ACU-T: 5001 Blower - Transient (Sliding Mesh)

This tutorial provides the instructions for setting up, solving and viewing results for a transient simulation of a centrifugal air blower utilizing the sliding mesh approach. In this simulation, AcuSolve is used to compute and visualize the motion of fluid in form of velocity field, streamlines and particle path animations for three revolutions after the blower has been operating for a long time. This tutorial is designed to introduce you to a number of modeling concepts necessary to perform simulations that use the sliding mesh motion feature.

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:
  • Mesh motion
  • Use of multiplier function to scale the time step size
  • Assigning and meshing interface surfaces
  • Mesh refinement
  • Projection of steady state solution as the initial condition
  • Post-processing using AcuFieldView to get velocity fields, streamlines and streaklines animation.

Prerequisites

In order to run this tutorial, you should have already run through ACU-T: 5000 Blower - Steady (Rotating Frame) and kept the solution in your working directory. It is assumed that you have some familiarity with AcuConsole, AcuSolve, and AcuFieldView. You will also need access to a licensed version of AcuSolve.

In case you do not have the steady state results, prior to running through this tutorial, copy AcuConsole_tutorial_input.zip from <AcuSolve installation directory>\model_files\tutorials\AcuSolve to a working directory and extract Centrifugal_Blower_MRF_Steady.acs from AcuConsole_tutorial_inputs.zip.

Analyze the Problem

The problem to be addressed in this tutorial is shown schematically in Figure 1 and Figure 2. It consists of a centrifugal blower with backward curved blades.

The diameter of the inlet is 0.1 m and the length is 0.150 m. The scroll width is 0.1 m and the radius varies from 0.113 m to 0.180 m.


Figure 1. Schematic of Centrifugal Blower
The fan blades have a mean chord length and width of 0.05 m. The maximum thickness of the blades is 0.003 m.


Figure 2. Schematic of Fan Blades

To capture the dynamic motion of the impeller blades, the simulation has to be run as transient. The converged steady state solution from the steady blower simulation is projected on the mesh and used as the initial state for the transient simulation.

The simulation will be run to model 0.12 s of the flow, which would constitute three revolutions of the fan blades with time step sizes scaled using a multiplier function.

t simulation =0.12 s

ω rot =1500 RPM=25 RPS= 9000  degrees s

Δ t initial = 10 9000 =0.00111 s

The multiplier function is chosen such that the impeller blades rotate at 10 degrees per time step for the first revolution, then ramp down from 10 degrees per time step to 3 degrees per time step during the second revolution and complete the third revolution at 3 degrees per time step.


Figure 3.
Note: Meaningful data should be taken after 2 or 3 revolutions as the initial conditions are flushed out of the domain. The multiplier function is selected such that the simulation completes in sufficient time for a tutorial exercise.

The time step size for the last revolution is based on prior investigations of a similar geometry, which indicate that this time step size is small enough to capture the transient behavior of the flow. It should be noted, however, that a time step size sensitivity study should always be performed to establish appropriate time step size when analyzing a new application.

The CFD analysis of this problem offers detailed information about the flow through a centrifugal blower. To investigate this behavior, it is necessary to select an appropriate set of boundary conditions to use. There are two different methods that are commonly used. One approach is to specify the mass flow rate at the inlet of the blower and allow AcuSolve to compute the pressure drop, that is, flow forces simulation. Another option is to specify the stagnation pressure at the inlet and allow AcuSolve to compute the flow rate that results from this specified pressure change between the inlet and outlet. The boundary conditions used in this example are the latter. That is, the inlet is taken as stagnation pressure rather than mass flow rate so that AcuSolve calculates mass flow rates and pressure rise based on impeller rotation.

The fluid in this problem is air, which has a density of 1.225 kg/m3 and a viscosity of 1.781 X 10-5 kg/m-s.

In addition to setting appropriate conditions for the simulation, it is important to generate a mesh that will be sufficiently refined to provide good results. For this problem the global mesh size is set to provide approximately 16 elements around the circumference of the inlet which results in a mesh size of 0.02 m.

meshSiz e global =  d inlet nElem s circ                       nElem s circ =16

meshSiz e global =0.02 m

Note that higher mesh densities are required where velocity, pressure, and eddy viscosity gradients are larger. In this application, the flow will accelerate as it passes through radial flow paths between the fan blades. This leads to the higher gradients that need finer mesh resolution. Proper boundary layer parameters need to be set to keep the y+ near the wall surface to a reasonable level. The mesh density used in this tutorial is coarse and is intended to illustrate the process of setting up the model and to retain a reasonable run time. A significantly higher mesh density is needed to achieve a grid converged solution.

