ALE Method for FSI

In the Eulerian description, the grid is fixed and fluid passes through it. It's robust for large deformations but poor at interface tracking. In the Lagrangian description, the grid moves with the material, so interfaces are sharp, but the mesh can become distorted under large deformations. The ALE method is a middle ground, where the grid velocity can be set arbitrarily (Arbitrary). At interfaces, the grid moves with the material (Lagrangian-like), while internally, the grid is moved appropriately to maintain mesh quality (Eulerian-like).

The momentum conservation law of the Navier-Stokes equations in the ALE description becomes this.

Here, $\mathbf{c} = \mathbf{u} - \hat{\mathbf{u}}$ is the relative velocity (convective velocity) between the fluid velocity $\mathbf{u}$ and the mesh velocity $\hat{\mathbf{u}}$.

Exactly. In FSI problems, on the fluid-structure interface, we set $\hat{\mathbf{u}} = \dot{\mathbf{d}}_s$ (the structure's velocity), and the internal mesh velocity is determined by a smoothing algorithm.

The most important is satisfying the GCL (Geometric Conservation Law). When the mesh moves, if the discretization of the conservation laws is not consistent, spurious source terms can appear even for a uniform flow.

This equation requires that the temporal change in cell volume matches the flux of the mesh velocity. In Fluent or STAR-CCM+, the GCL is automatically satisfied, but caution is needed for custom solvers in OpenFOAM.

Even with a uniform flow input, non-physical fluctuations in pressure or energy will occur. GCL errors become particularly pronounced with first-order time accuracy. It's important to use second-order time integration and correctly use the mesh positions from the previous step when calculating mesh velocity.

Let's compare typical methods.

In Fluent's Diffusion-based smoothing, setting the diffusivity as the inverse of the distance from the wall (the Boundary Distance option) suppresses mesh deformation near walls and preserves the quality of prism layers.

Stability and accuracy change significantly depending on the coupling strength.

Weak coupling has a one-step delay (time lag). It can remain stable for large density ratios $\rho_s/\rho_f$ (e.g., metal structure + air), but for $\rho_s/\rho_f \approx 1$ (e.g., blood vessel + blood, rubber + water), added mass instability occurs and weak coupling cannot be used.

For structures in air ($\rho_s/\rho_f \gg 1$), weak coupling is often stable enough. However, use strong coupling if accuracy is prioritized. For structures in water ($\rho_s/\rho_f \sim 1-10$), strong coupling is always necessary.

The Aitken $\Delta^2$ acceleration method is the simplest and most effective. It dynamically optimizes the relaxation factor for coupling iterations.

Here, $\mathbf{r}^k$ is the interface residual at the $k$-th iteration. While fixed relaxation factors (e.g., $\omega = 0.5$) often require 10-20 iterations, Aitken acceleration often converges in 3-5 iterations.

It's standard in preCICE. It was also recently added to Ansys System Coupling. In OpenFOAM, custom implementation is needed for coupling solidDisplacementFoam and pimpleFoam, but it's easy if you use the preCICE adapter.

When structural deformation becomes comparable to the original mesh size, smoothing alone cannot cope. At that point, automatic remeshing is necessary.

• Fluent: Remeshing option in Dynamic Mesh Zone. Automatically regenerates tetrahedral mesh locally when cell quality falls below a threshold.
• STAR-CCM+: Remeshing possible as a fallback when Morpher fails.
• OpenFOAM: Local refinement/coarsening with dynamicRefineFvMesh, remeshing with tetDecomposition.

However, remeshing introduces interpolation errors in the solution. Quality control is particularly difficult for remeshing boundary layer prism meshes. For extremely large deformations, consider switching to the Overset mesh method or IBM (Immersed Boundary Method).