Gambit: Viscous grid for naca0016 airfoil

In this tutorial we will learn how to generate a viscous unstructured grid for a NACA0016 airfoil using Gambit.

Open the Gambit GUI by clicking the Gambit icon in Windows or by typing gambit at the Linux prompt.

Step 1. Importing: 

1. Change the default tolerance by going to  Edit/Defaults/GEOMETRY/TOLERANCE. Change the EDGE_FACET value from 0.001 to 1.0e-08. This helps to build more accurate geometries.

Fig 2, Curves using NURBS

2. Import the airfoil coordinates by going to File/Import/Vertex Data/ and pickup the file naca0016.dat file from the computer.  The file should be a simple ascii file having 3 columns of x, y, z coordinates.

 Step 2. Creating the geometric domain:

1. Gambit is a single precision grid generator, so when we are having a boundary layer with first spacing as small as 1.0e-05 to 1.0e-07 we end up having distorted cells in the boundary layer. To avoid this, scale up the geometry by 1000 times or in other words use a geometry which is in millimeters.
  

Fig 3, Domain

2. Join the points by box picking or individually picking each vertices by using the nurb option. Go to Geometry/EDGE COMMAND BUTTON/NURBS. It is advised to split the airfoil into 3 parts namely le, upper and lower and use 3 NURBS as shown in  figure 4. This helps to get smoother le curve than by capturing the airfoil profile by one curve.

3. Create a surface out of the 3 curves representing the airfoil. Go to FACE/Create Face From Wireframe. Pick the 3 airfoil edges in Edges tab and press Apply.

4. Create a circular surface with a radius of 20 chord by going to FACE COMMAND BUTTON/CREATE FACE, right click and choose Create Real Circular Face. In the Radius tab put 20,000 and press Apply. 

Fig 4, Airfoil after boolean operation

5. Use boolean operation to substract the airfoil surface from the bigger circular surface. Go to BOOLEAN OPERATIONS, right click and choose Substract. In the first Face tab pick the big circular surface and in the second Substract Faces tab pick the airfoil surface. Press Apply. One surface with the airfoil profile is created. The geometric domain is ready for meshing.
   
 Step 3. Meshing the airfoil edges:

1. Edge meshing will be done using the sizing function tool. Firstly change the default setting of sizing function by going to  Edit/Defaults/TOOLS/SFUNCTION. Change the default value of BGRID_MAX_TREE_DEPTH from 16 to 25 and that of BGRID_NONLINEAR_ERR_PERCENT from 25 to 15. These parameters helps to get smoother point distributions.

2. Two sizing functions will be used to mesh the airfoil. One to capture the curvature of the airfoil and the other to put finer points at the trailing edge. Go to TOOL COMMAND BUTTON/Create Size Function.

3. Sizing function 1: Choose Curvature in Type, for Sources and Attachment pick all the edges of the airfoil.  Input the following parameters. Angle = 3, Growth rate = 1.125, Max. size = 13, Min. size = 0.01. Press Apply.

4. Sizing function 2: Choose Fixed in Type. For Source pick the trailing edge vertex and for Attachment pick the edges of the airfoil. Input the following parameters. Start size = 0.5, Growth rate = 1.125, Max. size = 13. Press Apply.

Fig 5, Edge meshing

5. Now to mesh the airfoil go to MESH COMMAND BUTTON/Mesh Edges. Pick all the 3 airfoil edges and press Apply. Edge mesh as shown in  figure 5 is generated.

Step 4. Applying boundary layer padding:

  

1. To resolve the boundary layer around the airfoil a viscous padding is created using the boundary layer template.

2.  Before creating the boundary layer template we will make a few changes in the default settings. Go to Edit/Defaults/MESH/BLAYER/. Modify USE_FACETS_EVALS from 1 to 0 and QUICK_N_DIRTY from 1 to 0. This helps to get more accurate boundary layer.

3. Go to MESH COMMAND BUTTON/BOUNDARY LAYER COMMAND BUTTON/Create Boundary Layer. Pick the option of Aspect ratio (last) under Algorithm. Make the following inputs for, First row (a) = 1.0e-02, Rows = 26, Last percent (c/w) = 50. We need a first spacing of 1.0e-05 meters  to resolve the boundary layer properly. Since we have already scaled the geometry by 1000 times, the input we will be making under First row (a) will be 1.0e-02. 

Fig 6,  Boundary layer template

Note: First spacing is calculated based on the Reynolds number, reference length and estimated Y plus using standard Y plus calculator available on internet.

4. To properly resolve the trailing edge, the option of Wedge corner shape is activated. Pick all the 3 edges forming the airfoil. Press Apply. A white boundary layer template as seen in  figure 6 is created.

Step 5. Creating the unstructured grid with boundary layer:

Finally to generate the unstructured hybrid grid we will make use of two more sizing functions.

Fig 7, Mesh around airfoil

Fig 8, Mesh for complete domain

Go to TOOLS COMMAND BUTTON /SIZING-FUNCTION COMMAND BUTTON/Create Sizing Function. 

1. Sizing function 3: Pick Meshed under Type, pick all the 3 edges of the airfoil as Source and  domain surface as Attachment. Let the Growth rate = 1.125 and Max.size =  20000.

2. Sizing function 4: Let Type be Fixed. Pick the trailing edge vertex as Source and the domain surface as Attachment. Input the following parameters, Start size = 0.01, Growth rate = 1.125, Max. size = 20000. 

3. Now to mesh the domain go to MESH COMMAND BUTTON/FACE COMMAND BUTTON/Mesh Faces. Pick the domain surface, let Elements  be Tri and Type be Pave. Press Apply. A hybrid grid as seen in figures 7, 8, 9 and 10 is generated.

Fig 10, Mesh around trailing edge

Fig 9, Mesh around leading edge

 Step 6. Quality check :

To check the quality of the cells in the grid pick the right bottom icon under Global Control called EXAMINE MESH.

Fig 11, Skewed cells at trailing edge

Fig 12, Node movement

Fig 13, Problem rectified

1. Pick Range under Display Type. Activate both quad and tria icons under 2D Element. Let the Quality Type be EquiSize Skew. Press Update. 

2. The  color the cells in the grid changes with the skewness quality level. To check the worst cell, activate the button Show worst element. Under Transcript a message saying that the worst element quality value is 0.95. This needs to be corrected.

3. To make corrections, come out of Examine Mesh and go to Move Face Nodes under face meshing options. Here pick the domain face in Face and pick the node which is making the 2 cells skewed and physically move to the proper location. Make sure that the button of Smooth is active. This will rectify the problem.  

 Step 7. Applying boundary conditions  and            exporting the mesh :

1. As a last step before exporting the mesh we will apply boundary conditions. Go to ZONE COMMAND BUTTON/Specify Boundary Types. 

2. Pick the edges forming the airfoil and Name it as airfoil. Apply  Type as WALL.
3. Pick the outer edge and Name it as farfield and  apply PRESSURE_FAR_FIELD under Type. Press Apply.
4. Now go to CONTINUUM TYPE COMMAND BUTTON in ZONE. Here pick the domain surface, Name it as fluid and apply FLUID as Type.

This completes applying boundary conditions. To export go to File/Export/Mesh/ and type out the name as naca0016.msh. Make sure to activate the button of Export 2-D(X-Y) Mesh.  If all the steps are done properly one will get the message "Mesh was successfully written to naca0016.msh" under Transcript.

This completes the tutorial on viscous grid for Naca0016 airfoil using Gambit.