Fluid-Structure Interaction General Workflow

Starting from an uncoupled set up with a fully defined fluid and solid domain, Simcenter STAR-CCM+ allows you to defined a general FSI problem.

To set up a fluid-structure interaction problem:
  1. Create the fluid-structure interface as a contact-mode interface (see Defining the Regions Layout).
    Boundary-mode interfaces are not supported as fluid-structure interfaces. By default, the Fluid Structure Coupling solver enforces the use of compatible settings (see Model Compatibility). If you run an FSI simulation with a boundary-mode fluid-structure interface, Simcenter STAR-CCM+ stops the simulation and issues a warning.
    • If you wish to continue the simulation despite the incompatible interface type, select the Solvers > Fluid Structure Coupling node and set Model Compatibility to Ignore.
  2. Make sure that the interface type is set to Mapped Contact Interface. To set this type, select the relevant Interfaces > [FSI Interface] node and set Type to Mapped Contact Interface.
    Simcenter STAR-CCM+ detects the fluid/solid interface and adds FSI controls under Regions > [Solid Region] > Boundaries > [FSI Interface] > Physics Conditions.

    As well as adding FSI control, Simcenter STAR-CCM+ adds the Fluid Structure Coupling solver to the Solvers node.

For two-way coupled problems you are strongly advised to use a stabilization method. As well as stabilizing the solution, the stabilization method accelerates the convergence of the coupled system.
  1. Apply one of the two stabilization methods available:
    • For transient simulations with large displacement of fluid volume, select Dynamic:
      1. Select the Solvers > Fluid Structure Coupling node and set Stabilization Method to Dynamic.
      2. Select the Regions > [Solid Region] > [FSI Interface] > Physics Conditions > FSI Dynamic Stabilization node and set the Method to either Automatic or Manual.
      3. If Method is set to Manual, select Regions > [Solid Region] > [FSI Interface] > Physics Values > FSI Dynamic Stabilization Coefficient and set Dynamic Coefficient to your chosen value. For example, for water flow in a slender pipe, the displaced fluid volume per unit area can be estimated as half the pipe inner diameter.
    • For steady simulations or simulations in which the displaced fluid volume is negligible, select Constant Displacement Under-relaxation:
      1. Select the Solvers > Fluid Structure Coupling node, and set Stabilization Method to Constant Displacement Under-relaxation.
      2. Select the Constant Displacement Under-relaxation node, and set the Under-Relaxation Factor value.
    If you select a stabilization method that is not appropriate to your setup (for example, you select the Dynamic in a steady simulation), Simcenter STAR-CCM+ resets the Stabilization Method to None.
  2. Select the Regions > [Solid Region] > Boundaries > [Interface Boundary] > Physics Conditions > FSI Coupling Specification node, and set Option to one of the following:
    • For one-way fluid-to-structure and two-way coupled problems — Fluid Load - Pressure and Wall Shear Stress (default).
    • For pressure dominant one-way fluid-to-structure and two-way coupled problems — Fluid Load - Pressure
    • For wall shear stress dominant one-way fluid-to-structure and two-way coupled problems — Fluid Load - Wall Shear Stress
    • For uncoupled problems — Uncoupled.
    The fluid region FSI Coupling Specification is a read-only property and is controlled by the motion of the coupled solid region (see FSI Region Motions).
As outlined in the FSI Solution Strategy, Simcenter STAR-CCM+ allows you to configure the force consistency through the ramping and clipping of the fluid traction.
  1. If you wish to set ramping:
    1. Select the Regions > [Solid Region] > Boundaries > [FSI Interface] > Physics Conditions > FSI Fluid Load Ramping node and set Option to Linear.
    2. Select the Physics Values > FSI Traction Linear Ramping node, and use the Starting Time and Stopping Time properties to set the ramping duration.
    注You must set the Stopping Time before you set the Starting Time property.
  2. If you wish to set clipping:
    1. Select the Regions > [Solid Region] > Boundaries > [FSI Interface] > Physics Conditions > FSI Fluid Load Clipping node and activate the Pressure, Shear, or Pressure and Shear properties.
    2. Select the Physics Values > FSI Pressure Clipping or FSI Shear Clipping node and set the Minimum and Maximum values.
  3. Expand the Tools > Motions node and define the motion of the fluid and solid regions.
    • For the solid region, you can define it as Stationary, or apply a rigid motion (such as Translation or Rotation), a Solid Displacement motion (which accounts for the solid deformation), or a superposition of rigid motions and Solid Displacement.

      Only include the Solid Displacement motion when modeling the effect of the solid deformation on the fluid. If you do not include the solid displacement motion, the Solid Displacement is still computed by not applied to the coordinates of the solid.

    • For the fluid, you can define it as Stationary, apply rigid motions, or use the Morphing motion. The Morphing motion adjusts the fluid mesh based on the solid motion and/or deformation.
    [Fluid Region] Motion [Solid Region] Motion Scenario
    Stationary or Prescribed Rigid Motion Stationary or Prescribed Rigid Motions Any simulation where you neglect the effects of the structure on the fluid. The rigid motions of the fluid and solid regions must be consistent.
    Morphing Stationary or Prescribed Rigid Motions Any simulation which neglect the effect of the structural deformation on the fluid, but takes into account the effect of any rigid motion of the structure.
    Morphing Solid Displacement+ any prescribed rigid motions Any simulation that takes into account the effects of the solid deformation on the fluid. This includes both one-way structure-to-fluid problems and two-way coupled problems.
To assign the motions to the fluid and solid regions:
  1. Select the Regions > [Fluid Region] > Physics Values > Motion Specification node and Regions > [Solid Region] > Physics Values > Motion Specification node, and set Motion to the motions you defined for the fluid and solid under the Tools > Motions node.
    If you change the [Solid Region] > Physics Values > Motion Specification to Stationary, the Reset Mesh option is not available in the Clear Solution dialog. For more information, see Reset Mesh.
  2. When morphing the fluid, for cases where the fluid boundary is not entirely mapped to the fluid-solid interface, set the morphing method for the unmapped boundary as follows:
    1. Expand the [Fluid Region] > Boundaries node.
    2. Select the [unmapped fluid boundary] > Physics Conditions > Morpher Specification node and set Specification to Floating.


  3. Set the Mesh Morpher solver properties:
    1. Select the Solvers > Mesh Morpher node and activate Morph At Inner Iterations. When enforcing compatible settings (see Model Compatibility for Fluid Structure Coupling), deactivating this property results in an error.
    2. To improve performance, you can activate Boundary Layer Morphing. However, this may come at the cost of accuracy in the fluid solution.
To prevent the FSI simulation from stopping after the first inner iteration, you must disable the global force and displacement stopping criteria.
  1. Within the Stopping Criteria node, multi-select the Force Criterion and Displacement Criterion nodes, and deactivate Enabled.