TUTORIAL#4. Marek Jaszczur. Turbulent Thermal Boundary Layer on a Flat Plate W1-1 AGH 2018/2019

Transcription

1 TUTORIAL#4 Turbulent Thermal Boundary Layer on a Flat Plate Marek Jaszczur AGH 2018/2019 W1-1

2 Problem specification TUTORIAL#4 Turbulent Thermal Boundary Layer - on a flat plate Goal: Solution for Non-isothermal Fluid FLow 1. Creating 2D simple geometry - DesignModeler 2. Creating 2D mesh Mesh 3. Solver Set-up 4. Results 5. Plots 6. Solution verification W1-2

3 Problem specification Turbulent Thermal Flat plate boundary layer For the case presented below take into account a non-isothermal turbulent fluid flow on a flat plate. The Reynolds number based on the plate length L is Re=1,000,000 and the plate length is L=1 m. For simplicity inlet fluid velocity in x-direction is U f =1 m/s while temperature T f =300 K, the fluid properties are: density is 1000 kg/m 3, viscosity m=10-6 Pas, heat capacity c p =1000J/kgK, thermal conductivity k=1.0 W/mK. Wall teperature T w =350 K and fluid Pr=1.0 For presented case solution is only Reynolds number and Prandtl number dependent U f =1.0m/s T f =300 K y x Re= Pr=1.0 L=1m T w =350 K W1-3

4 Mathematical model non-isothermal case steady, turbulent constant properties incompressible fluid thicknees of boundary layer can be calculated as and for end of the plat x=l=1m =0.024m. This area have to be resolved with large care, and the height of domain should be at least 10 times larger here H=0.5m top inlet fluid H=0.5m outlet L=1m plate W1-4

5 Let s go.. Open ANSYS Workbench Find WB Software in Menu Start --- Programs --- ANSYS Workbench 15.0 W1-5

6 Workbench Steady problem can be solved using different modules from ANSYS WORKBENCH In this tutorial most advanced module for Fluid for Simulation is used Fluid flow (FLUENT) (avaliable in Anaysis Systems) In order to select FLUENT module drag and drop or double-click W1-6

7 Geometry CREATING GEOMETRY in DESIGN MODELLER W1-7

8 Geometry 2 1. For Geometry in Properties set-up Analysis Type 2D!!!! If You leave default option 3D Your geometry will be three-dimensional 2. After 2D set-up double-click Geometry in order to start DESIGN MODELER 1 W1-8

9 Geometry DesignModeler This is DesignModeler.at the beginning 1. Select XYPlane (just select and click)) as a working plane 2. Then select view at Face by clicking on icon 3. In tab Sketching are tools for plotting W1-9

10 DesignModeler At this step we will draw simple geometry we will just plot and set-up dimension for rectanguar In this version ANSYS 15 for the geometry DesignModeler, is used as a default module for geometry This tools allow as to create geometry from the begining as well as to import geometry from other software for example from CAD software. The first step is to check units!!! In menu units check if You are working with meters (information about units can be also find in at rights bottom corner [METER]). You can swith units in menu Units > PLANE Sketch (Plot) will be create at XYPlane toto do that select To Look at Face select icon W1-10

11 Sketching At this step please select tab Sketching then Draw tools and Rectangle In order to have plot from (0,0) coordinates or atached to the axies select and enable constrains: Last step is to draw rectangle from begining of XY-coordinates HELP- is something goes wrong --- use UNDO W1-11

12 Dimensioning Now You should have rectangle but the size is probably wrong Under Sketching Toolboxes, select Dimensions tab, use the default dimensioning tools. Dimension the geometry as shown in image. (use what is default GENERAL dimension) 1. Then select top side of rectangle and move cursor a bit top next do the same with left (or right) side 2. You should get new LABELS for example V1 i H1 for vertical and horizontal dimension W1-12

13 Dimensioning After dimensioning in Details View (left bottom corner) it is possible to setup exact size for V1 and i H2. Under the Details View table (located in the lower left corner), set V1=0.5 m, H2=1 m. Don t worry if your labels for Dimensions are not V1 and H2. When You create and delete new dimensions new numbers are used. The same for new Sketches W1-13

