# ACU-T: 2000 Turbulent Flow in a Mixing Elbow

This tutorial provides the instructions for setting up, solving, and viewing results of a simulation of 3D turbulent flow in a mixing elbow. It is designed to introduce you to the AcuSolve tool set with a simple problem.

## Prerequisites

In order to run this simulation, you will need access to a licensed version of AcuSolve. As this is the first tutorial in the introductory tutorial sequence, no prior experience with AcuConsole, AcuSolve, or AcuFieldView is expected.

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 mixingElbow.x_t from AcuConsole_tutorial_inputs.zip.

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.

## 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 Figure 1. This is a typical industrial example for mixing in a pipe by injecting high-velocity fluid from a small inlet into relatively low-velocity fluid in the main pipe. It consists of a 90° mixing elbow with water entering through two inlets with different velocities. The geometry is symmetric about the XY midplane of the pipe, as shown in the figure. This symmetry allows the flow to be modeled with the use of a symmetry plane. The use of a symmetry plane leads to reduced computation time while still providing an accurate solution.

Details of the problem characteristics are shown in the following images extracted from a sample worksheet that was created prior to setting up the case for AcuSolve.

The diameter of the large inlet is 0.1 m, and the inlet velocity (v) is 0.4 m/s. The diameter of the small inlet is 0.025 m, and the inlet velocity is 1.2 m/s.

The fluid in this problem is water, with the following properties that do not change with temperature; a density (ρ) of 1000 kg/m3, a molecular viscosity (μ) of 1 X 10-3 kg/m-sec, a conductivity (k) of 0.598 W/m-K, and a specific heat (cp) of 4183 J/kg-K, as shown in the worksheet.

Based on mass conservation, the combined flow rate (Q) yields a velocity of 0.475 m/s downstream of the small inlet. This value is useful in determining the Reynolds number, which in turn can be used to determine if the flow should be modeled as turbulent, or if it should be modeled as laminar.

In order to determine whether the modeled flow would be turbulent or whether it would be laminar, the Reynolds number (Re) should be calculated. The Reynolds number is given by: $\mathrm{Re}=\frac{\rho VD}{\mu }$ where ρ is the fluid density, V is the fluid velocity, D is the diameter of the flow region, and μ is the molecular viscosity of the fluid. When the Reynolds number is above 4,000, it is generally accepted that flow should be modeled as turbulent.

The Reynolds numbers of 40,000 at the large inlet, 30,000 at the small inlet, and 47,500 for the combined flow indicate that the flow is turbulent throughout the flow domain.

The simulation will be set up to model steady state, turbulent flow.

In addition to setting appropriate conditions to capture the physics of the simulation, it is important to generate a mesh that is sufficiently refined to provide good results. In this tutorial the global mesh size is set to provide at least 30 mesh elements around the circumference of the large inlet. For this problem, the global mesh size is 0.0106 m. This mesh size was chosen to provide a quick turnaround time for the model. For real-world simulations, you would modify your mesh settings after an initial solution until a mesh-independent solution is reached (that is, a solution that does not change with further mesh refinement).

AcuSolve allows for mesh refinements in a user-defined region that is independent of geometric components of the problem such as volumes, model surfaces, or edges. It is useful to refine the mesh in areas where gradients in pressure, velocity, eddy viscosity, and the like are steep.

Once a solution is calculated, results of interest are the steady state velocity contours on the symmetry plane, velocity vectors on the symmetry plane, and pressure contours on the symmetry plane.

## Define the Simulation Parameters

### Start AcuConsole

AcuConsole is the workspace that is used for building simulations and running them with AcuSolve.

Start AcuConsole from the Windows Start menu by clicking Start > Altair <version> > AcuConsole.

Start AcuConsole on Linux by entering AcuConsole in a terminal window that has the AcuSolve environment configured. Please refer to the HyperWorks Installation Guide for instructions on configuring AcuSolve on Linux.

The main AcuConsole window is comprised of eight major components.

• Toolbar
• Data Tree
• Data Tree Manager
• View Manager toolbar
• modeling window
• Detail panels
• Information window

When AcuConsole is first opened, the Data Tree, detail panel, modeling window and Information window are empty. The following figure from a partially defined case is used to illustrate the parts of the workspace.

