### 5.2.1. Unidirectional (One-Way) FSI

In many FSI simulations, the coupling between the solution fields is predominantly unidirectional; a given field may strongly affect, but not be affected by other fields. In CFX, there are a variety of strategies to efficiently execute such simulations. These strategies are identified in the following examples.

#### 5.2.1.1. Using CFX Only

One of the most useful examples of unidirectional FSI within CFX involves prescribed mesh deformation of fluid or solid domains. This is possible using the CEL to specify the motion of sub-domains or domain boundaries, or by reading a sequence of pre-defined meshes.

#### 5.2.1.2. Using CFX and the Mechanical Application

In many FSI simulations, the capabilities of additional solvers are required to compliment those of CFX. In these circumstances, CFX provides tools to facilitate the import and export of solution data in a variety of formats.

##### 5.2.1.2.1. Importing Data from the Mechanical Application Solver

The recommended method for importing boundary condition data from the Mechanical application into CFX is via boundary profile data. For information about the creation and use of profile data files, refer to Unidirectional Load Transfer in the Mechanical APDL Coupled-Field Analysis Guide and Use Profile Data in the CFX-Pre User's Guide.

##### 5.2.1.2.2. Export Data to Other ANSYS Software Products

Two methods exist for exporting data from CFX for use in other ANSYS software products. The first method requires the use of the MFS variant of the ANSYS Multi-field solver and the second method does not.

- For information about exporting mechanical and thermal surface data and thermal volumetric data for use with the MFS solver, refer to Export to ANSYS Multi-field Solver Dialog Box in the CFX-Solver Manager User's Guide. For information about using the exported results and the MFS Solver, refer to The ANSYS Multi-field™ Solver - MFS Single-Code Coupling in the Mechanical APDL Coupled-Field Analysis Guide.

- For information about exporting mechanical and thermal surface data for general use, refer to Mechanical Import/Export Commands in the CFD-Post User's Guide. This method involves reading a Mechanical Coded Database (CDB) file and interpolating CFX solution data onto the mesh contained in that file. For more information about how these steps are automated in the Mechanical application, see Custom Systems in the Workbench User's Guide.

##### 5.2.1.2.3. Mechanical Import/Export Example: One-Way FSI Data Transfer

You can perform one-way FSI operations manually (by exporting CDB files from the Mechanical APDL application, importing the surface in CFD-Post, and exporting the SFE commands).

To create a Mechanical load file using CFD-Post to transfer FSI data:

1. Load the fluids results file, from which you want to transfer results, into CFD-Post

2. Select File > Import > Import Mechanical CDB Surface. The Import Mechanical CDB Surface dialog box appears.

3. In the Import Mechanical CDB Surface dialog box, either:

   - Select the CDB file that specifies the surface mesh of the solid object to which to transfer data. Also select the Associated Boundary for the surface to map onto, and make other selections as appropriate.

   - Select the XML document that provides all transfer information. Click OK, and the surface data is loaded.

4. Select File > Export > Export Mechanical Load File. The Export Mechanical Load File dialog box appears.

5. In the Export Mechanical Load File dialog box, select a filename to which to save the data. For the Location parameter value, select the imported ANSYS mesh object. Under File Format select ANSYS Load Commands (FSE or D). (Alternatively, you can select WB Simulation Input (XML) to get XML output.) Also select the appropriate data to export: Normal Stress Vector, Tangential Stress Vector, Stress Vector, Heat Transfer Coefficient, Heat Flux, or Temperature. Click Save, and the data file is created.

The one-way FSI data transfer described above is performed automatically when using the FSI: Fluid Flow (CFX) > Static Structural custom system in ANSYS Workbench. For details, see the FSI: Fluid Flow (ANSYS CFX) > Static Structural in the Workbench User's Guide section in the ANSYS documentation.

#### 5.2.1.3. Using CFX and Other CAE Software

Solution data can be exported from CFX in a variety of general formats during or after execution of the CFX-Solver. For information about the export of data in CGNS format during the execution of the solver, refer to Export Results Tab in the CFX-Pre User's Guide. For information about the extraction and export of CGNS, MSC Patran, FIELDVIEW, EnSight and custom data from CFX results files, refer to Generic Export Options in the CFX-Solver Manager User's Guide.

Release 18.2 - © ANSYS, Inc. All rights reserved.