14 Surface Body Creation Our Sketch READY but sketch can t be used for computations!!!. In order to performed simulations in ANSYS You need BODY", and not a SKETCH!!!!. To create BODY we can use Sketch. In case of 2D body it will be just surface To create BODY select tab Modelling (not Sketching) then select from menu Concept > Surface From Sketches, as bellow: W1-14

15 Surface Body Creation Then select XY Plane and Sketch 1. (or other number) After Sketch 1 selection press Apply to accept selected Sketch in Details View Details of SurfaceSk1 The last step is to find and click icon GENERATE is ready to use in the next step. Now Your BODY W1-15

16 Surface Body Creation If no ERROR we can enjoj with our PLATE-BODY (it should be with colour) NEW object 1 Body!!! Surface Body The thickness of our plate 2D is = 0m W1-16

17 2D PLATE is Ready Body of 2D Plate is ready. However if You find any problem please download 2D_PLATE geometry from my web (2D_TBL_geom file) W1-17

18 Geometry CREATING MESH in DESIGN MODELLER W1-18

19 Surface Body Creation Our 2D BL PLATE (Surface Body) is ready Now you can close DesignModeler: menu File > close DesignModeler At this step You can save whole Project in Workbench menu File under easy name (for exaple plate_2d): menu File > save the project Next step is to create MESH no.3 (Mesh) To RUN mesh module double- click 3. Mesh W1-19

20 Mesh At this step numerical mesh will be created. Mesh is required in order to performed computer simulations because of methodology used Continuous space will be replace by the discrete space Here the division is Nx=100(length -X direction) and Ny=30(height Y direction) As a results 3000 control volumes CV created (101x31 nodes) Ny=30 Nx=100 W1-20

21 Mesh In Mesh Tree select Mesh than Window Details of Mesh appear Check the Physics Preference it should be automatically set to CFD Solver preferences for Fluid Flow calculations have to be FLUENT Thus, in this case (complete block from Analysis System) it is not necessary to specify a preference in Meshing Options. W1-21

22 Mesh For easier work from anywhere in the MESH Graphics window, use RMB then View and select Front view This will make object orientation geometry Front to user so it will be easier to work with particulary after rotation or any other operation. W1-22

23 Mesh Edge Sizing From the Selection Toolbar, which is located near the top of the Meshing window, select Edge Filter to change the default selection filter from Face to Edge. Place the cursor over the left edge of plate and when the edge changes colour to a dotted red line, user LMB to select edge. The edge after selection should become green to indicate that it is selected. After selection use RMB > Insert > Sizing W1-23

24 Mesh Edge Sizing After choice sizing the selected edge is taken into account For this edge in window Details of Edge Sizing several settings can be applied (for example) for Left / Right Edge - select type- number of division - then type - number of divisions=30 - behaviour Hard - Bias Type (remember to revers bias for right edge) - Bias Factor 1000 Repeat this procedure for Right edge it is essential to use of finer elements near the edge of plate resolve the boundary layer along the plate. to have uniform grid in X direction Top/Bottom use the folowing settings (it is possible to select with Ctrl+ two edges) W1-24

25 Mesh Edge Sizing Select Face Filter Tap rectangle surface RMB > Insert > Mapped Face Meshing In Details of Mapped Face Meshing, Apply to make this surface the Geometry selection. This procedure create uniform structural mesh Click on Generate Mesh to create mesh W1-25

26 Mesh Now mesh is ready In Mesh details window you can see mesh size (nodes, elements) 3000 Elements W1-26

27 Mesh Before we will proceed next step and go to the solver it is very usefull to give names for all edges. This allso to easy recognise them in Fluent solver Select edge filter select edge you want put name then: RMB > Create Name Selection Then type desired name Repeat procedure for all egdes -inlet, outlet, top, plate It is also possible to give name for whole body (with Face Filter selection) fluid W1-27

28 2D plate MESH is Ready MESH for 2D Plate is ready to use. if You find any problem please download 2D_PLATE mesh file from my web (2D_TBL_mesh_30x100 file) W1-28

29 Geometry SOLVING in ANSYS FLUENT W1-29

30 Setup Before proceed to the next step Setup mesh update is required. To do that RMB and update symbol should change from into Then You can go to the next step SETUP W1-30

