CFD INSIGHT MODULE: FLOODING
The CFD Flooding module, an add-on product to the InsightCAE framework defines and solves the flooding for (ship)compartments and containers for investigating fluid flow, fill up time as well as resulting forces and moments in conjunction with other physical phenomena.
The CFD Flooding module provides the easy setup with a minimum of input of parameters and leads through the automated simulation process of
- incompressible two phase and
- turbulent flow
The capabilities are implemented through structured flow interfaces to define, solve and analyze time-dependent (transient) flooding problems in 3D. Silentdynamics provides best practice, robust and stable simulation parameters using OpenFOAM in the background. Meshing, solving and post-processing is automated. As result, the user get a PDF report including all (user)defined results.
Start the workbench through
and open a new analysis selecting the flooding module
The Input InsightCAE GUI will be displayed:
The needed simulation parameters are displayed at the right side of GUI. The user need to specify the yellow highlighted entries at least.
The filling fluid parameters defined in the fluid section. As default the parameters of water are set. Note: Initial air is inside the geometry (not to be changed). An appropriate turbulence model must be specified.
|PIM||Point inside flooding volume. Coordinates in geometry CS.|
|geomtreyFile||CAD input (STL)|
|inletName||Name of inlet patch in STL file. patchXX in case of binary STL file.|
|outletName||Name of inlet patch in STL file. patchXX in case of binary STL file.|
|outlet_submerged||Whether the outlet is submerged below the water surface (true) or connected to the atmosphere, e.g. by an air-filled pipe (false)|
The Point-In-Mesh(PIM) have to be specified inside the domain for meshing parameter. Loading the geometry could be done by a singleSTL file or multipleSTL files. If singleSTL is selected, the STL file must contain regions specifying the inlet and outlet part. The name of inlet inletName and name of the outlet outletName must be defined. Entry outlet_submerged needs to be set as true or false whether the outlet is submerged below the water surface (true) or connected to the atmosphere, e.g. by an air-filled pipe (false).
For mulipleSTL the STL files need to defined separately. Click on +Add new button to add the number of present stl files. Each STL file as a single array with the extended parameters:
|Parameter for multipleSTL||Description|
|extract_features||Whether to extract the feature edges from this geometry for meshing|
|geometryfile||STL file with geometry|
|name||Name of patch in CFD model which will be generated from this file. Must be unique|
|lm - Minimum refinement level on this geometry. This overrides the global settings|
|lx - Maximum refinement level on this geometry. This overrides the global settings.|
|patch_type||role of this patch in CFD model (inlet/outlet/wall)|
|frictionless_wall - Whether to set slip wall treatment for this geometry. Will be ignored, if this is not a wall.|
|include_in_forces - Whether to include the patch in force integration|
|unit||Unit of coordinates in file|
|linkmesh||If not empty, the mesh will not be generated, but a symbolic link to the polyMesh folder of the specified OpenFOAM case will be created.|
|lm||Minimum refinement level on geometry.|
|lx||Maximum refinement level on geometry and refinement level at feature curves.|
|ndiag||number of cells across geometry bounding box diagonal in template mesh|
|nlayers||Number of prism layers|
For the meshing process an intial mesh which is created with the given dimension from the input stl file(s). The parameter ndiag defines the number of cells across the diagional line of the overall dimension. Using the parameters lm and lx the mesh could be locally at the boundaries refined whereas the parameter ndiag controls the global mesh size.
|draught||[m] draught for which the simulation will be performed. The geometry is expected to be in a coordinate system with z=0 at the keel. The final grid will be shifted vertically by this value to meet z=0 at the free surface.|
|init_inlet||initialize water volume fraction in cells next to inlet|
|init_volume||initialize water volume fraction inside box|
|fillbox_max - maximum coordinates corner of fill box. Coordinates in geometry CS|
|fillbox_min - maximum coordinates corner of fill box. Coordinates in geometry CS.|
Parameter | Description ------------------------|:----------------------------- OFEname| (OFesi1806) Identifier of the OpenFOAM installation, that shall be used evaluateonly | Whether to skip solver run and do only the evaluation expected_flooding_time | [s] Expected time for flooding simulation. machine | Machine or queue, where the external commands are executed on. Defaults to 'localhost', if left empty. mapFrom | Map solution from specified case, if not empty. potentialinit is skipped if specified. np| Number of processors for parallel run (less or equal 1 means serial execution) np_mesh| Number of processors for meshing process numerics_setup| (stable/accurate) Tuning direction of numerical solver settings. output_intervall| [s] Interval between output times. Choose high, if no field output is needed. Adjust reasonably high, if movie rendering is intended. execution_directory| Directory to store data files during analysis. Leave empty for temporary storage.
Running the simulation
If all parameters are set. I start the simulation by clicking on the "Run" button in the upper right corner. The GUI switches to the tab "Run" and the progress is displayed in the log window and, as soon as the solver has started, the residuals, forces and so on are also displayed graphically:
Then the flow solver starts. While the flow solver is running, the most important parameters that CFD specialists are usually interested in are displayed online in various diagrams. These include residuals and continuity errors, both of which should be as small as possible, and the forces and moments that will eventually become stationary and should no longer change when the container is filled up.
The simulation runs for the expected flooding time. If one determines beforehand that the container is filled, one can force by clicking on the button "Write+Stop" that output is written immediately and the solver stops afterwards and starts the evaluation. By clicking on the button "Write now", a signal file is created in the case directory, which is recognized by the OpenFOAM solver and leads to immediate output of the current time step. This is useful, if Paraview is running with the current case loaded and an update is demanded.
Analogously, by hitting the button "Write+Stop", immediate output is triggered but the solver is gracefully stopped immediately. This is useful, if you recognize that the container has filled up and you do not want to wait any longer.
Once the solver has finished, the evaluation is run. A number of figures, renderings and graphs as filling volume over time, forces etc. are created and displayed in the "Output" tab.
If the generated renderings do not suffice, you can also perform further evaluations with Paraview afterwards. The generated OpenFOAM case with all results is left in the working directory of the simulation. A click on "Paraview" on the right side starts Paraview.
If something went wrong or the setup has to be changed click on the "Clean " button to delete all simulation files Change the parameters und
Generating the report
The displayed so-called result elements, can be compiled into a PDF-Report by selecting "Results > Create report..." in the menu. You can either create a TEX file or a PDF file. In the same directory as the report, a directory "report_data_[input filename]" is created. In this directory, all figures from the report (except the rendering images) are contained in script-readable ASCII format.