The items in the Data Tree are separated into two main areas, Global and Model. The Global tree item contains geometry independent settings that apply to the AcuSolve simulation, such as the physics to be modeled, the solution strategy, material properties and geometry independent mesh controls. The Model branch in the Data Tree contains settings that apply to specific portions of the geometry of the model, such as boundary conditions, material used for a volume region and meshing attributes that apply to a specific component of the model geometry.

In this tutorial, you will begin by creating a database, 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 visualize the results using AcuFieldView.

### Create the Simulation Database

In the next steps you will create a database for the storage of AcuConsole settings and set the location for saving mesh and solution information for AcuSolve.
1. Click the File menu, then click New to open the New data base dialog.
Tip: You can also open the New data base dialog by clicking on the toolbar.
2. 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.
3. Create a new folder named Mixing_Elbow and open this folder.
4. Enter Mixing_Elbow as the File name for the database.
Note: In order for other applications to be able to read the files written by AcuConsole, the database path and name should not include spaces.
5. Click Save to create the database.

### 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 physical models that you define for this tutorial correspond to steady state, turbulent flow. You will also provide some general information about the AcuSolve case, such as a title and subtitle.

1. Click BAS in the Data Tree Manager to switch to basic view in the Data Tree.
2. Expand the Global Data Tree item.
3. Double-click Problem Description to open the Problem Description detail panel.
Tip: You can also open a panel by right clicking a tree item and clicking Open on the context menu.
4. Enter Introductory Tutorial as the Title.
5. Enter Mixing Elbow – Turbulent as the Sub title.
6. Accept the default Analysis type.
Note: By default, AcuSolve cases are run as steady state simulations.
7. Set the Turbulence equation to Spalart Allmaras.
1. Click the Turbulence equation drop-down.
2. Click Spalart Allmaras from the list.
The robustness and accuracy of the Spalart Allmaras turbulence model makes it an excellent choice for simulation of steady state flows.
Note: The detail panel can be resized by dragging the right frame of the panel.

### Set Solution Strategy Parameters

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

1. Double-click Auto Solution Strategy to open the Auto Solution Strategy detail panel.
2. Enter 0.4 for the Relaxation factor.
The relaxation factor 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.

### Set Material Model Parameters

AcuConsole has three pre-defined materials, Air, Aluminum, and Water.

In the next steps you will verify that the pre-defined material properties of water match the desired properties for this problem.

1. Double-click Material Model in the Data Tree to expand it.
2. Double-click Water in the Data Tree to open the Water detail panel.

The Material type for water is Fluid.

3. Click the Density tab. Verify that the density of water is 1000.0 kg/m3.
4. Click the Specific Heat tab. Verify that the specific heat of water is 4183.0 J/kg-K.
5. Click the Viscosity tab. Verify that the viscosity of water is 0.001 kg/m-sec.
6. Click the Conductivity tab. Verify that the conductivity of water is 0.598 W/m-K.
7. 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 the Mixing Elbow Geometry

You will import the geometry in the next part of this tutorial. You will need to know the location of mixingElbow.x_t in order to complete these steps. This file contains information about the geometry in Parasolid ASCII format.
1. Click File > Import.
2. Browse to the directory containing mixingElbow.x_t.
3. Change the file name filter to Parasolid File (*.x_t *.xmt *X_T...).
1. Click the drop-down button to the right of the File name field.
2. Click Parasolid File (*.x_t *.xmt *X_T...) from the drop-down list.
4. Select mixingElbow.x_t and click Open to open the Import Geometry dialog.

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.

5. Click Ok to complete the geometry import.

At this point, your modeling window should look similar to what is shown in Figure 17.

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.

