Presentation on theme: "Introductory FLUENT Training"— Presentation transcript:
1Introductory FLUENT Training Chapter 3 Solver BasicsThis lecture follows the first tutorial. The purpose of this lecture is to confirm in the minds of the users what they have just seen in the demo and the first tutorial.Introductory FLUENT TrainingSharif University of TechnologyLecturer: Ehsan Saadati
2FLUENT 12 GUI NavigationThe FLUENT GUI is arranged such that the tasks are generally arranged from top to bottom in the project setup tree.Selecting an item in the tree opens the relevant input items in the center pane.GeneralModelsMaterialsBoundary ConditionsSolver SettingsInitialization and CalculationPostprocessingThis slide is meant to be an overview of this lecture and relates steps discussed in the Intro to CFD analysis to actions in the fluent GUI. Obviously, some of the actions have their own dedicated lectures. This lecture covers the rest.
3Scaling the Mesh and Selecting Units When FLUENT reads a mesh file (.msh), all physical dimensions are assumed to be in units of meters.If your model was not built in meters, then it must be scaled.Verify that the Domain Extents are correct after scaling the mesh.When importing a mesh under Workbench, the mesh does not need to be scaled; however, the units are set to the default MKS system.Any “mixed” units system can be used if desired.By default, FLUENT uses the SI system of units (specifically, MKS system).Any units can be specified in the Set Units panel, accessed from the top menu.DefineUnits…
4Text User InterfaceMost GUI commands have a corresponding TUI command.Many advanced commands are only available through the TUI.Press the Enter key to display the command set at the current level.q moves up one level.FLUENT can be run in batch mode or scripted using a journal file (see Appendix)A TUI user guide is available on the FLUENT User Services Center
5Mouse FunctionalityMouse button functionality depends on the chosen solver (2D / 3D) and can be configured in the solver.Default settings2D SolverLeft button translates/pans (dolly)Middle button zoomsRight button selects/probes3D SolverLeft button rotates about 2 axesMiddle click on point in screen centers point in windowRetrieve detailed flow field information at point with Probe enabled.Right-click on the graphics display.Mouse controls can be set to emulate those in Workbench!DisplayMouse Buttons…
6Material PropertiesFLUENT provides a standard database of materials and the ability to create a custom user-defined database.Your choice of physical models may require multiple materials and dictate which material properties must be defined.Multiphase (multiple materials)Combustion (multiple species)Heat transfer (thermal conductivity)Radiation (emissivity and absorptivity)Material properties can be directly customized as function of temperature/pressureUse of other solution variable(s) requires UDF.
7Materials Databases FLUENT materials database Provides access to a number of pre-defined fluid, solid and mixture materials.Materials can be copied to the case file and edited if required.Custom material database:Create a new custom database of material properties and reaction mechanisms from materials in an existing case file for reuse in future cases.Custom databases can be created, accessed and modified from the standard materials panel in FLUENT.
8Operating ConditionsThe Operating Pressure with a Reference Pressure Location sets the reference value that is used in computing gauge pressures.The Operating Temperature sets the reference temperature (used when computing buoyancy forces.Specified Operating Density sets the reference value for flows with widely varying density.
9Parallel ProcessingParallel processing can be used to run FLUENT on multiple processors to decrease turnaround time and increase simulation efficiency.Critical for cases involving large meshes and/or complex physics.FLUENT is fully parallelized and capable of running across most hardware and software configurations, such as compute clusters or multi-processor machines.Parallel FLUENT can be launched either using the system command prompt or using the FLUENT Launcher panel.For example, to launch an n-CPU parallel session, use the command fluent 3d –tnThe mesh can be partitioned either manually or automatically using a number of different methods.Non-conformal meshes, sliding mesh interfaces and shell conduction zones require partitioning in serial.A web-based lecture is available on the FLUENT User Services Center.To end the lecture, this single slide was included to make the users aware that they can run the solver in parallel. The intention of this slide is to make them aware of this functionality and the fact that the mesh has to be partitioned. You should not go into the details of the different ways a mesh can be partitioned.
10SummaryThis lecture has presented many basic tasks that are often performed during a CFD simulation setup.Parallel processing can be used to reduce calculation time. This is advantageous only on large meshes.A later lecture contains material related to the setup and solution of time-dependent problems.Other topics not discussed (see Appendix for information).Mesh heirarchy and relationships.Reordering and modifying the mesh in the solver.Polyhedral mesh conversion.Solution-based mesh adaption.
