OpenFOAM v11 User Guide - 2.2 Breaking of a dam

2.2 Breaking of a dam

In this example we shall solve a problem of a simplified dam break in 2 dimensions using the incompressibleVoF modular solver. The feature of the problem is a transient flow of two fluids separated by a sharp interface, or free surface. The two-phase algorithm in incompressibleVoF is based on the volume of fluid (VoF) method in which a phase transport equation is used to determine the relative volume fraction of the two phases, or phase fraction , in each computational cell. Physical properties are calculated as weighted averages based on this fraction. The nature of the VoF method means that an interface between the phases is not explicitly computed, but rather emerges as a property of the phase fraction field. Since the phase fraction can have any value between 0 and 1, the interface is never precisely defined, but occupies a volume around the region where a sharp interface should exist.

The test setup consists of a column of water at rest located behind a membrane on the left side of a tank. At time , the membrane is removed and the column of water collapses. During the collapse, the water impacts an obstacle at the bottom of the tank and creates a complicated flow structure, including several captured pockets of air. The geometry and the initial setup is shown in Figure 2.15 .

---

---

2.2.1 Mesh generation

The user should go to their run directory and copy the damBreak case from the $FOAM_TUTORIALS/incompressibleVoF/damBreakLaminar directory, i.e.

Go into the damBreak case directory and generate the mesh running blockMesh as described previously. The damBreak mesh consist of five blocks; the blockMeshDict entries are given below.

The mesh is written into a set of files in a polyMesh directory in the constant directory. The use can list the contents of the directory to reveal the set of files/

The files include: points, a list of the cell vertices; faces, a list of the cell faces; owner and neighbour, containing the indices of cells connected to a given face; boundary, a description of the boundary patches.

2.2.2 Boundary conditions

The boundary file can be read and understood by the user. The user should take a look at its contents, either by opening it in a file editor or printing out in the terminal window using the cat utility.

The file contains a list of five boundary patches: leftWall, rightWall, lowerWall, atmosphere and defaultFaces. The user should notice the type of the patches. Firstly, the atmosphere is a standard patch, i.e. has no special attributes, merely an entity on which boundary conditions can be specified. Then, the defaultFaces patch is formed of block faces that are omitted from the boundary sub-dictionary in the blockMeshDict file. Those block faces form a patch whose properties are specified in a defaultPatch sub-dictionary in the blockMeshDict file. In this case, the default type is set to empty since the patch normal is in the direction we will not solve in this 2D case.

The leftWall, rightWall and lowerWall patches are each a wall. Like the generic patch, the wall type contains no geometric or topological information about the mesh and only differs from the plain patch in that it identifies the patch as a wall. This is required by some modelling, e.g. turbulent wall functions and some turbulence models which include the distance to the nearest wall in their calculations.

With VoF specifically, surface tension models can include wall adhesion at the contact point between the interface and wall surface. Wall adhesion models can be applied through a special boundary condition on the alpha () field, e.g. the constantAlphaContactAngle boundary condition, which requires the user to specify a static contact angle, theta0.

This example ignores surface tension effects between the wall and interface. This can be done can do this by setting the static contact angle, , but a simpler approach is to apply the zeroGradient condition to alpha on the walls.

The top boundary is free to the atmosphere so needs to permit both outflow and inflow according to the internal flow. We therefore use a combination of boundary conditions for pressure and velocity that does this while maintaining stability. They are:

• prghTotalPressure, applied to the pressure field, minus the hydrostatic component, , given by Equation 6.3 ;
• pressureInletOutletVelocity, applied to velocity , which sets zeroGradient on all components of , except where there is inflow, in which case a fixedValue condition is applied to the tangential component;
• inletOutlet applied to other fields, which is a zeroGradient condition when flow outwards, fixedValue when flow is inwards.

At all wall boundaries, the fixedFluxPressure boundary condition is applied to the pressure field, which adjusts the pressure gradient so that the boundary flux matches the velocity boundary condition for solvers that include body forces such as gravity and surface tension.

The defaultFaces patch representing the front and back planes of the 2D problem, is, as usual, an empty type.

2.2.3 Phases

The fluid phases are specified in the phaseProperties file in the constant directory as follows:

It lists two phases, water and air. Equations for phase fraction are solved for the phases in the list, except the last phase listed, i.e. air in this case. Since there are only two phases, only one phase fraction equation is solved in this case, for the water phase fraction , specified in the file alpha.water in the 0 directory.

The phaseProperties file also contains an entry for the surface tension between the two phases, specified by the keyword sigma in units .

2.2.4 Setting initial fields

Unlike the previous cases, we shall now specify a non-uniform initial condition for the phase fraction where

(2.5)

This is done by running the setFields utility. It requires a setFieldsDict dictionary, located in the system directory, whose entries for this case are shown below.

The defaultFieldValues sets the default value of the fields, i.e. the value the field takes unless specified otherwise in the regions list. That list contains sub-dictionaries with fieldValues that override the defaults in a specified region. Regions are defined by functions that define a set of points, faces, or cells. Here boxToCell creates a box defined by minimum and maximum bounds that defines the set of cells of the water region. The phase fraction is specified as 1 in this region.

