snappyhexmesh Basic Training single Region meshing simulation of heat transfer with scalartransportfoam

Transcription

1 Basic Training single Region meshing simulation of heat transfer with scalartransportfoam 1 st edition, Aug Editor: Philipp Schretter (TU Wien)

2 Tutorial One: Single Region Meshing Mesh creation The procedure described in this tutorial is structured in the following order: Creation of the geometry data Meshing a geometry with one single region Run an OpenFOAM simulation with the generated mesh using scalartransportfoam The reference for this tutorial is a tutorial for meshing in OpenFoam. It is located in OpenFOAM/OpenFOAM-2.x.x/tutorials/mesh//flange Objectives The aim of the tutorial is to give a basic introduction to single region meshing with the meshing tool. Understanding the advantages of No commercial software package is ultimately necessary. For the meshing, the OpenFoam environment is sufficient and no further software is necessary. The geometry can be created with any CAD program like CATIA, FreeCAD, etc. As the geometry is to be only surface data, the files need to be in.stl,.nas or.obj. format. The meshing process can be run in parallel mode. If high computational capabilities are available, high quality meshes can be generated in little time. Understanding the three basic steps of Castellation: The cells which are beyond a region set by a predefined point are deleted Snapping: Reconstructs the cells to move the edges from inside the region to the required boundary Layering: Creates additional layers in the boundary region. Post processing Import your simulation to ParaView. Analyze the heat distribution in the flange 1

3 Step by step meshing Creation of the.stl files For the geometry data, the CAD software CATIA was used, to create the solid geometry. The creation of the.stl files for single region and multi-region is slightly different. Either way, it is necessary, to create the.stl files as ASCII.stl and not as binary.stl. For the single region case, only one.stl file for the whole geometry is necessary. In case the software CATIA is used, the file can easily be created by exporting the file as.stl. CATIA automatically exports the file as ASCII.stl. Nevertheless, with CATIA, it is not possible to export different surface areas of the flange, for example only the outside part or the inside part. Therefore, the geometry data is exported from CATIA in.stp format. This.stp file is then read into FreeCAD. With FreeCAD, the.stl files can be extracted from the.stp solid geometry: Open the.stp geometry file in the draft workbench and select the object in the tree view view-section. Then click on Downgrade in the combo view view-section. This gives a list of all faces of the geometry, which can be selected and exported as.ast format. In FreeCAD, it's necessary to distinguish between.stl, which is binary.stl, and.ast, which is ASCII.stl. In FreeCAD, the surface file is exported in.ast format and afterwards renamed to.stl. 2

4 Figure 1 Select the surfaces from a solid geometry In case which was prepared for this tutorial, the dimensions from from the.stl files exported from the CAD software are in meters. To convert the dimensinos, the open source software Blender can be used. Therefore, import the.stl files and use the scale tool with a factor to convert from m to mm. To export the file, it is necessary to tick the box for Ascii to save the.stl file in ascii format. Otherwise, OpenFoam won't be able to deal with the file. In the single region case, the header line and the base line of the.stl files, exported from blender need to be updated. For example the headers and baselines in the two available.stl files are renamed to flange_outside_surface and flange_inside_surface. This is necessary to have appropriate entries in the boundary file later on for the OpenFoam simulation. In order to create a.stl from a geometry which is already available in gambit, the geometry data can be exported in.stp or alternatively in.igs format. Afterwards, the.stp or.igs (msbo) file can be imported to FreeCAD and converted via export as.stl. The technical drawing with the dimensions of the geometry for this tutorial is depicted below. 3

5 4

6 The folder constant is necessary for the mesh files. The folder system is necessary for the system settings. constant directory The constant directory must initially have the following folders - polymesh: Which contains the base mesh as blockmeshdict. Here we define a base block mesh inside. The blockmesh will contain the flange geometry. The dimensions of the blockmesh are as follows. // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // converttometers 1; Eight coordinates of a rectangular block vertices ( ( ) ( ) ( ) ( ) ( ) ( ) ( ) ( ) ); blocks labels the vertices, define number of cells along the axes and expansion ratio of cells blocks ( hex ( ) ( ) simplegrading (1 1 1) ); edges ( ); boundary defines different faces if any, based on vertices label. In this case we do not define different boundaries like 'inlet' 'outlet' etc boundary 5

7 ( ); allboundary type patch; faces ( ( ) ( ) ( ) ( ) ( ) ( ) ); // ************************************************************************ // - trisurface: The folder trisurface should contain a file with the geometry data to be meshed (stl, nas, obj). The file name is to be used as a reference pointer in later stages. system directory The system directory may have the following files, - controldict - decomposepardict If the mesh is to be run in parallel using the decomposepar utility, this file defines the parameters for distributed processors - fvschemes - fvsolution - meshqualitydict minfaceweight- can be kept at the default value of Dict: // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // set castellatedmesh, snap, addlayers to true or false depending on the stages required castellatedmesh true; snap true; addlayers true; geometry lists all surfaces except the blockmesh geometry, in the constant/trisurface directory, and define a name for each of them to be used as reference a refinementbox() can be defined. This is a a region in the blockmesh geometry which has a refined mesh. The level of refinement of this box is defined in the section refinementregions below. geometry flange_single_region.stl type trisurfacemesh; name flange_single_region; 6

