ACU-T: 5100 Modeling of a Fan Component: Axial Fan

This tutorial provides the instructions for setting up, solving and viewing results for simulation of flow inside a pipe with an interior fan placed at the middle of the pipe. This middle portion of the pipe is considered to be fan volume which is modeled using the Fan_Component parameter. In this simulation, flow is passed from the pipe inlet and it enters the fan in axial direction and exits at the outlet causing pressure rise due to the fan. A lumped fan model is used to obtain fan pressure rise for a known inlet volume flow rate. This tutorial is designed to introduce the user to modeling concepts related to Fan_Components for axial fans.

The basic steps in any CFD simulation are shown in ACU-T: 2000 Turbulent Flow in a Mixing Elbow. The following additional capabilities of AcuSolve are introduced in this tutorial:
  • Specifying FAN_COMPONENT parameter in AcuConsole
  • Setting up Inflow boundary condition with volumetric flow rate

Prerequisites

You should have already run through the introductory tutorial, ACU-T: 2000 Turbulent Flow in a Mixing Elbow. It is assumed that you have some familiarity with AcuConsole, AcuSolve, and AcuFieldView. You will also need access to a licensed version of AcuSolve.

Prior to running through this tutorial, copy AcuConsole_tutorial_inputs.zip from <Altair_installation_directory>\hwcfdsolvers\acusolve\win64\model_files\tutorials\AcuSolve to a local directory. Extract AxialFan.x_t from AcuConsole_tutorial_inputs.zip.

The color of objects shown in the modeling window in this tutorial and those displayed on your screen may differ. The default color scheme in AcuConsole is "random," in which colors are randomly assigned to groups as they are created. In addition, this tutorial was developed on Windows. If you are running this tutorial on a different operating system, you may notice a slight difference between the images displayed on your screen and the images shown in the tutorial.

Analyze the Problem

An important step in any CFD simulation is to examine the engineering problem at hand and determine the important parameters that need to be provided to AcuSolve. Parameters can be based on geometrical elements (such as inlets, outlets, or walls) and on flow conditions (such as fluid properties, velocity, or whether the flow should be modeled as turbulent or as laminar).


Figure 1. Axial Fan Model Used for the Simulation

Figure 1 shows a simple axial fan component problem where fan is an interior fan with thickness “t” and tip radius as “r”. In this simulation, flow is passed from the pipe inlet and it enters the fan in axial direction and exits at the outlet causing pressure rise due to the fan. This fan pressure rise can be simulated for a given volume flow rate at the inlet surface which will be assigned as the inflow boundary condition. The volume flow rate at the inlet surface is considered to be 525.35 m3/hr.

The middle portion of the pipe is the Fan Component volume which has both Fan_Inlet and Fan_Outlet. The FAN_COMPONENT parameters are assigned to Fan_Inlet surface through Advance problem definition option. Basically, the fan model is applied to a surface, and the pressure jumps across that surface to model the effect of the fan. The outlet of the pipe geometry is assigned with Outflow BC to model the flow exit whereas the outer walls are defined to be Wall BC with slip condition. The fluid material considered for this simulation is air with density=1.225 kg/m3, viscosity=1.781e-005 kg/m-s.

The FAN_COMPONENT directly computes a body force term to yield the pressure rise within the volume of interest. It accomplishes this based on the following approach:
  • Evaluate the flow rate at the inlet to the domain that is assigned as a fan component (that is, the surface on which you have assigned the FAN_COMPONENT condition)
  • Evaluate the pressure rise resulting from this flow rate based on the fan curve that the user has input
  • Compute a body force per unit length that yields the required pressure rise based on fan_length input parameter and the target pressure rise.
  • The body force can be specified to be a function of the flow direction, that is, axial velocity, radial velocity, tangential velocity or combination of all these three.
  • Assign the body force to all elements of the element set that the FAN_COMPONENT is assigned to.