### Manipulate the View in the Modeling Window

In the next steps you will do some basic manipulations of the mixing elbow view to help you become familiar with the mouse actions in the modeling window. The mouse buttons that are used for rotating, panning, and zooming are shown in the following table:

Action Mouse Button
rotate left
move (pan) middle
zoom right
1. Rotate the view.
1. Left-click in the modeling window.
2. Drag the cursor to the right and observe the display.
The model should rotate to the right.
3. Drag the cursor to the left to rotate the model to the left.
4. Drag the cursor up or down to rotate the model up or down.
Note: You will only see half of the pipe when you manipulate the view. As this geometry is symmetric around the midplane only half of the geometry needs to be modeled, which reduces computation time.
5. Restore the initial view by clicking on the View Manager toolbar.
2. Pan the view.
1. Middle-click in the modeling window.
2. Drag the cursor to the right to move the model to the right.
3. Drag the cursor to the left to move the model to the left.
4. Restore the initial view by clicking on the View Manager toolbar.
3. Zoom in on and out from the view.
1. Right-click in the modeling window.
2. Drag the cursor up to zoom out from the view.
3. Drag the cursor down to zoom in on the view
4. Restore the initial view by clicking on the View Manager toolbar.
Note: You can also fit the model to the window by clicking on the View Manager toolbar.

### Apply Volume Parameters

Volume groups are containers used for storing information about a volume region. This information includes solution and meshing parameters applied to the volume and the geometric regions that these settings are applied to.

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 volume group, toggle the display, and assign the material for the volume as water.

1. Expand the Model tree item by clicking .
2. Expand the Volumes tree item.
3. 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.
4. Rename the default volume group.
1. Right-click default under Volumes and click Rename on the context menu.
2. Type Mixing Elbow and press Enter.
Note: When an item in the Data Tree is renamed, the change is not saved until you press Enter on your keyboard. If you move the input focus away from the item without entering it, your changes will be lost.
5. Set the material model used for the fluid in the simulation.
1. Expand the Mixing Elbow tree item.
Note: By default, when an item in the Data Tree is specified, the corresponding geometric elements are highlighted in the modeling window.
2. Double-click Element Set to open the Element Set detail panel.
3. Click the Material model drop down arrow.
4. Click Water.
For the next set of steps, it is useful to turn off the display of Elbow Volume by clicking so that it is in the off () state.

### Create Surface Groups and Apply Surface Boundary Conditions

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 attributes such as boundary conditions, surface outputs, and mesh sizing information.

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

#### Set Inflow Boundary Conditions for the Large Inlet

In the next steps you will define a surface group for the large inlet, set the inlet velocity, and add the main inlet from the geometry to the surface group.

1. Create a new surface group.
1. Right-click Surfaces in the Data Tree.
2. Click New.
2. Rename the surface to Large Inlet .
1. Right-click Surface 1 under Surfaces and click Rename from the context menu.
2. Enter Large Inlet and press Enter.
3. Expand the Large Inlet surface in the tree.
4. Double-click Simple Boundary Condition under Large Inlet to open the Simple Boundary Condition detail panel.
5. Change the Type to Inflow.
6. Change the Inflow type to Average Velocity.
This type of boundary condition is used by AcuSolve to approximate a fully developed flow with a given average velocity.
7. Set the Average velocity to 0.4 m/sec.
8. Add a geometry surface to the Large Inlet group.
1. In the Data Tree, right-click Large Inlet and click Add to.
The Add to dialog is used in conjunction with the modeling window to select geometry items to associate with model groups such as volumes, surfaces, or edges. When using the Add to capability, zoom, pan, and rotate actions are performed by holding down the Ctrl key and using the mouse buttons.
2. If needed, expose the modeling window, by dragging the Add to dialog to the side.
3. Rotate the model to expose the large inlet by Ctrl+left-clicking near the left side of the geometry and dragging the cursor to the right.
4. Click on the large inlet face.

At this point, the inlet should be highlighted.

5. Click Done to add this geometry surface to the Large Inlet surface group.
Note: You can also use the middle mouse button to complete the addition of geometry components to a group.

#### Set Inflow Boundary Conditions for the Small Inlet

In the next steps you will define a surface group for the small inlet, assign the appropriate attributes, and add the small inlet from the geometry to the surface group.

1. Create a new surface group.
2. Rename the surface to Small Inlet.
3. Expand the Small Inlet surface in the tree.
4. Double-click Simple Boundary Condition under Small Inlet to open the Simple Boundary Condition detail panel.
5. Change the Type to Inflow.
6. Change the Inflow type to Average Velocity.
7. Set the Average velocity to 1.2 m/sec.
8. Add a geometry surface to the Small Inlet group.
1. In the Data Tree, right-click Small Inlet and click Add to.
2. Rotate the model to expose the small inlet by Ctrl+left-clicking near the bottom of the geometry and moving the cursor toward the top of the window.
Note: If you need to zoom in or out, Ctrl+right-click and drag the cursor down or up. You can also restore the initial view by clicking .
3. Left-click on the small inlet face.

