ACU-T: 5000 Blower - Steady (Rotating Frame)

This tutorial provides the instructions for setting up, solving and viewing results for a steady simulation of a centrifugal air blower utilizing reference frames. In this simulation, AcuSolve is used to compute the motion of fluid due to the rotation of the impeller blades as well as the resulting pressure drop created between the inlet and outlet after the blades have been rotating for a long time. This tutorial is designed to introduce you to a number of modelling concepts necessary to perform simulations that use multiple reference frames.

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:
  • Rotating reference frame
  • Assigning of reference frame to volume and surface sets
  • Post-processing using user function with AcuProbe
  • Post-processing the nodal output with AcuFieldView to get pressure fields.

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 Centrifugal_Blower.x_t 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 a wheel of forward curved blades, and a housing with inlet and outlet ducts. The fluid through the inlet plane enters the hub of the blade wheel, radially accelerates due to centrifugal force as it flows over the blades, and then exits the blower housing through the outlet plane. Because they're relatively cheaper and simpler than axial fans, centrifugal blowers have been widely used in HVAC (heating, ventilating, and air conditioning) systems of buildings.

The diameter of the inlet plane is 0.1 m and the length of the inlet duct is 0.15 m. The housing width is 0.1 m and the radius of the housing from the blade wheel hub varies from 0.113 to 0.18 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. The fan blades have an angular velocity of -1500 RPM. The negative sign describes the direction of the angular velocity vector which in this case is in the –Z direction (clockwise rotation).


Figure 2. Schematic of Fan Blades

The boundary condition at 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 (ρ) of 1.225 kg/m3 and a viscosity (μ) of 1.781 X 10-5 kg/m-sec.

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. 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 mass flow rate at the outlet and the pressure drop across the inlet and outlet. These parameters define the performance characteristics.

Define the Simulation Parameters

Start AcuConsole and Create the Simulation Database

In this tutorial, you will begin by creating a database, populating the geometry-independent settings, loading the geometry, creating groups, setting group parameters, 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 compute the steady state solution. Finally, you will visualize the results using AcuFieldView.

In the next steps you will start AcuConsole, and create the database for storage of the simulation settings.

  1. Start AcuConsole from the Windows Start menu by clicking Start > Altair <version> > AcuConsole.
  2. Click the File menu, then click New to open the New data base dialog.
  3. 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.
  4. Create a new directory in this location. Name it Blower_MRF_Steady and open it.
  5. Enter Blower_MRF_Steady 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.
  6. Click Save to create the database.

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 physical models that you define for this tutorial correspond to steady state, turbulent flow.

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


    Figure 3.
  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 4.
  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 - Reference Frame as the Sub title.
  6. Accept the default Analysis type as Steady State.
  7. Change the Turbulence equation to Spalart Allmaras.
  8. Accept the default Mesh type of Fixed.


    Figure 5.

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. Check that the Analysis type is set to Steady State.
  3. Set the Max time steps as 100.
  4. Check that the Convergence tolerance is set to 0.001.
  5. Set the Relaxation factor to 0.4.
    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.


    Figure 6.

Set Material Model Parameters

AcuConsole has three pre-defined materials, Air, Aluminum, and Water, with standard parameters defined. In the next steps you will verify that the pre-defined material properties of air match the desired properties for this problem.
  1. Double-click Material Model in the Data Tree to expand it.


    Figure 7.
  2. Double-click Air in the Data Tree to open the Air detail panel.

    The material type for air is Fluid. Fluid is the default material type for any new material created in AcuConsole.

  3. Click the Density tab. The density of air is 1.225 kg/m3.
  4. Click the Viscosity tab. The viscosity of air is 1.781 x 10-5kg/m – sec.
  5. 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 Geometry

You will import the geometry in the next part of this tutorial. You will need to know the location of Centrifugal_Blower.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 Centrifugal_Blower.x_t.
  3. Change the file name filter to Parasolid File (*.x_t *.xmt *X_T …).
  4. Select Centrifugal_Blower.x_t and click Open to open the Import Geometry dialog.


    Figure 8.

    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.


    Figure 9.

    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 Reference Frame

A reference frame is used to specify a rotating frame of reference. When specified for a volume set in domain, the elements in that volume set are assumed to be solved in the given rotating reference frame and rotational body forces are added for that volume set. In this tutorial, the fluid region near the impeller blades is assigned a rotating reference frame.

In the next steps you will create a reference frame.

