTANTS option. These are defined in terms of the local Abaqus coordinate system of each element.
Preparing the Abaqus input file for analysis
Once the abaqus moldflow translator has created the Abaqus input file, you must complete the input file manually before submitting it for analysis (see “Defining a model in Abaqus,” Section 1.3.1, for details).
Preparing for a shrinkage and warpage analysis
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.
Preparing for a service loading analysis
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.
Preparing for other analysis types
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.
Command line options
This option specifies the input and output file names to use during results translation. The job-name value is used to construct the default SIM database file name, job-name.sim. The output modal neutral file is given the name job-name.mnf.
If this option is omitted from the command line, the user will be prompted for this value.
This option is used to specify the name of the files containing the Moldflow interface data if it is different from job-name.
This option is used to translate the results of a midplane simulation to an Abaqus model with three-dimensional (shell) elements.
This option is used to translate the results of a three-dimensional solid simulation to an Abaqus model with solid elements.
This option is used to specify the order of elements created in the partial input file for three-dimensional solid simulations. Possible values are 1 to create first-order elements (C3D4) and 2 to create second-order elements (C3D10). The default value is 2. This option is valid only when using the 3D option.
This option specifies whether or not initial stress will be included in the model. This option is valid only when using the 3D option.
If the initial_stress option is not included or if initial_stress=off, initial stresses will not be translated.
If initial_stress=on, initial stresses will be written to the input file.
This option is used to specify where the material properties are written. If material=traditional, the material properties will be written to the input file. Otherwise, the material properties will be written to the (binary) .mpt file. Using material=traditional is not recommended for large models for performance reasons since every element will have its own *MATERIAL definition.
This option is used to specify where the orientations are written. If orientation=traditional, the orientations are written to the input file. Otherwise, the orientations will be written to the (binary) .opt file. Using orientation=traditional is not recommended for large models for performance reasons since every element will have its own *ORIENTATION definition.