At this point, the small inlet should be highlighted.

4. Click Done to add this geometry surface to the Small Inlet group.

#### Set Wall Boundary Conditions for the Large Pipe

In the next steps you will define a surface group for the pipe walls, assign the appropriate attributes, and add the elbow pipe walls from the geometry to the surface group.

1. Create a new surface group.
2. Rename the surface to Large Pipe.
3. Expand the Large Pipe surface in the tree.
4. Double-click Simple Boundary Condition under Large Pipe to open the Simple Boundary Condition detail panel.
The default wall settings will be used for the pipe wall.
5. Add geometry surfaces to this group.
1. Right-click Large Pipe and click Add to.
2. Click on the pipe near the large inlet, the pipe near the elbow, and the pipe near the outlet to select the three surfaces that make up the main pipe wall.

At this point, the pipe walls should be highlighted.

3. Click Done to add these geometric surfaces to the Large Pipe group.

#### Set Wall Boundary Conditions for the Small Pipe

In the next steps you will define a surface group for the side pipe wall, assign the appropriate attributes, and add the side pipe wall from the geometry to the surface group.

1. Create a new surface group.
2. Rename the surface to Small Pipe.
3. Expand the Small Pipe surface in the tree.
4. Double-click Simple Boundary Condition under Small Pipe to open the Simple Boundary Condition detail panel.
As with the large pipe, the default boundary condition Type is Wall. The default is appropriate for this group and no other changes are needed.
5. Add geometry surfaces to this group.
1. Right-click Small Pipe and click Add to.
2. Click on the pipe near the side inlet.

At this point, the side pipe wall should be highlighted.

3. Click Done to associate this geometry surface with the Small Pipe surface container.

#### Set Outflow Boundary Conditions for the Outlet

In the next steps you will define a surface group for the outlet, assign the appropriate attributes and add the outlet from the geometry to the surface group.

1. Create a new surface group.
2. Rename the surface to Outlet.
3. Expand the Outlet surface in the tree.
4. Double-click Simple Boundary Condition under Outlet to open the Simple Boundary Condition detail panel.
5. Change the Type to Outflow.
6. Add a geometry surface to the Outlet surface container.
1. In the Data Tree, right-click Outlet and click Add to.
2. Rotate the model to expose the outlet by Ctrl+left-clicking near the top of the geometry and moving the cursor toward the bottom of the window.
3. Click on the outlet face.

At this point, the outlet should be highlighted.

4. Click Done to associate this geometry surface with the surface settings of the Outlet group.

#### Set Symmetry Boundary Conditions for the Symmetry Plane

This geometry is symmetric about the XY midplane, and can therefore be modeled with half of the geometry. In order to take advantage of this, the midplane needs to be identified as a symmetry plane. The symmetry boundary condition enforces constraints such that the flow field from one side of the plane is a mirror image of that on the other side.

In the next steps you will rename the default surface and apply appropriate settings.

When the geometry was loaded into AcuConsole, all geometry surfaces were placed in the default surface group. In the previous steps, you selected geometry surfaces to be placed in the groups that you created. At this point, all that is left in the default surface group is the symmetry plane. Rather than create a new container, add the symmetry surface in the geometry to it, and then delete the default surface container, you will rename the existing container.

1. Rename the default surface to Symmetry
2. Expand the Symmetry surface in the tree.
3. Double-click Simple Boundary Condition under Symmetry to open the Simple Boundary Condition detail panel.
4. Change the Type to Symmetry.

## 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.

In the next steps you will set global meshing parameters. In subsequent steps you will create zone and surface meshing parameters.

1. Click MSH in the Data Tree Manager to filter the settings in the Data Tree to show only the controls related to meshing.
2. Expand the Global Data Tree item.
3. Double-click Global Mesh Attributes to open the Global Mesh Attributes detail panel.
4. Change the Mesh size type to Absolute.
5. Enter 0.0106 m for the Absolute mesh size.
This absolute mesh size is chosen to ensure that there are at least 30 mesh elements around the circumference of the main pipe.
6. Turn off the Curvature refinement parameters option.

