3D Wing Tutorial by Ryan Babigian
PURPOSE
The purpose of this tutorial is to instruct the reader on the methods involved in creating, meshing, solving, and analyzing a complex wing geometry using CATIA, Gambit, and Fluent Computational Fluid Dynamics (CFD) software. This tutorial is directed at an intermediate to advanced audience with knowledge of CFD theory and software. Although there are several resources available to the CFD student for the creation and meshing of airfoils and finite (quasi-2D) wings, this tutorial provides the CFD student with an approach to creating and analyzing complex wing geometry. In this tutorial a finite wing with dihedral, taper, and sweep will be analyzed. Additionally, most true-scale 3D wing meshes require an enormous amount of computational power and memory in order to run the CFD solution. This tutorial allows the CFD student to run the solution on a single computer. The geometry will be created using CATIA software and exported to Gambit, where the geometry will be meshed. The geometry will then be imported into Fluent for the CFD processing and post-processing. This tutorial is comprised of four parts:
1. Wing Geometry Creation Using CATIA
2. Wing Meshing Using Gambit
3. Wing Processing Using Fluent
4. Wing Post-processing Using Fluent
1
Lesson 1: Wing Geometry Creation Using CATIA CATIA SETUP 1. The first step is to start the CATIA software. Go to Start → College of Engineering → CATIA → CATIA V5R17. 2. Change the unit system in CATIA by selecting Tools → Options →Parameters and Measure → Units and change the length parameter to ‘foot (ft)’. 3. Note: The airfoil file is an IGES file (.igs) and can be found in the ERAU T drive. The location of the file is T:\AE Resources\Airfoil data. 4. Open the airfoil file that will be used for the 3D wing cross-section by selecting File → Open. For this tutorial the b737a airfoil, as seen below in Figure 1.1, will be used.
Figure 1.1: B737a Airfoil Used for 3D Wing Cross-section 2
CREATING THE AIRFOIL 1. After the b737a.igs file has been opened in CATIA, highlight all of the airfoil vertices by selecting ‘Geometrical Set.1’. Right-click on the mouse and select ‘copy’ to copy all of the airfoil vertices. 2. Begin a new part by selecting File → New. In the window that appears, select ‘Part’. 3. In the part tree, highlight the xy plane and left-click on the sketcher icon sketcher mode.
to enter into
4. Next, right-click on the mouse and select ‘paste’, to paste all of the airfoil vertices into the current sketch. When all of the airfoil vertices have been pasted, exit sketcher mode. Left-click on the ‘Fit all In’ button. The screen should appear similar to that seen in Figure 2:
Figure 2: Airfoil Vertices Upon Completion of Step 6 5. Create an axis system at the origin by selecting the axis icon dialogue box appears, select ‘OK’.
. When the axis
6. Next, select ‘Geometrical Set.1’ in the part tree to highlight all of the airfoil vertices. Left-click on the rotate icon
to rotate the airfoil vertices about the z-axis. 3
7. In the rotation dialogue box that appears, left-click in the axis field to make it active and select the z-axis from the axis system that was created in step 5. Next, type 270 for the angle and select ‘Hide/Show initial element’ and select ‘OK’. 8. In the part tree, expand the ‘Part Body’ by left-clicking on the plus (+) sign to the left of it. Select the ‘Multi Output.1 (Rotate)’ to highlight the airfoil vertices. 9. Left-click on the rotate icon to rotate the airfoil vertices about the x-axis. Repeat step 7, but select the x-axis rather than the z-axis. After completing these steps, the window should appear similar to that seen in Figure 3, below.
Figure 3: Rotation of the Airfoil Vertices about the Z and X Axes 10. In the part tree, highlight the xy plane and left-click on the sketcher icon sketcher mode.
to enter
11. In the part tree, locate and expand the ‘Multi Output.2 (Rotate)’ and highlight all of its sub elements (the airfoil vertices). 12. Select the project 3D elements icon. This will create a projection of the airfoil vertices onto the sketch so that the vertices can be connected to create the edges of the airfoil.
