# 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 HyperWorks tutorial, ACU-T: 1000 HyperWorks UI Introduction, and have a basic understanding of AcuSolve and HyperMesh. 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-T5100_AxialFanComponent.hm and AxialCoefficient.txt 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 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 0.146 m3/sec (~525.35 m3/hr). The problem is simulated as a steady state run and the pressure rise across the fan region is computed.

## 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-T5100_AxialFanComponent.hm and click Open.
4. Click File > Save As.
The Save Model As dialog opens.
5. Create a new directory named AxialFan 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 AxialFan 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, change the Turbulence model to Spalart Allmaras.
3. Ensure that the Analysis type is Steady State.

## Set the Boundary Conditions

By default, all components are assigned to the wall boundary condition. In this step, you will change them to the appropriate boundary conditions and assign material properties to the fluid volumes.
1. In the Solver Browser, expand 12.Surfaces > WALL.
2. Click Inlet. In the Entity Editor,
1. Change the Type to INFLOW.
2. Set the Inflow type to Flow rate.
3. Set the Flow rate 0.146 m3/sec.
3. Click Fan_Inlet. In the Entity Editor,
1. Change the Type to FAN_COMPONENT.
2. Set the Rotational speed to 377 rad/sec.
3. Set the Tip radius to 0.11 m.
4. Set the Fan thickness to 0.06 m.
5. Change the Axial coefficient type to Piecewise Bilinear.
6. For the Axial coefficient curvefit file, click the open file icon and browse to the location where you saved AxialCoefficient.txt and select it. Click Open.
7. Verify that the Radial coefficient and Tangential coefficient are set to 0.
4. Click Outlet. In the Entity Editor, change the Type to OUTFLOW.
5. Click Walls. In the Entity Editor, verify that the Type is set to WALL.

When component type is assigned as Wall, all the elements in the surface set are automatically re-grouped into surface sets based on the parent volume they belong to and also if they are internal or external. Auto_Wall is an advanced feature in AcuSolve which takes care of this process internally, without you having to do it manually and hence reducing the number of steps in the workflow.

6. Click Downstream_Duct. In the Entity Editor,
1. Change the Type to FLUID.
2. Select Air_HM as the Material.
7. Similarly, set the Fan and Upstream_Duct component Type to FLUID and select Air_HM as the Material for both components.
8. Save the model.

## 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 with AcuProbe

As the solution progresses, the AcuProbe window is launched automatically. AcuProbe can be used to monitor various variables over solution time.

1. In the AcuProbe Data Tree, expand Residual Ratio.
2. Right-click on Final and select Plot All.
Note: You might need to click on the toolbar in order to properly display the plot.
3. Once the solution is converged, right-click again on Final and select Plot None.
4. Click the User Function icon from the toolbar.
5. In the dialog, enter the Name as dP.
6. In the Data Tree, expand Surface Output > Fan_Inlet > Pressure
7. Right-click on pressure and select Copy name.
8. In the Function field of the User Function dialog, type Fan_In = then paste the name you just copied.
9. Type Fan_Out = on a new line.
10. In the Data Tree, expand Surface Output > AUTO Fan internal > Pressure.
11. Right-click on pressure and select Copy name.
Here, the surface output (AUTO Fan internal) is the Auto_Wall generated surface output corresponding to the internal surface at the outlet of the fan component volume.
12. Paste the name in the Function field after Fan_Out =.
13. On a new line, type value = Fan_Out - Fan_In.
Note: The word “value” is case sensitive and should always be in lower case. If you use a capital letter, an error window appears.
14. Click Apply.
15. In the Data Tree, expand User function then right-click on dP and select Plot.

You can zoom into the plot by clicking then selecting an area at the end of the curve. As shown in the figure below, for the given flow rate of 525.35 m3/hr (0.146 m3/sec), the pressure rise is 494.182 Pa.

## Summary

In this tutorial you successfully learned how to set up and solve a simulation involving a fan component. You imported the meshed geometry and then assigned the material properties and boundary conditions to all the regions. Once the solution was computed, you defined a user function to create a plot of the pressure rise across the fan component volume.