Once a solution is calculated, the flow properties of interest are the velocity magnitude, stream – lines and streak – lines animations as the blower goes through three revolutions of the impeller blades.

Define the Simulation Parameters

Start AcuConsole and Create the Simulation Database

In the next steps you will start AcuConsole, and open a database that is set up for a steady state simulation for the centrifugal blower using a rotating reference frame. You will then run AcuSolve to calculate a steady state solution, view the results with AcuFieldView, and save the database for the transient simulation.

  1. Start AcuConsole from the Windows Start menu by clicking Start > All Programs > Altair <version> > AcuConsole.
  2. Click File > Open and open Centrifugal_Blower_MRF_Steady.acs.


    Figure 4.
  3. Run AcuSolve to solve the steady state problem.
    1. Click on the toolbar to open the Launch AcuSolve dialog.
      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.



      Figure 5.

View Steady State Results

The steady state flow field was calculated as the starting point for the transient simulation of temperature. For instructions on visualising steady state results, refer to ACU-T: 5000 Blower - Steady (Rotating Frame).

Set General Simulation Parameters

In next steps you will set parameters that apply globally to the simulation. To make this simple, the basic settings applicable for any simulation can be filtered using the BAS filter in the Data Tree Manager. This filter enables display of only a small subset of the available items in the Data Tree and makes navigation of the entries easier.

The general parameters that you will set for this tutorial are for turbulent flow, transient analysis, and mesh type as fully specified, which means that the motion is fully specified at the beginning of each time step and hence no mesh equation needs to be solved.

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


    Figure 6.
  2. 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 7.
  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 AcuSolve Tutorial as the Title.
  5. Enter Centrifugal Blower - Sliding Mesh as the Sub title.
  6. Change the Analysis type to Transient.
  7. Change the Turbulence equation to Spalart Allmaras.
  8. Set the Mesh type to Fully Specified.
    This option indicates that the simulation will contain a moving mesh, but the motion of the mesh will be fully specified, that is, no differential equations will be solved to determine the deformation of the elements. Since the mesh is undergoing a simple rotational motion, this option provides the most efficient solution.


    Figure 8.

Set Solution Strategy Parameters

In the next steps you will set attributes 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. Check that the Analysis type is set to Transient.
  3. Set the Max time steps as 0.
    AcuSolve will calculate the number of time steps based on the final time and the multiplier function, which you will specify in the next section.
  4. Set the Final time as 0.12.
  5. Set the Initial time increment to 0.00111.
  6. Check that the Convergence tolerance is set to 0.001.
    Note that for a transient analysis, the convergence tolerance corresponds to the tolerance that the equations are converged to before proceeding to the next time step. However, since we are performing a maximum of 2 iterations per step, the solver will be limited in the number of iterations it can perform while attempting to reach this tolerance.
  7. Set the Max stagger iterations to 2.
    This setting determines the maximum number of iterations that will occur at each time step.
  8. Set the Relaxation factor to 0.
    The relaxation factor is used to improve convergence of the solution. 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. When solving transient solutions, the relaxation factor should be set to zero. A non-zero relaxation factor causes incremental updates of the solution, which will impact the time accuracy of the solution for transient cases.


    Figure 9.

Create a Multiplier Function for the Time Increment

AcuSolve provides the ability to scale values as a function of time and/or time step during a simulation. This is achieved through the use of a multiplier function. In this tutorial, the time steps sizes are scaled against time to set up a robust solution.

In the next steps you will create a multiplier function for the time increment. The multiplier function is chosen such that the impeller blades rotate at 10 degrees per time step for the first revolution (0 s– 0.04 s), then ramp down from 10 degrees per time step to 3 degrees per time step during the second revolution (0.04 s – 0.08 s) and complete the third revolution at 3 degrees per time step (0.08 s – .12 s)

Δ t initial =10 deg per step= 10 9000 =0.00111 s

Δ t final =3 deg per step=0.3 Δ t initial

To make the creation of the multiplier functions as simple as possible, you will use the PB* filter in the Data Tree Manager.

