ACU-T: 2100 Turbulent Flow Over an Airfoil Using the SST Turbulence Model

This tutorial provides the instructions for setting up and using the SST and K-Omega turbulence models in AcuSolve. The application that is investigated is the flow over a NACA0012 airfoil at an angle of attack of 5 degrees. AcuSolve is used to extract the lift and drag forces on the airfoil. This tutorial is designed to introduce you to the modeling concepts necessary to perform external aerodynamic simulations using the SST and K-Omega turbulence models.

The basic steps in any CFD simulation are shown in ACU-T: 2000 Turbulent Flow in a Mixing Elbow. The following additional capabilities of AcuSolve are introduced in this tutorial:

Use of the SST and/or K-Omega turbulence models
Use of the farfield boundary condition type
Use of the Variable Manager to store variables and expressions
Entry of expressions into the panel area.

Prerequisites

You should have already run through the introductory tutorial, ACU-T: 2000 Turbulent Flow in a Mixing Elbow. It is assumed that you have some familiarity with AcuConsole, AcuSolve, and AcuFieldView. You will also need access to a licensed version of AcuSolve.

Prior to running through this tutorial, copy AcuConsole_tutorial_inputs.zip from <Altair_installation_directory>\hwcfdsolvers\acusolve\win64\model_files\tutorials\AcuSolve to a local directory. Extract NACA0012.x_t from AcuConsole_tutorial_inputs.zip.

Analyze the Problem

An important first step in any CFD simulation is to examine the engineering problem to be analyzed and determine the settings that need to be provided to AcuSolve. Settings can be based on geometrical components (such as volumes, inlets, outlets, or walls) and on flow conditions (such as fluid properties, velocity, or whether the flow should be modeled as turbulent or as laminar).

The problem to be addressed in this tutorial is shown schematically in the figure below. It consists of a cylindrical bounding region containing air that flows past a NACA0012 airfoil profile. The simulation is performed as 2D by including only a single layer of extruded elements in the airfoil span direction. The velocity vector at the far field boundary of the domain is specified to yield an angle of attack of 5 degrees and a Reynolds Number of 1.0e6. The airfoil chord is 1 meter, and standard air material properties are used for the simulation.

Figure 1.

The diameter of the cylindrical bounding volume for the airfoil is set to 500 times the airfoil chord. This large bounding volume is selected to ensure that the farfield boundaries are sufficiently far from the airfoil to prevent any influence of blockage of the domain on the solution.

The initial simulation of this airfoil will be considered fully turbulent and use the SST turbulence model. These simulation conditions correspond to a scenario where the boundary layer on the leading edge of the airfoil is tripped with some type of roughness elements to produce a fully turbulent boundary layer over the length of the airfoil.

Define the Simulation Parameters

Start AcuConsole and Create the Simulation Database

In this tutorial, you will begin by creating a database and loading some predefined variables, populating the geometry-independent settings, loading the geometry, creating groups, setting group attributes, adding geometry components to groups and assigning mesh controls and boundary conditions to the groups. Next you will generate a mesh and run AcuSolve to converge on a steady state solution. Finally, you will review the results using AcuFieldView and AcuProbe.

In the next steps you will start AcuConsole, create the database for storage of AcuConsole settings and set the location for saving mesh and solution information for AcuSolve.

Start AcuConsole from the Windows Start menu by clicking Start > Altair <version> > AcuConsole.
Click the File menu, then click New to open the New data base dialog.

Note: You can also open the New data base dialog by clicking on the toolbar.
Browse to the location that you would like to use as your working directory.
This directory is where all files related to the simulation will be stored. The AcuConsole database file (.acs) is stored in this directory. Once the mesh and solution are created, additional files and directories will be created within this directory.
Create a new folder named TurbulentAirfoil_SST and open this folder.
Enter Turbulent_Airfoil_SST as the File name for the database.

Note: In order for other application to be able to read the files written by AcuConsole, the database path and name should not include spaces.
Save the database to create a backup of your settings.

Define Expressions and Variables Using the Variable Manager

In this step, you will use the Variable Manager in AcuConsole to create a list of expressions that will be used during the model setup process.

The Variable Manager is a useful utility that allows you to define variables and expressions that can later be referenced as inputs to the various settings used throughout the process of building your model. When a model is constructed in terms of variables, it is very easy to update the entire model with a simple change of a single parameter from the Variable Manager. This process will be illustrated in this tutorial.