  1. Click PB* in the Data Tree Manager to display all the available settings related to general problem setup in the Data Tree.
  2. Expand the Global Data Tree item.
  3. Right-click Reference Frame and click New to create a new reference frame.
  4. Rename the new reference frame.
    1. Right-click Reference Frame 1.
    2. Click Rename.
    3. Type Impeller_RF and press Enter.
  5. Double-click Impeller_RF to open the detail panel.
  6. Click the Open Array button next to Rotation center to open the Array Editor.
  7. Enter 0.05 as the Z-coordinate.


    Figure 10.
  8. Click OK to close the dialog.
  9. In the detail panel, click the Open Array button next to Angular velocity to open the Array Editor.
  10. Change the units to RPM and enter -1500 in the Z-component field.
    Note: The negative sign specifies the clockwise direction of rotation. Note that the rotation direction is determined using the “right-hand rule”.


    Figure 11.
  11. Click OK to close the dialog.

Apply Volume Parameters

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

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

In the next steps you will create a new volume group, assign a volume to that group, rename the default volume group container, assign the materials for the groups, and set the reference frame for the impeller volume.

  1. Click BAS in the Data Tree Manager to switch to basic view in the Data Tree.
  2. Expand the Model Data Tree item.
  3. 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.
  4. Create a new volume group.
    1. Right-click on Volumes.
    2. Click New.
  5. Rename the new volume group to Fluid_main.
  6. Add the fluid volume to the Fluid_main volume group.
    1. Right-click on the Fluid_main volume group.
    2. Click Add to and select the volume to add it to the volume group.
      The fluid main volume should now be highlighted in a grey color.


      Figure 12.

When the geometry was loaded into AcuConsole, all geometry volumes were placed in the default volume group container. At this point, all the remaining volumes are in the default volume group. Rather than create a new container, add the flow volume in the geometry to it, and then delete the default volume container, you will rename the container and modify the parameters for this group.

  1. Rename the default volume group to Fluid_Impeller.
  2. Check that the material model for the volumes is set as Air.
    1. Double click Element Set under Fluid_Main to open it in the detail panel.
    2. Ensure that the Material model is set to Air.
  3. Assign the reference frame Impeller_RF to Fluid_Impeller.


    Figure 13.

Create Surface Groups and Apply Surface Boundary Conditions

Surface groups are containers used for storing information about a surface or a set of surfaces. 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 settings for the different characteristics of the problem and add surfaces to the group containers.
  • Inlet
  • Outlet
  • Walls
  • Interface
  • Fan Blades

Set Parameters for the Inlet

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

  1. Collapse Volumes in the Data Tree.
  2. Create a new surface group.
  3. Rename the new surface to Inlet.
  4. Expand Inlet in the Data Tree.
  5. Double-click Simple Boundary Condition to open the detail panel.
  6. Change the Type to Inflow.
  7. Change the Inflow type to Stagnation Pressure.
  8. Change the Turbulent input type to Viscosity Ratio.
    This allows you to automatically compute the eddy viscosity value based on the material model and the ratio of the turbulent to molecular viscosity.
  9. Set the Turbulence viscosity ratio to 10.


    Figure 14.
  10. Add geometry to the Inlet group.
    1. In the tree, right-click on Inlet and select Add to.
    2. Click on the inlet face on the model.
      At this point, the inlet should be highlighted grey.


      Figure 15.
    3. Click Done to add this geometry surface to the Inlet surface group.
      Tip: You can also use the middle mouse button to complete the addition of geometry components to a group.

Set Parameters for the Outlet

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

  1. Create a new surface group.
  2. Rename the new surface to Outlet.
  3. Expand Outlet in the Data Tree.
  4. Double-click Simple Boundary Condition to open the detail panel.
  5. Change the Type to Outflow.


    Figure 16.
  6. Add geometry to the Outlet surface container.
    1. In the tree, right-click on Outlet and select Add to.
    2. Click on the outlet face on the model.
      At this point, the outlet should be highlighted grey.


      Figure 17.
    3. Click Done to add this geometry surface to the Outlet surface group.

Set Parameters for the Walls

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

  1. Create a new surface group.
  2. Rename the new surface to Walls.
  3. Expand Walls in the Data Tree.
  4. Double-click Simple Boundary Condition to open the detail panel.
  5. Check that the Type is set to Wall.
  6. Add geometric faces to the Wall group.
    1. In the tree, right-click on Walls and select Add to.
    2. Select all the wall surfaces.
      At this point, the wall surfaces should be highlighted grey.