  1. Click PB* in the Data Tree Manager to display all the available settings related to general problem setup in the Data Tree.
  2. In the Data Tree, under Global, right-click Multiplier Function and click New to create a new multiplier function.
  3. Rename the multiplier function.
    1. Right-click the newly created Multiplier Function 1 and click Rename.
    2. Type Time_Function and press Enter.
  4. Double-click Time_Function to open the Time_Function detail panel.
  5. Set the Type to Piecewise Linear.
    This option indicates that you will enter an array of numbers that will be used by AcuSolve to interpolate the value of the multiplier function at each time step. In this example, the curve fit is a function of time.


    Figure 10.
  6. Add the curve-fit values for the large inlet temperature profile.
    1. Click Open Array to open the Array Editor dialog.
    2. Enter the values shown as calculated earlier and shown in the following image.


      Figure 11.
  7. Click Plot to expand the Array Editor dialog to display the plot of the curve fit values.
    Note: You may need to expand the dialog by dragging the right edge in order to see the plot.


    Figure 12.
  8. Close the dialog.

Modify the Advanced Solution Strategy Parameters

AcuSolve provides additional features to modify some advanced solution strategy attributes separately, such as individual staggers (flow, mesh, turbulence, and so on), time increments, linear solver parameters and many more. In this tutorial the time increment feature is turned on in order to scale the time step sizes based on a multiplier function.

In the next steps you will work with the time increment feature under advanced solution strategy to assign the multiplier function.

  1. Double-click Advanced Solution Strategy to expand the tree.
  2. Double-click Time Increment to display the Time Increment detail panel.
  3. Turn on the Modify advanced settings option.
  4. Check that the Initial time increment has been set as 0.00111.
  5. In the Multiplier function drop-down menu, select Time_Function.


    Figure 13.

Create the Mesh Motion

This command is used to simplify the specification of boundary conditions on mesh displacement and it can be used to simulate the dynamic motion of a rigid body. In this tutorial, the fluid region near the impeller blades is assigned a rotating mesh motion. The parameters defined for this would be the angular speed of the impeller blades and the center of rotation of the motion.

In the next steps you will create a mesh motion.

  1. Click ALE in the Data Tree Manager to see all the settings related to mesh motion.
  2. Double-click the Global Data Tree item to expand it.
  3. Right-click Mesh Motion and click New to create a new mesh motion.
  4. Rename the new mesh motion to Impeller_Motion.
  5. Double-click Impeller_Motion to open the detail panel.
  6. Set the Type to Rotation.


    Figure 14.
  7. Set the mesh motion parameters.
    1. Click Open Array next to Rotation center to open the Array Editor.
    2. Enter 0.05 as the Z-coordinate.
      This is the coordinate for the centre of the rotating fluid domain, that is, Fluid_Impeller.
    3. Click OK to close the dialog.
    4. Click Open Array next to Angular velocity to open the Array Editor.
    5. Change the units to RPM and enter -1500 in the Z-component field.
      The negative sign specifies the clockwise direction of rotation.
      Note: The rotation direction is determined using the “right-hand rule”.
    6. Click OK to close the dialog.

Set the Nodal Output Frequency

The Nodal Output Frequency determines at what frequency or time interval the solution results would be stored to be used for post processing within AcuFieldView.

  1. Click OUT in the Data Tree Manager to filter the settings in the Data Tree to show only those controls related to outputs written to the solution files.
  2. Double-click Output to expand it.
  3. Double-click Nodal Output.
    1. Change the time step frequency to 3.
      This setting will save results every 3 steps and will allow you to create an animation of the results once the simulation is complete.
  4. Set Output Initial Condition to On.
    This writes the initial condition file.


    Figure 15.

Modify 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.

  1. Click PRB from the Data Tree Manager.
  2. Expand Model, and then expand Volumes.
  3. Assign the mesh motion Impeller_Motion to Fluid_Impeller.
    1. Expand Fluid_Impeller.
    2. Under Fluid_Impeller, double-click Element Set to open the Element Set detail panel.
    3. Click the drop-down control next to Mesh motion and click Impeller_Motion.
      This step assigns the mesh displacement boundary conditions specified by the Impeller Motion mesh motion on all the nodes of Fluid_Impeller Element Set. All the nodes in the Fluid_Impeller element set would be assigned the angular velocity and center of rotation defined in the mesh motion.
  4. Set the Reference frame as None.


    Figure 16.

Modify Surface Parameters

Surface groups are containers used for storing information about a surface, including solution and meshing parameters, and the corresponding surface in the geometry that the parameters will apply to.

In the next steps you will modify the parameters for:
  • Fan Blades
  • Interface

Modify Parameters for the Fan Blades

In the next steps you will specify the mesh motion associated with fan blades.