The AcuConsole expression syntax has two different types of entry methods. The first entry method is known as immediate evaluation, and uses the = sign to perform assignments of values to a variable. For example, consider an inlet boundary to a model with an area of 2 m and an average velocity of 2 m/s. If you want to create a variable called volumeFlowRate, you can enter the expression into the Variable Manager as follows:

Name	Expression
volumeFlowRate	=2*2

When using the = syntax, the expression is immediately evaluated when you click out of the text entry area and the equation used to compute that expression is not stored in the database. However, if you wish to store the expression as a relationship, you can use the relational expression definition by replacing the = with :=. In that case, AcuConsole stores the expression and evaluates it when needed. This means that you can define expressions that are functions of other expressions and changes to one will be propagated to all other dependent expressions. For example, if you want to redefine the inlet flow rate using a relational expression, you can do that as follows:

Name	Expression
inletArea	2.0
averageVelocity	2.0
volumeFlowRate	:=inletArea*averageVelocity

Using this syntax, the formula for volumeFlowRate is stored in the database and will automatically update whenever the inletArea or averageVelocity are updated. Any variables that are defined in the Variable Manager can be referenced when specifying an integer or floating point value in the panels area. The same expression syntax can be used.

Click the Variable List icon from the main toolbar:

Figure 2.

The Variable Manager opens.
To create new variables in the Variable Manager, click Add.
To create new variables in the Variable Manager, you will need to click Add, then populate the columns of the table with appropriate inputs. The columns in the table represent the name of the variable, the expression that defines it, the current value, and a description of the expression.
For Name, enter ReynoldsNumber.
For Expression enter 1000000.
For Description, enter Target Reynolds number for the simulation.

Repeat this process for the remaining variables shown in the table below:

Name	Expression	Description
ReynoldsNumber	1000000	Target Reynolds number for the simulation
rho	1.225	Density of air
mu	1.781e-5	Molecular viscosity of air
chord	1.0	Airfoil chord
alpha	5.0	Angle of attack (degrees)
windSpeed	:=ReynoldsNumbermu/(rhochord)	Velocity of air (m/s)
xVelocity	:=windSpeedcos(alphadeg)	X component of velocity
yVelocity	:=windSpeedsin(alphadeg)	Y component of velocity
turbIntensityPercent	0.025	Turbulence intensity percentage
viscosityRatio	0.03	Viscosity ratio (turbulent viscosity / molecular viscosity)
globalMeshSize	:=200*chord	Global maximum element size
surfaceMeshSize	:=.02*chord	Maximum surface element size
firstLayerHeight	1.2e-5	Boundary layer first layer height
stretchRatio	1.2	Boundary layer element growth rate
totalLayerHeight	0.004	Total height of boundary layer element stack
sweepAngle	7.0	Sweep angle for boundary layer blends at sharp edges

Once the expressions are entered, the Variable Manager should appear similar to what is shown below:

At this point all variables and expressions are defined and you can close the Variable Manager by selecting Close.

Set General Simulation Parameters

In the next steps you will set parameters that apply globally to the simulation. To simplify this task, you will use the BAS filter in the Data Tree Manager. The BAS filter limits the options in the Data Tree to show only the basic settings.

The general attributes that you will set for this tutorial are for turbulent flow, and steady state time analysis.

Click BAS in the Data Tree Manager to switch to basic view in the Data Tree.

Figure 4.
Double-click the Global Data Tree item to expand it.

Tip: You can also expand a tree item by clicking next to the item name.

Figure 5.
Double-click Problem Description to open the Problem Description detail panel.
Enter NACA0012 Airfoil as the Title for this case.
Enter Fully turbulent as the Sub title for this case.
Change the Analysis type to Steady State.
Change the Turbulence equation to SST
The SST and K-Omega models both require the same set of inputs, so the steps in this tutorial also apply to the K-omega model. If you wish to use the K-Omega model instead of SST, you can select it from this menu.

Figure 6.

Set Solution Strategy Parameters

In the next steps you will set the parameters that control the behavior of AcuSolve as it progresses during the transient solution.