4
13. In order to create the edges of the airfoil, one more point must be made to define the trailing edge of the airfoil. To do this, select the point by using coordinates the dialogue box that appears enter the following: H: V:
icon. In
0.08375 0
Select ‘OK’. 14. Next, select the spline tool. Zoom in as necessary and select the trailing edge point that was created in step 13. 15. Connect the spline to each vertex, or point, along the upper surface of the airfoil. Start at the trailing edge and connect the vertices along the upper airfoil, continuing along the lower surface of the airfoil, back to the trailing edge vertex. When completed, all the vertices of the airfoil should be connected, and should appear similar to that shown in Figure 4, below.
Figure 4: Connected Airfoil Vertices using the Spline Tool 16. Exit the sketcher mode by selecting the exit workbench in the part tree and enter sketcher mode again. 5
icon. Highlight the xy plane
17. Project the two edges of the airfoil by left-clicking on them and select the project 3D elements icon. In the part tree, locate and highlight all of the sub elements of ‘Multi Output.2 (Rotate)’ and right-click and select ‘Hide/Show’. Next, select ‘Sketch 1’ and right-click and select ‘Hide/Show’. The airfoil vertices and original edges created in step 15 should be hidden. 18. Next, the airfoil needs to be scaled. To do this, select the upper and lower edges of the airfoil and left-click on the scale tool. In the dialogue box that appears, uncheck the ‘Duplicate mode’ option. Next, left-click on the origin (0,0) of the sketch and enter a value of 477.6 for the ‘Scale value’. Select ‘OK’. 19. To create the flow domain geometry, select the rectangle tool and create a rectangle around the airfoil. The dimensions of the rectangle are shown in Figure 5:
Figure 5: Flow Domain Dimensions 20. After the flow domain has been created, exit sketcher mode.
6
CREATING THE 3D WING Note: The following steps to create the 3D wing are based on the geometry of a 787 wing. The wing geometry used in this tutorial has the following characteristics: Span, b =87 feet Leading edge sweep, Λ = 36 degrees Root chord, cr = 40 feet Tip chord, ct = 5.5 feet Tip-to-chord ratio, λ = 0.1375 Dihedral, Г = 8 degrees These geometrical wing characteristics are illustrated in Figure 6:
Figure 6: Dimensions of 787 Wing used in Tutorial
7
1. Two profiles of the airfoil and flow domain will be created to generate the wing. The first profile will be at the planform break, and the second at the wingtip. First, create two planes by selecting the plane
icon.
2. In the dialogue box that appears, left-click in the reference box to make it active. Select the xy plane by highlighting it in the parts tree. Select ‘Reverse direction’, such that the plane is in the negative z-direction. 3. In the ‘Offset’ box, enter the value 29. Select ‘OK’. A plane is created parallel to the xy plane, 29 feet in the negative z-direction. 4. Next, create the second plane by repeating steps 1-2. In the ‘Offset’ box, enter the value 87. A plane is created parallel to the xy plane, 87 feet in the negative z-direction. 5. Select the first plane that was created and enter the sketcher mode by clicking on the sketcher icon
.
6. Select the top and bottom root airfoil edges and the 4 edges of the root rectangular flow domain by holding the control button down and left-clicking on each of them. After all 6 edges are highlighted, project them onto the current sketch by selecting the project 3D elements icon. Move the cursor over one of the new edges, right-click, and select Selected objects → Isolate. 7. With the edges of the airfoil and domain still highlighted, left-click on the scale tool. In the dialogue box that appears, uncheck the ‘Duplicate mode’ box. Left-click on the origin (0,0) of the sketch, and in the ‘Scale value’ field enter 0.4733. Select ‘OK’. 8. Next, translate the profile by left-clicking on the translate icon. Again, select the origin (0,0) of the sketch. In the ‘Length value’ field enter 21.07. Click ‘OK’. In the lower right toolbar, enter the following values for the ‘End point’: H: V:
21.07 4.076
9. Hit enter. Exit sketcher mode by selecting the exit workbench icon. If done correctly, the sketch should be similar to that shown in Figure 7, on page 9.
