Presentation slides for the course CFD with OpenSource Software 2015

Transcription

1 Presentation slides for the course CFD with OpenSource Software 2015 Sebastian Kohlstädt Applied Mechanics/Fluid Dynamics, Chalmers University of Technology, Gothenburg, Sweden Sebastian Kohlstädt Modeling hpdc / 28

2 Principal setup of a high-pressure die caster What is high-pressure die casting? locking unit casting unit moving clamping plate unit ejector unit tie bar fixed plate plunger hydraulic aggregate Figure : The layout and components of a high-pressure die casting machine according to DIN Sebastian Kohlstädt Modeling hpdc / 28

3 Three process phases of high-pressure die casting The three phases in high-pressure die casting (1) Figure : Phase one: pre-filling. Sebastian Kohlstädt Modeling hpdc / 28

4 Three process phases of high-pressure die casting The three phases in high-pressure die casting (2) Figure : Phase two: die-filling. Sebastian Kohlstädt Modeling hpdc / 28

5 Three process phases of high-pressure die casting The three phases in high-pressure die casting (3) Figure : Phase three: after-pressure. Sebastian Kohlstädt Modeling hpdc / 28

6 Focus of tutorial: CFD in shot sleeve The fluid mechanics processes in the shot sleeve Figure : Impact of increasing plunger propagation. The velocity increases from the left to the right picture. Sebastian Kohlstädt Modeling hpdc / 28

7 Overview Ways to create mesh with open source software blockmesh: included in openfoam R. Usable for very simple geometries. Somewhat spread in academia. Of limited usability for industrial cases. Salome: Salome comes along with meshing tools. They are quite intuitively usable, however can not entirely compete with commercial alternatives. snappyhexmesh: included in openfoam R. Requires however some work with the.stl file mostly in additional pre-processing software in order to be appropriately usable. Sebastian Kohlstädt Modeling hpdc / 28

8 Overview Ways to create mesh with open source software author s recommendation The author of this tutorial found out that for industrial applications with complex shapes the combination of pre-processing the (stl-) geometry in Salome and then applying snappyhexmesh is for the majority of cases the best option. Unless the user has access to proprietary software such as ANSA. Sebastian Kohlstädt Modeling hpdc / 28

9 Salome tutorial A brief tutorial in Salome Open Salome, please! We will now create a geometry together! Sebastian Kohlstädt Modeling hpdc / 28

10 Generating the mesh for the tutorial Envisioned geometry/mesh for the tutorial The aim is to create a mesh like the one shown underneath for the tutorial. How would you proceed? Sebastian Kohlstädt Modeling hpdc / 28

11 Generating the mesh for the tutorial Envisioned geometry/mesh for the tutorial The author did it by using his self-developed template of the blockmeshdict for boxes. Some excerpts of it will be shown in the following slides and beneath the text. minxcor -30; minycor -30; minzcor -300; //This is the first paragraph my maxxcor 30; //blockmeshdict starts with maxycor 30; // I do convert the values to meters by 1e-3 maxzcor -20; Sebastian Kohlstädt Modeling hpdc / 28

12 Generating the mesh for the tutorial How to create the geometry/mesh for the tutorial (1) The vertices only use the priorly defined coordinates. vertices ( ($minxcor $minycor $minzcor) ($maxxcor $minycor $minzcor) ($maxxcor $maxycor $minzcor) ($minxcor $maxycor $minzcor) ($minxcor $minycor $maxzcor) ($maxxcor $minycor $maxzcor) ($maxxcor $maxycor $maxzcor) ($minxcor $maxycor $maxzcor) ); Sebastian Kohlstädt Modeling hpdc / 28

13 Generating the mesh for the tutorial How to create the geometry/mesh for the tutorial The faces of the so created blocks can be easily assigned to the patches because they were previously assigned to XY, XZ, YZ planes. boundary ( slipwalls { type wall; faces ( ( ) //maxxzblock0 ( ) //minxzblock0 ); } Sebastian Kohlstädt Modeling hpdc / 28

14 Generating the mesh for the tutorial Envisioned geometry/mesh for the tutorial The faces of the so created blocks can be easily assigned to the patches because they were previously assigned to XY, XZ, YZ planes. fixedwalls { type wall; faces ( ( ) //minxzblock1 ( ) //maxxyblock1 ( ) //minxyblock2 ( ) //maxxyblock2 ); The same is done for movingwalls, outlet and frontandback (empty patches in 2D case). Sebastian Kohlstädt Modeling hpdc / 28