12FLUENT Journals FLUENT can be run in batch mode using journal files. A journal file is a text file which contains TUI commands which FLUENT will execute sequentially.The FLUENT TUI accepts abbreviations of the commands; for example,ls Lists the files in the working folderrcd Reads case and data fileswcd Writes case and data filesrc/wc Reads/writes case filerd/wd Reads/writes data fileit IterateTUI commands in a batch file can be used to automate operations in a non-interactive mode.The TUI commands file/read-bc and file/write-bc can be used for reading and writing the settings for a FLUENT session to and from a file, respectively.A web-based training module is available which explains this processSample Journal File; Read case filerc example.cas.gz; Initialize the solution/solve/initialize/initialize-flow; Calculate 50 iterationsit 50; Write data filewd example50.dat.gz; Calculate another 50 iterations; Write another data filewd example100.dat.gz; Exit FLUENTexityes
13Reading the Mesh – Zones plateplate-shadowwalloutletDefault-interior zone(s) can always be ignored.inletfluid (cell zone)In this example, there are two cell zones (fluid-upstream and fluid-downstream).Because of this, FLUENT splits the exterior wall zone into two zones (wall and wall:001). This is because an external boundary cannot span multiple cell zones.FLUENT also splits the orifice plate into two walls also (plate and plate-shadow) since the plate zone is an internal wall.They should have seen most of this in the demo. Now some of it can be reviewed here as well as the concepts of shadow-wall and default-interior.
14Mesh Information and Hierarchy All mesh information is stored in the mesh file.Node coordinatesConnectivityZone definitionSimilar to the way geometry is defined, mesh entities obey a hierarchy:Node Edge intersection / grid pointEdge Boundary of a face (defined by two nodesFace The boundaries of cells, defined by a collection of edgesCell The control volumes into which the domain is discretized.Zone A collection of nodes, edges, faces or cells.The computational domain is defined by all members of the hierarchyFor fluid flow simulation only, the domain consists only of the fluid region.For conjugate heat transfer or fluid-structure interaction problems, the domain needs to include any solid parts that are present.Boundary data is assigned to face zones.Material data and source terms are assigned to cell zones.NodeBoundary FaceCellCell CenterCell FaceSimple 2D MeshNodeBoundary FaceCellEdgeThis slide was taken from the Tgrid lecture. Here the grid structure is formally defined; necessary to make later discussions clear.Simple 3D mesh
15Reordering and Modifying the Grid The grid can be reordered so that neighboring cells are near each other in the zones and in memoryImproves efficiency of memory access and reduces the bandwidth of the computationReordering can be performed for the entire domain or specific cell zones.The bandwidth of each partition in the grid can be printed for reference.The face/cell zones can also be modified by the following operations in the Grid menu:Separation and merge of zonesFusing of cell zones with merge of duplicate faces and nodesTranslate, rotate, reflect face or cell zonesExtrusion of face zones to extend the domainReplace a cell zone with another or delete itActivate and Deactivate cell zonesGridReorderDomainGridReorderZonesGridReorderPrint Bandwidth
16Polyhedral Mesh Conversion A tetrahedral or hybrid grid can be converted to polyhedra in the FLUENT GUI (not in the preprocessor).Generate a tetrahedral mesh then convert inside FLUENT.AdvantagesImproved mesh quality.Can reduce cell count significantly.User has control of the conversion process.Disadvantages:Cannot be adapted or converted again.Cannot use tools such as smooth, swap, merge and extrude to modify the mesh.Two conversion options are available in the Grid menu:Convert all cells in the domain (except hex cells) to polyhedraCannot convert meshes with hanging nodesHexCore mesh can be converted using the tpoly standalone utility.Convert only highly skewed cells to polyhedraTet/Hybrid MeshPolyhedral MeshGridPolyhedraConvert DomainGridPolyhedraConvert Skewed Cells
17Profile Data and Solution Data Interpolation FLUENT allows interpolation of selected variable data on both face zones and cell zones by using profile files and data interpolation files, respectively.For example, a velocity profile from experimental data or previous FLUENT run at an inlet, or a solution interpolated from a coarse mesh to fine mesh.Profile files are data files which contain point data for selected variables on particular face zones, and can be both written and read in a FLUENT session.Similarly, Interpolation data files contain discrete data for selected field variables on particular cell zones to be written and read into FLUENT.FileProfile…WriteFileProfile…ReadFileInterpolate…
18Mesh AdaptionMesh adaption refers to refinement and/or coarsening cells where needed to resolve the flow field without returning to the preprocessor.Mark cells satisfying the adaption criteria and store them in a “register.”Display and modify the register if desired.Click Adapt to adapt the cells listed in the register.Registers can be defined based on:Gradients or isovalues of all variablesAll cells on a boundaryAll cells in a region with a defined shapeCell volumes or volume changesy+ in cells adjacent to wallsTo assist adaption process, you can:Combine adaption registersDraw contours of adaption functionDisplay cells marked for adaptionLimit adaption based on cell size and number of cellsRefine Threshold should be set to 10% of the value reported in the Max field.The mechanics of using grid adaption is discussed here. When to use it is still in the Solvers lecture.
19Adaption Example – Supersonic Projectile Adapt grid in regions of large pressure gradient to better resolve the sudden pressure rise across the shock.Large pressure gradient indicating a shock (poor resolution on coarse mesh)Initial Mesh (Generated by Preprocessor)Pressure Contours on Initial Mesh
20Adaption Example – Supersonic Projectile Solution-based mesh adaption allows better resolution of the bow shock and expansion wave.Mesh adaption yields much better resolution of the bow shock.Adapted cells in locations of large pressure gradientsAdapted Mesh (Multiple Adaptions Based on Gradients of Pressure)Pressure Contours on Adapted Mesh