8
Figure 7: Root and Planform Break Profile Sketches 10. Next, the profile at the wingtip needs to be created. To do this, left-click on the second plane that was created in step 4, and enter sketcher mode. Repeat steps 6-8. When scaling, enter a value of 0.1375 in the ‘Scale value’. When translating, enter a value of 63.21 in the ‘Length value’ field. For the ‘Endpoint’ values enter the following: H: V:
63.21 12.227
11. Hit enter. Exit sketcher mode by selecting the exit workbench the sketch should be similar to that shown in Figure 8, below.
icon. If done correctly,
Figure 8: Root, Planform Break, and Tip Profile Sketches 9
12. Before the upper and lower surfaces of the wing can be created, each profile (root, planform break, and tip) need to be disassembled. To do this, select the disassemble tool. Left-click on the root profile and select ‘OK’ in the dialogue box that appears. 13. Repeat step 10 for both the planform break profile and the tip profile. 14. To create the upper and lower surfaces of the wing, select the multi-section surface tool. Select the top edge of the root airfoil and the top edge of the planform break airfoil by left-clicking on them. Select ‘OK’. 15. Next, select the multi-section surface tool again and select the top edge of the planform break airfoil and the top edge of the tip airfoil. Click ‘OK’. After completing steps 12 and 13, the upper surface of the wing should have been created. 16. Create the lower surface of the wing by selecting the bottom edges of the airfoils in the same manner outlined in steps 12 and 13. 17. The next step is to fill in the root and tip airfoil cross-sections. To do this, select the fill tool and left-click the top and bottom edges of the root airfoil. Select ‘OK’. 18. Repeat step 15 on the tip airfoil cross-section to fill in the tip airfoil. When all of the surfaces and both fills have been completed successfully, the geometry should be similar to that seen in Figure 9:
Figure 9: Wing Geometry with Filled Surfaces 10
CREATING THE FLOW DOMAIN 1. To allow for 3D effects on the wing geometry, one last profile needs to be created. To do this, select the plane tool. Select the xy plane as the reference and enter a value of 117 in the ‘Offset’ field. Just as before, select ‘Reverse direction’ and select ‘OK’. 2. Left-click on the plane and enter sketcher mode by clicking on the sketcher icon . Select the 4 edges of the rectangular tip domain by holding down the control button and selecting each 3. Next, left-click on project 3D elements . Move the cursor over one of the new edges, right-click, and select Selected objects → Isolate. Exit sketcher mode by selecting the icon. 4. To create the flow domain, the 4 rectangular profiles (root, planform break, tip, and last profile) that have been created need to be connected. To do this, select the line tool. Left-click on the upper left corner of the root rectangular flow domain. Next, left-click on the upper left corner of the planform break rectangular flow domain to create a line connecting the two. Select ‘OK’. 5. Select the line tool again and left-click on the upper left corner of the planform break rectangular flow domain. Next, left-click on the upper left corner of the tip rectangular flow domain to create a line connecting the two. Select ‘OK’. 6. Again, select the line tool and left-click on the upper left corner of the tip rectangular flow domain. Next, left-click on the upper left corner of the last rectangular flow domain, that was created in step 3, to create a line connecting the two. Select ‘OK’. 7. Repeat steps 4-6 for the lower left, upper right, and lower right corners of the rectangular flow domains. When completed correctly, the wing geometry and flow domain should appear similar to that seen in Figure 10, on page 12. Now that the wing geometry has been created using CATIA, the last step is to prepare the geometry for export into the preprocessing software, Gambit.
