Interface to ANSYS

The interface to ANSYS enables you to export the mesh and key material and analysis data for further stress analyses in ANSYS.

Injection molding specific distributions of initial stress, and material properties such as the orthotropic mechanical properties, and linear thermal expansion coefficients, are the key elements of this interface.

Prerequisites

The interface to ANSYS requires the following:

• A Midplane or 3D meshed model
  Note: A multi-cavity model is separated into individual cavities.
• Results of a Fill+Pack analysis, with or without Fiber orientation results

Restrictions

The following restrictions apply to the interface to ANSYS:

• The following model features are not exported:
  • Runners, sprues, and gates
  • Cooling channels, bubblers, baffles
  • Mold boundary
  • Gas-assisted injection molding parts
• The following molding simulation features are not considered in the ANSYS analysis:
  • Corner effects
  • Mold thermal expansion

Assumptions

When working with layered, spatially varying materials, the ANSYS Interface for Autodesk assumes the following:

• 20 laminates will be output.
  Note: Fill+Pack outputs 12 laminates by default and will therefore be interpolated to 20 laminates for ANSYS.

Data exported / files created

The interface to ANSYS creates the following files:

• one *.cdb (command database) file
• one *.ist (initial stress) file

The data exported by the interface includes:

• For all Midplane/3D meshes:
  • Node position and element connectivity data
  • Material IDs and section IDs needed for element and laminated properties
  • Section data
• For a Midplane model and unfilled material:
  • Elastic modulus, shear modulus, and Poisson's ratio values from the material properties database
  • Coefficient of thermal expansion (CTE) value from the material properties database
  • Per-element and per-layer residual stress values in elemental local coordinate system
  • Per-element and per-layer section orientation angle defined with respect to layer element coordinate system
• For a Midplane model and fiber-filled material:
  • Per-element and per-layer elastic moduli, shear moduli, and Poisson's ratio values in principal directions
  • Per-element and per-layer coefficient of thermal expansion (CTE) values in principal directions
  • Per-element and per-layer residual stress values in elemental local coordinate system
  • Per-element and per-layer section orientation angle defined with respect to layer element coordinate system
• For a 3D model and unfilled material:
  • Elastic modulus, shear modulus, and Poisson's ratio values from the material properties database
  • Coefficient of thermal expansion (CTE) value from the material properties database
  • Per-element initial stress values
  • If the unfilled material is transversely isotropic, the flow direction of each element will be the first principal direction
• For a 3D model and fiber-filled material:
  • Per-element and per-layer elastic modulus, shear modulus and Poissons ratio values in the three global coordinate directions
  • Per-element and per-layer coefficient of thermal expansion (CTE) values in the three global coordinate directions
  • Per-element initial stress values in the three global coordinate directions

Additional notes

The interface automatically creates a set of three fixities such that the nodes construct a maximum inscribed circle to fix the rigid body motion only for warpage calculation. You may wish to apply alternate displacement constraints within ANSYS prior to analysis.

ANSYS has stricter rules regarding element aspect ratio so the molding simulation mesh may generate a number of warnings within ANSYS. These warnings may be ignored.

For a Midplane mesh, the interface creates shell181 elements. If there are structural beams in the model, they are created as beam4 elements. You can use a different element type that supports laminate initial stress and material property data by providing a suitable mapping in the *.cdb (command database) file generated by the interface.

For a 3D mesh that comprises four-node tetrahedra, the interface creates 10-node solid187 elements. This requires a mid-point generation command to be run in the ANSYS pre-processor. You can use a different solid element that supports orthotropic properties by providing a suitable mapping in the *.cdb file generated by the interface.

The ANSYS SHELL181 element includes the effects of transverse shear deformation. This requires the shear moduli G23 and G13 to be used in this element, which is different to what the Warp solver does.

ANSYS cannot be automatically instructed to run a large deflection analysis; a linear analysis with one loading step is run by default. If you have selected a large deflection analysis in this product, you need to make appropriate changes to the ANSYS command script to also run a large deflection analysis; otherwise, the results of the two products will not be comparable.

The 3D Warp analysis is based on proprietary solver technology, and the element type(s) used in ANSYS can differ from those used in 3D Warp models. Therefore, there may be a difference in the magnitude of the deflections calculated by ANSYS 3D and 3D Warp analyses. However, the warped shape should be the same in both results.