31 Setup When You click on Setup FLUENT solver will run Welcome window will appear with few settings - Dimension (here because of geometry is 2D) - Double precision (please enable!!!) - Serial/Parallel computation (leave default) (each CPU may require license!!) - Then procceed OK. W1-31

32 FLUENT v15 This is default solver Fluent v15 window (with plate) Object Selection tree Graphical window Text window - You can also type here W1-32

33 FLUENT v15 Check Mesh It is good idea to check the mesh in order to verify that it has been properly read/import. -go to General in right window press button CHECK or from menu Mesh>Check if no error mesh is OK -It is also possible to get more -information about mesh from menu mesh: Mesh > Info > Size Mesh > Info > Quality Mesh > Info > Memory use W1-33

34 Fluent - General First step is to select General Check Settings: -Steady -Planar Then go to the next step Models W1-34

35 Fluent - Models At this step set-up Model for Energy double-click or Edit Energy from avaliable models Enable this model ON The same can be done from Menu > Define > Models W1-35

36 Fluent - Models At this step set-up Viscous model double-click or Edit Viscous from avaliable models for fluid flow select k-epsilon(2-eq)model (we assume flow is turbulent) check if k-epsilon Stardard version is used as well as Standard Wall Function Then click OK The same can be done from Menu > Define > Models W1-36

37 Fluent Models - Theory We will first use the k-epsilon Standard Model version. In the Near-Wall Treatment selection observe the Standard Wall Function option, which deals with the resolution of the boundar layer in our symulation. Turbulent boundary contain three different regions that are important. Starting at the wall we can define: - Laminar sublayer up to the distance y+ < 5 - Buffer region at the distance 5 < y+ < 30 -Turbulent region for the distance y+ > 30 where y+ is a mesh-dependent dimensionless distance that quantifies to what degree the wall layer is resolved. After calculating flow, this value will be calculated for different meshes used in this example. The Wall Function Model option serves to solve the boundary layer in the case when the mesh is only fine enough to resolve to the turbulent region (y+ > 30). For current mesh, FLUENT will be able to resolve the laminar sublayer, thus Wall Model does not improve the accuracy of our solution with this mesh. It make a difference when coars mesh will be used. It has to be noticed that the thickness of the boundary layer is significantly smaller than the height of our domain. Resolving the laminar sub-layer is computationally burden, especially when flow has high Reynolds Number. For this reason resolving only the turbulent region is often the only choice. Thus it is good practice to use more advanced than Standard Wall Function Models. The numbers in the Model Constants window are typically used in the k-epsilon turbulence equations. Such values for the Model are well-accepted for a wide range of wall-bounded shear flows in the literature. Leave all constant as a default values. W1-37

38 Fluent - Materials Select Materials then select in Material window air and Create/Edit For air material type new properties as in problem specyfication density is 1000 kg/m 3, viscosity m=10-6 Pas, heat capacity c p =1000J/kgK, thermal conductivity k=1.0 W/mK. it is possible to type new name airx to keep original air When you press Change/Create new window appear select No to Not overwrite original air, then Close W1-38

39 Fluent - Materials At present in the list of avaliable materials for Fluid materials airx appears as possible choice with new material we can go to the Cell Zone Condition settings (see next page) W1-39

40 Fluent Cell Zone conditions We have create in database airx material but up to now this material it is not taken into consideration To set-up material airx: -go to Cell Zone Condition -select fluid (or any other name object if you don t give name fluid) -check if Zone-fluid Type is set to Fluid Type -Press Edit and in next window select Material Name airx W1-40

41 Fluent Cell Zone conditions For all flows, FLUENT solver need gauge pressure internally. All the time an absolute pressure is required. Pressure is generated by adding the operating pressure to the gauge pressure. To set-up Operating Pressure go to Operating Conditions In new window set-up (if necessary) the default value of 1 atm pressure (101,325 Pa) as the Operating Pressure. then OK W1-41

42 Fluent Boundary conditions At this step boundary condition have to be set-up for all boundaries select inlet boundaries You can see that Type is velocity-inlet (as default for the B.C. name inlet_xxx) Edit and set-up in Momentum Tab in Thermal Tab Velocity Magnitude=1.0 m/s Turbulent Intensity=1% Turbulent Viscosity Ration=1 Fluid Temperature=300K then OK W1-42