8 ; The refinement box has to be larger than one cell of the blockmesh. In Order to reach a fine region in the blockmesh, several refinement boxes can be defined whereas always a smaller box is refined inside the refined box. It is always necessary to keep each box larger than the smallest cell in that region. refinementbox CASTELLATING castellatedmeshcontrols maxlocalcells ; maxglobalcells ; minrefinementcells 0; maxloadunbalance 0.0; ncellsbetweenlevels 1; The section features is used for user-defined edge refinement. It uses The emesh files, created with the surfacefeatureextract command. These.eMesh files are extracted parts from the.stl surfaces, specified in The surfacefeatureextractdict. Also the extendedfeatureedgemesh file from the constant/extendedfeatureedgemesh folder can be used. In this case,both files give the same result. features ( file "flange_single_region.emesh"; level 3; ); All surfaces defined in the geometry subdirectory must be listed here. List of the surfaces, which need to be listed in in the boundary files In constant/polymesh/boundary refinementsurfaces flange_single_region level (3 3); resolvefeatureangle is an important setting. Edges, whose adjacent surface normals are at an angle higher than the value set, are resolved. The lower the value, the better is the resolution at sharp edges resolvefeatureangle 30; refinementregions()- the refinement of the refinement box is defined. The cells in this box are split up to the number of levels defined, or until the max number of cells is reached. In this case, no refined regions are defined. refinementregions locationinmesh()- Important coordinate for single region cases, to define a region which is to be kept from the blockmesh locationinmesh (6 0 0); allowfreestandingzonefaces false; SNAPPING Important parameters are number of mesh displacement iterations, nsolveiter and the number of feature edge snapping iterations, nfeaturesnapiter. snapcontrols nsmoothpatch 4; tolerance 1.2; nsolveiter 185; nrelaxiter 6; nfeaturesnapiter 5; 7

9 implicitfeaturesnap false; explicitfeaturesnap true; multiregionfeaturesnap false; LAYERING addlayerscontrols relativesizes false; layers The label for the layering is equal to the labeling of the Boundary surface in the boundary file in the constant/polymesh folder flange_single_region_flange_inside define the number of surface layers nsurfacelayers 3; flange_single_region_flange_outside nsurfacelayers 3; define the expansion ratio of the surface layers expansionratio 1.005; define the min and the final thickness of the surface layers finallayerthickness ; minthickness ; ngrow 0; featureangle 85; slipfeatureangle 25; nrelaxiter 5; nsmoothsurfacenormals 4; nsmoothnormals 3; nsmooththickness 10; maxfacethicknessratio 0.5; maxthicknesstomedialratio 0.2; minmedianaxisangle 90; nbuffercellsnoextrude 0; nlayeriter : If not snapped smoothly enough, the max number of layer addition iteration can be increased nlayeriter 50; meshqualitycontrols #include "meshqualitydict" nsmoothscale 4; errorreduction 0.75; writeflags ( scalarlevels layersets layerfields ); mergetolerance 1e-6; // ******************************************************************* // - surfacefeatureextractdict: // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // flange_single_region.stl 8

10 extractionmethod extractfromsurface; extractfromsurfacecoeffs All edges are refined, whose surface normals include angles with less than the angle specified. For the included angels, a special level of refinement can be set in the Dict in the features subdictionary. includedangle 150; writeobj yes; // ******************************************************************** // Setting Refinement level in Dict and surfacefeatureextractdict In the first step, the castellatedmeshcontrols, the initial mesh can be refined with levels. The level depends on the refinement set in the blockmesh, and the required refinement on the surfaces. Therefore, levels can be set in the subdirectories features, refinementsurfaces and refinementregions. Level 0 stands for no refinement and each level splits the cell into 4 separate cells. Figure 2 Refinement level 0, level 1, level 2, level 3 Only the relevant changes, which were used in the sample flange case, are commented in the Dict. For more information see the literature in [1], [2], [3], [4]. The background mesh is created with the command blockmesh. >blockmesh To ensure that also the sharp edges are refined properly, it is very important to create perfect cubes in the first place. In this case, the mesh was created with 30 cells in x- and y direction and with 20 cells in z direction. Thus, according to the settings in the blockmeshdict each cube has a length of 2mm in each direction. 9

11 Figure 3 Block mesh for flange One.stl file is needed with the information about the surfaces inside and outside of the flange to set the appropriate boundary conditions. So both surfaces are are combined to a single file. As mentioned above, this is necessary to have appropriate entries in the boundary file. >cat cad/flange_inside.stl cad/flange_outside.stl > constant/trisurface/flange_single_region.stl In this case, the combined.stl can look similar to the following extract. solid flange_inside facet normal outer loop vertex vertex vertex endloop endfacet... facet normal outer loop vertex vertex vertex endloop endfacet endsolid flange_inside solid flange_outside facet normal outer loop vertex vertex vertex endloop endfacet. 10