  1. Click BC from the Data Tree Manager.
  2. Expand Surfaces.
  3. Assign the mesh motion Impeller_Motion to Fan_Blades.
    1. Expand Fan_Blades.
    2. Double-click Simple Boundary Condition under Fan_Blades to open the Simple Boundary Condition detail panel.
    3. Click the Mesh motion drop-down menu and select Impeller_Motion.
      This step assigns the center of rotation and angular velocity assigned to Impeller_Motion mesh motion to the fan_blades surface.
  4. Set the Reference frame as None.


    Figure 17.

Modify Parameters for the Interface

In the next steps you will assign Interface Surface properties to the Interface.

The Interface acts as a sliding boundary and is used to connect pairs of elements that share (approximately) the same surface but are not conformal. An Interface Surface allows the flow to pass from one side of the surface to the other when the nodes are not connected to each other. This step would become clear when you split the nodes on the interface surface in the later steps.
Note: Internal surfaces in AcuConsole are handled in a special manner. When a geometry with internal surfaces is imported, AcuConsole creates two identical copies of the surface. One copy of the surface is associated with each volume. This allows you to control meshing parameters independently on each side of the surface. When assigning boundary conditions to internal surfaces, it is important to remember that there are 2 sides of the surface that need to be dealt with. When selecting an internal surface, the side corresponding to the outer volume is the first pick target that is encountered when both faces are visible. The inner surface can be selected directly by changing the display of the outer surface.
  1. Click ALE in the Data Tree Manager to see all the settings related to mesh motion.
  2. Expand Model, and then expand Surfaces.
  3. Activate Interface Surface for Interface.
    1. Double-click Interface.
    2. Check Interface Surface under Interface.
    3. Double-click Interface Surface.
    4. Set the Gap factor to 0.
      Gap factor is non-dimensional (with respect to the length of an element face) maximum gap allowed for two element faces to be in contact.
      A gap factor of 0 means the maximum gap allowed is zero.


      Figure 18.

Assign Mesh Controls

Set Zone Meshing Attributes

In addition to setting meshing characteristics for the whole problem, you can assign meshing attributes 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 following steps you will add mesh refinement in the zone around the impeller blades closest to the housing wall as shown in figure 3.

  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. Under Global, right-click Zone Mesh Attributes and then click New.
  3. Rename Zone Mesh Attributes 1 to Refine_1.
  4. Double-click Refine_1 to open the Zone Mesh Attributes detail panel.
  5. Change the Mesh zone type to Cylinder.
  6. 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 the coordinate values as shown in the following image.


      Figure 19.
    3. Click OK to close the dialog.
  7. In the detail panel, enter 0.05 m for the Radius.
    This radius is used to define a cylinder that encloses the gap in the modeled section near the impeller blades and housing wall.
  8. Enter 0.005 m for the Mesh size.
    This will result in a zone where the mesh size provides at least 10 cells between the impeller and the housing wall at their nearest distance.


    Figure 20.

Set Surface Meshing Parameters for the Interface

In the following steps you will set meshing attributes that will allow for localized control of the mesh size near on the interface.

  1. Expand the Model Data Tree item.
  2. Expand Surfaces, and then expand Interface.
  3. Click the check box next to Surface Mesh Attributes to enable the settings and open the Surface Mesh Attributes detail panel.
  4. Change the Mesh size type to None.
  5. Turn the Boundary layer flag option to On.
  6. Set the Boundary layer type to Total Layer Height.
  7. Enter the value 0.002 m for First element height.
  8. Enter 1.3 for the Growth rate.
  9. Enter 1 for Number of layers.
  10. Change the Boundary layer elements type to Mixed.

    This is used to generate prism/hexahedral elements in the boundary layer.



    Figure 21.
  11. 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.
    For this case, the default settings will be used.
  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.



    Figure 22.
    Note: The actual number of nodes and elements, and memory usage may vary slightly from machine to machine.
  3. Visualize the mesh in the modeling window. For the purposes of this tutorial, the following steps lead to the display of inlet, outlet, walls and fan blades.
  4. Right-click Volumes in the Data Tree and click Display off.
  5. Right-click Surfaces in the Data Tree and click Display on.
  6. Right-click Surfaces in the Data Tree, select Display type and click solid & wire.
  7. Rotate and zoom in the model to analyze the various mesh regions.
  8. Right-click on the model and select cut plane visualization to view the mesh near the fan blades.


    Figure 23. Mesh Details of the Geometry


    Figure 24. Mesh Details Near the Fan Blades
  9. Save the database to create a backup of your settings.