11
Figure 10: Final Wing and Flow Domain Geometry
PREPARING THE WING MODEL FOR EXPORT 1. From the parts tree, locate and select all of the parts of the geometry entitled ‘Sketch’. Right-click and select ‘Hide/Show’. Locate and select the 4 planes that were created as well as the axis system and right-click and choose ‘Hide/Show’. 2. To save the file, select File → Save As. In the window that appears, give the file a name, such as ‘tutorial 787 wing’. Under the ‘Save as type’ drop-down list, select ‘.igs’. Browse to the Gambit directory and left-click on ‘save’. Note: The wing geometry file should be saved in an iges file format. It is important to save the file into the Gambit directory, otherwise Gambit will not be able to import the .igs file. The default directory is C:\Fluent.Inc\Gambit2.4.6.
12
Lesson 2: Wing Pre-Processing Using Gambit FILE IMPORT AND SETUP 1. The first step is to start the Gambit software. Go to Start → College of Engineering → Fluent Inc Products → Gambit 2.4.6 → Gambit 2.4.6. 2. After Gambit opens, select File → Import → IGES. The screen that appears is shown in Figure 1:
Figure 1: IGES import file screen 3. The page defaults should be: Translator: Spatial Model Scale Factor: 1 Make Tolerant Shortest Edge. 1
4. Leave all defaults unchanged and click on the browse button next to the file name. Search for the file tutorial 787 wing.igs that was saved in Lesson 1: Wing Geometry Creation Using CATIA. The default location is C:\Fluent.Inc\Gambit2.4.6\tutorial 787 wing.igs. 5. Once the file tutorial 787 wing.igs is located, select ‘Accept’ on the IGES import screen. 6. Once Gambit imports the IGES file, the Graphics User Interface (GUI) should appear similar to that shown in Figure 2:
Figure 2: Wing Geometry After Import Into Gambit
2
PREPARING THE WING GEOMETRY FOR MESHING Before the wing geometry can be meshed, a volume containing the wing geometry must be created. To do this, faces must be made of each side of the flow domain and of the wing surfaces. Note: When creating faces from edges, all edges that are to form the face must be selected in a consecutive and continuous order, from start to finish. 1. When the wing geometry is imported, Gambit automatically creates a volume out of the wing geometry, represented by the color green in Figure 2, above. To create a volume from the flow domain, select the Face command button
under geometry and the
Create face from wireframe button under face. While holding down the shift button, select the 4 edges that define the root rectangular flow domain by left-clicking on them in a continuous order. After all 4 edges have been selected, the edges will turn red. By selecting ‘Apply’, the edges will turn blue indicating that a face has been created. 2. Repeat step 1 for all 14 sides of the flow domain: 3 sides on the left of the domain; 3 sides on the right of the domain; 3 sides on the top of the domain; 3 sides on the bottom of the domain; 1 side on the front or root of the domain (created in step 1); and 1 side on the rear of the domain. Once all of these sides have been converted into faces, the wing geometry should appear similar to that seen in Figure 3:
3
Figure 3: Wing Geometry After All Faces Are Generated 3. Next, a volume must be created using the faces generated in steps 1 and 2. Select the Volume command button under geometry and select the stitch faces button. While holding down the shift key, select all of the 14 faces created in step 2. When all faces are selected, click ‘Apply’. The flow domain will turn green, indicating that a volume has been created.
4. Under Boolean operations, select the Subtract button. In the dialogue box that appears, left-click in the ‘Volume’ field to make it active. Select the domain volume by holding down the shift button and left-clicking on any face of the flow domain volume. 5. Next, left-click in the ‘Subtract Volumes’ field to make it active. While holding down the shift button, left-click on any face of the wing volume. Select ‘Apply’. If done correctly, the final volume consisting of the wing inside the flow domain should appear similar to that seen in Figure 4, below.
