Exporting

Send the results of Advanced Material Exchange to the structural package for analysis.

Export

  1. Click Home > Export > Export to Structural Package.
  2. After the Export to Structural Package dialog appears, click Browse, navigate to the directory where the files should be exported, and give the file a name.
  3. Review the material model information and select the environment to use (if multiple environments are present).
  4. Review the options for element deletion and residual strains.
  5. Click Export.

After the Export button is selected, an input file (.inp, .cdb, or .dat) and an interface file (.sif) will be saved in the directory of your choosing for use with the structural analysis. The input file contains the part geometry, mesh, load and boundary conditions, and the user material definition. The interface file contains the mapped fiber orientations and(or) the residual strains.

Models that use Abaqus S3, S4, S4R, or C3D8R elements will have the extraneous stiffness parameters calculated automatically during the export. This will add the *HOURGLASS STIFFNESS keyword to the section definition. Models with S3, S4, and S4R elements will also have the POISSON and THICKNESS MODULUS parameters added to the shell section definition. The *TRANSVERSE SHEAR STIFFNESS keyword is also added for the shell element types listed.

If the Enable element deletion check box is turned on, an additional parameter is added to the input file during the export. Refer to the Element Deletion section for further details. If the Output residual strains check box is turned on, the residual strain data from Moldflow will be stored in the .sif file. Additionally, a HIN file is created that contains the keyword *CURE STRESS. This keyword will tell the solver to include the effects of thermal residual stresses and strains in the structural analysis. Refer to the Model Thermal Residual Stresses section for further details.

Run the Analysis

  1. Ensure that both the input file and structural interface file are in the same directory (and the HIN file if applicable). All job files must have the same name. For example MyJob.inp and MyJob.sif.
  2. Open a command prompt by clicking the Command Shell icon on your desktop (any Windows command prompt will work as well).
  3. Navigate to the directory where the files are stored.
  4. Enter the appropriate syntax for the Abaqus or ANSYS job. See the examples below for reference.

The example below demonstrates how to submit an Abaqus model (example.inp and example.sif) from the command prompt (in this case with Abaqus 6.13-1): 
>>abq6131 job=example

The example below demonstrates how to submit a model (example.cdb and example.sif) from the command prompt with ANSYS 15.0: 
>>ansys-helius 150 example.cdb

Environment File Considerations

Prior to running a job with Abaqus, you will need to setup the abaqus_v6.env file. The usub_lib_dir variable in the abaqus_v6.env file should point to the directory holding the user material subroutine. The user material subroutine is located in the installation directory (usually C:\Program Files\Autodesk\Helius PFA 2016\). As an example, consider the case for a model run with Abaqus 6.13: 
usub_lib_dir = 'C:/Program Files/Autodesk/Helius PFA 2016/bin/abaqus/613'
Use forward slashes (/) rather than back slashes (\).

Only double precision analyses are supported. Set the double_precision parameter in the abaqus_v6.env file as follows: 
double_precision = BOTH
Parent topic: User's Guide