Double-click Auto Solution Strategy to open the Auto Solution Strategy detail panel.
Enter 0.4 for Relaxation factor.
This value is used to improve convergence of the solution. Typically a value between 0.2 and 0.4 provides a good balance between achieving a smooth progression of the solution and the extra compute time needed to reach convergence. Higher relaxation factors cause AcuSolve to take more time steps to reach a steady state solution. A high relaxation factor is sometimes necessary in order to achieve convergence for very complex applications.

Figure 7.

Set Material Model Parameters

In the next steps you will modify the pre-defined material properties of air using an expression that was created in the Variable Manager.

Double-click Material Model in the Data Tree to expand it.

Figure 8.
Double-click Air in the Data Tree to open the Air detail panel.
Click the Density tab and in the Density value field, enter :=rho.
This sets the value of density to be equal to the value entered in the Variable Manager.
Click the Viscosity tab and enter :=mu in the Viscosity field.
This sets the value of viscosity to be equal to the value entered in the Variable Manager.
Save the database to create a backup of your settings. This can be achieved with any of the following methods.
- Click the File menu, then click Save.
- Click on the toolbar.
- Click Ctrl+S.
Note: Changes made in AcuConsole are saved into the database file (.acs) as they are made. A save operation copies the database to a backup file, which can be used to reload the database from that saved state in the event that you do not want to commit future changes.

Import the Geometry and Define the Model

Import Airfoil Geometry

You will import the geometry in the next part of this tutorial. You will need to know the location of NACA0012.x_t in order to complete these steps. This file contains information about the geometry in Parasolid ASCII format.

Click File > Import.
Browse to the directory containing NACA0012.x_t.
Change the file name filter to Parasolid File (*.x_t *.xmt *X_T …).
Select NACA0012.x_t and click Open to open the Import Geometry dialog.

Figure 9.

For this tutorial, the default values for the Import Geometry dialog are used to load the geometry. If you have previously used AcuConsole, be sure that any settings that you might have altered are manually changed to match the default values shown in the figure. With the default settings, volumes from the CAD model are added to a default volume group. Surfaces from the CAD model are added to a default surface group. You will work with groups later in this tutorial to create new groups, set flow parameters, add geometric components, and set meshing parameters.
Click OK to close the dialog.
Rotate and zoom in the visualization to view the entire model.

Figure 10.

The color of objects shown in the modeling window in this tutorial and those displayed on your screen may differ. The default color scheme in AcuConsole is "random," in which colors are randomly assigned to groups as they are created. In addition, this tutorial was developed on Windows. If you are running this tutorial on a different operating system, you may notice a slight difference between the images displayed on your screen and the images shown in the tutorial.

Create a Volume Group and Apply Volume Parameters

Volume groups are containers used for storing information about volumes. This information includes the list of geometric volumes associated with the container, as well as parameters such as material models and mesh sizing information.

When the geometry was imported into AcuConsole, all volumes were placed into the default volume container.

In the next steps you will rename the default group to Fluid, set the material for that group and add the volume from the geometry to that volume group.

Expand the Model Tree.
Expand Volumes.
Toggle the display of the default volume container by clicking and next to the volume name.

Note: You may not see any change when toggling the display if Surfaces are being displayed, as surfaces and volumes may overlap.
Rename the default group.
1. Right-click default.
2. Click Rename.
3. Enter Fluid.
Expand Fluid in the Data Tree.
Double-click Element Set to open the Element Set detail panel.
Ensure that the Material model is set to Air.

Figure 11.

Create Surface Groups and Apply Surface Parameters

Surface groups are containers used for storing information about a surface. This information includes the list of geometric surfaces associated with the container, as well as parameters such as boundary conditions, surface outputs and mesh sizing information.

In the next steps you will define surface groups, assign the appropriate parameters for each group in the problem and add surfaces to the groups.

Set Farfield Boundary Conditions

In the next steps you will define a surface group for the farfield boundary, set the inlet velocity and add the corresponding surface from the geometry to this group.

Add a new surface group by right-clicking Surfaces and click New.
Rename Surface 1 to Far Field.
Expand the Far Field surface in the tree.
Right-click Far Field in the Model Tree.
Select Add to.
Select the edge surface in the visualization window (highlighted in gray below) and then select Done.