Figure 4: Final Volume of the Wing Inside of the Flow Domain
6. Create a face on the root airfoil by selecting the Face command button
under
geometry and the Create face from wireframe button under face. Hold down the shift button and select the top edge and the bottom edge of the root airfoil by left-clicking on them. Select ‘Apply’. 4
CREATING A BOUNDARY LAYER MESH ON THE WING
1. To create a boundary layer on the root airfoil, select the Mesh command button under operation, then select the edge command button mesh edges
under mesh. Select the
button.
2. In the dialogue box that appears, left-click in the ‘Edges’ field to make it active. Select the top edge of the airfoil, and enter the following values in the dialogue box: Type: Successive Ratio: 1 Change ‘interval size’ to ‘interval count’ and enter 50 3. Leave all other values at their default setting, at select ‘Apply’. 4. Repeat step 2 for the bottom edge of the root airfoil. 5. Next, select the Boundary layer command button appears is shown in Figure 5:
under mesh. The dialogue box that
Figure 5: Boundary Layer Dialogue box 5
6. Enter the following values in the boundary layer dialogue box: First row: 0.05 Growth Factor: 1.15 Rows: 18 7. Check the ‘Internal continuity’ and ‘Wedge corner shape’ options and leave all other settings at their default values. 8. Left-click in the ‘Attachment’ field to make it active and select the top and bottom edges of the root airfoil. Select ‘Apply’. Figure 6, below, shows the boundary layer generated over the root airfoil. Note: The top and bottom edges of the root airfoil will be need to be selected twice each. In order to get the proper boundary layer, deselect the edges that do not generate an appropriate boundary layer mesh.
Figure 6: Boundary Layer Created Over the Root Airfoil
6
MESHING THE WING AND FLOW DOMAIN 1. In order to create a volume mesh on the flow domain, the individual edges of the domain and wing need to be meshed. To do this, select the Mesh command button operation, then select the edge command button edges
under
under mesh. Select the mesh
button.
2. In the dialogue box that appears, left-click in the ‘Edges’ field to make it active. Select the horizontal edges, edge 1 and edge 2, as shown below in Figure 7. Enter the following values in the dialogue box: Type: Successive Ratio: 1 Change ‘interval size’ to ‘interval count’ and enter 25 Select ‘Apply’.
Edge 1
Edge(s) 6 Edge 3
Edge 4
Edge 2
Figure 7: Edge Selection for Edge Meshes (Rear Edges Hidden) 7
Edge 1
3. Next, select the vertical edges of the root face, edge 3 and edge 4, and enter the following values in the mesh edges dialogue box: Type: Successive Ratio: 1 Change ‘interval size’ to ‘interval count’ and enter 10 Select ‘Apply’. 4. Select the 4 edges shown in Figure 7, labeled ‘edge(s) 6’, and enter the following values in the mesh edges dialogue box: Type: Successive Ratio: 1 Change ‘interval size’ to ‘interval count’ and enter 20 Select ‘Apply’. 5. Select the 2 edges, labeled ‘edges(s) 7’ in Figure 8 on page 9. Enter the following values in the mesh edges dialogue box: Type: Successive Ratio: 1 Change ‘interval size’ to ‘interval count’ and enter 20 6. Select the 4 edges, labeled ‘edge(s) 8’ in Figure 8, on page 9. Enter the following values in the mesh edges dialogue box: Type: Successive Ratio: 1 Change ‘interval size’ to ‘interval count’ and enter 30 7. Next, repeat step 6 for the 2 edges, labeled ‘edge(s) 9’ in Figure 8 on page 9. 8. Finally, select the 4 edges, labeled ‘edge(s) 10’ in Figure 8 on page 9. Enter the following values in the mesh edges dialogue box: Type: Successive Ratio: 1 Change ‘interval size’ to ‘interval count’ and enter 20 8
If completed correctly, the current wing and flow domain edge meshes should appear similar to that seen in Figure 9, below. Edge(s) 10
Edge(s) 9
Edge(s) 8
Edge(s) 7
Figure 8: Edge Selection for Edge meshes of Wing and Flow Domain (Front Edges Hidden)
Figure 9: Final Edge Meshes of Wing and Flow Domain 9
VOLUME MESHING THE WING AND FLOW DOMAIN 1. To mesh the wing and flow volume, select the Mesh command button operation, then select the volume command button
under
, then select the mesh volumes
button. 2. Left-click in the ‘Volumes’ field to make it active, then hold down the shift button and left-click anywhere on the flow domain volume to select it. The entire volume will turn red. 3. In the ‘Elements’ field, select Hex/Wedge. Left-click in the ‘Sources’ field to make it active. Select the root rectangular face, the wing tip face, and the face located farthest from the root face. These 3 faces are shown in red in Figure 10:
Farthest face
Wing tip face
Root face
Figure 10: Sources Face Selection for the Volume Mesh 10
4. Keep all other default values in the dialogue box, and select ‘Apply’. When the volume mesh is completed, the meshed geometry should appear similar to that seen in Figure 11, on page 11.
