# Numerical Modeling of Fluid Flows (BMEGEÁTAM5) 2014. 02. 19.

## Presentation on theme: "Numerical Modeling of Fluid Flows (BMEGEÁTAM5) 2014. 02. 19."— Presentation transcript:

Numerical Modeling of Fluid Flows (BMEGEÁTAM5) 2014. 02. 19.

Farkas, Balázs farkas [at] ara.bme.hu www.ara.bme.hu/~farkas/CFD/workbench http://www.ara.bme.hu/oktatas/tantargy/NEPTUN/BMEGEATAG26/M AGYAR_kepzes/2013-2014-II/ea http://www.ara.bme.hu/oktatas/tantargy/NEPTUN/BMEGEATAG26/M AGYAR_kepzes/2013-2014-II/ea

Most Important Rule NO SPECIAL CHARACTERS AND SPACE ALLOWED DURING USE OF ANSYS WORKBENCH USE: - UPPER- and lowercase - Latin characters - Numbers - Character _ NEVER: ÖÜÓŐÚÉÁŰÍ Öüóőúéáűí space GOOD: Path: C:/Work/Andras_Job_01 Named Selection: „Velocity_inlet1” BAD: C:/Asztal/András Jób 01 Named Selection: „Velocity inlet 1”

Aim of Exercise 2 – Pump (2D, periodic boundary conditions)

1. Chapter: The geometry

Start Screen of ANSYS Workbench Drag and drop the element Fluid Flow(Fluent) Into the Project Schematic area

Starting Design Modeler 1) Click on Advanced Geometry Options Change Analysis type to 2D 2) Double-click on Geometry to start Design Modeler

Setting units Select Millimeter unit in Units menu

Workplane selection Select XYPlane, right click, then select Look At to align plane to forntal view

Reading construction points To generate basic construction points onto the plane, Use File/Run Script Find and select the downloaded script file

Constraints 2) At Constraints group, find Auto Constarints and check the Cursor box 1) After the appearance of points, change to Sketching panel

Drawing circular arcs Use Draw/Arc by 3 points command to draw the pressure (upper) side of blade (first select endpoints, then middle point)

Drawing circular arcs Do the same with leading edge and suction (lower) side

Drawing circular arcs Trailing edge is an Origin- centered arc (use Arc by center)

Constraints Fix endpoints of leading edge and leading edge arc using Constraints/Fixed command

Drawing a Spline Connect with a spline the endpoints of computational domain (you may have to roll down in menu) – After endpoint, right click and select Open End in the context menu

Copy/Paste the periodic boundary 1)Modify/Copy 2)Select spline 3)Right click:End/Use plane origin as handle – (you close the selection and set the Origin as the basepoint of Paste command 1 2 3

Copy/Paste the periodic boundary Automatic change to Paste command 1)Cahnge r value to 60° 2)Right click: Rotate by –r 1 2

Copy/Paste the periodic boundary Click on Origin with the cursor: Copy/Paste finished

Drawing in let and aoutlet boundaries Inlet/Outlet boundaries are Origin centered arcs (Arc by center)

Publication of input parameters 1)Select Dimensions/Radius command 2)Set (type) trailing edge radius to 125 mm 3)By checking the box, Publish parameter and name it as R_out 1 2 2 3

Creating Surface 1)Go to Modelling panel 2) Select Sketch1 3) Select Concept/Surface from sketches 1 2 3

Contd. Apply

Contd. 2) Click on Generate to apply command and make surface 3) Close Design Modeler 1) Select Add frozen

2. Chapter: The Mesh

Mesher start Double click on Mesh Mesher is started Save Project (NO spaces and \$pecial chäracters WHATSOEVER)

Initial mesh In Project Tree, Click on Mesh then on Update to see current mesh

Setting boundaries as Named Selections 1)Select Line Selection Tool 2)Select inlet boundary 3)Right click on line, select Create Named Selection command form the context menu 1 2 3

Setting boundaries as Named Selections Name it as velocity_inlet

Setting boundaries as Named Selections Similarly create: 1)Pressure_outlet 2)Per1 3)Per2 4)Leading_edge 5)Trailing_edge 6)Pressure_side 7)Suction_side 1 3 2 6 7 5 4

Setting mesh sizing Open (explore) Sizing menu -Set Min size: 1 mm -Set Max Face Size: 2 mm -Set Max Size larger than both if conflict appears Publish Max Face Size by checking box

Refining boundary layer mesh Update mesh Right click on Mesh  Insert  Inflation

Refining boundary layer mesh 1)Select Surface Selection Tool 2)Geometry: whole surface 3)Apply 1 2 2,3