### Set Zone Meshing Parameters

In addition to setting meshing characteristics for the whole problem, you can assign meshing parameters to a zone within the problem where you want to be able to resolve flow with a mesh that is more refined than the global mesh. A zone mesh refinement can be created using basic shapes to control the mesh size within that shape. These types of mesh refinement are used when refinement is needed in an area that does not correspond to a geometric item.

In the next steps you will define mesh controls for a region around the small pipe and extending into the main pipe by using a zone mesh control. The region of interest for this refinement is a cylinder that encloses the small pipe and extends into the main pipe.

1. Turn off the display of volumes.
2. Turn off the display of all surfaces except Symmetry.
3. Restore the initial view by clicking on the View Manager toolbar.
4. Right-click Zone Mesh Attributes under the Global branch in the Data Tree and click New.
5. Rename Zone Mesh Attributes 1 to Small pipe refinement.
6. Double-click Small pipe refinement to open the Zone Mesh Attributes detail panel.
7. Change the Mesh zone type to Cylinder.
8. Set the location of the mesh refinement by defining the center points of the end faces of the cylinder.
1. Click Open Array to open the Array Editor dialog.
2. Enter 0.143 for X-coordinate 1 and 2.
3. Enter -0.232 for Y-coordinate 1.
4. Enter -0.025 for Y-coordinate 2.
5. Enter 0.0 for Z-coordinate 2.
6. Click OK.
9. Enter 0.0254 m for the Radius.
This radius is used to define a cylinder that is larger than the small inlet.
10. Enter 0.0053 m for the Mesh size.
This will result in a zone where the mesh size is half of the mesh size in the rest of the pipe.
Note: When setting mesh size for refinement zones, the best practice is to choose a value that is the global mesh size divided by a power of two, that is, 1/2, 1/4, 1/8, and the like.

### Set Meshing Parameters for Surface Groups

In the following steps you will set meshing parameters that will allow for localized control of the mesh size on surface groups that you created earlier in this tutorial. Specifically, you will set local meshing parameters that control the growth of boundary layer elements normal to the surfaces of the main pipe and of the side pipe.

#### Set Meshing Parameters for the Large Pipe

In the next steps you will set parameters that control the mesh size normal to the large pipe wall (boundary layer mesh controls).
1. Expand the Model > Surfaces > Large Pipe tree item.
2. Click the check box next to Surface Mesh Attributes to enable the settings and open the Surface Mesh Attributes detail panel.
3. Change the Mesh size type to None.
This option indicates that the mesher will use the global meshing parameters when creating the mesh on the surface of the pipe walls.
4. Turn on the Boundary layer flag option.

This option allows you to define how the meshing should be handled in the direction normal to the walls.

5. Set the Resolve option to Total Layer Height.

Mesh elements for a boundary layer are grown in the normal direction from a surface to allow effective resolution of the steep gradients near no-slip walls. The layers can be specified using a number of different options. In this tutorial you will specify the height of the first layer, a stretch ratio for successive layers (growth rate), and the total number of layers to generate. AcuConsole will resolve the total layer height from the attributes that you provide. That is, total layer height will be computed based on the height of the first element, the growth rate, and the number of layers that you provide in the next few steps.

6. Keep the default value, 0.001 m, for First element height.
7. Enter 1.3 for the Growth rate.
8. Enter 4 for the Number of layers.

#### Set Meshing Parameters for the Small Pipe

In the following steps you will set meshing parameters that will allow for localized control of the mesh size near the walls of the small pipe.

1. Expand the Small Pipe tree item.
Note: You will set the same attributes as for the large pipe.
2. Click the check box next to Surface Mesh Attributes to enable the settings and open the Surface Mesh Attributes detail panel.
3. Change the Mesh size type to None.
4. Turn on the Boundary layer flag option.
5. Set the Resolve option to Total Layer Height.
6. Enter 1.3 for the Growth rate.
7. Enter 4 for the Number of layers.
8. Save the database to create a backup of your settings.

### Generate the Mesh

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

1. Click on the toolbar to open the Launch AcuMeshSim dialog.
2. Click Ok to begin meshing.

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.