Figure 11: Successful Volume Mesh of the Wing and Flow Domain Now that the wing and flow volume geometry has been meshed, the last step is to assign boundary conditions in Gambit.
11
Assigning Boundary Conditions 1. Select the Zones Command Button
under Operation. Next, select Specify Boundary
Types Command Button under Zones. The boundary conditions dialogue box will appear, as seen in Figure 12:
Figure 12: Boundary Conditions Dialogue Box 2. In the ‘Type’ field, select wall. Change the edges field beneath ‘Entity’ to faces. Leftclick in the faces field to make it active. Select the 5 faces that comprise the wing geometry: 2 faces for the top surface of the wing; 2 faces for the bottom surface of the wing; and the 1 wing tip face. In the ‘Name’ field, type “wing” and select ‘Apply’. 3. Next, change the ‘Type’ field to symmetry. Select the following 8 faces of the volume: the 3 top faces of the volume; the 3 bottom faces of the volume; the root face of the volume; and the farthest face of the volume. In the ‘Name’ field, type “symmetry” and select ‘Apply’.
12
4. Next, change the ‘Type’ field to pressure inlet, and select the 3 faces that define the left side of the volume. In the ‘Name’ field, type “inlet” and select ‘Apply’. 5. Finally, change the ‘Type’ field to pressure far field, and select the 3 faces that define the right side of the volume. In the ‘Name’ field, type “outlet” and select ‘Apply’. 6. At this point, save the diamond mesh. To do this, select File → Save As and choose a name for the mesh, such as ‘wing mesh tutorial’. 7. The last step is to export the mesh to the Fluent solver. To do this, select File → Export→ Mesh, and be sure that the box next to ‘Export 2-D (X-Y) Mesh’ is unchecked and select ‘Accept’.
13
Lesson 3: Wing Processing Using Fluent File Import and Setup 1. The first step is to start the Fluent software. Go to Start → College of Engineering → Fluent Inc Products → Fluent 6.3.26 → Fluent 6.3.26. 2. Next, a prompt screen will appear before Fluent starts as seen in Figure 1 below:
Figure 1: Fluent Prompt Screen 3. Highlight the ‘3D’ selection and select ‘Run’. 4. After Fluent opens, select File → Read → Case, and browse for the 3-D Gambit mesh that was exported in the previous lesson. Select ‘OK’ to import the 3-D wing case into the Fluent solver. When Fluent is finished reading the case, the word ‘done’ will be displayed. 5. Next, it is important to check the mesh to be sure that it is free of errors. To do this, select Grid → Check. If the grid check is successful, the word ‘done’ will appear. This is seen below in Figure 2, on page 2.
