ACU-T: 2300 Atmospheric Boundary Layer Problem – Flow Over Building

Prerequisites

Prior to starting this tutorial, you should have already run through the introductory HyperWorks tutorial, ACU-T: 1000 HyperWorks UI Introduction. To run this simulation, you will need access to a licensed version of HyperMesh and AcuSolve.

Prior to running through this tutorial, copy HyperMesh_tutorial_inputs.zip from <Altair_installation_directory>\hwcfdsolvers\acusolve\win64\model_files\tutorials\AcuSolve to a local directory. Extract ACU-T2300_Building.hm from HyperMesh_tutorial_inputs.zip.

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 addressed in this tutorial is shown schematically in Figure 1. As an example, this problem shows the capability of Atmospheric Boundary Layer modelling in AcuSolve.



Figure 1.

In this tutorial, you will simulate the air flow over a building with a ground roughness of 0.03. In this case, User Defined Atmospheric Roughness Type is considered.

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-T2300_Building.hm and click Open.
  4. Click File > Save As.
    The Save Model As dialog opens.
  5. Create a new directory named Building_ABL 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 Building as the file name for the database, or choose any name of your preference.
  7. Click Save to create the database.

Set the General Simulation Parameters

  1. Go to the Solver Browser, expand 01.Global, then click PROBLEM_DESCRIPTION.
  2. In the Entity Editor, enter Building as the Title.
  3. Verify that the Analysis Type is set to Steady State.
  4. Set the Turbulence Model to Spalart Allmaras.


    Figure 2.
  5. In the Solver Browser, expand the 02.SOLVER_SETTINGS group then click SOLVER_SETTINGS to open it in the Entity Editor.
  6. Set Convergence Tolerance 0.001.
  7. Set the Relaxation Factor to 0.4.


    Figure 3.

Set Up Boundary Conditions and Material Model Parameters

In this step, you will define the Boundary Conditions (BCs) for the problem and assign material properties to the fluid volume.

Set Up Material Model Parameters

  1. In the Solver Browser, expand 02.Materials > FLUID then click on Air_HM.
  2. Set the Material Type to FLUID if it's not already set. Leave the remaining default values as is.


    Figure 4.

Set Up Fluid Volume Material

  1. In the Solver Browser, expand 11.Volumes > FLUID then click on fluid.
  2. Set the Type to FLUID.
  3. Set the Material to Air_HM.


    Figure 5.

Set Up Boundary Conditions

  1. In the Solver Browser, expand 12.Surfaces > INFLOW then click on Inflow. In the Entity Editor,
    1. Set the Type to INFLOW.
    2. Set the Inflow Type to Atmospheric.
    3. Set the Atmospheric Roughness Type to User value.
    4. Set the Atmospheric Ground Roughness to 0.001.
    5. Set the Atmospheric Reference Vel Type to Friction velocity.
    6. Set the Atmospheric Friction Velocity to 0.106.
    7. For Atmospheric Ground Origin, set the coordinates to (0, 0, 0).
    8. For Atmospheric Ground Normal Direction, set the coordinates to (0, 0, 1).
    9. For Atmospheric Flow Direction, set the coordinates to (1, 0, 0).


    Figure 6.
  2. Expand OUTFLOW then click on Outflow. In the Entity Editor, change the Type to OUTFLOW.


    Figure 7.
  3. Expand WALL then click on Building. In the Entity Editor, change the Type to WALL.


    Figure 8.
  4. Under WALL, click on Wall. In the Entity Editor,
    1. Change the Type to WALL.
    2. Set the Roughness height to 0.03.


    Figure 9.
  5. Expand SLIP then click on Slip. In the Entity Editor, change the Type to SLIP.


    Figure 10.

Set Up Nodal Initial Conditions

  1. In the Solver Browser, expand 01.GLOBAL > 03.NODAL_INITIAL_CONDITIONS then click on NODAL_INITIAL_CONDITION.
  2. Verify that the Pressure Default value is 0.0.
  3. Verify that the Velocity in all direction is 0.0.
  4. Change the Eddy viscosity to 0.0001


    Figure 11.

Compute the Solution

In this step, you will launch AcuSolve directly from HyperMesh and compute the solution.

Run AcuSolve

  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. The Output time steps can be set to All or Final. Since this is a steady state analysis, the Final time step output is sufficient.
  5. Leave the remaining options as default and click Launch to start the solution process.