Figure 12.
Double-click Simple Boundary Condition under Far Field to open the Simple Boundary Condition detail panel.
Change the Type to Far Field.
When using the Far field boundary condition, you need to enter the vector direction of the flow velocity. Based on this direction, AcuSolve determines whether each element face should be acting as an inlet or an outlet. Using this direction vector, in conjunction with the outward facing normal at each element, it applies the appropriate boundary conditions to the faces of the model. For faces where the flow is entering the model, a nodal boundary condition for velocity and turbulence variables is assigned. For faces where the flow is exiting the model, an element boundary condition for pressure is assigned, that is, an outflow condition.

To facilitate ease in changing the angle of attack for this simulation, you will set the inlet velocity vector at the far field boundary using the variables that were previously defined. Set the values using the following inputs.
For X Velocity, enter :=xVelocity.
For Y Velocity, enter :=yVelocity.

When using the SST or k-omega turbulence models, you need to provide values for the Kinetic energy and Eddy frequency at inflow/farfield boundaries. AcuConsole supports various options of doing this. You can specify the values directly using turbulence input type = Direct, or you can have AcuConsole compute the values based on an estimation of the Turbulence Intensity and Length Scale, or based on an estimation of the Turbulence Intensity and Viscosity Ratio. Besides these options, AcuConsole can also automatically set the values for turbulence inputs to simplify this task for the user. This automatic selection of inputs is based on parameters like flow type, etc. While using the automatic option to compute the values is convenient for generic cases, users are advised to use the other available options if they have suitable input data available.

For this case, you will make use of the auto option to allow AcuConsole to calculate the kinetic energy and eddy frequency values on the farfield boundary.
Set Turbulence input type to Auto.
Set Turbulence intensity type to Auto.

Figure 13.

You can see the value of Percent turbulence intensity is set to 0.5. This value is automatically selected by AcuConsole based on parameters like the turbulence model selected, flow type, etc.

Set Remaining Boundary Conditions

In the next steps you will define surface groups for slip and wall boundaries.

Add a new surface group by right-clicking Surfaces and click New.
Rename Surface 1 to +z slip.
Expand the +z slip surface in the tree.
Right-click +z slip.
Select Add to.
Select the edge surface in the visualization window (highlighted in gray below) and then select Done.

Figure 14.
Click Simple Boundary Condition.
Set Type to Symmetry.
Add another new surface group by right-clicking Surfaces and click New.
Rename Surface 1 to -z slip.
Expand the -z slip surface in the tree.
Right-click -z slip in the Model Tree.
Select Add to.
Select the edge surface in the visualization window (highlighted in gray below) and then select Done.

Figure 15.
Click Simple Boundary Condition.
Set Type to Symmetry.
In the tree, rename the default surface to airfoil.
Expand the airfoil surface in the tree.
Turn off the display of the other surfaces in the Model Tree and then zoom into the remaining surface.
Right-click airfoil in the Model Tree.
Select Add to.
Select the edge surface in the visualization window (shown below) and then select Done.

Figure 16.
Click Simple Boundary Condition.
Set Type to Wall. Leave all the default settings.

Define Nodal Initial Conditions

In the next steps you will define the nodal initial conditions.

In the Data Tree, double-click Nodal Initial Conditions.
Set the X velocity to :=xVelocity.
Set the Y velocity to :=yVelocity.
This will set the X and Y velocities equal to the values specified in the Variable Manager.

For the SST and K-Omega turbulence models, you need to enter the initial values for Kinetic energy and Eddy frequency. If you have a reasonable estimate of these values, you can enter them directly in the fields. One option is to use the same values that are assigned at the inlet boundary. In the absence of good estimates for the initial conditions, it is also possible to let AcuSolve perform an automatic initialization of the turbulence variables. By leaving these values set to zero, AcuSolve will trigger an automatic initialization of these variables.

Set the Kinetic energy and Eddy frequency to 0.0 to trigger the automatic initialization.

Figure 17.

Assign Mesh Controls

Set Global Meshing Parameters

Now that the simulation has been defined, parameters need to be added to define the mesh sizes that will be created by the mesher.

AcuConsole supports three levels of meshing control, global, zone and geometric.

Global mesh controls apply to the whole model without being tied to any geometric component of the model.
Zone mesh controls apply to a defined region of the model, but are not associated with a particular geometric component.
Geometric mesh controls are applied to a specific geometric component. These controls can be applied to volume groups, surface groups or edge groups.

