ACU-T: 5001 Blower - Transient (Sliding Mesh)

Prerequisites

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 Centrifugal Air Blower with Moving Reference Frame (Steady) and kept the solution in your working directory. It is assumed that you have some familiarity with HyperMesh, HyperMesh, and HyperView.

Before you begin, copy the file(s) used in this tutorial to your working directory.

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 discussed in this tutorial is shown schematically in Figure 1. The simulation is divided into two components, steady state and transient. The steady state solution will be computed first and then projected onto the mesh and used as the initial state for the transient simulation. Please refer to the tutorial ACU-T: 5000 Centrifugal Air Blower with Moving Reference Frame (Steady) to learn the step by step procedure to obtain the steady state solution for this problem. Once the transient solution is computed, you will post-process the results using HyperView.


Figure 1.

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 ACU-T5001_BlowerTransient.hm and click Open.
  4. Click File > Save As.
    The Save Model As dialog opens.
  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 as the file name for the database, or choose any name of your preference.
  7. Click Save to create the database.

Run the Steady State Simulation

In this step, you will run the steady state simulation with the model file provided and then create the nodal initial condition files needed for the transient simulation.
  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. Leave the remaining options as default and click Launch to start the solution process.
  5. Once the solution has converged, close the AcuTail and AcuProbe windows. Also, close the Solver job launcher and the AcuSolve Control tab.
  6. Start AcuSolve Command Prompt from the Windows Start menu by clicking Start > Altair <version> > AcuSolve Cmd Prompt .
  7. In the Command Prompt, change the directory to the working directory using the cd command.
  8. Type the command acuProj -crd HYPERMESH.DIR\Blower_Transient.crd -run 1 and press Enter.
  9. Verify that the working directory is populated with the new files Blower_Transient.pres.nic, Blower_Transient.vel.nic, and Blower_Transient.eddy.nic
  10. Move these files into the HYPERMESH.DIR directory.

Set the Transient Simulation Parameters

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

Set the General Simulation Parameters

  1. Go to the Solver Browser, expand 01.Global, then click PROBLEM_DESCRIPTION.
  2. Change the Analysis type to Transient.
  3. Set the Turbulence model to Spalart Allmaras.
  4. Set the Mesh type to Fully Specified.


    Figure 2.

Specify the Solver Settings

  1. In the Solver Browser, click 02.SOLVER_SETTINGS under 01.Global.
  2. Set the Max time steps to 0 and press Enter.
  3. Set the Final time to 0.12.
  4. Set the Initial time increment to 0.00111
  5. Change the Max stagger iterations to 2.
  6. Change the Relaxation factor to 0.


    Figure 3.

Set the Nodal Output Frequency

  1. In the Solver Browser, expand 17.Output then click on NODAL_OUTPUT.
  2. Set the Time step frequency to 1.
  3. Turn On the Output initial condition field.


    Figure 4.
  4. Save the model.

Define Mesh Motion and Set Up Boundary Conditions

Create Mesh Motion

  1. In Solver Browser, right-click on 06.Mesh_Motion and select Create.
  2. Rename the mesh motion as Impeller_Motion in the Entity Editor.
  3. Set the Type to Rotation.
  4. Enter (0, 0, 0.05) as the coordinates of the Rotation center.
  5. Set the Angular velocity - Z to -157.08 rad/sec.


    Figure 5.

Modify the Boundary Conditions

  1. In the Solver Browser, expand 11.Volumes > FLUID.
  2. Click Fluid_Impeller. In the Entity Editor,
    1. Set the Reference frame to Unspecified.
    2. Set the Mesh motion to Impeller_Motion.


    Figure 6.

Specify the Nodal Initial Conditions

  1. In the Solver Browser, expand 01.Global then click on 03.NODAL_INITIAL_CONDITION.
  2. In the Entity Editor, under the Pressure tab,
    1. Set the Type to Nodal Values.
    2. Change Select nodes by to NIC file.
    3. Click the open file icon in the NIC file field and browse to the HYPERMESH.DIR folder located in your working directory. Select the file Blower_Transient.pres.nic.


