# 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, copy HyperWorksCFD_tutorial_inputs.zip from <Altair_installation_directory>\hwcfdsolvers\acusolve\win64\model_files\tutorials\AcuSolve to a local directory. 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 meshing.

## 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.

## 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.
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.

## Set Up Flow

### Set the General Simulation Parameters

1. From the Flow ribbon, click the Physics tool.
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.
3. Click the Solver controls setting and verify that the parameters are set as shown in the figure below.
4. Close the dialog and save the model.

### Assign Material Properties

1. From the Flow ribbon, click the Material tool.
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.
2. Select the middle solid as the fan component volume.
3. On the guide bar, click Surfaces then select the face shown below as the inlet of the fan component.
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.
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.
7. Enter 0.06 for Thickness.
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.
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.
2. Click the inlet face highlighted in the figure below.
3. In the microdialog, enter 0.146 for the flow rate.
4. On the guide bar, click to execute the command and exit the tool.
5. Click the Outlet tool.
6. Select the face highlighted in the figure below and then click on the guide bar.

## 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.
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).
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.
The Launch AcuSolve dialog opens.
2. Enter the following text in the additional arguments field: -tlog -lprobe.
This will instruct AcuSolve to launch the AcuTail and AcuProbe windows, which can be used to monitor the solution as the simulation progresses.
3. Set the Parallel processing option to Intel MPI.
4. Optional: Set the number of processors to 4 or 8 based on availability.
5. Leave the remaining options as default and click Run to launch AcuSolve.

## 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 > FanComponent-FanComponent > 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 AxialFan-1.1 SolidBody_2_2 internal > Pressure.
11. Right-click on pressure and select Copy name.
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.

As shown in the plot below, for the given problem, the pressure rise is 494.514 Pa.

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 494.514 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 defined a user-function in AcuProbe in order to create a plot of the pressure rise across the fan volume.