Split the Nodes on the Interface

At this point, the interface surface has one set of nodes which are either attached to the Fluid_Main or Fluid_Impeller volume sets. In order for the nodes inside the Fluid_Impeller volume and Interface to rotate based on the mesh motion prescribed, a duplicate set of nodes needs to be created, so that one set of the nodes follow the motion of the Fluid_Impeller and another set stays attached to Fluid_Main.

Splitting the nodes on the interface would allow the nodes attached to Fluid_Impeller to slide over the nodes on Fluid_Main, hence simulating the rotation on the fluid domain with the impeller blades.

In the next steps you will split the nodes on the interface using the Mesh Op. tool.

Right-click on Interface, select Mesh Op > Split internal faces.
The information window showing the modified number of nodes displays.


Figure 25.

Project Steady State Solution to Use as Initial Conditions

In the next steps you will use the Project Solution to project the steady state solution onto the transient case in form on Nodal Initial Conditions.

  1. From the Tools menu, select Project Solution.
    The AcuSolve solution projection dialog opens.
  2. Click Browse to read in the log file from the steady state solution.
  3. Browse to the location where the steady state solution is stored and select the log file.
    Once the log file is selected, the Information Window displays, showing the details of the projection process.

    The AcuSolve solution projection dialog updates and displays the step ID and the variables to project.



    Figure 26.
  4. Close the Information Window.
  5. Select velocity, pressure and eddy_viscosity from the list by using Shift+click.
  6. Click Project.
    The Information Window displays and shows that all the three variables have been projected.
  7. Close the Information Window and the AcuSolve solution projection dialog.
  8. Click BAS in the Data Tree Manager to switch to basic view in the Data Tree.
  9. In the Data Tree, expand Global, and double-click on Nodal Initial Condition.
  10. Set the pressure, velocity and eddy viscosity initial condition type as Nodal Values.
  11. Click Open Array next to Nodal values for Pressure to check that the values have been assigned.


    Figure 27.
  12. Click OK to close the Array Editor.
  13. Similarly check the values for velocity and eddy viscosity.

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.


    Figure 28.

    For this case, the default values will be used. AcuSolve will run using four processors and it will calculate the transient 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.



    Figure 29.
  3. Close the AcuTail window and save the database to create a backup of your settings.

View Transient 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 following steps you will start AcuFieldView, display the pressure contours on the mid coordinate surface and generate animations for pressure, streamlines and particle paths.

Start AcuFieldView

  1. Click on the AcuConsole toolbar to open the Launch AcuFieldView dialog.
  2. Click Ok to start AcuFieldView.
    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. You will see that the pressure contours have already been displayed on all the boundary surfaces with mesh.


    Figure 30.

    These steps are provided with the assumption that you are able to manipulate the view in AcuFieldView to have a white background, perspective turned off, outlines turned off, and the viewing direction set to +Z. If you are unfamiliar with basic AcuFieldView operations, refer to Manipulate the Model View in AcuFieldView.

Animate the Pressure Contours on the Mid Coordinate Surface

  1. In the Boundary Surface dialog, turn off the visibility for the boundary surfaces by unchecking the Visibility check box.
  2. From the View menu, uncheck Perspective view to disable it.
  3. From the View menu, uncheck Axis markers to disable them.
  4. From the View menu, select Defined Views.
  5. In the Defined Views dialog, change the view to +Z.
  6. Close the dialog.
  7. Click to open the Coordinate Surface dialog.
  8. Click Create to create a new surface at the mid –Z coordinate surface.
  9. Under Coord Plane, change the Current value to 0.05.
    This is the z coordinate for the mid plane between the blower front and back walls.
  10. Change the Display Type to Smooth.
  11. Change the Coloring to Scalar.
  12. Select pressure as the Scalar Function to be displayed.
  13. Click the Colormap tab and activate the Local check box to change the coloring to local.
  14. Click on the Legend tab,and activate the Show Legend check box to display the velocity magnitude values on the coordinate plane.
  15. Activate the Frame check box to display the frame for the legend.