    Figure 7.
  3. Repeat the above step for the Velocity and Eddy viscosity fields. Select the Blower_Transient.vel.nic and Blower_Transient.eddy.nic files, respectively.
  4. Save the model.

Compute the Solution

In this step, you will launch AcuSolve directly from HyperMesh and compute the solution.
  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. Observe that the Output time steps is set to All. This means that AcuSolve will write solution at all the time steps specified in the Nodal Output Frequency.
  5. Leave the remaining options as default and click Launch to start the solution process.


    Figure 8.
    Once the solution is launched, the AcuSolve Control tab opens. Also, the AcuTail and AcuProbe windows are launched automatically in which the solution progress can be monitored.

Post-Process the Results with HyperView

Once the solution has converged, close the AcuProbe and AcuTail windows. Go to the HyperMesh window and 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 BlowerTransient.2.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 Animation

In this step, you will start by creating a pressure contour on a cut plane on the z-axis. Then, you will create an animation of the pressure contour.
  1. Click on the Results toolbar to open the Contour panel.
  2. In the panel area, set the Result type to Pressure (s).
  3. Click Apply to display the velocity contour.
  4. In the panel area, under the Display tab, turn off the Discrete color option.


    Figure 9.
  5. Click the Legend tab then click Edit Legend. In the dialog, change the Type to Dynamic scale and the Numeric format to Fixed then click OK.


    Figure 10.


    Figure 11.
  6. Click on the Display toolbar to open the Section Cut panel.
  7. In the panel area, click Add.
  8. Under the Define plane section, change the plane to Z-Axis then click Apply.
  9. Set the Z-coordinate of the Base to 0.05 then press Enter
  10. Under the Display options section, activate the Cross section option.
  11. Click Girdline.... In the dialog, turn off the Show Grid Line option then click OK.


    Figure 12.
  12. Orient the display to the xy-plane by clicking on the Standard Views toolbar.


    Figure 13.
  13. From the Animation toolbar, click the Animation controls icon.


    Figure 14.
  14. In the panel area, set the Max Frame Rate to 15 Frames/Sec by dragging the slider.
  15. Click on the Start/Pause Animation icon to play the velocity magnitude animation.


    Figure 15.

Create Streamlines

  1. Click on the Display toolbar to open the Section Cut panel.
  2. In the panel area, toggle off the Section 1 check box.
    This will turn off the display of the section cut, showing the complete model.
  3. In the Results Browser, expand the list of Components and turn off all components except the Inlet, Outlet, AUTO Fluid_Main wall and AUTO Fluid_Impeller wall.


    Figure 16.
  4. Change the element display mode to Transparent Elements and Feature Lines.


    Figure 17.
  5. Rotate the model so that you have a clear view of all the components that are being displayed.
  6. Go to the Contour panel, change the Result type to Velocity (v), and set the drop-down menu below it to Mag.
  7. Click Apply to plot the velocity magnitude.


    Figure 18.
  8. Click on the Results toolbar to open the Streamlines panel.
  9. In the panel area, click Add, then change the Rake type to Area.
  10. Click the Component entity collector then select By ID.
  11. In the Select by ID dialog, enter 6 in the value field of Component ID then click OK.
  12. In the panel area, change the Integration mode to Both.
  13. Set the Number of seeds to 50.
  14. Toggle on the Draw as tube checkbox then click Create Streamlines to generate the streamlines.


    Figure 19.
    This will generate streamlines originating from the Inlet surface with seeds that are distributed over the surface area of the fan blades and end at the outlet.


    Figure 20.
  15. In the panel area, click the Tracers tab.
  16. Change the Pule to Endless.
  17. Leave the other default values unchanged then click Create to generate the tracers.


    Figure 21.


    Figure 22.

Summary

In this tutorial, you successfully learned how to set up and solve a transient simulation of a centrifugal air blower using the sliding mesh approach. You started by importing the meshed geometry and then ran the steady state simulation. Then, you used the steady state result as the starting point for the transient simulation using the AcuProj tool to specify the nodal initial conditions and then solved the transient simulation using the sliding mesh approach instead of the moving reference frame approach. Once the transient solution was computed, you launched HyperView and created an animation of pressure contours and streamlines.