      Figure 18.


      Figure 19.
    3. Click Done to associate this geometry surface with the Walls surface container.

Set Parameters for the Interface

In the next steps you will define a surface group for the Interface, assign the appropriate settings, and add the Interface surfaces from the geometry to the surface group.
Note: Internal surfaces in AcuConsole are handled in a special manner. At import time, 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 two 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. Turn off the display of the Inlet, Outlet, and Walls surfaces.
  2. Create a new surface group.
  3. Rename the new surface to Interface.
  4. Expand Interface in the Data Tree.
  5. Turn off the Simple Boundary Condition by unchecking the box next to it.


    Figure 20.
  6. Add geometry surfaces Interface group.
    1. In the tree, right-click on Interface and select Add to.
    2. Select all the surfaces on the interface.
    3. Click Done to associate this geometry surface with the Walls surface container.


      Figure 21.
  7. Turn off the display for the interface.

There are two sets of surfaces for the interface which belong to different volume sets. In this case they can be moved into the same surface group.

  1. Right-click Interface and click Add to.
  2. Select the remaining interface surfaces.
  3. Click Done to associate this geometry surface with the surface settings of the Interface group.
    Note: Note that no boundary conditions are applied to this surface at this point. The grouping operation was performed to identify that these surfaces are internal and that flow will be allowed to pass through them freely. These surfaces can still be used for output purposes, however.

Set Parameters for the Fan Blades

In the next steps you will define a surface group for the Fan_Blades, assign the appropriate settings, and add the fan blades from the geometry to the surface group.

  1. Rename the default surface to Fan_Blades.
  2. Expand Fan_Blades in the Data Tree.
  3. Double-click Simple Boundary Condition to open the detail panel.
    The default Type for a default surface is Wall.
  4. Set the Reference frame as Impeller_RF.


    Figure 22.

Assign Mesh Controls

Set Global Mesh Parameters

Now that the flow characteristics have been set for the whole problem and for the individual surfaces, attributes need to be added to make sure that a sufficiently refined mesh is generated.
  • 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 the global mesh attributes. In subsequent steps you will set the surface meshing attributes.

  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. Double-click the Global Data Tree item to expand it.
  3. Double-click Global Mesh Attributes to open the Global Mesh Attributes detail panel.
  4. Change the Mesh size type to Absolute.
  5. Enter 0.02 m for the Absolute mesh size.
    This absolute mesh size is chosen to ensure that there are at least 50 mesh elements on the inlet.
  6. Set the Maximum sweep angle as 30.0 degrees.
    This option allows you to set the maximum sweep angle for edge blend meshing on a global basis which creates a radial array of elements around sharp edges to provide better resolution of the flow features. The sweep angle is used to control how many degrees each radial division spans.


    Figure 23.

Set Surface Mesh Parameters

In the following steps you will set the meshing attributes that will allow for localized control of the mesh size on the surface groups that you created earlier. Specifically, you will set local meshing attributes that control the growth of boundary layer elements normal to the surfaces of the walls and fan blades.
  • Walls
  • Fan Blades

Set Surface Mesh Parameters for the Walls

In the following steps you will set meshing attributes that will allow for localized control of the mesh size near the walls. The mesh size on the wall will be inherited from the global mesh size that was defined earlier. The settings that follow will only control the growth of the boundary layer from the walls.

  1. Expand the Model Data Tree item.
  2. Under the Model branch, expand Surfaces, and then expand Walls.
  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.
    This option indicates that the mesher will use the global meshing attributes when creating the mesh on the surface of the walls.
  5. Switch the Boundary layer flag to On.
    This option allows you to define how the meshing should be handled in the direction normal to the walls.
  6. Set the Boundary layer type to Full Control.
    Mesh elements for a boundary layer are grown in the normal direction from a surface to allow efficient resolution of the steep gradients near no-slip walls. The layers can be specified using a number of different options.

    When Boundary layer type is set to Full Control, the First layer height, Number of layers and the Growth rate are specified. Boundary layer elements will be grown until the mesh size of the top layer matches the mesh size of the volume into which the boundary layer elements are grown.

  7. Set the remaining settings as follows:
    Option Description
    First element height 0.002
    Number of layers 3
    Boundary layer bends flag On
    Maximum sweep angle 15.0


    Figure 24.