    Figure 31.
  16. From the Tools menu, click on Transient Data to open the Transient Data Controls dialog.
    For a transient case, the data displayed by launching AcuFieldView from AcuConsole is for the last time step. The Transient Data Controls allows you to visualize the data at rest of the time steps. The time steps at which the data can be post processed depends on the nodal output value set in AcuConsole. In this case the nodal output is stored at every third time step.
  17. Move the slider all the way to the back to zero to visualize the data at the zeroth time step.
    This is done in order to build the animation from the beginning of the simulation.
  18. From the Tools menu, click on Flipbook Build Mode.
    A Flipbook size warning dialog appears.
  19. Click OK.
    In the Transient Data Controls dialog, the Sweep option under Sweep Control changes to Build.
  20. Click Build.
    AcuFieldView will build the frame by frame animation of the solution progressing through all of the available time steps. You will be able to see the progress in a Building Flipbook dialog.
  21. In the Flipbook Controls dialog, click on Speed to open the Minimum Time Between Frames dialog.


    Figure 32.
  22. Enter 0.1 seconds as the minimum time.
  23. Pause the animation and click Save to save the animation.
  24. Close the Minimum Time Between Frames, Flipbook Controls, and Transient Data Controls dialogs.

Set up Streamlines

  1. Click to open the Coordinate Surface dialog.
  2. Turn off the visibility.
  3. Click to open the Boundary Surface dialog.
  4. Turn on the visibility.
    Pressure is already selected as the Scalar Function.
  5. In the Boundary Types list, select OSF: walls and click OK.
  6. Change the Coloring to Geometric and select grey from the color panel.
  7. Turn off the mesh display by unchecking Show Mesh.
  8. Set the Transparency field to 75 %.
  9. Set the Scalar Function to velocity_magnitude.
  10. Turn off the visibility for this surface.
  11. Click Create to create a new boundary surface.
  12. Select OSF: Inlet and OSF: Outlet from the Boundary Types list.
  13. Turn on the visibility for this surface.
  14. Change the Coloring to Scalar.
  15. Set the Transparency to 0.
  16. Create another boundary surface and select OSF: Fan_Blades from the Boundary Types list.
  17. Click the Colormap tab and activate the Local check box to change the coloring to local.
  18. From the Visualization Panels menu, select Streamlines.
    The Streamlines panel opens.
  19. Select Create to create a new set of streamlines.
  20. Click the Mode toggle button and select Seed a Surface.
    In order to display streamlines you will need to seed a surface from where the streamlines are generated.


    Figure 33.
  21. Set the Seeds to Add value to 200.
  22. Ctrl + left click to select boundary surface 3 (Fan_Blades) as the surface to be seeded and click OK.
    The seeds are displayed on the fan blades.


    Figure 34.
  23. Uncheck Show Seeds to turn off the display of seeds.
  24. Open the Boundary Surfaces dialog and turn on the display for Surface 1 (walls).
  25. Return to the Streamlines dialog. Under Calculation Parameters, change the Step counter to 5.
    The Step size determines the time step intervals at which the streamlines would be calculated.
  26. Change the Direction to Both.
    The direction determines the direction of flow (upstream, downstream or both) in which the streamlines would be generated from the surface selected.


    Figure 35.
  27. Click Calculate to generate the streamlines.


    Figure 36.
  28. Change Coloring to Scalar and Display Type to Filament and Arrows.
  29. Click the Colormap tab.
  30. Click the Colormap drop-down arrow and select NASA-1.
  31. Click the Legend tab.
  32. Activate the Show Legend and Frame checkboxes to turn them on.
  33. Orient the geometry so that all the surfaces are visible, as shown below:


    Figure 37.
  34. In the Steamlines panel, click Animate to see the streamlines.


    Figure 38.

Set up Streaklines

  1. Click Tools > Flipbook Build Mode.
  2. Click OK to skip the warning.
  3. Click Tools > Transient Data.
  4. Move the slider back to 0 to show the contours for the 0th time step.
  5. Click Build.
  6. Click Yes in the Streakline Export panel.
  7. Save the .fvp export file.
    The export file will save streaklines to a particle path file, and simplifies future import and display.
  8. Change the Frame rate to 0.16.
  9. Pause the animation and click Save to save the animation.


    Figure 39.

Summary

In this tutorial, you worked through a basic workflow to set up a transient simulation with a sliding mesh in a centrifugal blower. Once the case was set up, you modified the mesh to include refinement zones, projected the steady state solution onto the refined mesh and generated a solution using AcuSolve.

Results were post-processed in AcuFieldView to allow you to create contour views for the pressure on the mid coordinate surface of the blower as well as the impeller blades along with new features for creating animations for contours, streamlines, streaklines and particle paths.

New features introduced in this tutorial include creating a rotational mesh motion, use of interface surfaces, projection of steady state solution in form of nodal initial conditions, creating pressure, streamlines and particle path animations.