solidTraction

Overview

solidTraction imposes a known surface traction $\mathbf{t}$ and/or normal pressure $p$ on the displacement field D of a solid region. It is the uncoupled counterpart of the FSI traction BC: use it for loaded or traction-free solid surfaces that are not coupled to another region. The class derives from fixedGradient (vector only). In each update it recomputes the displacement normal gradient so that the stress on the patch matches the prescribed load. The traction and the pressure can each be given as a constant field, as a time series, or as a separate volume field. It was ported from the foam-extend solid-mechanics toolbox (Cardiff, Tuković). It reads the fields of solidStVK (impK, rImpK, gradD, sigma, Finv).

Mathematical Formulation

The target condition is a traction balance in the current (deformed) configuration:

It is imposed through the normal gradient of D, in the segregated “implicit stiffness” form used by solidStVK:

$\boldsymbol{\sigma}$ and $\nabla\mathbf{D}$ are the current patch values. When the iteration has converged, $\mathbf{g} = \mathbf{n}_0\cdot\nabla\mathbf{D}$, so the bracket requires $\mathbf{n}_c\cdot\boldsymbol{\sigma} = \mathbf{t} - p\,\mathbf{n}_c$. The $K\,\mathbf{n}_0\cdot\nabla\mathbf{D}$ term mirrors the implicit/explicit Laplacian pair in the solidStVK momentum equation.

The patch value is then reconstructed from the gradient:

with $\mathbf{k} = (\mathbf{I}-\mathbf{n}_0\mathbf{n}_0)\cdot\boldsymbol{\Delta}$.

Note on OpenFOAM.com. In OpenFOAM.com, fvPatch::delta() is patch-normal for non-coupled patches, so $\mathbf{k} \equiv \mathbf{0}$ and the non-orthogonal term in $\mathbf{D}_b$ has no effect.

Implementation

Construction. The dictionary constructor reads secondOrder, setEffectiveTraction and relaxationFactor. It reads gradient and value if present, otherwise it starts from zero gradient and the patch-internal value. It then sets up the traction and the pressure. For each, exactly one of three forms is allowed. Giving two forms of the same quantity stops the run (FatalError):

If neither a series nor a field is given, traction and pressure are read as plain patch fields, so both are required.

updateCoeffs() (skipped if already updated in this evaluation):

1. Once per time step (tracked through curTimeIndex_), calls correctBoundaryConditions() on the tractionField / pressureField, if one is used.
2. Updates $\mathbf{t}$ and $p$ from the field or the series.
3. If setEffectiveTraction is on, subtracts the patch values of a volScalarField named p from the pressure. This applies the effective rather than the total traction, which is meant for poro-elastic solids.
4. Looks up impK, rImpK, gradD, sigma and Finv on the patch. All are mandatory.
5. Computes $\mathbf{n}_c$ and the relaxed gradient $\mathbf{g}$ above, then calls fixedGradient::updateCoeffs().

evaluate() calls updateCoeffs() if needed. It looks up the cell gradient field named grad<fieldName> (i.e. gradD for D), sets $\mathbf{D}_b$ by the formula above and resets the updated flag. The matrix coefficients are those of the stock fixedGradient condition: the gradient $\mathbf{g}$ enters the Laplacian as an explicit flux.

Interaction with solidStVK. D boundary conditions are updated when the momentum equation for D is assembled. sigma, gradD and Finv come from the previous Picard / DNA iteration (updated in solidStVK::postSolve()), so the traction is enforced iteratively. It converges together with the PICARD loop on D. The relaxationFactor gives extra under-relaxation of the gradient if this loop oscillates.

write() writes the form actually used for traction and pressure (tractionField/tractionSeries/traction, and likewise for pressure), then secondOrder, setEffectiveTraction, relaxationFactor, value and gradient.

Dictionary Entries

In the series sub-dictionary, outOfBounds defaults to warn and readerType to openFoam. Both are standard OpenFOAM interpolationTable keywords.

Required registered fields on the solid mesh:

Usage

Traction-free surface (0/<solid>/D):

freeSurface
{
    type            solidTraction;
    traction        uniform (0 0 0);
    pressure        uniform 0;
    value           uniform (0 0 0);
}

Uniform pressure ramped in time from a table file:

loadedSurface
{
    type            solidTraction;
    traction        uniform (0 0 0);
    pressureSeries
    {
        file        "$FOAM_CASE/constant/solid/pressureSeries";
        outOfBounds clamp;
    }
    relaxationFactor 0.8;
    value           uniform (0 0 0);
}

with constant/solid/pressureSeries in the openFoam table format, e.g. ( (0 0) (1 1e4) ).

Known Limitations

• Only for solidStVK. The fields impK, rImpK, gradD, sigma and Finv are looked up unconditionally. No other compiled region type provides all of them.
• Field and series data are uniform or per face only. tractionSeries / pressureSeries give a value that is uniform over the patch. traction / pressure are constant in time. For space- and time-varying loads, use tractionField / pressureField and drive that field’s own boundary conditions (they are corrected once per time step).
• setEffectiveTraction needs a p field on the solid mesh. No shipped solid region type registers one.
• Non-orthogonal correction has no effect in OpenFOAM.com (patch-normal delta(); see the note above).
• Copies lose the field link. The mapping and copy constructors do not copy tractionFieldPtr_ / pressureFieldPtr_. A cloned patch field (e.g. a stored old-time or previous-iteration copy) keeps the last traction/pressure values and stops following the field. The original boundary condition of D is not affected.
• Inconsistent gradient names. updateCoeffs() always reads gradD, while evaluate() reads grad<fieldName>. On a field other than D the two differ.

Tutorials

No tutorial uses solidTraction. The FSI tutorials use regionCoupledTraction on the coupled solid surface and fixedValue / solidSymmetry elsewhere.

References

• Cardiff, P., Karač, A., De Jaeger, P., Jasak, H., Nagy, J., Ivanković, A., Tuković, Ž., An open-source finite volume toolbox for solid mechanics and fluid-solid interaction simulations, arXiv:1808.10736, 2018.
• Alkfri, A., Habes, C., Marschall, H., multiRegionFoam: A Unified Multiphysics Framework for Multi-Region Coupled Continuum-Physical Problems, Engineering with Computers, 2023. DOI: 10.1007/s00366-024-01974-4