The Inherent Strain method provides an alternative to a coupled thermal-structural additive process simulation available in Mechanical. With the Inherent Strain method, strains are calculated not from material properties and thermal loads but from the use of a calibration factor, or Strain Scaling Factor. The strain is equal to the Strain Scaling Factor multiplied by yield strength and divided by elastic modulus:
The Strain Scaling Factor (SSF) is an important factor quantifying the variables unique to each build scenario. It must be experimentally determined for each machine and material combination of interest. We recommend you perform the same calibration procedure used for Ansys Additive, as described in the Additive Print and Science Calibration Guide.
The SSF value is a direct multiplier to the predicted strain values. Using a value of 1 (default) will result in strain magnitudes as calculated by the solver. Some material and geometry combinations result in bulging/expansion rather than shrinkage and so a negative SSF is possible. Values between -1 and 1 will reduce displacement and stress while values outside of that range will amplify them. Using a value of 0 will result in no strain and the final displacement will match the input geometry.
You can define calibration factors that are different in each direction (X, Y, and Z) based on the Global coordinate system by choosing Anisotropic Inherent Strain Definition. The properties of materials will differ in different directions. If Inherent Strain Definition = Scan Pattern or Thermal Strain, individual calibration factors, called anisotropic scaling coefficients (ASCs), may be entered based on the local orientation of scan vectors within the part, that is, parallel and perpendicular to scanning direction and in the build direction.
The steps in a typical additive manufacturing simulation are shown in the table below. Considerations unique to using the Inherent Strain method are described.
| Inherent Strain Workflow at a Glance | |
|---|---|
| Simulation Step | Considerations for Inherent Strain Method |
| 1. Create analysis system | Select the AM LPBF Inherent Strain custom system in Workbench. |
| 2. Define Engineering Data | Necessary only if you are using your own user-defined material. (Ansys-supplied sample AM materials are automatically available if you used AM LPBF Inherent Strain custom system.) |
| 3. Attach geometry and launch Mechanical | No special considerations. |
| 4. Identify geometry | No special considerations. |
| 5. Assign materials | No special considerations. |
| 6. Apply mesh controls and generate mesh | No special considerations, other than if you will be using AM octree adaptive meshing, in which case Cartesian meshing with voxelization option is required. Adaptive meshing is available only with Inherent Strain simulations. |
| 7. Identify and/or generate supports | No special considerations. |
| 8. Define connections | No special considerations. |
| 9. Define AM process steps | Note there is no cooldown step. |
| 10. Define build settings | Set Inherent Strain = Yes (Automatic if you used AM LPBF Inherent Strain custom
system.) Set Inherent Strain Definition to isotropic, anisotropic, scan pattern, or thermal strain. The thermal strain definition uses the machine learning (ML) method. Define process parameters. Required inputs depend on the selected strain definition. Enter strain scaling factors, usually determined by a calibration procedure. |
| 11. Establish structural analysis settings | Review and change output controls as needed. Most items are not stored during solution to reduce result file size. Consider suppressing the calculation of stresses and strains if you are interested only in distortion. |
| 12. Apply structural boundary conditions | Apply a fixed condition to the underside of the base assuming the base is rigid with no distortion. |
| 13. Solve the static structural analysis | No special considerations. |
| 14. Review results | No special considerations. |