1
Figure 2: Successful Grid Check
2
Solver Setup 1. The wing mesh must be setup for processing. First, the solver needs to be selected. To do this select Define → Models → Solver. Depending on the version of Fluent, the screen that appears should be similar to that shown in Figure 3 below:
Figure 3: Solver Setup 2. Select coupled or density based (depending on the version). Be sure that the steady, 3D, and implicit options are selected. Leave all other settings at their default values, and select ‘OK’. 3. Next, the geometry needs to be scaled because it was created in feet, and the default unit of measure in Fluent is meters. To do this select Grid → Scale. In the ‘Scale grid’ window that appears, select ‘ft’ from the drop down list next to ‘Grid was created in’. Left-click on the ‘Scale’ button to scale the grid. 4. Next, the material model must be defined. To do this, select Define → Materials. For this tutorial the fluid being modeled is air, which is the default setting. Under ‘Properties’, change ‘Density’ to ideal-gas. Change the ‘Viscosity’ to Sutherland and click ‘OK’. Leave all other settings at their default values and left-click on the ‘Change/Create’ button.
3
5. Next, the viscous model needs to be selected. Select Define → Models → Viscous and choose the Spalart-Allmaras viscous model. Leave all settings at their default values and select ‘OK’. 6. Next, the operating condition must be set. To do this, select Define → Operating Conditions. Change the value under ‘Operating Pressure’ to zero and select ‘OK’. 7. Note: Because the fluid (air) is being modeled as an ideal gas and the solution will involve compressible flow, Fluent recommends setting the ‘Operating Pressure’ value to zero. 8. The next step is to set the initial boundary conditions. Select Define → Boundary Conditions. The boundary conditions window will appear, seen in Figure 4 below:
Figure 4: Boundary Conditions Window For this tutorial, only the inlet and outlet boundaries need be set. To do this, select inlet, then select ‘Set’. The default inlet boundary is pressure inlet (as defined in lesson 2). The window that appears should be similar to that seen in Figure 5 on page 5. Note: The boundary conditions for the solver are based on typical 787 jet airliner cruise conditions. The altitude and cruise speed corresponding to these conditions are 37,000 ft and Mach 0.85, respectively.
4
In the pressure inlet boundary condition window, enter the following: Gauge Pressure: 21728 Total Temperature: 216 Direction Specification Method: Direction Vector X-component of Flow Direction: 1 Y-component of Flow Direction: 0 Z-component of Flow Direction: 0
Figure 5: Inlet Boundary Condition Window After the values have been inputted, select ‘OK’. 1. For the outlet boundary condition, a pressure far field is the default outlet boundary (as specified in lesson 2). Highlight ‘outlet’ and select ‘Set’. The window that appears should be similar to that seen in Figure 6, on page 5. Input the following values for the outlet: Gauge Pressure: 21728 Mach Number: 0.85 Temperature: 216 X-component of Flow Direction: 1 Y-component of Flow Direction: 0 Z-component of Flow Direction: 0 5
After the values have been inputted, select ‘OK’.
Figure 6: Outlet Boundary Condition Window 2. In order to monitor the convergence of the solution, one more parameter must be set. Select Solve → Monitors →Residual. The window that appears is seen in Figure 7, below. Leave all default values unchanged, check the box next to ‘Plot’, and select ‘OK’.
Figure 7: Residual Monitors Window 6
3. Next, the solver must be initialized to begin the solution. Select Solve → Initialize → Initialize. Figure 8, below, shows the Solution Initialization window. Select inlet from the ‘Compute from’ drop-down list. Select ‘Outlet’. 4. To begin the iteration process, select Solve → Iterate. Input ‘600’ for the ‘Number of Iterations’ and select ‘iterate’. The solution will begin iterating, and should converge after approximately 580 iterations.
Figure 8: Solution Initialization Window Figure 9, below, shows the convergence history of the solution. The last step is to analyze the results of the solution.
