OpenFOAM now includes avalanche modelling, based on the newly integrated finite area functionality. This contribution includes a new solver with many submodels to include the effects of:
- Source code
- $WM_PROJECT_DIR/modules - see the avalanche directory
- $WM_PROJECT_DIR/modules - see the avalanche/tutorials directory
- This project is the work of Matthias Rauter and described by the
- Rauter and Tukovic (submitted to Computer & Fluids): A finite area scheme for shallow granular flows on three-dimensional surfaces
- The code has been integrated into OpenFOAM by OpenCFD as a new module
A new Arrenius laminar transport model is available for incompressible flows where the fluid viscosity is dependent on another field variable, e.g. on temperature for glass, syrup.
The viscosity is calculated using:
This model is provided as a wrapper for the existing viscosity models, e.g. BirdCarreau, Casson, etc.. and selected in the constant/transportProperties dictionary, e.g.:
- Source code
The new energyTransport function object enables users to evolve a simplified energy transport equation for incompressible flows, available to all incompressible solvers.
Inertial, conduction and convection terms are included, plus a run-time selectable source term using the fvOption framework. An incompressible flow assumption is employed whereby the temperature is modelled as a passive scalar and does not influence the fluid physical properties.
- The field name entry must represent a temperature field and its boundary conditions specified in the start time directory, e.g.0/T
- The turbulence model should be incompressible
- For incompressible multi-phase cases a list of thermal properties must be provided
- Source code
The externalCoupled function object has been extended to offer greater flexibility when coupling OpenFOAM to external applications. In previous versions, the presence of the lock file was used to identify which application should execute. The lock file now contains additional information that can be used to terminate the OpenFOAM application, acting similarly to the abort function object, i.e.
- action=writeNow: write at next time-step and terminate
- action=nextWrite: terminate at the next write
- action=noWriteNow: terminate at the next time-step without writing.
- Source code
Sub-looping has been added to the Conjugate Heat Transfer (CHT) solvers as a convergence aid for the energy solution.
The sub-looping is defined, e.g. in the SIMPLE dictionary in the $FOAM_CASE/system/fvSolution file:
// timeStart 0;
// timeEnd 100;
// Convergence criteria to stop looping
// Names of function objects to fire with execute(int) when looping
onLoop ( );
// Names of function objects to fire with execute(int) when converged
onConverged ( externalCoupled );
// Names of function objects to fire with execute(int) when loop ends
// without convergence
onEnd ( );
The effectivenessHeatExchangerSource fvOption has been extended to operate according to a target heat rejection. This is applicable to steady state cases whereby the user wishes to evolve, e.g. the top hose temperature to achieve the target heat rejection.
The standard entries, e.g.
secondaryInletT 375.75; // Initial temperature only
can now be extended by the optional entries:
// Optional controls
// targetQdotCalcInterval 5;
// targetQdotRelax 0.5;
As an example, when operating to acheieve a target heat rejection of the secondary inlet temperature converged to :
and when operating with a fixed secondary inlet temperature of , the predicted heat rejection was shown to be :
confirming that the model operates symetrically.
The new heatTransferCoeff function object provides several methods to compute the heat transfer coefficient [W/m2/K] for a set of user-specified patches.
The methods include:
- ReynoldsAnalogy: coefficient derived from the local skin friction
- localReferenceTemperature: based on the temperature difference between the patch internal cells and patch faces; note: sensitive to the mesh
- fixedReferenceTemperature: based on the temperature difference between a user-specified reference temperature (typically the inlet temperature) and patch faces
The heat transfer coefficient should be described in the functions sub-dictionary of the $FOAM_CASE/system/controlDict file, e.g. for an incompressible solver:
UInf (20 0 0);
The result is stored on the mesh database, and written to disk as a volScalarField according to the usual write controls.
The kOmega family of turbulence models has been extended to include turbulence decay control, as described in the reference:
Spalart, P. R. and Rumsey, C. L. (2007). Effective Inflow Conditions for Turbulence Models in Aerodynamic Calculations. AIAA Journal, 45(10), 2544 - 2553.
The model is particularly suited to wind-tunnel-like cases, whereby the user wishes to maintain the inlet turbulence levels upstream of any obstacles.
Decay control is inactive by default, and enabled using:
kInf <far-field k value>;
omegaInf <far-field omega value>;
The new viscousDissipation fvOption provides a mechanism to include viscous dissipation effects in the energy equation. It can be applied to both compressible solvers with a ‘native’ energy equation configured using the thermophysicalProperties dictionary, and incompressible solvers when combined with the new energyTransport function object.
rho rho; //rho Field