The setFields utility reads fields from file and, after re-calculating those fields, will write them back to file. In the damBreak case, the alpha.water field is initially stored in its original form with the name alpha.water.orig. A field file with the .orig extension is read in when the actual file does not exist, so setFields will read alpha.water.orig but write the resulting output to alpha.water (or alpha.water.gz if compression is switched on). This way the original file is not overwritten, so can be reused.

The user should execute setFields like any other utility by:

Using paraFoam, check that the initial alpha.water field corresponds to the desired distribution as in Figure 2.16.

---

---

2.2.5 Fluid properties

The physical properties for the air and water phases are specified in physicalProperties.air and physicalProperties.water files, respectively, in the constant directory. Physical properties describe characteristics of the fluid in a absence of flow. Each file specifies the viscosity model through the viscosityModel keyword, which is set to constant to indicate the value is unchanging. The viscosity is then specified by the nu keyword in units . The density of each fluid is also specified by the keyword rho in units . The physicalProperties.air file is shown below as an example:

If the viscosity does change according to the flow, e.g. as in non-Newtonian or visco-elastic fluids, then those models are specified through the momentumProperties file, as described in section 8.3 .

2.2.6 Gravity

Gravitational acceleration is uniform across the domain and is specified in a file named g in the constant directory. Unlike a normal field file, e.g. U and p, g is a uniformDimensionedVectorField and so simply contains a set of dimensions and a value that represents for this case:

2.2.7 Turbulence modelling

As in the cavity example, the choice of turbulence modelling method is selectable at run-time through the simulationType keyword in momentumTransport dictionary. In this example, we wish to run without turbulence modelling so we set laminar:

2.2.8 Time step control

The simulation of the damBreak case is fully transient so the time step requires attention. The Courant number is an important consideration relating to time step. It is dimensionless parameter which can be defined for each cell as:

(2.6)

where is the time step, is the magnitude of the velocity through that cell and is the cell size in the direction of the velocity. With explicit solution, stability requires the maximum at least; stricter limits exist depending on the choice of advection scheme. Implicit solutions do not have the same stability limit of the maximum , but temporal accuracy becomes more relevant as increased beyond 1.

Time step control is particularly important with interface-capturing. The incompressibleVoF solver module uses the multidimensional universal limiter for explicit solution (MULES), created by Henry Weller, to maintain boundedness of the phase fraction. needs to be limited depending on the choice of MULES algorithm. With the original explicit MULES algorithm, an upper limit of for stability is typically required. However, there is also the semi-implicit version of MULES, specified by the MULESCorr switch in the fvSolution file. For semi-implicit MULES, there is really no upper limit in for stability, but instead the level is determined by requirements of temporal accuracy.

In general it is difficult to specify a fixed time-step to satisfy the criterion since is changing from cell to cell during the simulation. Instead, automatic adjustment of the time step is specified in the controlDict by switching adjustTimeStep to on and specifying the maximum for the phase fields, maxAlphaCo, and other fields, maxCo. In this example, the maxAlphaCo and maxCo are set to 1.0. The upper limit on time step maxDeltaT can be set to a value that will not be exceeded in this simulation, e.g. 1.0.

By using automatic time step control, the steps themselves are never rounded to a convenient value. Consequently if we request that OpenFOAM saves results at a fixed number of time step intervals, the times at which results are saved are somewhat arbitrary. However with automatic time step adjustment, results can be written at fixed times using the adjustableRunTime option for writeControl in the controlDict dictionary. With this option, the automatic time stepping procedure further adjusts their time steps so that it ‘hits’ on the exact times specified by the writeInterval, set to 0.05 in this example. The controlDict dictionary entries are shown below.

2.2.9 Discretisation schemes

The MULES method, used by the incompressibleVoF modular solver, maintains boundedness of the phase fraction independently of the underlying numerical scheme, mesh structure, etc. The choice of schemes for convection are therefore not restricted to those that are strongly stable or bounded, such as upwind differencing.

The convection schemes settings are made in the divSchemes sub-dictionary of the fvSchemes dictionary. In this example, the convection term in the momentum equation, , denoted by the div(rhoPhi,U) keyword, uses Gauss linearUpwind grad(U) to produce good accuracy.

The term, represented by the div(phi,alpha) keyword uses a bespoke interfaceCompression scheme where the specified coefficient is a factor that controls the compression of the interface where: 0 corresponds to no compression; 1 corresponds to conservative compression; and, anything larger than 1, relates to enhanced compression of the interface. We generally use a value of 1.0, as in this example.

The other discretised terms use commonly employed schemes so that the fvSchemes dictionary entries is as follows.

2.2.10 Linear-solver control

In the fvSolution file, the sub-dictionary in solvers for alpha.water contains elements that are specific to the MULES algorithm as shown below.