43 Fluent Boundary conditions select outlet boundaries You can see that Type is pressure-outlet as default for the name outlet_xxx Edit and check if Gauge pressure is 0 Pa then press OK. Also set-up Backflow conditions W1-43

44 Fluent Boundary conditions select plate boundaries You can see that Type is wall as default for the names diferent from mentioned Edit and check if in Momentum Tab Wall motion is Stationary Wall and Shear Condition is No Slip in Thermal Tab Plate Temperature is 350K then press OK. W1-44

45 Fluent Boundary conditions select top boundaries You can see that Type is wall as default for the names diferent from mentioned however this Type is not correct, top edge should be considered as a free flow or surface one of the option is to use Type symmetry Confirm selection Yes then press OK. W1-45

46 Fluent Solution Methods Under Solution Methods set-up all methods to be at least second order Spatial Discretization Confirm selection Yes then press OK. W1-46

47 Fluent Monitors Under Monitors select Residuals then double-click and set-up all Residuals to be 10-6 Confirm selection - press OK. W1-47

48 Fluent Solution Initialization Before we proceed Run Calculation it is necessary to go to Solution Initialization in order to initialise the solution starting value More close value less iteration is required Here use Standard Initialization and Compute from from inlet After that x-velocity at initial step will be everywhere 1m/s then press Initialize Button W1-48

49 Fluent RUN calculation The last step is to Run Calculation Set-up (maximum) number of iteration and Calculate (in case of initialisation question click OK) if no error calculation should iterate and Residuals plot should appears Your solution is READY (about 300 iterations) W1-49

50 Fluent Results To plot Velocity vectors go to Graphics & Animations. double click on Vectors under Graphics. Click on Display to see vectors (Zoom-in vectors) W1-50

51 Fluent Results Use zoom icon to zoom-in or zoom-out vectors W1-51

52 Fluent Velocity Profile To plot velocity profile at the channel outlet go to the: Results > Plots > XY Plot then set-up as follows: Then press Plot buton to see velocity profile W1-52

53 Fluent Skin friction calculation -FLUENT can calculate different coefficents. -However, to do this Software need to set-up Reference Values -go to the Reference Values -then set-up all References Values as in Right Figure W1-53

54 Fluent Y+ Profile To plot Y+ non-dimensional distance profile go to the: Results > Plots > XY Plot then set-up as follows: Then press Plot buton to see Y+ profile As can be seen wall y+ dystance is in the range y+ <5-3> point are in viscous sub-layer W1-54

55 Fluent Y+ Save calculated Y+ profile to the file y_30x100_ke_s.xy Plot and write to the file heat_30x100_ke_s.xy Skin Friction Coefficient profile Do the same (plot and write file name heat_30x100_ke_s.xy) for Total Heat Flux Profile W1-55

56 Fluent Drag To calculate the average drag on the plate. go to Reports then in Reports window select Forces and double click then set-up as follow: C d = (theoretical) In text window You should see Viscous Force and Drag Coeffcient W1-56

57 Fluent Drag To calculate the Drag coefficient on the plate the following formula is used: C d = F d 2 A 0.5 ρ ref V ref At home calculate theoretical drag coeffcient for Turbulent Boundary Layer (find it in Fluid Mechanic Book) and compare with obtained value W1-57

58 Appendix 1 k-e RNG Turbulent Model W1-58

59 Fluent - Models At this step set-up Viscous model double-click or Edit Viscous from avaliable models for fluid flow select k-epsilon(2-eq)model (we assume flow is turbulent) check if k-epsilon RNG version is used as well as Standard Wall Function Then click OK W1-59

60 Fluent Solution Initialization Before we proceed Run Calculation it is necessary to go to Solution Initialization in order to initialise the solution starting value More close value less iteration is required Here use Standard Initialization and Compute from from inlet After that x-velocity at initial step will be everywhere 1m/s then press Initialize Button W1-60

61 Fluent RUN calculation The last step is to Run Calculation Set-up (maximum) number of iteration and Calculate (in case of initialisation question click OK) if no error calculation should iterate and Residuals plot should appears Your solution is READY With this model calculations requires less iterations (270) W1-61

62 Fluent Results To plot Velocity vectors go to Graphics & Animations. double click on Vectors under Graphics. Click on Display to see vectors (Zoom-in vectors) W1-62