Click MSH in the Data Tree Manager to filter the settings in the Data Tree to show only the controls related to meshing.
Double-click the Global Data Tree item to expand it.
Double-click Global Mesh Attributes to open the Global Mesh Attributes detail panel.
Change the Mesh size type to Absolute.
Set Absolute mesh size to :=globalMeshSize.
Set the Curvature refinement parameters to Off.
Set the Mesh growth rate to 1.2.
When this option is set, the mesher will ensure that the mesh grows smoothly when transitioning between different size. Note that the growth rate of 1.2 does not directly corresponds to a change in length scale of adjacent elements of 1.2, but rather a gradual expansion. The mesh growth rate can be adjusted between a value of 1 and 2. Values closer to 1.0 indicate a smoother transition, whereas a value closer to 2.0 indicates a faster transition. A value of 1.0 disables this setting and reverts to the default meshing behavior. It should be noted that this option can significantly increase the time necessary to produce the mesh as well as the total number of nodes/elements created by the mesher.
Set Maximum sweep angle to :=sweepAngle.
This setting instructs the mesher to use the sweepAngle parameter to define the maximum angle between radial element lines when creating radial edge blends during the boundary layer meshing process.

Figure 18.

Set Mesh Process Parameters

Due to the large range of mesh sizes that will be created on the surface of the airfoil, you will need to instruct the boundary layer mesher how to resolve poor quality elements that result from the requested boundary layer controls. For example, you request the boundary layers to grow to a constant height across the airfoil surface, but the local surface element size varies drastically. So, in some areas this will lead to boundary layer elements that are much taller than they are wide. The mesher views this as a poor quality element and needs to resolve this in some manner. There are two mechanisms by which to resolve this:

Locally reduce the number of layers in the boundary layer stack to maintain high quality boundary layer elements.
Locally reduce the height of the boundary layer stack, but keep the total number of layers constant. Using this approach, the height of each layer is scaled by a constant factor to reduce the total height of the stack and avoid the creation of the poor quality boundary layer elements.

For this simulation, the mesher will locally reduce the height of the boundary layer stack.

Under the Global Tree, double-click on Mesh Process Attributes.
In the detail panel, set the Shrink mixed flag to On.
Set the 2D Boundary layer adjacent height smoothing ratio to 0.25.
This parameter controls how smoothly the local boundary layer heights vary from one element to the next after the layers height are adjusted locally to resolve poor quality elements. A low value of this parameter smooths the variation in height over a large distance, while a value closer to 1.0 enforces a more abrupt change in height. Note that there are separate values of this setting for 2D and 3D boundary layers. For this application, you will be creating a 2D mesh and extruding it in the third direction to create the volume. Therefore, the 2D setting will control the behavior of the mesh in this case.

Figure 19.

Set Surface Mesh Parameters

The surface mesh size on the airfoil is controlled through a combination of the mesh size set on the perimeter edges of the airfoil and the mesh size applied directly to the surface. In this tutorial you will also use the region of influence option of the surface mesh to create a refined mesh at a specified distance from the airfoil surface.

Expand Model > Surfaces > Airfoil.
Activate the Surface Mesh Attributes option.
Select Absolute as the Mesh size type.
Enter :=surfaceMeshSize as the Absolute mesh size.
This assigns a constant mesh size on the surface that corresponds to the value created in the “surfaceMeshSize” variable.
Set the Region of influence parameters to On.
Set the Influence type to Simple.
When using a region of influence type = Simple, the mesh size that was assigned on the surface is maintained for a specified distance from the surface. The distance from the surface at which the surface mesh size is retained is defined by the "Influence distance”. It is also possible to scale the mesh size as a function of distance from the surface. This can be achieved by setting the influence size factor. When this value is set, the local mesh size is linearly interpolated from the size specified on the surface to the scaled value at the furthest extent of the refinement distance. Note that the size used by the “region of influence” meshing is the absolute mesh size that is defined in the surface mesh attributes parameter. It does not take into account any local variation of the mesh size due to curvature refinement, and so on. Therefore, the current settings on the airfoil surface are only used to drive the region of influence sizing. The desired element size on the surface to resolve the shape of the airfoil will be controlled with edge meshing.
Set the Influence size factor to 1.0.
Set the Influence distance to :=chord*0.1.
Set Boundary layer flag to On.
Set the Boundary layer type to Full Control.
For the Resolve field, select Number of Layers.
With this setting, you will specify the first layer height of the boundary layer elements, the total layer height and the growth rate. The total number of layers required to satisfy these settings will be computed by AcuConsole.
For First element height, enter :=firstLayerHeight.
For Total layer height, enter :=totalLayerHeight.
For Growth rate, enter :=stretchRatio
Set the Boundary layer blends flag to On.
Set the Boundary layer element type to Tetrahedron.
For Maximum sweep angle, enter :=sweepAngle.
With these settings, the boundary layer mesher will create radial edge blends with a maximum angle defined by the sweepAngle variable.