So, when deciding how to set up the FAN_COMPONENT model, you also need to consider how your fan is modeled. If it is purely axial flow, then the relevant pressure rise relationship is just in the axial direction, and the fan_length is the distance from inlet to outlet of the fan section.

Basically the FAN_COMPONENT is modelled by adding axial, radial and tangential body forces to the momentum equations. For an axial fan type, these forces increase the pressure across the component by

Δ P axial =  1 2 α axial ρ u tip 2 +  1 2 ρ u ¯ 2

where α a x i a l : axial coefficient

ρ : density

u t i p : tip velocity = ω r tip

ω : fan angular rotational speed (rad/sec)

r t i p : fan tip radius

u ¯ : mass averaged velocity through the inlet (m/sec)

Since piecewise_bilinear curve fit values used in FAN_COMPONENT are functions of the normalized flow rate (Q1) and axial coefficient (αaxial), you need to convert them from the fan performance curve.

Normalized flow rate (Q1): Actual flow rate ( Q ) Inlet area ( A )*Utip

Axial co-efficient (αaxial) = 2ΔP− ρ u ¯ 2 ρ u tip 2

For example, evaluate the axial coefficients and normalized flow rate from the fan performance data. The following tables are inputs for the calculations.
Table 1. Fan Characteristics
Fluid Density 1.225 kg/m3
Tip Radius ( r t i p ) 0.11 m
Rotational Speed ( ω ) 3600 RPM = 376.99 rad/sec
Inlet Area, Ai 0.03801 m2
Tip Velocity ( u t i p ) 41.47 m/sec
Table 2. Fan Performance Parameters
  Volume Flow Rate (Q), m3/hr Pressure rise (ΔP), Pa
1 525.35 494.91
2 890.21 474.63
3 1161.63 424.9
4 1272.76 389.11
5 1356.57 350.42
6 1431.84 308.18
7 1494.69 268.35
8 1551.39 230.89
You can calculate the normalized flow rate and axial coefficient for first two volume flow rates (Q) from Table 2. The same procedure is followed for the other volume flow rates.
  1. For Q = 525.35 m3/hr:

    Q1 = Q A * U t i p = 0.0926

    α a x i a l = 2 Δ P −   ρ u ¯ 2 ρ u t i p 2 = 0.4613

  2. For Q = 890.21 m3/hr:

    Q1 = Q A * U t i p = 0.1569

    α a x i a l = 2 Δ P −   ρ u ¯ 2 ρ u t i p 2 = 0.426

In this manner you can calculate Ql and αaxial for the remaining volume flow rates, shown in the following table.
Table 3. Normalized Flow Rates and Axial Coefficients
S. No Normalized Flow Rate (Q1) Axial Coefficients ( αaxial )
1 0.0926 0.4613
2 0.1569 0.426
3 0.2047 0.3615
4 0.2243 0.3191
5 0.2391 0.2755
6 0.2523 0.2289
7 0.2634 0.1854
8 0.2734 0.1445
The same information is entered as input for axial curve fit values for the FAN_COMPONENT parameter as shown in Figure 2.


Figure 2. Fan Component Array Editor

The first column of array is the normalized radius which varies between 0 and 1 which implies that at the centre of the fan, this value is 0 whereas at the tip of the fan, this value is 1.

Define the Simulation Parameters

Start AcuConsole and Create the Simulation Database

In this tutorial, you will begin by creating a database, populating the geometry-independent settings, loading the geometry, creating volume and surface groups, setting group parameters, adding geometry components to groups, and assigning mesh controls and boundary conditions to the groups. Next you will generate a mesh and run AcuSolve to solve for the number of time steps specified. Finally, you will visualize some characteristics of the results using AcuFieldView.

In the next steps you will start AcuConsole, and create the database for storage of the simulation settings.