63 Fluent Results Use zoom icon to zoom-in or zoom-out vectors W1-63

64 Fluent Y+ Plot and write to the file heat_30x100_ke_rng.xy Skin Friction Coefficient profile Plot and write to the file heat_30x100_ke_rng.xy for Total Heat Flux profile W1-64

65 Fluent Drag To calculate the average drag on the plate. go to Reports then in Reports window select Forces and double click then set-up as follow: C d = (theoretical) In text window You should see Viscous Force and Drag Coeffcient W1-65

66 Appendix 2 k-e RNG Turbulent Model W1-66

67 Fluent - Models At this step set-up Viscous model double-click or Edit Viscous from avaliable models for fluid flow select k-epsilon(2-eq)model (we assume flow is turbulent) check if k-epsilon Realizable version is used as well as Standard Wall Function Then click OK W1-67

68 Fluent Solution Initialization Before we proceed Run Calculation it is necessary to go to Solution Initialization in order to initialise the solution starting value More close value less iteration is required Here use Standard Initialization and Compute from from inlet After that x-velocity at initial step will be everywhere 1m/s then press Initialize Button W1-68

69 Fluent RUN calculation The last step is to Run Calculation Set-up (maximum) number of iteration and Calculate (in case of initialisation question click OK) if no error calculation should iterate and Residuals plot should appears Your solution is READY With this model calculations requires more iterations (352) W1-69

70 Fluent Y+ Plot and write to the file skin_30x100_ke_r.xy Skin Friction Coefficient profile Plot and write to the file heat_30x100_ke_r.xy for Total Heat Flux profile W1-70

71 Fluent Drag To calculate the average drag on the plate. go to Reports then in Reports window select Forces and double click then set-up as follow: C d = (theoretical) In text window You should see Viscous Force and Drag Coeffcient W1-71

72 Fluent Skin Friction Coefficient comparision Now compare all three Skin Friction Coefficient profiles. -to to Plot >XYPlot> select settings a folows. Press Load File botton and load profiles from previous calculations: -skin_30x100_ke_s.xy -skin_30x100_ke_rng.xy We got 3 different results which is correct???? k-e Standard C d = k-e RNG C d = k-e R C d = At home compare all 3 local Skin Friction Coeffcient profiles with literature data. Additionaly compare averaged value W1-72

73 Appendix 3 k-e RNG Turbulent Model with Enhanced Wall Treatment W1-73

74 Fluent - Models At this step set-up Viscous model double-click or Edit Viscous from avaliable models for fluid flow select k-epsilon(2-eq)model (we assume flow is turbulent) check if k-epsilon Realizable version is used as well as Enhanced Wall Treatment Then click OK W1-74

75 Fluent Solution Initialization Before we proceed Run Calculation it is necessary to go to Solution Initialization in order to initialise the solution starting value More close value less iteration is required Here use Standard Initialization and Compute from from inlet After that x-velocity at initial step will be everywhere 1m/s then press Initialize Button W1-75

76 Fluent RUN calculation The last step is to Run Calculation Set-up (maximum) number of iteration and Calculate (in case of initialisation question click OK) if no error calculation should iterate and Residuals plot should appears Your solution is READY With this model calculations requires (300) iterations W1-76

77 Fluent Y+ Plot and write to the file heat_30x100_ke_rnga.xy Skin Friction Coefficient profile Plot and write to the file heat_30x100_ke_rnga.xy for Total Heat Flux profile W1-77

78 Fluent Drag To calculate the average drag on the plate. go to Reports then in Reports window select Forces and double click then set-up as follow: C d = (theoretical) In text window You should see Viscous Force and Drag Coeffcient W1-78

79 Fluent Drag To calculate the average drag on the plate. go to Reports then in Reports window select Forces and double click then set-up as follow: C d = (theoretical) In text window You should see Viscous Force and Drag Coeffcient W1-79

80 Fluent Homework At HOME compare: 1. The (a) Skin friction coefficient and (b) average drag on the plate calculated using Fluent solver with Literature data 2. The Total Surface Heat Flux calculated using Fluent solver with Literature data use - Fluid mechanic book - Reynolds, W.C., Kays, W.M., Kline, S.J. "Heat Transfer in the Turbulent Incompressible Boundary Layer." NASA Memo W. December W1-80