MULES calculates two limiters to keep the phase fraction within the lower and upper bounds of 0 and 1. The limiter calculation is iterative, with the number of iterations specified by nLimiterIter. As a rule of thumb, nLimiterIter can be set to 3 + to maintain boundedness.

The semi-implicit version of MULES is activated by the MULESCorr switch. It first calculates an implicit, upwind solution before applying MULES as a higher-order correction. The linear solver must be configured for the implicit, upwind solution, through the solver, smoother, tolerance and relTol parameters.

The nAlphaCorr keyword which controls the number of iterations of the phase fraction equation within a solution step. The iteration is used to overcome nonlinearities in the advection which are present in this case due to the interfaceCompression scheme.

2.2.11 Running the code

Running of the code has been described in the previous tutorial. Try the following, that uses tee, a command that enables output to be written to both standard output and files:

The code will now be run interactively, with a copy of output stored in the log file.

2.2.12 Post-processing

Post-processing of the results can now be done in the usual way. The user can monitor the development of the phase fraction alpha.water in time, e.g. see Figure 2.17 .

---

---

2.2.13 Running in parallel

The results from the previous example are generated using a fairly coarse mesh. We now wish to increase the mesh resolution and re-run the case. Using a finer mesh, we can then demonstrate the parallel processing capability of OpenFOAM.

The user should first clone the damBreak case, e.g. by

Enter the new case directory and change the blocks description in the blockMeshDict dictionary to Here, the entry is presented as printed from the blockMeshDict file; in short the user must change the mesh densities, e.g. the 46 10 1 entry, and some of the mesh grading entries to 1 2 1. Once the dictionary is correct, generate the mesh by running blockMesh.

As the mesh has now changed from the damBreak example, the user must re-initialise the phase field alpha.water in the 0 time directory since it contains a number of elements that is inconsistent with the new mesh. Note that there is no need to change the U and p_rgh fields since they are specified as uniform which is independent of the number of elements in the field.

The user should then rerun the setFields utility. However, the mesh size is now inconsistent with the number of elements in the alpha.water file in the 0 directory, so the user must delete that file so that setFields uses the original alpha.water.orig file.

Parallel computing uses domain decomposition, in which the geometry and associated fields are broken into pieces and allocated to separate processors for solution. The first step required to run a parallel case is therefore to decompose the domain using the decomposePar utility. There is a dictionary associated with decomposePar named decomposeParDict which is located in the system directory. Also, sample dictionaries can be found within the etc directory in the OpenFOAM installation, which can be copied to the case directory by running the foamGet script, e.g. (you do not need to do this):

The first entry is numberOfSubdomains which specifies the number of subdomains into which the case will be decomposed, usually corresponding to the number of processors available for the case.

This example uses the simple method of decomposition. It requires the simpleCoeffs to be configured according to the following criteria. The domain is split into pieces, or subdomains, in the , and directions, the number of subdomains in each direction being given by the vector . As this geometry is 2 dimensional, the 3rd direction, , cannot be split, hence must equal 1. The and components of split the domain in the and directions and must be specified so that the number of subdomains specified by and equals the specified numberOfSubdomains, i.e.  numberOfSubdomains.

It is beneficial to keep the number of cell faces adjoining the subdomains to a minimum so, for a square geometry, it is best to keep the split between the and directions should be fairly even. For example, let us assume we wish to run on 4 processors. We would set numberOfSubdomains to 4 and n to (2, 2, 1). The user should run decomposePar by the following command.

The terminal output shows that the decomposition is distributed evenly between the sub-domains. The decomposition writes the mesh and fields of each sub-domain into separate sub-directories named processor<N>, where N is the sub-domain ID, e.g. 0, 1, 2, etc. The user should list the files in the case directory to confirm that four directories processor0, processor1, processor2 and processor3 exist.

This example presents running in parallel with the openMPI implementation of the standard message-passing interface (MPI). The following command runs on 4 cores of a local multi-processor CPU.

The user can consult section 3.4 for more details of how to run a case in parallel. For example, the user may run on more nodes over a network by creating a file that lists the host names of the machines on which the case is to be run as described in section 3.4.3 .

2.2.14 Post-processing a case run in parallel

When the case runs in parallel, the results are written into time directories within the processor<N> sub-directories. The user can confirm this by listing the time directories for the processor0 directory.

It is possible to post-process an individual sub-domain by treating the individual processor directory as a case in its own right. For example, to view the processor1 sub-domain in ParaView, the user can launch paraFoam by running the following command.

Figure 2.18 shows the mesh from this sub-domain, following the decomposition of the domain using the simple method.

---

---

Alternatively, the decomposed fields and mesh can be reassembled for post-processing in serial. The reconstructPar utility takes the field files from time directories for the processor sub-domain and builds equivalent field files for the complete domain. The user should run the utility as follows.

The fields are reconstructed are written to solution time directories in the case directory. These fields can be visualised as normal in ParaView. The results from the fine mesh are shown in Figure 2.19. The user can see that the resolution of interface has improved significantly compared to the coarse mesh.

---

---