TUTORIAL#3. Marek Jaszczur. Boundary Layer on a Flat Plate W1-1 AGH 2018/2019

Transcription

1 TUTORIAL#3 Boundary Layer on a Flat Plate Marek Jaszczur AGH 2018/2019 W1-1

2 Problem specification TUTORIAL#3 Boundary Layer - on a flat plate Goal: Solution for boudary layer 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 Flat plate boundary layer For the case presented bellow take into account a fluid flow on a flat plate. The Reynolds number based on the plate length is Re=10,000 and the plate length is L=1 m. For simplicity inlet fluid velocity V o in x-direction is 1 m/s and the fluid density is 1.0 kg/m 3, viscosity m=10-4 Pas. For presented case solution is only Reynolds number dependent y x Re=10000 L=1m W1-3

4 Mathematical model isothermal case Steady, laminar/turbulent constant properties incompressible thicknees of boundary layer can be calculated as and for end of the plat x=l=1m =0.05m. This areal have to be resolved with large care, and the height of domain should be at least 10 times larger 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 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 W1-7

8 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 W1-8

9 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 W1-9

10 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 W1-10

11 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 W1-11

12 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 W1-12

13 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: W1-13

14 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 W1-14

15 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 = 0 but You can change that W1-15

16 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_BL_geom file) W1-16

17 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 W1-17

18 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=50(height Y direction) As a results 5000 control volumes CV created (101x51 nodes) Ny=50 Nx=100 W1-18

19 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. W1-19

20 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. W1-20

21 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 W1-21

22 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 - select number of division - then type number of div=50 - behaviour HARD - Bias Type (remember to revers bias for right edge) - Bias Factor. try 10, 30, 50, and.70 it is essential to use of finer elements near the edge of plate resolve the boundary layer along the plate. Repeat this procedure for all edges to have uniform grid in X direction and non uniform in Y direction (it is possible to select with Ctrl+ two edges) W1-22

23 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 W1-23

24 Mesh Now mesh is ready In Mesh details window you can see mesh size (nodes, elements) 5000 Elements W1-24

25 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 W1-25

26 2D plate MESH is Ready MESH for 2D Plate is ready to use. However if You find any problem please download 2D_PLATE mesh file from my web (2D_BL_mesh file) W1-26

27 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 W1-27

28 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. W1-28

29 FLUENT v15 This is default solver Fluent v15 window (with plate) Object Selection tree Graphical window Text window - You can also type here W1-29

30 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 W1-30

31 FLUENT v15 Display Mesh It is also possible to Display mesh -go to General in right window press button Display -new window will appear, select surfaces to display -and press Display button -to zoom in/out or move mesh use icons -to zoom In: Hold down the Middle Mouse Button &drag box from the Upper Left Hand Corner to the Lower Right Hand Corner over the to zoom in on. -to zoom Out: Hold down the Middle Mouse Button &drag a box anywhere from the Lower Right Hand Corner to the Upper Left Hand Corner. W1-31

32 Fluent - General First step is to select General Check Settings: -Steady -Planar Then go to the next step Models W1-32

33 Fluent - Models At this step set-up Viscous model double-click or Edit from avaliable models for fluid flow select Laminar flow (we assume laminar) The same can be done from Menu > Define > Models W1-33

34 Fluent - Materials Select Materials then select in Material window air and Create/Edit For air material type new properties as in problem specyfication (1.0 and ), it is also possible to type new name air1 to keep original air When you press Change/Create new window appear select No to Not overwrite original air, then Close W1-34

35 Fluent - Materials At present in the list of avaliable materials for Fluid materials air1 appears as possible choice with new material we can go to the last settings step: Boundary Conditions W1-35

36 Fluent Boundary conditions At this step boundary condition have to be set for all boundaries select inlet boundaries You can see that Type is velocity-inlet as default for the name inlet_xxx Edit and set-up Velocity Magnitude=1.0 m/s then OK W1-36

37 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. W1-37

38 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 Wall motion is Stationary Wall and Shear Condition is No Slip then press OK. W1-38

39 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. W1-39

40 Fluent Cell Zone conditions We have create in database air1 material but up to now it is not taken into consideration To set-up material air1: -go to Cell Zone Condition -select fluid (or any other name object if you don t give name fluid) -see that Type is automaticaly switchs to Fluid Type -Press Edit and in next window select Material Name air1 W1-40

