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

## Prerequisites

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

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 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.

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.
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.

## 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.

### 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.

### 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).
2. Expand OUTFLOW then click on Outflow. In the Entity Editor, change the Type to OUTFLOW.
3. Expand WALL then click on Building. In the Entity Editor, change the Type to WALL.
4. Under WALL, click on Wall. In the Entity Editor,
1. Change the Type to WALL.
2. Set the Roughness height to 0.03.
5. Expand SLIP then click on Slip. In the Entity Editor, change the Type to SLIP.

## 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

## 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.

## Post-Process the Results with HyperWorks HV

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

Start HyperView from the Windows Start menu by clicking Start > Altair <version> > HyperWorks HV.

1. Once the HyperWorks HV window is loaded, 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 Building.1.Log.
4. Click Open.
5. Click Apply in the panel area to load the model and results.

### Coordinate the Surface for Showing Velocity Magnitude on the Y Plane

1. From the View Controls toolbar, click to create a new coordinate surface on the y plane.
2. Click in the microdialog to only display the section cut.
3. Click the Left face on the View Cube to orient the section cut.
4. From the Results ribbon, click the Contour tool.
5. In the panel area, under Result type, verify that Velocity (v) and Mag are selected.
6. Click the Components entity selector. In the Extended Entity Selection dialog, select Displayed.
7. Click Apply.

### Coordinate the Surface for Showing Velocity Vectors on the Y Plane

1. From the Results ribbon, click the Vector tool.
2. In the panel area, under Result type, verify that Velocity (v) is selected.
3. Click the arrow next to the Components entity selector and select Sections.
4. Activate X+Y+Z for Resultant.
5. Set Size scaling to 0.05.
6. Click Apply.

## 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 HyperWorks HV. 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 HyperWorks HV to post-process the results and create contour and vector plots.