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, AcuSolve, and HyperView. To run this simulation, you will need access to a licensed version of HyperWorks CFD and AcuSolve.

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

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.
    The Save File 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.

Validate the Geometry

  1. From the Geometry ribbon, click the Validate tool.


    Figure 4.
    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.

    The current model doesn’t have any of the issues mentioned above. Alternatively, if any issues are found, they are indicated by the number in the brackets adjacent to the tool name.

    Observe that a blue check mark appears on the top-left corner of the Validate icon. This indicates that the tool found no issues with the geometry model.


    Figure 5.
  2. Press Esc or right-click in the modeling window and select Exit from the context menu to exit the tool.
  3. Save the database.

Set Up the Problem

Set Up the Simulation Parameters and Solver Settings

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


    Figure 6.
    The Setup dialog opens.
  2. Click the Time setting and ensure that Steady is selected.


    Figure 7.
  3. Click the Flow setting.
  4. Check that the flow type is set to Turbulent.
  5. 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 8.
  6. Click the Solver controls setting and verify that the parameters are set as shown in the figure below.


    Figure 9.
  7. Exit the Setup dialog.

Assign Material Properties

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


    Figure 10.
  2. Using window selection, draw a box around the entire model.
    Both the centrifugal blower and the housing solids are selected.


    Figure 11.
  3. In the dialog that appears, 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 12.
  2. From the Flow ribbon, click the Reference Frame tool.


    Figure 13.
  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 14.
    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 15.
  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.

Assign Flow Boundary Conditions

Set Boundary Conditions for the Inlet

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


    Figure 16.
  2. Click the face of the inlet.


    Figure 17.
  3. In the dialog that appears, click the Turbulence tab.
  4. Set the Turbulence input type to Viscosity Ratio.
  5. Set the Turbulence viscosity ratio to 10.


    Figure 18.
  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.

Set Boundary Conditions for the Outlet

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


    Figure 19.
  2. Click the face of the outlet.


    Figure 20.
  3. In the dialog that appears, make sure both Static pressure and Pressure loss factor are 0.


    Figure 21.
  4. 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 Batch tool.


    Figure 22.
    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 23.
  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.

Run AcuSolve

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


    Figure 24.
    The Launch AcuSolve dialog opens.
  2. Enter -lprobe as an additional argument.
    This launches AcuProbe, which you will use to post-process the results once the run is complete.
  3. Set the Parallel processing option to Intel MPI.
  4. Optional: Set the number of processors to 4 or 8 based on availability.
  5. Deactivate the Automatically define pressure reference option.
  6. Leave the remaining options as default and click Run to launch AcuSolve.


    Figure 25.
    The Run Status dialog opens. Once the run is complete, the status is updated and you can close the dialog.
    Tip: While AcuSolve is running, right-click on the AcuSolve job in the Run Status dialog and select View Log File to monitor the AcuSolve solution process.

Post-Process the Results

Create a Pressure-Rise Plot in AcuProbe

As the solution progresses, the AcuProbe window is 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 - Output > 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 26.
    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 27.
  8. Close the AcuProbe window.
In the next steps you will use HyperView to create a pressure contour on a section on the z-plane.

Open HyperView and Load the Model and Results

  1. Start HyperView from the Windows Start menu by clicking Start > All Programs > Altair <version> > 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 28.
  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 29.

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 pressure rise using AcuProbe and created a contour plot for pressure on a cut plane using HyperView.