Figure 20.

Set Edge Mesh Parameters

To create an optimum mesh on the surface of the airfoil, it is necessary to have high levels of refinement near the leading and trailing edges and a large element size near the mid chord. Since the surface mesh size was set to constant to serve as the size that is propagated into the volume for the region of influence refinement, you will use an edge mesh parameter to control the placement of nodes along the airfoil surface. To accomplish this, you will first need to create an edge group that contains the perimeter edges of the airfoil.

Add a new edge by right-clicking Edges and click New.
Rename Edge 1 to Perimeter Edges.
Select the two perimeter edges of the airfoil to add them to this group.
1. Right-click Perimeter Edges and click Add to.
2. Select the two perimeter edges of the airfoil shown below.
  
  Figure 21.
3. Select Done.
Activate Edge Mesh Attributes and then double-click on it.
Set the Mesh size type to Absolute Expression.

Figure 22.
Click on the Absolute mesh size expression button to open a text editor where you can write an expression for the mesh size.
This expression will be evaluated by the mesher to determine the local mesh size that should be used at each location on edges in the edge set.
Enter the following expression:
```
sizeMin  = 0.0025
sizeMax = 0.1 

xMin =(0.0)
xMax =(1.0) 

xCenter =((xMin+xMax)/2.0)
dx = ((xMax-xMin)/2.0) 

fac = ((dx - abs(x-xCenter) )/dx ) 

power = (ln(sizeMax/sizeMin))
expVal = sizeMin*exp(power*fac) 

linVal = sizeMin+(sizeMax-sizeMin)*fac 

value = expVal
```
This expression takes the min and max surface mesh size (sizeMin and sizeMax) along with the location of the leading and trailing edge (xMin and xMax) and computes a logarithmic expansion of the surface mesh size as a function of distance from the leading and trailing edges. The mesh size at the leading and trailing edge corresponds to sizeMin and the size at the mid chord location corresponds to sizeMax.

Figure 23.
Click Ok to close this text editor area and accept the expression.

Set Mesh Extrusion Parameters

The final step in the setup of the meshing for the airfoil is the creation of a mesh extrusion attribute. This extrusion will be defined such that a single element is created across the span of the airfoil.

Create a new Mesh Extrusion.
1. Right-click Mesh Extrusions and select New.
2. Right-click Mesh Extrusion 1 and select Rename.
3. Rename it to Z extrusion.
Double-click Z extrusion to open the settings dialog.
Two types of extrusion are supported with the mesh extrusion attributes. The first type is surface. When selecting this type, the input to the mesher is a set of two surfaces for which the mesh will be extruded between. The resulting mesh is an extruded volume mesh. The second type of extrusion that is supported is an edge extrusion. Using this type of extrusion, two edges are chosen and the resulting mesh is an extruded surface mesh that lies between the two edges. For this application, you will set Geometry type to surface to generate an extruded volume mesh.
Ensure the Geometry type is set to surface.
For Side 1, from the drop down, select +z slip.
For Side 2, from the drop down, select –z slip.
Set the Extrusion type to Number of layers.
Enter 1 for the total number of layers.
Under Extrusion options, select Mixed elements to create a single layer of extruded prism elements across the span of the airfoil.
Click OK to accept these settings.

Figure 24.

Generate the Mesh

In the next steps you will generate the mesh that will be used when computing a solution for the problem.

Click on the toolbar to open the Launch AcuMeshSim dialog.
Leave the default settings and select OK.

During meshing an AcuTail window opens. Meshing progress is reported in this window. A summary of the meshing process indicates that the mesh has been generated.
Inspect the mesh around the surface of the airfoil.
Note the refinement at the leading and trailing edge of the airfoil that resulted from the expression that was used for edge mesh attributes. Also note the refinement of the mesh around the airfoil surface. This was caused by the region of influence meshing.
Zoom in on the trailing edge of the airfoil to see the impact of setting the boundary layer blends flag to on. The radial edge blend at the trailing edge of the airfoil is clearly evident.

