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 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 HyperWorks CFD and AcuSolve. To run this simulation, you will need access to a licensed version of HyperWorks CFD 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 HyperWorks CFD database (.hm file) uses the ACU-T:5000 Blower-Steady model, this tutorial skips the geometry clean-up and inlet boundary conditions as well as the mesh settings.

Problem Description

The model consists of a centrifugal blower with a wheel of backward 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.

Figure 1. Schematic of Centrifugal Blower

Figure 2. Schematic of Fan Blades

Start HyperWorks CFD and Open the HyperMesh Database

  1. Start HyperWorks CFD from the Windows Start menu by clicking Start > Altair <version> > HyperWorks CFD.
  2. From the Home tools, Files tool group, click the Open Model tool.

    Figure 3.
    The Open File 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.
  5. Create a new directory named BlowerTransient 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 BlowerTransient_solved as the file name for the database, or choose any name of your preference.
  7. Click Save to create the database.

Set Up Flow

Set Up the Simulation Parameters and Solver Settings

  1. From the Flow ribbon, click the Physics tool.

    Figure 4.
    The Setup dialog opens.
  2. Under the Physics models settings:
    1. Set Time marching to Transient.
    2. Set the Time step size to 0.0005 and the Final time to 0.05.

    Figure 5.
  3. Click Solver controls.
  4. Set the Minimum stagger iterations and Maximum stagger iterations to 2 and 6, respectively.

    Figure 6.
  5. Close the dialog and save the model.

Define Flow Boundary Conditions

  1. From the Flow ribbon, Pressure tool group, click the Stagnation Pressure tool.

    Figure 7.
  2. Click the face of the inlet.

    Figure 8.
  3. In the microdialog, click the Turbulence tab.
  4. Set the Turbulence input type to Auto.
  5. Set the Turbulence flow type to Internal.

    Figure 9.
  6. Rename the inlet.
    1. From the legend on the left side of the modeling window, double-click on Stagnation pressure.
    2. Type Inlet and press Enter.
  7. On the guide bar, click to execute the command and exit the tool.
  8. Click the Outlet tool.

    Figure 10.
  9. Click the face of the outlet.

    Figure 11.
  10. In the microdialog, make sure both Static pressure and Pressure loss factor are 0.

    Figure 12.
  11. On the guide bar, click to execute the command and exit the tool.

Set Up Mesh Motion

Define the Mesh Motion Type

  1. From the Motion ribbon, click the Settings tool.

    Figure 13.
    The Setup dialog opens.
  2. Change the Mesh motion type to Specified.
  3. Click the Solver controls setting and make sure the Mesh deformation checkbox is unchecked.

Define the Rotating Mesh Motion

  1. Hide the housing solid.
    1. Set the entity selector to Solids.
    2. Select the centrifugal housing.
    3. Right-click and select Hide or press H on your keyboard.

    Figure 14.
  2. Click the Rotation tool.

    Figure 15.
  3. Select the solid in the modeling window.
  4. On the guide bar, click Axis.
  5. Define the axis of rotation.
    1. Use the Surf Center snap point to place the axis in the middle of the centrifugal blower.

      Figure 16.
    2. In the microdialog, click Z to align the axis with the global z axis.
    3. Click to change the rotational direction.
    4. Enter a value of 157.09 in the text field.

    Figure 17.
  6. On the guide bar, click to execute the command and exit the tool.
  7. Right-click in the modeling window and select Show All or press A on your keyboard to return to the full model view.

Define Nodal Output Frequency

  1. From the Solution ribbon, click the Field tool.

    Figure 18.
    The Field Output dialog opens.
  2. Check the Write initial conditions checkbox.
  3. Check the Write results at time step interval checkbox.
  4. Set the Time step interval to 1.

    Figure 19.

Run AcuSolve

  1. From the Solution ribbon, click the Run tool.

    Figure 20.
  2. Set the Parallel processing option to Intel MPI.
  3. Optional: Set the number of processors to 4 or 8 based on availability.
  4. Deactivate the Automatically define pressure reference option.
  5. Leave the remaining options as default and click Run to launch AcuSolve.

    Figure 21.
    Tip: While AcuSolve is running, right-click on the AcuSolve job in the Run Status dialog and select View Log File to monitor the solution process.

Plot Surface Output

  1. Right-click on the AcuSolve run in the Run Status dialog and select Plot time history.
    The plot utility shows the residuals of the equations as the solution progresses through each time step.

    Figure 22.
  2. Click to add a new plot.
  3. Under the Y-Axis heading, click the arrow besides Run Data and select Surface Output

    Figure 23.
  4. Click the arrow besides area and select moment.
  5. For the Selector, choose z_moment.
  6. Select blades for the surface output.

    Figure 24.
  7. Click Create.

    Figure 25.

Post-Process the Results with HW-CFD Post

In this step, you will plot the pressure on a slice plane.
  1. Navigate to the Post ribbon.
  2. From the menu bar, click File > Open > Results.
  3. Select the AcuSolve log file in your problem directory to load the results for post-processing.
    The solid and all the surfaces are loaded in the Post Browser.
  4. Click the Slice Planes tool.

    Figure 26.
  5. Select the x-y plane in the modeling window.
  6. In the microdialog, click and move the plane along its normal direction a distance of -0.07.

    Figure 27.
  7. Press Esc to exit the Move tool context.
  8. In the slice plane microdialog, click to create the slice plane.
  9. In the display properties microdialog, toggle the Legend radio button and set the bounds to -120 and 43.
  10. Click and set the Colormap Name to Rainbow Uniform.

    Figure 28.
  11. On the guide bar, click to execute the command and exit the tool.
  12. In the Post Browser, hide all the Parts and Flow Boundaries.
  13. Click the play button on the Animation toolbar.

    Figure 29.
  14. Go to File > Export > Results to save the pressure contour animation.


In this tutorial, you worked through a basic workflow to set up a transient simulation with a sliding mesh in a centrifugal blower. You started by importing the mesh; once the case was set up, you generated a solution using AcuSolve. Then, you computed the blower momentum using the Plot Utility and created a contour plot for pressure on a cut plane using HW-CFD post.