ProductsAbaqus/Standard Using the translatorThe following procedure summarizes the typical usage of the abaqus moldflow translator:
The Moldflow interface filesThe 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.
Finite element mesh dataThe Moldflow interface files contain finite element mesh data.
Material property dataThe 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 dataThe 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.
Assumptions used to translate the Moldflow data for midplane simulationsFor 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 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 simulationsFor 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.
Files created for a midplane simulationThe 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) fileThe 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 propertiesMaterial 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:
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) fileResidual 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. Files created for a three-dimensional solid simulationThe 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 fileThe 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 dataMaterial 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. Orientation (.opt) file containing element orientation dataOrientations defining the directions for material properties and initial stresses are computed and placed in this binary file. Thermal expansion (.tpt) file containing element thermal expansion coefficient dataThe 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. Preparing the Abaqus input file for analysisOnce 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). Preparing for a shrinkage and warpage analysisA 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:
Preparing for a service loading analysisA 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 typesAny 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 summaryabaqus
moldflowjobjob-nameinputinput-namemidplane3Delement_order{12}initial_stress{onoff}materialtraditionalorientationtraditional
Command line options
|