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

Prerequisites

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 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, click here to download the tutorial models. Extract ACU-T5000_BlowerSteady.hm from HyperWorksCFD_tutorial_inputs.zip.

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

The boundary condition at the inlet is taken as stagnation pressure rather than mass flow rate so that AcuSolve calculates 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.

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 ACU-T5000_BlowerSteady.hm and click Open.
  4. Click File > Save As.
  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.

Validate the Geometry

The Validate tool scans through the entire model, performs checks on the surfaces and solids, and flags any defects in the geometry, such as free edges, closed shells, intersections, duplicates, and slivers.

To focus on the physics part of the simulation, this tutorial input file contains geometry which has already been validated. Observe that a blue check mark appears on the top-left corner of the Validate icon on the Geometry ribbon. This indicates that the geometry is valid, and you can go to the flow set up.


Figure 4.

Set Up the Problem

Set Up the Simulation Parameters and Solver Settings

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


    Figure 5.
    The Setup dialog opens.
  2. Under the Physics models setting:
    1. Verify that the Incompressible option is selected under Single phase flow.
    2. Set the Time marching to Steady.
    3. Select Spalart-Allmaras as the Turbulence model.
      The robustness and accuracy of the Spalart Allmaras turbulence model makes it an excellent choice for simulation of steady state flows.


    Figure 6.
  3. Click the Solver controls setting and verify that the parameters are set as shown in the figure below.


    Figure 7.
  4. Close the dialog and save the model.

Assign Material Properties

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


    Figure 8.
  2. Using window selection, draw a box around the entire model.
    Both the centrifugal blower and the housing solids are selected.


    Figure 9.
  3. In the microdialog, click the drop-down menu next to Material and select Air.
  4. On the guide bar, click to execute the command and exit the tool.

Define the 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. Hide the housing solid.
    1. Set the entity selector to Solids.
    2. Select the centrifugal housing.
    3. Right-click and select Hide form the context menu or press H.
    Only the solid for the centrifugal blower displays in the modeling window.


    Figure 10.
  2. From the Flow ribbon, click the Reference Frame tool.


    Figure 11.
  3. Make sure the Include bounding surfaces option is active on the guide bar.
  4. Select the solid in the modeling window.
    Bounding surfaces are automatically selected.
  5. On the guide bar, click Axis.
  6. Define the axis of rotation.
    1. Use the Surf Center snap point to place the axis in the middle of the centrifugal blower.


      Figure 12.
    2. In the microdialog, click Z to align the axis with the global z axis.
    3. Click to flip the spin direction.
    4. Enter a value of 157.09 in the text field.


      Figure 13.
  7. On the guide bar, click to execute the command and exit the tool.
  8. Right-click in the modeling window and select Show All from the context menu or press A to return to the full model display.

Define Flow Boundary Conditions

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


    Figure 14.
  2. Click the face of the inlet.


    Figure 15.
  3. In the microdialog, click the Turbulence tab.
  4. Set the Turbulence input type to Viscosity Ratio.
  5. Set the Turbulence viscosity ratio to 10.


    Figure 16.
  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 17.
  9. Click the face of the outlet.


    Figure 18.
  10. In the microdialog, make sure both Static pressure and Pressure loss factor are 0.


    Figure 19.
  11. On the guide bar, click to execute the command and exit the tool.

Generate the Mesh

The meshing parameters for this tutorial are already set in the input file.
  1. From the Mesh ribbon, click the Volume tool.


    Figure 20.
    The Meshing Operations dialog opens.
    Note: If the model has not been validated, you are prompted to create the simulation model before running the batch mesh.
  2. Check that the Average element size is 0.01061.
  3. Accept all other default parameters.


    Figure 21.
  4. Click Mesh.
    The Run Status dialog opens. Once the run is complete, the status is updated and you can close the dialog.
    Tip: Right-click on the mesh job and select View log file to view a summary of the meshing process.