Set Surface Mesh Parameters for the Fan Blades

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

  1. Under Fan Blades, click the check box next to Surface Mesh Attributes to enable the settings and open the Surface Mesh Attributes detail panel.
  2. Change the Mesh size type to Absolute.
  3. Enter 0.005 m as the Absolute mesh size.
  4. Switch the Boundary layer flag to On.
  5. Set the Boundary layer type to Full Control.
  6. Set the Resolve field to Total Layer Height.
  7. Set the remaining settings as follows:
    Option Description
    First element height 0.001 m
    Growth rate 1.3
    Number of layers 3


    Figure 25.
  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.



    Figure 26.
    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 27. Mesh Details of the Geometry
    Figure 28. Mesh Details Near the Fan Blades


  9. 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.


    Figure 29.
  2. Enter 4 for Number of processors, if your system has 4 or more processors.
    The use of multiple processors can reduce solution time.
  3. Accept all other default settings.
    Based on these settings, AcuConsole will generate the AcuSolve input files and then launch the solver.
  4. 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 30.
  5. Close the AcuTail window and save the database to create a backup of your settings.

Monitor the Solution with AcuProbe

AcuProbe can be used to monitor various variables over solution time.

  1. Open AcuProbe by clicking on the toolbar.
  2. In the Data Tree on the left, expand Residual Ratio.
  3. Right-click on Final and select Plot All.
    The residual ratio measures how well the solution matches the governing equations.
    Note: You might need to click on the toolbar in order to properly display the plot.


    Figure 31.
    After AcuSolve has finished running, a summary of the solution process showing the “End Time Step” data indicates that the simulation has been completed.

Post-Process with AcuProbe

The pressure rise between the Inlet and Outlet can be viewed using a User Function at the end of simulation using AcuProbe.

  1. In the AcuProbe window, double-click on .
  2. Enter the name in the User Function window as Pres_Rise.
  3. In the function window, type P_Outlet =.
  4. Expand Surface Output > Outlet > Pressure.
  5. Right-click on pressure and select Copy Name.
  6. Paste the value in the function window for Outlet pressure.
  7. Type P_Inlet = on a line line.
  8. Repeat steps 4 - 6 for Inlet pressure.
  9. Type value = P_Outlet – P_Inlet.


    Figure 32.
  10. Click Apply to display the plot.
    Note: You might need to click on the toolbar in order to properly display the plot.


    Figure 33.

View Results with AcuFieldView

Now that a solution has been calculated, you are ready to view the flow field using AcuFieldView. AcuFieldView is based on a third-party post-processing tool that has been tightly integrated toAcuSolve. 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.

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.

View the Boundary Surface Showing Pressure for the Outer Surfaces with Mesh

  1. Click Viewer Options.


    Figure 34.
  2. Click axis markers to disable them.
  3. Uncheck Perspective to disable perspective view.
  4. Close the Viewer Options dialog.
  5. Change the background color to white
  6. Orient the geometry so you can see inlet, outlet and wall surfaces as shown in Figure 35.
  7. In the Boundary Surfaces dialog, ensure that Pressure is selected as the Scalar function.
  8. In the Boundary Types list, select the Inlet, Outlet and Wall surfaces from boundary types.
  9. Click on the Colormap tab and check Local to display the local range of values of pressure for the selected surfaces.
  10. 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.


    Figure 35.

Coordinate the Surface Showing Pressure on the Mid Coordinate Surface

  1. Click to open the Coordinate Surface dialog.
  2. Click Create to create a new surface.
  3. Set the new surface at the mid –Z coordinate surface.
  4. In the Coord Plane fields, enter 0.05 as the Current value.
    This is the z coordinate for the mid plane between the blower front and back walls.
  5. Change the Display Type to smooth.
  6. Change the Coloring to scalar.
  7. Select pressure as the scalar function to display.
  8. Click the Colormap tab and change the coloring to local.
  9. Turn on the legend to display the pressure values on the coordinate plane.
  10. Orient the geometry for a better view of the results.


    Figure 36.

Summary

In this tutorial, you worked through a basic workflow to set up a steady state simulation with a rotating reference frame in a centrifugal blower. Once the case was set up, you generated a mesh and generated a solution using AcuSolve. AcuProbe was used to post-process the pressure rise in the blower. Results were also post-processed in AcuFieldView to allow you to create contour views for the pressure along the walls and on the mid coordinate surface of the blower. New features introduced in this tutorial include creating a rotating reference frame and creating a user function in AcuProbe.