Figure 9: Convergence History 7
Lesson 4: Wing Post-processing Using Fluent DISPLAYING THE WING 1. The first step in the post-processing of the CFD solution is to setup the wing display. For the purposes of this tutorial the wing will be displayed with full span, lighting, and surface shading. 2. Select Display → Views to bring up the ‘Views’ window in Fluent. The ‘Views’ window should be similar to that seen in Figure 1:
Figure 1: Views Window 3. To create a full span wing, the wing must be mirrored about the origin. To do this, select ‘Define Plane’. In the dialogue box that appears, enter the following values: X: Y: Z:
0 0 40
4. Select ‘Add’, then select ‘OK’. In the ‘Views’ window, highlight the ‘40z = 0’ and select ‘Apply’. The wing is now displayed in full span. 5. To create lighting on the wing surface, select Display → Options. In the window that appears, leave all values at their default setting and check the box next to ‘Lights On’. Select ‘Apply’. 1
6. Next, select Display → Grid to open the ‘Grid Display’ window. The ‘Grid Display’ window is seen in Figure 2:
Figure 2: Grid Display Window 7. Be sure that the only box that is checked in the ‘Options’ field is that of faces. Select only the wing in the ‘Surfaces’ field. Leave all other values at their default settings and click ‘Display’. The wing geometry should appear similar to that seen in Figure 3:
Figure 3: Wing With Full Span and Lighting
2
DISPLAYING CONTOURS 1. First, the contours of pressure on the surface of the wing will be displayed. To do this, select Display → Contours. In the ‘Contours’ window that appears, check the box next to ‘Filled’ and for ‘Levels’ enter 100. The default setting is ‘Contours of’ Pressure…Static Pressure. In the ‘Surfaces’ field, select only wing and select ‘Display’. Figure 4, below, is a contour plot of the static pressure on the surface of the wing.
Figure 4: Contours of Static Pressure 2. Next, display the contours of Mach number on the wing surface in a manner similar to that outlined in step 1. In the ‘Contours of’ drop-down list select Velocity…Mach number. Select ‘Display’. Figure 5, below, is a contour plot of the Mach number on the surface of the wing.
Figure 5: Contours of Mach Number 3
Displaying Vorticity Vectors 3. To display the vortices at the wingtips, planes must be created. To do this, select Surface → Plane. In the ‘Plane Surface’ window that appears, check the ‘Bounded’ and the ‘Plane tool’ boxes. 4. Create the first plane by entering the following values into the ‘Plane Surface’ dialogue window: x0(m): 21 y0(m): -30 z0(m): -35
x1(m): 21 y1(m): -30 z1(m): 0
x2(m): 21 y2(m): 30 z2(m): 0
Select ‘Create’. 5. Create the second plane by repeating step 2 using the following values: x0(m): 25 y0(m): -30 z0(m): -35
x1(m): 25 y1(m): -30 z1(m): 0
x2(m): 25 y2(m): 30 z2(m): 0
Select ‘Create’. 6. Create the third plane by repeating step 3 using the following values: x0(m): 29 y0(m): -30 z0(m): -35
x1(m): 29 y1(m): -30 z1(m): 0
x2(m): 29 y2(m): 30 z2(m): 0
7. To display the vorticity vectors at the wingtips, select Display → Vectors. The ‘Vectors’ window appears, as seen in Figure 6 on page 5. Check the box next to ‘Draw grid’ and select ‘OK’. In the ‘Surfaces’ field, highlight the 3 planes that were created in steps 2-4. Choose ‘Vectors of’ Velocity, and ‘Color by’ Velocity…Vorticity Magnitude. Select ‘Display’. Deselect the box next to ‘Auto range’ and enter 5 in the ‘Min’ field and 50 in the ‘Max’ field. Select ‘Display’ again. Figure 7, on page 5, shows the vortices in the wake region of the wingtip.
4
Figure 6: Vectors Window
Figure 7: Wingtip Vorticity vectors
5
The limit of the detail of the results (corresponding to the mesh size of the flow domain) was a result of processing a complex geometry on a single computer. By refining the mesh size on the wing and flow domain, more detailed results can be obtained. This lesson was a brief overview of post-processing techniques, in which the contours of pressure and Mach number, as well as vorticity vectors, were realized. Further analysis of the computational results can be conducted and is encouraged.
6