Define a Surface Monitor and Run AcuSolve

  1. Set the entity selector to Solids.
  2. Select the centrifugal housing.
  3. Right-click and select Hide form the context menu or press H.
    The solid for the centrifugal blower should be displayed in the modeling window


    Figure 22.
  4. From the Solution ribbon, click the Surfaces tool.


    Figure 23.
  5. Select the blower interface and verify that the arrow is heading toward the blower, as shown in figure below.


    Figure 24.
  6. On the guide bar, click to execute the command and exit the tool.
  7. Rename surface_output to blowerInterfaceFront.
  8. From the Solution ribbon, click the Run tool.


    Figure 25.
    The Launch AcuSolve dialog opens.
  9. Set the Parallel processing option to Intel MPI.
  10. Optional: Set the number of processors to 4 or 8 based on availability.
  11. Deactivate the Automatically define pressure reference option.
  12. Leave the remaining options as default and click Run to launch AcuSolve.


    Figure 26.
    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 Ratios and Surface Output

  1. Right-click on the AcuSolve run in the Run Status dialog and select Plot time history.
  2. In the Plot Utility dialog, double-click on Residual Ratio to open the corresponding plot.


    Figure 27.

    The plot shows the residuals of the equations as the solution progresses through each time step.

    You can see the residuals dropping smoothly. Once the pressure and velocity residual ratios reach a value less than the specified convergence tolerance (0.001), the solution is considered to be converged.

    By default, the eddy viscosity convergence tolerance is set to a magnitude of one order higher than the specified convergence tolerance (0.01).

  3. Return to the Library tab then double-click on Solution Ratio to open the plot.
  4. Click the Logarithm icon to change the solution ratio into a log scale.


    Figure 28.

    The plot shows the solution convergence.

    Once the pressure and velocity residual ratios reach a value less than the specified convergence tolerance (0.01), the solution is considered to be converged.

    By default, the eddy viscosity convergence tolerance is set to a magnitude of one order higher than the specified convergence tolerance (0.1).

  5. Click to add a new plot.
  6. Under the Y-Axis heading, click the arrow besides Run Data and select Surface Output


    Figure 29.
  7. Click the arrow besides area and select moment.
  8. For the Selector, choose z_moment.
  9. Select blades for the surface output.


    Figure 30.
  10. Click Create.


    Figure 31.
  11. Click to add a new plot.
  12. Under the Y-Axis heading, click the arrow besides Run Data and select Surface Output
  13. Click the arrow besides area and select mass_flux.
  14. Select blowerInterfaceFront for the surface output.
  15. Click Create.


    Figure 32.

Post-Process the Results with HW-CFD Post

Plot 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 33.
  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 34.
  7. Press Esc to exit the Move tool.
  8. In the slice plane microdialog, click to create the slice plane.
  9. In the display properties microdialog, toggle the Legend radio button.
  10. Click and set the Colormap Name to Rainbow Uniform.


    Figure 35.
  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.


    Figure 36.

Plot Velocity Streamlines

  1. Hide the slice plane and show the Inlet and Outlet boundaries in the Post Browser.
  2. Click the Streamlines > Circle tool.


    Figure 37.
  3. Select the x-y plane in the modeling window.
  4. In the microdialog, click and move the plane along its normal direction a distance of -0.07.


    Figure 38.
  5. Press Esc to exit the Move tool.
  6. In the slice plane microdialog, click and set the circle radius to 0.1.
  7. On the guide bar, click Seeds.
  8. In the microdialog, set the Generation method to Uniform and set the Point count to 100.
  9. Click Calculate.


    Figure 39.
  10. In the display properties microdialog, set the Display to Velocity and set the Colormap Name to Rainbow Uniform.
  11. On the guide bar, click to execute the command and exit the tool.
  12. In the Post Browser, show the Auto boundary condition, then right-click on Auto and select Edit.
  13. In the microdialog, adjust the transparency slider until you can see the velocity streamlines.
  14. Click on the guide bar.


    Figure 40.

Summary

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 blower momentum using the Plot Utility and created a contour plot for pressure and velocity streamlines using HyperWorks CFD post.