12 .. facet normal outer loop vertex vertex vertex endloop endfacet endsolid flange_outside The command surfacefeatureextract creates the.emesh files from the.stl files and creates the folder extendedfeatureedgemesh in the /constant directory. Refining certain parts of the surface geometry with the surfacefeatureextract tool is optional. >surfacefeatureextract 11

13 a) Run on one processor The meshing process with can be run in on one processor or on several processors in parallel. The command to mesh the flange geometry on one processor is > The command creates a folder with the mesh files for each mesh step. If, for example, in the Dict, only castellatedmesh is set to true and snap and addlayers are set to false, only one folder is created. If also snap is set to true, 2 folders are created and if also addlayers is set to true, 3 folders with 3 polymesh folders are created. In order to avoid the creation of these folders and only keep the final mesh, the following command can be used to overwrite the previous meshing steps. In this case, only one polymesh folder exits in the /constant directory. > -overwrite 12

14 b) Run on several processors in parallel For running the simulation in parallel, a decomposepardict file is necessary in the system folder. In this file, the decomposition method can be specified. This can be hierarchical, simple, scotch or manual. Note: It is recommended, not to use the scotch method to decompose the region. Rather, the hierarchical or the simple method should be used. In case of scotch method, errors can occur while executing or while reconstructing the mesh, so that more domains are reconstructed than have been decomposed before. // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // numberofsubdomains 2; method //method //method //method hierarchical; simple; scotch; manual; hierarchicalcoeffs n (1 2 1); delta 0.001; order xyz; simplecoeffs n (1 2 1); delta 0.001; manualcoeffs datafile "celldecomposition"; // ************************************************************************* // >decomposepar After executing decomposepar, the processor* folders are created. The number of created folders are according to the number of subdomains specified in the decomposepardict. >mpirun -np 2 -parallel 13

15 To examine, what each of the steps in the Dict really does, the following commands can be used. To reconstruct and examine the castelleting step >reconstructparmesh -time 1 Figure 4 flange mesh for step castellate with surface refinement level 2 Figure 5 flange mesh for step castellate with surface refinement level 3 14

16 To reconstruct and examine the snap step >reconstructparmesh -time 2 Figure 6 flange mesh for step snap with surface refinement level 3 To reconstruct and examine the layering step >reconstructparmesh -time 3 In case, only the latest timestep available needed, also the following command can be used >reconstructparmesh -latesttime Figure 7 flange mesh for step addlayers with surface refinement level 3 15

17 The figures 4 to 7, are slice views taken with paraview from the center of the flange. The slices are depicted by the red plain in figure XX on the right Figure 8 flange with sectional plain The following command only creates a single folder 0 in the processor* folders whereas the preceding mesh folders 1 or 2 are overwritten. 16

18 >mpirun -np 2 -parallel -overwrite By overwriting the previous time steps, the mesh can be reconstructed with >reconstructparmesh constant Review the mesh quality with the tool checkmesh >checkmesh In case the checkmesh tool finds erros, the corrupted cells or faces are written to the folder sets in the folder polymesh. These cells or faces can be examined with paraview by converting the files to the VTK format. Depending on the sort of corrupted cells depicted in the terminal output from checkmesh, the following commands can be used among others >foamtovtk region insidezone faceset nonorthofaces >foamtovtk region outsidezone faceset skewfaces >foamtovtk region insidezone cellset zerovolumecells 17

19 Running OpenFoam simulation with scalartransportfoam The mesh files, created with are copied to the scalartransportfoam tutorial sample case pitzdaily which is provided by OpenFoam. Some adjustments are necessary to run the case and check if the mesh quality is satisfactory. - Delete the entry defaultfaces in the boundary file in the polymesh folder - In the controldict file change the endtime to 0.05 and the writeinterval to Update the file temperature where the flange has an initial temperature of 293K and is heated up from the inside with 350K. The outside of the flange is adiabatic // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [ ]; internalfield uniform 293; boundaryfield flange_single_region_flange_inside type fixedvalue; value uniform 350; flange_single_region_flange_outside type zerogradient; // ******************************************************************** // - Update the file velocity where the whole velocity in the flange and at the boundaries is zero. // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [ ]; internalfield uniform (0 0 0 ); boundaryfield flange_single_region_flange_inside type fixedvalue; value uniform (0 0 0); flange_single_region_flange_outside type fixedvalue; value uniform (0 0 0); 18

20 // ******************************************************************** // Run the solver with the command >scalartransportfoam Convert the results with >foamtovtk 0.01s 0.02s 0.03s 0.04s 0.05s Figure 7 Heating of the flange from 0.01 to 0.05s 19

21 Literature [1] [2] [3] [4] 20