41 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 time will be everywhere 1m/s then press Initialize Button W1-41

42 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 W1-42

43 Fluent Results To plot Velocity vectors go to Graphics & Animations. double click on Vectors under Graphics. Click on Display to see vectors W1-43

44 Fluent Results Use zoom icon to zoom-in or zoom-out vectors W1-44

45 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 W1-45

46 Fluent Velocity Profile To cut not interesting range of the far velocity region from the wall, the range of the y axis will be truncated, as on picture: in Solution XY Plot window select Axes Then set-up Axes window as follow: W1-46

47 Fluent Velocity Profile Now the plot should be like this In order to compare this with Blasius profile download file Blasius.xy from my web and load it to compare both data At home compare profile with Your calculated Blasius profile W1-47

48 Fluent Skin friction calculation skin friction calculation: c f = τ w ρ ref V ref -FLUENT can calculate different coefficents. -However, to do thisfluent need to set-up Reference Values -go to the Reference Values -then set-up Density and Velocity equal 1 W1-48

49 Fluent Skin friction calculation go to Plots then in Plots window select > XY Plot and put settings as presented skin friction calculation plot: W1-49

50 Fluent Skin friction calculation As previously compare calculated skin friction with Blasius skin friction. Download file skin.xy and load to the XY-Plot Press Plot botton and see new plots base on analitycal solution At home compare profile with Your calculated skin profile W1-50

51 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: In text window You should see Viscous Force and Drag Coeffcient W1-51

52 Fluent Drag To calculate the drag coeficient 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 laminar BL (find it in Fluid Mechanic Book) and compare with obtained value W1-52

53 Appendix 1 Solution refinement W1-53

54 Fluent Drag To calculate the drag coeficient on the plate BUT more accurate than NOW there are at least 4 choices: for our case C d = (A) performed more iterations (B) use higher order discretisation (C) create manually new mesh (D) automatically mesh refinement Save velocity calculated velocity profile (file vel1.xy) and skin friction profile (file skin1.xy) as well as write down average drag coefficient to see the effect of our selection then go to the next page W1-54

55 Fluent Appendix 1 (A) performed more iterations To performed more iteration it is necessary to decrease residuum convergence criteria from 10-5 to 10-6 go to Monitors in window Monitors double click Resuduals and change convergenge settings from 10-5 into 10-6 Then press OK. and Run calculations 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: In text window You should see Viscous Force and Drag Coeffcient W1-56

57 Fluent Appendix 1 (B) use higher order discretisation To change derivatives aproximation order go to Solution Methods All available discretisations are there Change Momentum discretisation from second order Upwind into Third order MUSCL also and enable High Order Term relaxation Then press OK. and Run calculations W1-57

58 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: In text window You should see Viscous Force and Drag Coeffcient W1-58

59 Fluent Appendix 1 (C) automatically mesh refinement To refine mesh automatically several critera can be used. In this tutorial mesh will be defined base on the velocity gradient. In places with high Y velocity gradient more grid points will be added To do that go to menu Adapt >Gradient set up windows as follow When You press botton Compute min and max gradient range will be display Base on that information set-up Refine Treshold for example W1-59

60 Fluent Appendix 1 (C) automatically mesh refinement When You press botton Mark grid point for refinement and coarsening will be selected Number of marked points You can see in Text window After pressing Adapt botton mesh will be adopted. Check new size dimension (in menu mesh > info> size) and see new mesh (in Graphich and Animation, Graphics, Mesh) Then press OK. and Run calculations W1-60

61 Fluent Appendix 1 (C) automatically mesh refinement The Fluent window display how many cells is selected for refining and coarsening. However the coarsening cells can be ignored since solver is unable to coarsen the original grid To see where the grid is adapted, click Manage> Display. Locations for mesh refinement will be highlighted. W1-61

62 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: In text window You should see Viscous Force and Drag Coeffcient W1-62

63 Fluent Appendix 1 (D) create manually new mesh To refine mesh manually go close Fluent go back to Workbench and enter Mesh module to create new mesh. Create mesh with size 100x100 Then update new mesh and repeat all calculations Compare drag coeffcient W1-63