3. Display the mesh on surfaces.
1. Right-click Zone Mesh Attributes under Global in the Data Tree and click Display off.
2. Right-click Volumes in the Data Tree and click Display off.
3. Right-click Surfaces in the Data Tree and click Display on.
4. Right-click Surfaces in the Data Tree, select Display type and click solid & wire.
4. Rotate, move, or zoom the view to examine the mesh.

Details of the mesh on the side pipe are shown in Figure 41. The view was obtained by turning off the display of all surfaces except Symmetry, then zooming in on the regions where the side pipe joins the main pipe.

Note that the mesh size in the main pipe decreases from left to right in the transition from a region where global settings determine the size to the zone around the small pipe where the settings are for a finer mesh.

5. Save the database to create a backup of your settings.

## Compute the Solution and Review the Results

### Run AcuSolve

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

1. Click on the toolbar to open the Launch AcuSolve dialog.

For this case, the default values will be used.

Based on these settings, AcuConsole will generate the AcuSolve input files, then launch the solver. AcuSolve will run on four processors to calculate the steady state solution for this problem.

2. Click 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.

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

### View Results with AcuFieldView

Now that a solution has been calculated, you are ready to view the flow field using AcuFieldView. AcuFieldView is a third-party post-processing tool that is tightly integrated to AcuSolve. AcuFieldView can be started directly from AcuConsole, or it can be started from the Start menu, or from a command line. In this tutorial you will start AcuFieldView from AcuConsole after the solution is calculated by AcuSolve.

In the next steps you will start AcuFieldView, manipulate the view of the model, display velocity contours and vectors on the symmetry plane, and display pressure contours on the symmetry plane.

#### Start AcuFieldView

1. Click on the AcuConsole toolbar to open the Launch AcuFieldView dialog.
2. Click Ok to start AcuFieldView.
When AcuFieldView is started from AcuConsole, the main window and the Boundary Surface dialog are displayed. The main window is comprised of six components as shown in Figure 44.
• Main toolbar
• Transform Controls toolbar
• Viewer toolbar
• modeling window
• Side toolbar

When you start AcuFieldView from AcuConsole, the results from the last time step of the solution that were written to disk will be loaded for post-processing.

#### Manipulate the Model View in AcuFieldView

When AcuFieldView is started directly from AcuConsole, the model will be displayed in an isometric view with a Boundary Surface dialog open. The initial view is shown in perspective, with an outline around the model. You will manipulate the view in the next steps, and in later steps will view different flow characteristics using the Boundary Surface dialog.

1. Change the background color to white.
1. Click on the View menu.
2. Click Background / Enviroment.
3. Click the white swatch, then click Close.
2. Turn off the display of the outline around the model by clicking on the toolbar.
3. Change the view from perspective to orthographic.
1. Click on the View menu.
2. Click Perspective to disable this option.
4. Orient the model to view it from the positive Z direction (+Z).
1. Click on the toolbar to open the Defined Views dialog.
2. Click .

You will see the view change as soon as you click a button in the Defined Views dialog.

3. (Optional) Close the dialog.

You can move, zoom, and rotate the view in AcuFieldView in a similar fashion as in AcuConsole. AcuFieldView uses a different mapping for mouse-button actions.

Action Mouse Button
move (pan) left
rotate middle
zoom right

#### Display Contours of Velocity Magnitude on the Symmetry Plane

In the next steps you will create a boundary surface to display contours of velocity magnitude on the symmetry plane.

1. Click to open the Boundary Surface dialog.
Note: The dialog may already be open. This step will put the focus on the dialog.
2. Disable the Show Mesh option.
3. Set velocity_magnitude as the scalar field to display.
1. Click Select in the Scalar Function control group to open the Function Selection dialog.
2. Select velocity_magnitude from the list.
Note: You may need to scroll down in the list to find velocity_magnitude.
3. Click Calculate.
4. Set the symmetry plane as the location for display of the contours.
1. Click OSF: Symmetry in the list of BOUNDARY TYPES.
2. Click OK.
The contours reflect the velocity profiles at the inlets, and show that at the elbow there is a momentum transfer between the high-velocity side inlet flow and the flow in the main pipe, represented by the change in the velocity magnitude.
5. Add a legend to the view.
1. In the Boundary Surface dialog, click the Legend tab .
2. Enable the Show Legend option.
3. Enable the Frame option.
4. In the Color group, next to Geometric, click the white color swatch, and then select the black color swatch to set the color for the legend values to black.
5. Click the white color swatch next to the Title field and set the color for the title to black.
6. Move the legend by Shift+left-clicking and dragging the legend to the left.

