ACU-T: 5000 Centrifugal Air Blower with Moving Reference Frame (Steady)


Prior to starting this tutorial, you should have already run through the introductory HyperWorks tutorial, ACU-T: 1000 HyperWorks UI Introduction, and have a basic understanding of HyperMesh, AcuSolve, and HyperView. To run this simulation, you will need access to a licensed version of HyperMesh and AcuSolve.

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

Since the HyperMesh database (.hm file) contains meshed geometry, this tutorial does not include steps related to geometry import and mesh generation.

Problem Description

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.

Figure 1. Schematic of Centrifugal Blower

Figure 2. Schematic of Fan Blades

Open the HyperMesh Model Database

  1. Start HyperMesh and load the AcuSolve user profile.
    Refer to the HM introductory tutorial, ACU-T: 1000 HyperWorks UI Introduction, to learn how to select AcuSolve from User Profiles.
  2. Click the Open Model icon located on the standard toolbar.
    The Open Model dialog opens.
  3. Browse to the directory where you saved the model file. Select the HyperMesh file and click Open.
  4. Click File > Save As.
    The Save Model As dialog opens.
  5. Create a new directory named CentrifugalBlower and navigate into this directory.
    This will be the working directory and all the files related to the simulation will be stored in this location.
  6. Enter Blower_Steady as the file name for the database, or choose any name of your preference.
  7. Click Save to create the database.

Set the General Simulation Parameters

In this step, you will set the simulation parameters that apply globally to the simulation.

  1. Go to the Solver Browser, expand 01.Global, then click PROBLEM_DESCRIPTION.
  2. Change the Turbulence model to Spalart Allmaras.

    Figure 3.

Create a Moving Reference Frame

In this step, you will create a rotating reference frame for the fluid in the impeller region so that the elements in those regions are solved in the given rotating reference frame and rotational body forces are added to that volume set.

  1. In the Solver Browser, right-click on 04.REFERENCE_FRAME and select Create.
  2. In the Entity Editor, rename the reference frame as Impeller_RF.
  3. Set the Rotation center to (0, 0, 0.05).
  4. Set the Angular velocity-Z to -157.08 rad/sec.

    Figure 4.

Set Up Boundary Conditions and Material Model Parameters

By default, all components are assigned to the wall boundary condition. In this step, you will change them to the appropriate boundary conditions and assign material properties to the fluid volumes.
  1. In the Solver Browser, expand 12.Surfaces > WALL.
  2. Click Inlet. In the Entity Editor,
    1. Change the Type to INFLOW.
    2. Set the Inflow type to Stagnation Pressure.
    3. Set the Turbulence input type to Viscosity Ratio.
    4. Set the Material to Air_HM.
    5. Set the Turbulence viscosity ratio to 10.0.

    Figure 5.
  3. Click Outlet. In the Entity Editor, change the Type to OUTFLOW.

    Figure 6.
  4. Click Walls. In the Entity Editor, verify that the Type is set to WALL.

    Figure 7.

    All the surface elements that make up the outer wall of the blower, the fan blades and the interface between the impeller and main fluid can be grouped into one surface set. Auto_Wall, which is an advanced feature in AcuSolve, re-groups these elements into external and internal walls and applies appropriate wall and interface conditions. In this case, the surface elements on the fan blades are grouped together (AUTO Fluid_Impeller wall) and the reference frame assigned to the impeller fluid will be inherited. The surface elements on the interface will be grouped into (AUTO Fluid_Impeller internal) and the elements on the outer casing will be grouped into (AUTO Fluid_Main wall). This entire process of grouping is done internally without you having to do it manually

  5. Click Fluid_Main. In the Entity Editor,
    1. Change the Type to FLUID.
    2. Select Air_HM as the Material.

    Figure 8.
  6. Click Fluid_Impeller. In the Entity Editor,
    1. Change the Type to FLUID.
    2. Select Air_HM as the Material.
    3. Select Impeller_RF as the Reference frame.

    Figure 9.
  7. Save the model.

Compute the Solution

In this step, you will launch AcuSolve directly from HyperMesh and compute the solution.

Run AcuSolve

  1. Turn on the visibility of all mesh components.
    For the analysis to run, the mesh for all active components must be visible.
  2. Click on the ACU toolbar.
    The Solver job Launcher dialog opens.
  3. Optional: For a faster solution time, set the number of processors to a higher number (4 or 8) based on availability.
  4. The Output time steps can be set to All or Final. Since this is a steady state analysis, the Final time step output is sufficient.
  5. Leave the remaining options as default and click Launch to start the solution process.

    Figure 10.

Post-Process the Results

Create a Pressure-Rise Plot in AcuProbe

As the solution progresses, the AcuTail and AcuProbe windows are launched automatically. In this step, you will create a User Defined Function (UDF) and generate a plot of the pressure rise between the inlet and outlet.

  1. Once the solution has converged, click the User Function icon in the AcuProbe window.
    A User Function dialog opens.
  2. Enter Pres_Rise as the function name.
  3. Type P_Outlet = in the Function field.
  4. Expand Surface Output > Outlet > Pressure. Right-click on pressure and select Copy Name. Paste the value in the Function field after P_Outlet =.
  5. On the next line, type P_Inlet = and repeat the above step for inlet pressure.
  6. On the next line, type value = P_Outlet - P_Inlet.

    Figure 11.
    Note: The word “value” is case sensitive and should always be in lowercase characters. If it starts with a capital letter, it will give you an error window.
  7. Click Apply to display the plot.
    Note: You might need to click on the toolbar in order to properly display the plot.

    Figure 12.
In the next steps you will use HyperView to create a pressure contour on a section on the z-plane. Close the AcuProbe and AcuTail windows. In the HyperMesh window, close the AcuSolve Control tab.

Open HyperView and Load the Model and Results

  1. In the HyperMesh main menu area, click Applications > HyperView.
    Once the HyperView window is loaded, the Load model and results panel should be open by default. If you do not see the panel, click File > Open > Model.
  2. In the Load model and results panel, click next to Load model.
  3. In the Load Model File dialog, navigate to your working directory and select the AcuSolve .Log file for the solution run that you want to post-process. In this example, the file to be selected is Blower_Steady.1.Log.
  4. Click Open.
  5. Click Apply in the panel area to load the model and results.
    The model is colored by geometry after loading.

Create a Pressure Contour on a Section Cut Plane

  1. Right-click on empty space in the Results Browser and select Create > Section Cut > Planar.
    A new entity named Section 1 is created
  2. Right-click on Section 1 and select Edit.
  3. In the Define plane section in the panel area, select Z-axis and click Apply.
  4. Enter (0,0,0.05) for the Base values and press Enter.
  5. Change the Display options from Clipping plane to Cross section.
  6. Click Gridline. In the dialog, uncheck the Show option then click OK.
  7. Click on the Results toolbar to open the Contour panel.
  8. Select Pressure(s) as the Result type.
  9. Click the Components collector and select All.
  10. Click Apply.
  11. In the panel area, under the Display tab, turn off the Discrete color option.

    Figure 13.
  12. Click the Legend tab then click Edit Legend. In the dialog, change the Numeric format to Fixed then click OK.
  13. Adjust the orientation in the graphics window for a better view of the results and verify that the contour plot looks like the figure below.

    Figure 14.


In this tutorial, you successfully learned how to set up a steady state simulation involving a rotating reference frame in a centrifugal blower. You started by importing the mesh and then once the case was set up, you generated a solution using AcuSolve. Then, you computed the pressure rise using AcuProbe and created a contour plot for pressure on a cut plane using HyperView.