One-Way Fluid to Structure Coupling with Pre-recorded Flow Solution

For one-way fluid to structure coupled problems, where the effect of the structure on the fluid can be neglected, it is often convenient to solve the fluid and the structure sequentially instead of simultaneously. This approach allows you to record a transient flow solution and to reuse the recorded fluid loads in multiple stress analyses without rerunning the flow solver.

In the following workflow, you first run the flow solver to compute the fluid loads, recording the transient solution in a simulation history file. You then map the fluid loads recorded during the first time-step onto the structure and run the stress solver, which in turn computes the solid displacements in response to the mapped loads. You can automate the mapping and running process for subsequent time-steps using a macro.

  1. Define the fluid and solid regions in the same simulation.
    It is not necessary to create a fluid-structure interface, as you directly map data from the fluid boundary to the solid boundary.
  2. Define the physics continua for the fluid and the solid regions, as required.
    For one-way fluid to structure coupling with sequential run, the simulation does not require the Fluid-Structure Coupling solver, as this solver controls implicit data exchange at the fluid-structure interface.
  3. Record the flow solution in a simulation history file:
    1. Right-click the Solution Histories node and create a new solution history file named, for example, fluidLoads.simh.
    2. Edit the Solution Histories > [fluidLoads] node and set the following properties:
      Node Property Setting
      [fluidLoads] Functions Select the field functions that represent the fluid loads acting on the structure, for example pressure (Static Pressure), or traction (Static Pressure and Wall Shear Stress).
      Regions Select the fluid region.
      Input By default, Simcenter STAR-CCM+ records the specified functions for the entire fluid region. Optionally, you can use this property to select the fluid boundaries in contact with the solid, so that the solution is only recorded at these boundaries.
      Update Trigger Time Step
      Time-Step Frequency Frequency Specify the frequency of recording in terms of the simulation time-step. The default frequency is 1, meaning that Simcenter STAR-CCM+ records the specified functions at each time-step.
Run a standalone flow analysis:
  1. Select the Solvers > Solid Stress Solver node and activate Solver Frozen.
  2. Run the simulation.
To use the computed fluid loads for stress analysis:
  1. Right-click the Solution Histories > [fluidLoads] node and select Create Recorded Solution View.
    Within Solution Views, Simcenter STAR-CCM+ adds a node named after the solution history.
  2. Right-click the Tools > Data Mappers node and select New Data Mapper > Surface Data Mapper.
  3. Edit the [Surface Data Mapper] node and set the following properties:
    Property Setting
    Source Surfaces Select the fluid FSI boundary.
    Source Stencil Select Face.
    Scalar Field Functions Select the field functions representing the fluid loads.
    Scalar/Vector Field Functions
    Mapped Names When you execute the mapping operation, the mapped loads become available as field functions. Assign the mapped field functions a suitable name, using this property.
    Representation Select the recorded flow solution.
Specify the solid mesh as the mapping target:
  1. Edit the [Surface Data Mapper] > Target Specifications > Surface node and set the following properties:
    Property Setting
    Target Surfaces Select the solid FSI boundary.
    Target Stencil Vertex
  2. Execute the mapping operation (for instructions, see Executing the Mapping Operation).
    When executed, the data mapper maps the fluid loads that were recorded at the Time-Step that is selected under the Solution Views > [fluidLoads] node.
Use the mapped field functions to define the loads on the structure:
  1. Create a surface segment, with the following properties:
    Node Property Setting
    [Segment] Type Load
    Surfaces Select the part surfaces corresponding to the FSI solid boundary.
    Physics ConditionsSolid Stress Loads Method Select the appropriate method, depending on the recorded fluid loads.
    Physics Value[Load] (for example Force) Method Field Function
    Scalar Function or Vector Function Select the field functions representing the mapped fluid loads. These are named based on the Mapped Names property that you defined for the data mapper.
Run a standalone solid analysis with the mapped fluid loads:
  1. Expand the Solvers node.
  2. Select the Solid Stress Solver node and deactivate Solver Frozen, then freeze the flow solver.
  3. Run the simulation.
    To obtain a transient solution for the solid, automate the mapping and running process using a macro. In the macro, include the following loop:
    1. For the Solution Views > [fluidLoads] node, increase the Time-Step property by 1.
    2. Execute the mapper.
    3. Run the stress solver for one time-step.