15 Generating the mesh for the tutorial Envisioned geometry/mesh for the tutorial In the end the patches that form internal borders are stitched together. This is necessary because of point doubling. mergepatchpairs // Remember: This only works if in both cases the master box // (the box to which the master patch belongs) stays the same. ( (internalborderblock10 internalborderblock01) (internalborderblock12 internalborderblock21) ); Sebastian Kohlstädt Modeling hpdc / 28

16 How to make the mesh moving Which solvers handle moving meshes? Moving meshes in openfoam R Solvers handling moving meshes are distinguished from solvers that do not by the expression DyM in their name, i.e. compressibleinterdymfoam they additionally require the dictionary dynamicmeshdict this dictionary is located in $CASE_DIR/constant/dynamicMeshDict the specialty of this DyM-solver family is that they inside call another solver that solves for mesh motion an additional library has to be included in dynamicmeshdict the mesh solution can be looked at independently from the flow solution by simply typing movedynamicmesh into a terminal in the case folder an example of the dynamicmesh I used will be given on the following pages Sebastian Kohlstädt Modeling hpdc / 28

17 How to make the mesh moving The layout of the dynamicmeshdict The example of the dynamicmeshdict I used. Particularly difficult to figure out was the line that includes the motionsolverlibs as openfoam R does not tell you it needs it and which options are available. /*openfoam header */... dynamicfvmesh dynamicmotionsolverfvmesh; motionsolverlibs ( "libfvmotionsolvers.so" ); solver velocitycomponentlaplacian z; velocitycomponentlaplaciancoeffs { component z; diffusivity directional ( ); } Sebastian Kohlstädt Modeling hpdc / 28

18 How to make the mesh moving Available dynamicfvmesh types Available dynamicmesh types in openfoam R You can see them by applying the banana trick. 6 ( dynamicinkjetfvmesh dynamicmotionsolverfvmesh dynamicrefinefvmesh multisolidbodymotionfvmesh solidbodymotionfvmesh staticfvmesh ) Sebastian Kohlstädt Modeling hpdc / 28

19 How to make the mesh moving Selection the motion solver What to do if the motion solver table is missing? --> FOAM FATAL ERROR: solver table is empty From function motionsolver::new(const polymesh& mesh) in file motionsolver/motionsolver/motionsolver.c at line 1 FOAM exiting You are probably missing the line motionsolverlibs ( "libfvmotionsolvers.so" ); inside your dynamicmeshdict. Sebastian Kohlstädt Modeling hpdc / 28

20 How to make the mesh moving Available solvers from the libfvmotionsolvers.so library Which solvers can you select? Valid solver types are: 7 ( displacementcomponentlaplacian displacementinterpolation displacementlaplacian displacementlayeredmotion displacementsbrstress velocitycomponentlaplacian velocitylaplacian ) Sebastian Kohlstädt Modeling hpdc / 28

21 Mesh motion Running the mesh motion For only calculating the mesh motion one has to type blockmesh > log.blockmesh movedynamicmesh > log.movedynamicmesh & parafoam to a terminal window in which the case directory is selected. Sebastian Kohlstädt Modeling hpdc / 28

22 CFD solution Computing the flow The commands for running the case are fairly similar to all other openfoam R cases. One opens a terminal sources the bashrc and navigates to the case directory. Typing blockmesh > log.blockmesh cp 0/alpha.melt.org 0/alpha.melt setfields > log.setfields compressibleinterdymfoam > log.compressibleinterdymfoam & parafoam will run the case. The results can then be viewed parafoam. Sebastian Kohlstädt Modeling hpdc / 28

23 Mesh motion Results from movedynamicmesh (1) Something like this should appear in ParaView after you executed the command movedynamicmesh in the tutorial s case folder. At t = 0 Sebastian Kohlstädt Modeling hpdc / 28

24 Mesh motion Results from movedynamicmesh (2) Something like this should appear in ParaView after you executed the command movedynamicmesh in the tutorial s case folder. At t = Sebastian Kohlstädt Modeling hpdc / 28

25 Mesh motion Results from movedynamicmesh (3) Something like this should appear in ParaView after you executed the command movedynamicmesh in the tutorial s case folder. Sebastian Kohlstädt Modeling hpdc / 28

26 CFD solution Results from compressibleinterdymfoam (1) Something like this should appear in ParaView after you executed the commands as stated above in the tutorial s case folder. At t = 0 Sebastian Kohlstädt Modeling hpdc / 28

27 CFD solution Results from compressibleinterdymfoam (2) Something like this should appear in ParaView after you executed the commands as stated above in the tutorial s case folder. At t = Sebastian Kohlstädt Modeling hpdc / 28

28 CFD solution Results from compressibleinterdymfoam (3) Something like this should appear in ParaView after you executed the commands as stated above in the tutorial s case folder. Sebastian Kohlstädt Modeling hpdc / 28