A boundary condition is used to identify the interface where the transfer of loads to and from external fluid solvers CFX or Fluent occur.
is available for the following analysis types:
A Static Structural analysis coupled with other physics is intended to work with one substep (specified in the Analysis Settings). When a Fluid Solid Interface is present, program controlled sub-stepping will always use one substep regardless of any nonlinearities present. See Steps and Step Controls for Static and Transient Analyses under the Configuring Analysis Settings section of the Help.
When one or more FSI loads are present, any components defined in the Mechanical APDL input file are exported using the CMWRITE command to the file, file.cm, before the solution is completed. This aids the post-processing of results in CFD-Post.
There is currently a limitation associated with making a name change to your Fluid Solid Interface object in Mechanical. The Setup cell on the Project Schematic for System Coupling is not automatically updated. You need to perform an action in the application in order to update the Setup cell so that it receives the new name.
Once Fluid Solid Interfaces are identified, loads are transferred to and from body faces in the Mechanical APDL model using the MFX variant of the ANSYS Multi-field solver (see “Chapter 4. Multi-field Analysis Using Code Coupling” in the Coupled-Field Analysis Guide for details). This solver is accessed from either the Mechanical APDL Product Launcher or CFX-Solver Manager, and requires both the Mechanical APDL and CFX input files. To generate the Mechanical APDL input file, select the Solution object folder in the Mechanical Outline View, and then select . To generate the CFX input file, use the CFX preprocessor, CFX-Pre.
Run time-monitoring is available in both the Mechanical APDL Product Launcher and CFX-Solver Manager. Postprocessing of the Mechanical APDL results is available in the Mechanical application, and simultaneous postprocessing of both the Mechanical APDL and CFX results is available in the CFX postprocessor, CFD-Post.
Fluid-solid interfaces define the interfaces between the solid or shell elements in the Mechanical system and the fluid in the Fluent system. These interfaces are defined on faces in the Mechanical model. Data is exchanged across these interfaces during the execution of the simulation using the System Coupling component of Workbench. System Coupling is the mechanism allowing the Mechanical application and Fluent to send boundary condition results back and forth to one another (one or two-way communication is available).
Mechanical’s Static Structural and Transient Structural systems can be coupled with Fluent for a fluid force and structural displacement analysis, or a fluid-thermal-structural analysis. For more information about settings and elements needed for the thermal-structural analysis, see Thermal-Fluid-Structural Analyses using System Coupling.
The integer Interface Number, found in the Details view, is incremented by default each time a new interface is added. This value can be overridden if desired.
Fluid-solid interfaces define the interfaces between the acoustic and the structural regions. These interfaces are defined on acoustic regions faces. You can use the contextual (right-click) menu option > on the environment object to automatically identify fluid solid interfaces.
Fluid-solid interfaces define the interfaces between the thermal solid or shell elements in the Mechanical system and the fluid in the Fluent system. These interfaces are defined on faces in the Mechanical model. Data is exchanged across these interfaces during the execution of the simulation as described in Fluid-Structure Interaction (FSI) - One-Way Transfer Using System Coupling.
For transferring temperature and heat flows from Mechanical, interfaces may only be defined on the following types of faces:
On faces having heat fluxes.
On faces having convections.
On faces with a temperature load.
On faces without any loads specified (adiabatic). In this case, only temperatures are exchanged.
This section describes the characteristics of the boundary condition, including the application requirements, support limitations, and loading definitions and values.
Dimensional Types
3D Simulation: Supported.
2D Simulation: Not Supported.
Geometry Types: Geometry types supported for the boundary condition include:
Solid: Supported.
Surface/Shell: Supported.
Wire Body/Line Body/Beam: Not Supported.
Topology: The following topology selection options are supported for .
Body: Not Supported.
Face: Supported.
Edge: Not Supported.
Vertex: Not Supported.
Nodes: Not Supported.
To apply a :
On the Environment context toolbar: click Loads>. Or, right-click the Environment tree object or the Geometry window and select Insert>.
Define the Scoping Method.
The selections available in the Details view are described below.
| Category | Fields/Options/Description |
|---|---|
| Scope |
Scoping Method: Options include:
|
| Definition |
Type: Read-only field that displays boundary condition type - . Interface Number: Incremental value for each new interface. This value can be overridden if desired. Export Results: Thermal analyses only. The default value for this property is . When this property is set to , thermal data is written to .axdt files for use with External Data and System Coupling, which can connect to Fluent to transfer thermal data to a CFD analysis for a one-way transfer of static data. The file format for an External Data File (.axdt) is described in the External Data File Format Help section in the Workbench User Guide. Data to Transfer [Expert]: The default for this property is Program Controlled. When set to All System Coupling Data Transfers, the fluid solid interface regions can participate in force, displacement, and thermal coupling through System Coupling. You need to set All System Coupling Data Transfers for Mechanical to participate in a thermal-structural analysis. Suppressed: Include ( - default) or exclude () the boundary condition. |