ACU-T: 5100 Modeling of a Fan Component: Axial Fan

Prerequisites

This simulation provides instructions for running a steady state simulation of flow inside a pipe with an interior fan placed at the middle of the pipe. Prior to starting this tutorial, you should have already run through the introductory tutorial, ACU-T: 1000 Basic Flow Set Up, 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-T5100_AxialFan.hm and AxialCoefficient.csv from HyperWorksCFD_tutorial_inputs.zip.

Note: This tutorial does not cover the steps related to geometry cleanup and mesh settings.

Problem Description

The problem to be solved in this tutorial is shown schematically in the figure below. It consists of an interior fan which rotates at a speed of 377 rad/sec (~3600 RPM) and has a thickness of 0.06 m and a tip radius of 0.11 m. The volumetric flow rate at the inlet is 0.322675 m3/sec (~1212.3 m3/hr). The problem is simulated as a steady state run and the pressure rise across the fan region is computed.



Figure 1.

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 2.
    The Open File dialog opens.
  3. Browse to the directory where you saved the model file. Select the HyperMesh file ACU-T5100_AxialFan.hm and click Open.
  4. Click File > Save As.
  5. Create a new directory named Axial_Fan 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 Axial_Fan 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 3.

Set Up Flow

Set the General Simulation Parameters

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


    Figure 4.
    The Setup dialog opens.
  2. Under the Physics models setting:
    1. Verify that Time marching is set to Steady.
    2. Select Spalart-Allmaras as the Turbulence model.


    Figure 5.
  3. Click the Solver controls setting and verify that the parameters are set as shown in the figure below.


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

Assign Material Properties

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


    Figure 7.
  2. Verify that the Air material has been assigned to all three volumes.
  3. Click on the guide bar to exit the tool.

Define the Fan Component

  1. From the Flow ribbon, click the arrow next to the Domain tool set, then select Fan Component.


    Figure 8.
  2. Select the middle solid as the fan component volume.


    Figure 9.
  3. On the guide bar, click Surfaces then select the face shown below as the inlet of the fan component.


    Figure 10.
  4. From the View Controls toolbar, change the geometry visualization mode from Shaded Geometry to Transparent Geometry.
    This allows you to view the axis direction vector in the next step.


    Figure 11.
  5. On the guide bar, click Axis.
    In the modeling window, you can see that the axis points in the -X direction.
  6. Click in the microdialog to flip the axis vector to the +X direction.


    Figure 12.
  7. Enter 0.06 for Thickness.


    Figure 13.
  8. Click beside P-Q Curve Type to open the Profile Editor.
  9. Click , browse to the location where you saved AxialCoefficient.csv, and open it.


    Figure 14.
  10. On the guide bar, click to execute the command and exit the tool.
  11. Save the model.

Define Flow Boundary Conditions

  1. From the Flow ribbon, Profiled tool group, click the Volumetric Flow Rate tool.


    Figure 15.
  2. Click the inlet face highlighted in the figure below.


    Figure 16.
  3. In the microdialog, enter 0.322675 for the flow rate.


    Figure 17.
  4. On the guide bar, click to execute the command and exit the tool.
  5. Click the Outlet tool.


    Figure 18.
  6. Select the face highlighted in the figure below and then click on the guide bar.


    Figure 19.

Generate the Mesh

To focus on the solver setup, the mesh settings are predefined in the input file given to you.
  1. From the Mesh ribbon, click the Volume tool.


    Figure 20.
  2. In the Meshing Operations dialog, set the Average element size to 0.01 and the Mesh growth rate to 1.1 (if not set already).


    Figure 21.
  3. 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.
  4. Save the model.

Run AcuSolve

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


    Figure 22.
    The Launch AcuSolve dialog opens.
  2. Set the Parallel processing option to Intel MPI.
  3. Optional: Set the number of processors to 4 or 8 based on availability.
  4. Leave the remaining options as default and click Run to launch AcuSolve.


    Figure 23.

Post-Process with the Plot Tool

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


    Figure 24.
  2. Click next to the Library tab.
  3. Keep the X-axis set to Step. For the Y-axis, click the tree browser and select pressure under Surface Output.
  4. Check the boxes for FAN_Inlet and FAN_outlet under Selector.


    Figure 25.
  5. Click Create to plot the surfaced average pressure.


    Figure 26.

    From the above figure, the pressure got stabilized at around the 6th iteration and remains constant with pressure difference between the FAN_inlet and FAN_outlet of 423.97 Pa for a given volume flow rate 0.322675 m3/sec (~ 1212.3 m3/hr), which is very near compared to the reference pressure increase of 424.9 Pa.

Summary

In this tutorial, you successfully learned how to set up and solve a simulation involving a fan component using HyperWorks CFD. You imported the geometry and then defined the simulation parameters, fan component, and flow boundary conditions. Once the solution was computed, you used the HW-CFD Plot tool to plot the pressure at fan inlet and fan outlet.