Figure 25.

Compute the Solution and Review the Results

Run AcuSolve and Examine the .log File

In the next steps, you will launch AcuSolve to compute the solution for this case.

Click on the toolbar to open the Launch AcuSolve dialog.
Enter 4 for Number of processors, if your system has 4 or more processors.
The use of multiple processors can reduce solution time.
Ensure the Restart radio button is set to Off.
Accept all other default settings.
Based on these settings, AcuConsole will generate the AcuSolve input files, then launch the solver. AcuSolve will run on four processors to calculate the transient solution for this problem.
Select Ok to start the solution process.

While computing the solution, an AcuTail window opens. Solution progress is reported in this window. A summary of the solution process indicates that the run has been completed.

The information provided in the summary is based on the number of processors used by AcuSolve. If you use a different number of processors than indicated in this tutorial, the summary for your run may be slightly different than the summary shown.
Once the analysis is complete, scroll up to the top of the file and look for the message about initializing turbulence field values.
This is because the nodal initial conditions were set to 0. Notice that it reports the min, max and average values of the initialized variables.

Figure 26.
Review a single time step.
One thing to notice is that eddy frequency and kinetic energy are solved for three times in each time step. This is the most efficient way to get a converged solution when using the SST and k-omega turbulence models.

Figure 27.
Close the AcuTail window and save the database to create a backup of your settings.

Monitor the Solution with AcuProbe

While AcuSolve is running, you can monitor the kinetic energy using AcuProbe.

Open AcuProbe by clicking on the toolbar.
Clear the plot by right-clicking on Residual Ratio and selecting Plot None.
Expand Residual Ratio > All.
Right-click kinetic_energy and select Plot.

Figure 28.
Right-click kinetic_energy and select Don’t Plot to clear the plot.
Right-click on Final and select Plot All.

Figure 29.
Close the AcuProbe dialog.

Start AcuFieldView

Click on the AcuConsole toolbar to open the Launch AcuFieldView dialog.
Click OK to start AcuConsole.
When you start AcuFieldView from AcuConsole, the results from the last time step of the solution that were written to the disk will be loaded for post-processing.

Display Square Root of the Eddy Period

In the next steps you will create a boundary surface to display contours of a new variable, called the square root of the eddy period. When solving for the SST and k-omega turbulence models, AcuSolve introduces three new variables to the output; kinetic_energy (k), eddy_frequency (ω) and sqrt_eddy_per ( $\frac{1}{\sqrt{ω}}$ ). The sqrt_eddy_per variable is useful for visualizing the turbulent time scale since the eddy_frequency variable has such a large range of values, it is often times easier to visualize sqrt_eddy_per.

These steps are provided with the assumption that you are able to manipulate the view in AcuFieldView. If you are unfamiliar with basic AcuFieldView operations, refer to Manipulate the Model View in AcuFieldView.

Click on the side toolbar to open the Boundary Surface dialog.

Note: The dialog may already be open. This step will put the focus on the dialog.
Under Scalar Function, click Select.
Select sqrt_eddy_period and then select Calculate.

Note: You may have to scroll down to find sqrt_eddy_period. This is a new variable and it represents one over the square root of omega. It has been added as it is a more well bounded variable to plot, as compared to the eddy frequency.

Figure 30.
Zoom into the airfoil to view the sqrt_eddy_period around the airfoil.

Figure 31.

Post-Process to Calculate Flow Coefficients

AcuSolve is shipped with a number of utility scripts to facilitate the pre and post-processing of a problem solved using the solver. You will be introduced to two of these scripts, AcuLiftDrag and AcuGetCpCf in this section, and their usage. These two scripts are focused on aerodynamic simulations as the ones solved in this tutorial.

Run AcuLiftDrag

AcuLiftDrag is a utility script used to calculate the lift and drag coefficients for an airfoil. The following options are required as input to run this script.