  1. Start AcuConsole from the Windows Start menu by clicking Start > Altair <version> > AcuConsole.
  2. Click the File menu, then click New to open the New data base dialog.
  3. Browse to the location that you would like to use as your working directory.
    This directory is where all files related to the simulation will be stored. The AcuConsole database file (.acs) is stored in this directory. Once the mesh and solution are created, additional files and directories will be created within this directory.
  4. Create a new directory in this location. Name it Axial_Fan and open it.
  5. Enter AxialFan as the file name for the database.
    Note: In order for other applications to be able to read the files written by AcuConsole, the database path and name should not include spaces.
  6. Click Save to create the database.

Set General Simulation Parameters

In next steps you will set parameters that apply globally to the simulation. To make this simple, the basic settings applicable for any simulation can be filtered using the BAS filter in the Data Tree Manager. This filter enables display of only a small subset of the available items in the Data Tree and makes navigation of the entries easier.

The physical models that you define for this tutorial correspond to steady state, turbulent flow.

  1. Click BAS in the Data Tree Manager to switch to basic view in the Data Tree.


    Figure 3.
  2. Double-click the Global Data Tree item to expand it.
    Tip: You can also expand a tree item by clicking next to the item name.


    Figure 4.
  3. Double-click Problem Description to open the Problem Description detail panel.
  4. Enter AcuSolve Tutorial as the Title.
  5. Enter Axial Fan as the Sub title.
  6. Change the Analysis type to Steady State.
  7. Change the Turbulence equation to Spalart Allmaras.


    Figure 5.

Set Solution Strategy Parameters

In the next steps you will set parameters that control the behavior of AcuSolve as it progresses during the solution.

  1. Double-click Auto Solution Strategy to open the Auto Solution Strategy detail panel.
  2. Check that the Analysis type is set to Steady State.
  3. Set the Max time steps as 50.
  4. Set the Relaxation factor to 0.5.
  5. Check the Flow and Turbulence are set to On.


    Figure 6. Auto Solution Detail Panel

Set Material Model Parameters

AcuConsole has three pre-defined materials, Air, Aluminum, and Water, with standard parameters defined. In the next steps you will verify that the pre-defined material properties of air match the desired properties for this problem.
  1. Double-click Material Model in the Data Tree to expand it.


    Figure 7.
  2. Double-click Air in the Data Tree to open the Air detail panel.

    The material type for air is Fluid. Fluid is the default material type for any new material created in AcuConsole.

  3. Click the Density tab. The density of air is 1.225 kg/m3.
  4. Click the Viscosity tab. The viscosity of air is 1.781 x 10-5kg/m – sec.
  5. Save the database to create a backup of your settings. This can be achieved with any of the following methods.
    • Click the File menu, then click Save.
    • Click on the toolbar.
    • Click Ctrl+S.
    Note: Changes made in AcuConsole are saved into the database file (.acs) as they are made. A save operation copies the database to a backup file, which can be used to reload the database from that saved state in the event that you do not want to commit future changes.

Import the Geometry and Define the Model

Import the Geometry

You will import the geometry in the next part of this tutorial. You will need to know the location of AxialFan.x_t in order to complete these steps. This file contains information about the geometry in Parasolid ASCII format.
  1. Click File > Import.
  2. Browse to the directory containing AxialFan.x_t.
  3. Change the file name filter to Parasolid File (*.x_t *.xmt *X_T …).
  4. Select AxialFan.x_t and click Open to open the Import Geometry dialog.


    Figure 8.

    For this tutorial, the default values for the Import Geometry dialog are used to load the geometry. If you have previously used AcuConsole, be sure that any settings that you might have altered are manually changed to match the default values shown in the figure. With the default settings, volumes from the CAD model are added to a default volume group. Surfaces from the CAD model are added to a default surface group. You will work with groups later in this tutorial to create new groups, set flow parameters, add geometric components, and set meshing parameters.

  5. Click Ok to complete the geometry import.


    Figure 9.

Apply Volume Parameters

Volume groups are containers used for storing information about a volume region. This information includes the list of geometric volumes associated with the container, as well as attributes such as material models and mesh size information.