#### Add Velocity Vectors to the View

In the next steps you will create a new boundary surface and display velocity vectors on that surface.

1. In the Boundary Surface dialog, in the Surface tab, click Create.

The new Surface ID will be 2.

2. Click the Geometric radio button in the COLORING group.
This sets the color of the vectors to a constant color. By default, the color is black.
3. Set vector options.
1. Click the Vectors radio button.
2. Click Options next to Vectors to open the Vector Options dialog.
3. Enable Head Scaling and set it to 0.5.
This option determines the size of the arrow head compared to the vector.
4. Set the Length Scale to 2.
The length scale determines the length of the vectors.
5. Enable the Skip option and set it to 37.5%.
The Skip option determines the percentage of vectors to skip from being displayed. The setting of 37.5% will result in 62.5% of the vectors being displayed.
6. Close the dialog.
4. Set the symmetry plane as the location for display of the vectors.
1. Click OSF: Symmetry in the BOUNDARY TYPES list.
2. Click OK.
5. Zoom in on the junction of the small inlet with the main pipe to view details of velocity vectors.
1. Click on the toolbar.
2. Draw a box around the junction of the two pipes.
Note: The Show Legend option for the velocity contour (Surface ID 1) is disabled in order to capture this image.
The velocity vectors indicate the direction of flow. Notice that the velocity vector length corresponds with the velocity contours. The vectors in the high-velocity region (red) are longest, and those in the low-velocity region (blue) are shortest.

#### Display Contours of Pressure on the Symmetry Plane

In the next steps you will create a boundary surface and display contours of pressure on the symmetry plane.

1. In the Boundary Surface dialog, in the Surface tab, click Create.
The new Surface ID will be 3.
2. Enable the Smooth option in the DISPLAY TYPE control group.
3. Enable the Scalar option in the COLORING control group.
4. Set pressure as the scalar property to display.
1. Click Select in the Scalar Function control group to open the Function Selection dialog.
2. Select pressure from the list.
3. Click Calculate.
5. Set the symmetry plane as the location for display of the contours.
1. Click OSF: Symmetry in the list of BOUNDARY TYPES.
2. Click OK.
6. Turn off the visibility of the vectors and velocity contours.
1. Change the Surface ID to 2 or by clicking .
2. Disable the Visibility option to hide the velocity vectors.
3. Change the Surface ID to 1.
4. Disable the Visibility option to hide the velocity contours.
Note: Click on the Transform Controls toolbar to resize and center the view.
7. Change the color mapping to better resolve differences in the pressure contours.
When the scalar function for pressure is calculated by AcuFieldView, minimum and maximum values are calculated for use in a colormap for the contour display. You can edit the coloring to better resolve differences in the pressure distribution.
1. Set the Surface ID in the Boundary Surface dialog to 3.
Note: You could also make this the current surface by double-clicking the surface in the modeling window.
2. Click the Colormap tab.
3. Enable the Local option.
4. Enter 200 for the upper SCALAR COLORING value.
5. Enter -60 for the lower SCALAR COLORING value.
Note: Decimal entries for values will be converted to scientific notation.
Notice that the Min: value for the Function Range changes when the Local option is toggled.

Notice also that the contours, especially near junction of the small pipe and the inside of the bend in the main pipe, change as the option is toggled.

8. Add a legend to the view.
1. Click the Legend tab in the Boundary Surface dialog.
2. If needed, change the Surface ID to 3.
3. Enable the Show Legend option.
4. Enable the Frame option.
5. Move the legend by Shift+left-clicking and dragging the legend to the left.

## Summary

In this tutorial you worked through a basic workflow to set up a simulation of flow through a mixing elbow. Once the case was set up, you generated a mesh and computed a solution using AcuSolve. Results were post-processed in AcuFieldView to allow you to create contour and vector views along the symmetry plane of the model. In other tutorials, this basic workflow will be reinforced while additional modeling capabilities are introduced.