Option Name	Description
-pb	problem name
-dir	working directory. The default working directory is ACUSIM.DIR, which contains all the solution files for the problem.
-run	run number (0, use last)
-osis	comma separated list of surface outputs to use for force computation (all for all)
-angle_of_attack / aoa	angle of attack of the wing (in degrees)
-reference_velocity / ref_vel	reference velocity
-wing_chord / chord	chord of the wing
-wing_span / span	span of the wing
-density / rho	density of the air
-drag_direction / drag_dir	direction of drag at zero angle of attack: x, y, z. The default drag direction is x.
-lift_direction / lift_dir	direction of lift at angle of attack: x, y, z. The default drag direction is y.
-x_axis_vars / x_vars	x axis variable for the exported data: step, time, both. The default is step.

In the Analyze the Problem section, it was described that the simulation is performed as 2D by including only a single layer of extruded elements in the airfoil span direction. When solving a problem in such a way, the span of the airfoil should be set equal to the thickness of the domain in the extrusion direction. When solving a 3D problem, the actual span of the airfoil should be used.

To execute the AcuLiftDrag script for this position, follow the steps below:

Start AcuSolve Command Prompt from the Start menu by clicking Start > All Programs > Altair HyperWorks <version> > AcuSolve > AcuSolve Cmd Prompt.
Change the directory to the present problem directory using the 'cd' command.
Enter the following command at the prompt:
```
acuLiftDrag -osis airfoil -aoa 5 -ref_vel 14.54 -chord 1 -rho 1.225 
-span 50  
```
The output of the command should look like the image below:

Figure 32.

The value C_l corresponds to the lift coefficient, and C_d corresponds to the drag coefficient. The final keyword refers to the respective coefficient values at the last time step of the simulation. The rest of the values provide the basic statistics for these coefficients over all the time steps of the simulation. These statistics are more meaningful if the simulation is transient.

The script also creates the file Turbulent_Airfoil_SST.liftDrag.dat in the problem directory. The file contains the lift and drag data for all the available time steps in a determined tabular arrangement. The first column is the time step, the second column is the lift coefficient, and the third column is the drag coefficient.

Run AcuGetCpCf

AcuGetCpCf is another utility script used to calculate the pressure coefficient (Cp) for the airfoil. The following options are required as input to run this script.

Option Name	Description
-pb	problem name
-dir	working directory. The default working directory is ACUSIM.DIR, which contains all the solution files for the problem.
-run	run number (0, use last)
-ts	time step to extract (0=use last)
-osis	comma separated list of surface outputs to use for force computation (all for all)
-type	type of data to generate: cp, cf
-point_type	method used to generate the points for the curve: file, auto
-points_file / pts	comma separated list of files to read points from (used with type=file)
-radial_locations / rad_locs	list of radial locations
-z_direction / z_dir	direction of iso-cut: x, y, z. Default is z.
-reference_pressure / ref_pres	reference pressure
-density / rho	density of the air
-reference_velocity / ref_vel	reference velocity
-wing_chord / chord	chord of the wing
-normalize_chord / nc	normalize the local chord to unity. Default is True.
-chord_scale_fac / csf	chord scale factor
-cp_scale_fac / cpsf	c_p / c_f scale factor
-pressure_type / ptype	pressure field to use: standard, time_ave, running_ave. Default is standard.

To execute the AcuGetCpCf script for this problem, follow the steps below:

Start AcuSolve Command Prompt from the Start menu by clicking Start > All Programs > Altair HyperWorks <version> > AcuSolve > AcuSolve Cmd Prompt.
Change the directory to the present problem directory using the 'cd' command.
Enter the following command at the prompt:
```
acuGetCpCf -osis airfoil -type cp -ref_vel 14.54 -rho 
1.225 -no_nc
```
The output of the command should look like the image below:

Figure 33.

The script prints the minimum and maximum values for the pressure coefficient. It also creates a file, cp.1.dat, in the problem directory. The file contains the pressure coefficient data along the chord of the airfoil. The first column is the x-coordinate along the chord, and the second column is the pressure coefficient. You can use an external plotting utility to the plot the data. The resulting plot is shown below.

Figure 34.

Change the Angle of Attack and Compute the Solution

Because this database was set up using variables and expressions, it is easy to re-run the simulation again using a different angle of attack. To accomplish this, open the Variable Manager, and set “alpha” to 0.0. Because the xVelocity and yVelocity variables that were defined for the initial and boundary conditions are a function of this parameter, the database will automatically be updated to reflect the new settings. You can simply write the input again and run the solver to obtain a different angle of attack solution.