When the geometry was imported into AcuConsole, all volumes were placed into the "default" volume container.

In the next steps you will rename the default volume group container, assign the materials for that group, and set mesh motion for the fluid volume.

  1. Click BAS in the Data Tree Manager to switch to basic view in the Data Tree.
  2. Expand the Model Data Tree item.
  3. Expand Volumes. Toggle the display of the default volume container by clicking and next to the volume name.
    Note: You may not see any change when toggling the display if Surfaces are being displayed, as surfaces and volumes may overlap.
  4. Right-click on Volumes and select Volume Manager.
  5. In the Volume Manager, click New twice to create two new volume groups.
  6. Turn off the display of all volumes, except default.
  7. Rename the default volume to UpstreamDuct.
  8. Rename Volume 1 and Volume 2, and set the columns as per the image below:


    Figure 10.
  9. Assign the respective volumes to their volume groups:
    1. In the Fan row, click Add To.
    2. Select the volume as shown in figure below and click Done.


      Figure 11.
    3. In the DownstreamDuct row, click Add To.
    4. Select the volume as shown in figure below and click Done.


      Figure 12.

      When the geometry was loaded into AcuConsole, complete geometry volume was placed in the default volume group. This default volume group was renamed to UpstreamDuct. In the previous steps, you assigned some volumes to various other volume groups that you created. At this point, all that is left is the UpstreamDuct volume group wherein the flow enters through the volume.

    5. Repeat the process with UpstreamDuct.


      Figure 13.
    6. Close the dialog.

Create Surface Groups and Apply Surface Parameters

Surface groups are containers used for storing information about a surface, including solution and meshing parameters, and the corresponding surface in the geometry that the parameters will apply to.

In the next steps you will define surface groups, assign the appropriate settings for the different characteristics of the problem, and add surfaces to the group containers.

In the process of setting up a simulation, you need to move into different panels for setting up the boundary conditions, mesh parameters, and so on, which can sometimes be cumbersome, especially for models with too many surfaces. To make it easier, less error prone, and to save time, two new dialogs are provided in AcuConsole. Use the Volume Manager and Surface Manager to verify and provide the information for all surface or volume entities at once. In this section some features of Surface Manager are exploited.

  1. Turn-off display for Volumes by right-clicking on Volumes and selecting Display off .
  2. Right-click on Surfaces in the Data Tree and select Surface Manager.
  3. In the Surface Manager dialog, click New eight times to create eight new surface groups.
  4. If you cannot see the Simple BC Active and Simple BC Type columns, click on Columns and select these two columns from the list and click Ok.


    Figure 14.
  5. Turn off the display for all surfaces except for the default surface.
  6. Rename Surface 1 through Surface 9 according to the image below.
  7. Set the Simple BC Active and Simple BC Type columns as per Figure 15.


    Figure 15.
  8. Assign the surfaces to the respective surface groups.
    1. In the Inlet row in the Surface Manager, click Add to .
    2. Select the planar symmetry surfaces as shown in the image, and click Done.


      Figure 16.
    3. Rotate the model to see the other side of the surface.
    4. In the Outlet row, click Add to, and select the surface shown below:


      Figure 17.
    5. Assign the surface for the Wall_Up group.


      Figure 18.
    6. Assign the surface for the Wall_Fan group.


      Figure 19.
    7. Assign the surface for the Wall_Down group.


      Figure 20.
    8. Assign the surface for the Upstream_Out group.


      Figure 21.
    9. Assign the surface for the Fan_Inlet group.


      Figure 22.
    10. Assign the surface for the Fan_Outlet group.


      Figure 23.

      When the geometry was loaded into AcuConsole, all geometry surfaces were placed in the default surface group container. This default surface group was renamed to Downstream_Inlet. In the previous steps, you assigned some surfaces to various other surface groups that you created. At this point, all that is left is the Downstream_Inlet surface group which makes up the inlet of the DownstreamDuct volume.