    Figure 12.

Post-Process the Results with AcuFieldView

Once the solution has converged, close the AcuProbe and AcuTail windows. Go to the HyperMesh window and close the AcuSolve Control tab.

Click on the AcuFieldView icon to launch the AcuFieldView dialog.

Load Model and Results

  1. In the AcuFieldView dialog, click next to File.
  2. 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 Building.1.Log
  3. For Solver exec dir, click , then navigate to the AcuSolve installation directory (<AcuSolve_installation_directory>hwcfdsolvers/acusolve/win64/) and select the bin folder if it is not selected by default.
  4. Click Launch.
    All the surfaces, with mesh, are displayed in AcuFieldView.
  5. Click Viewer Options.


    Figure 13.
  6. In the Viewer Options dialog:
    1. Deselect Perspective to turn off the perspective view.
    2. Click Axis Markers to disable the axis markers.
    3. Click Close.
  7. On the toolbar, click the Colormap icon .
  8. In the Scalar Colormap Specification dialog, click Background and select White.
  9. Close the Scalar Colormap Specification dialog.
  10. Click the Toggle Outline icon on the toolbar to turn off the outline display.

Coordinate the Surface for Showing Velocity Magnitude on the Y Plane

  1. From Boundary Surface dialog, Surafce tab, disable the Visibility option for the active boundary surfaces.
  2. Click to open the Coordinate Surface dialog.
  3. Click Create to create a new Coordinate Surface.
  4. Set the Coord Plane to Y.
  5. Change the Coloring to Scalar.
  6. Set the Display Type to Smooth.
  7. In the Scalar Function list, select velocity_magnitude as the scalar function to be displayed.
  8. In the Colormap tab, change Scalar Coloring to Local.
  9. In the Legend tab, check the Show Legend checkbox to display the velocity magnitude on the coordinate plane.
  10. From the Defined Views, select viewing direction as -Y.


    Figure 14.

Coordinate the Surface for Showing Velocity Vectors on the Y Plane

  1. From the Surface tab, disable the Visibility option for Surface ID 1.
  2. Click Create to create a new Coordinate Surface.
  3. Set the Coord Plane to Y.
  4. Change the Coloring to Scalar.
  5. In the Scalar Function list, select velocity_magnitude as the scalar function to be displayed.
  6. Set the Display Type to Vectors.
  7. Next to Vectors, click Options.
  8. Set the VECTOR HEAD type to 2D.
  9. Activate Head Scaling and set it to 0.2.
  10. Set the Length Scale to 1.
  11. Activate the Skip option and set the value to 75%.


    Figure 15.

Coordinate the Surface for Showing Velocity Magnitude on the Z Plane

  1. Delete the Coordinate Surfaces with Surface Ids 1 and 2.
  2. Click Create to create a new Coordinate Surface.
  3. Set the Coord Plane to Z.
  4. Change the Coloring to Scalar.
  5. Set the Display Type to Smooth.
  6. In the Scalar Function list, select velocity_magnitude as the scalar function to be displayed.
  7. In the Colormap tab, change Scalar Coloring to Local.
  8. In the Legend tab, check the Show Legend checkbox to display the velocity magnitude on the coordinate plane.
  9. From the Defined Views, select viewing direction as +Z.


    Figure 16.

Coordinate the Surface for Showing Velocity Vectors on the Z Plane

  1. From the Surface tab, disable the Visibility option for Surface ID 1.
  2. Click Create to create a new Coordinate Surface.
  3. Set the Coord Plane to Z.
  4. Change the Coloring to Scalar.
  5. In the Scalar Function list, select velocity_magnitude as the scalar function to be displayed.
  6. Set the Display Type to Vectors.
  7. Next to Vectors, click Options.
  8. Set the VECTOR HEAD type to 2D.
  9. Activate Head Scaling and set it to 0.2.
  10. Set the Length Scale to 1.
  11. Activate the Skip option and set the value to 75%.


    Figure 17.

Summary

In this tutorial, you worked through a basic workflow to set up a CFD model, carry out a CFD simulation, then post-process the results using HyperWorks products, namely AcuSolve, HyperMesh and AcuFieldView. You started by importing the model in HyperMesh. Then, you defined the simulation parameters and launched AcuSolve directly from within HyperMesh. Upon completion of solution by AcuSolve, you used AcuFieldView to post-process the results and create contour plots.