Refining boundary layer mesh 1)Select Line Selection Tool 2)Boundary: 4 edges of blade (hold ctrl to select multiple lines) 3)Apply 1 2 2,3

Refining boundary layer mesh Transition ratio: 0.6 Maximum layers: 4 Growth rate: 1.5

Refining boundary layer mesh Update

Refining boundary layer mesh – transition ratio Use transition ratio to set relative thickness of boundary layer mesh. Range: 0-1 transition ratio: 0.6transition ratio: 0.2

Refining boundary layer mesh – # of layers Use # of layers to… set… number of layers?! (number of cell layers generated by the Inflation, belonging to the Boundary layer mesh) Numb. of layers: 4Numb. of layers: 10

Refining boundary layer mesh – growth rate Use Growth rate to set the thicknes ratio of two consecutive cell layers Growth rate: 1.5Growth rate: 1.1

Close Mesher

3. Chapter: Physical model Setup, Running simulation

FLUENT start Double click on Setup FLUENT starts

FLUENT start Launcher Window of FLUENT Possible input: -Number of Processors -Number Precision -Color Scheme of GUI Leave as it is, just click OK now

Definiton of periodicity In Boundary Conditions menu, Type of per1 and per2 Zones must be set from wall to interface 1 2

Definiton of periodicity Set periodicity of computational domain by using Mesh Interfaces/Create command: -Mesh Interface: per -interface zone1: per1 -interface zone2: per2 -interterface options: periodic boundary condition -Type: rotational -Check Auto Compute Offset -Click Create -(Click Close if needed) 2

Turbulence model Set turbulence model in Models/Viscosus menu: -k-epsilon -Realizable -Enhanced wall treatment

Material properties In Materials menu, we obtain water material properties by: 1)Double click on Fluid: air 2)Click on Fluent Database…. 3)Search and select water-liquid ( ) 4)Copy 5)Close both windows 1 2 3 4

Fluid Zones In Cell Zones menu, Set the properties of our single zone 1)Material name: water liquid 2)Frame motion: check 3)Rotational velocity: 62.8 rad/s 3 1 2

Velocity inlet In Boundary Conditions slecet velocity_inlet and click on Edit: 1)Velocity magnitude 3.5 m/s, Absolute refernce frame 2)Turbulence Intesity, 10% Hydr. Diam, 0.01 m 1 2

Solution methods A Solution Methods menu: Set Schemes: -Pressure-velocity coupling: Coupled -Second Order upwind wherever possible

Convergence Monitors In Monitors menu, Turn off automatic convergence detection by given residual values 1)Double click on Monitors/Residuals 2)Convergence criterion: none 1 2

Convergence Monitors Let’s create a New convergence monitor: Torque on the blade: - Monitors/Residuals, Statistic and Force monitors - Create/Moment…

Convergence Monitors 1)Plot 2)Select Wall Zones belonging to the blade 3)Moment axis: z=1, Center: 0,0 1 2 3

Initialize Initialize simulation by -Selecting Hybrid Initialization and -clicking on Inizialize

Runing the simulation 1)Set the screen layout to be 2-divided 2)Go to Run Calculataion menu 3)Change Number of Iterations to 500 4)Hit Calculate 1 3 2 4

Reports for surface integrals In Reports menu, select Surface integrals, and click Set Up: 1)Field variable: Pressure / Static Pressure 2)Report type: area weighted average 3)Surfaces: select ONLY velocity-inlet 4)Click on Save output Parameter…. 5)Name it as Pressure-in Do one single iteration step (or a few) by running the simulation again Close FLUENT 1 3 2 4 5

4. Chapter: Results

Postprocessing Double click on Results CFD-post starts

Displaying varibale distributions 1)Volume rendering 2)Name: ex. pressure 3)Domains: all 4)Variable: pressure 5)Apply 3 4 5 2 1

Displaying the pressure distribution

Displaying the streamlines 1)Hide Volume rendering 1 by turning off checkbox in model tree 2)Streamlines 3)Name: stramline1 3 2 1

Displaying the streamlines 1)Start from: velocity inlet 2)Number of points: as you like 3)Apply 3 2 1

Displaying velocity vektors 1)Vectors 2)Domains: surface body 3)Location: surface body 3 2 1

Changing the published parameters Double click on Parameters 3

Run the case with different published parameters Fill up input parameters of Table of Design points as in Excel to set parametric runs (above image is illustration) Click Update All Design Points to start parametric runs and obtain output parameters Actual simulation starts, it takes time Two recommended variations: Change mesh size to 0.0015 m Radius to 110 mm (Disproportional values will result in impossible geometry and kill the simulation)

Bruce Willis