  9. Assign the surface for the Downstream_Inlet group.


    Figure 24.
  10. Close the Surface Manager.

Inlet

The Inlet group defines that the flow enters through the pipe and flows across length of the pipe. The correct boundary condition type for this surface is Inflow.

  1. Expand the Inlet surface in the tree.
  2. Double-click Simple Boundary Condition under Inlet to open the Simple Boundary Condition detail panel.
  3. Ensure that the Type is set to Inflow.
  4. Change Inflow type from Velocity to Flow Rate.
  5. In the Flow rate field, change the units to m3/hr.
  6. Enter the Flow rate value as 525.35.


    Figure 25.

Outlet

The Outlet group defines the exit of the pipe. The correct boundary condition type for this surface is Outflow.

  1. Expand the Outlet surface group in the tree.
  2. Double click Simple Boundary Condition to open the detail panel.
  3. Ensure that the Type is set to Outflow.
  4. Leave the remaining settings at their default values.


    Figure 26.

Wall_Up

The walls enclose the fluid volume on the outside. The correct boundary condition type for this surface is Wall.

  1. Expand the Wall_Up surface group in the tree.
  2. Double click Simple Boundary Condition under inner_wall to open the Simple Boundary Condition detail panel.
  3. Ensure that the Type is set to Wall.
  4. Leave the remaining settings at their default values.


    Figure 27.

Wall_Fan and Wall_Down

The surface groups Wall_Fan and Wall_Down will have the same settings as Wall_Up group. In order to not to repeat the steps again, you can propagate the settings to those two groups.

  1. Expand the Wall_Up surface group.
  2. Right-click on Simple Boundary Conditions, and select Propagate.
  3. Select Wall_Fan and Wall_Down from the menu.
  4. Click Propagate.


    Figure 28.

Fan_Outlet

Uncheck the Simple Boundary Condition for this surface.

Upstream_Out

Uncheck the Simple Boundary Condition for this surface.

Downstream_Inlet

Uncheck the Simple Boundary Condition for this surface.

Fan_Inlet

This surface corresponds to the inlet of the Fan component volume. For this particular surface you need to assign the FAN_COMPONENT parameter, which requires data related to fan speed, tip radius, axial coefficients, and so on. This parameter is available under advanced options in AcuSolve.
  1. Click ALL in the Data Tree Manager to show all the settings in the Data Tree.
  2. Uncheck the Simple Boundary Condition for the Fan_Inlet surface
  3. Expand Advanced Options.
  4. Check the Fan Component check box to open the detail panel.
  5. Ensure that the Type is set to Axial.
  6. Next to Center, click Open Array.
  7. In the dialog, enter 0.0 for all the fields.
  8. Click OK.
  9. Next to Direction, click Open Array.
  10. Enter 1.0 for X-Direction, and 0.0 for the other fields.
  11. Click OK.
  12. For Rotational Speed change the units from rad/sec to RPM.
  13. Set the Rotational Speed to 3600 RPM.
  14. Set Tip Radius to 0.11 m.
  15. Set Fan thickness to 0.06 m.
  16. Change Axial coefficient type from Constant to Piecewise Bilinear.
  17. Next to Axial curve fit values, click Open Array.
  18. Click Add Col seven times and enter the following as shown in the figure below.


    Figure 29.
  19. Click OK to close the dialog.
  20. Set Radial coefficient and Tangential coefficient to 0.
  21. Leave the remaining settings at their default values.


    Figure 30.

Assign Mesh Controls

Set Global Mesh Parameters

Now that the flow characteristics have been set for the whole problem, a sufficiently refined mesh has to be generated.

Global mesh attributes are the meshing parameters applied to the model as a whole without reference to a specific geometric volume, surface, edge, or point. Local mesh attributes are used to create mesh generation controls for specific geometry components of the model.

In the next steps you will set the global mesh attributes.

  1. Click MSH in the Data Tree Manager to filter the settings in the Data Tree to show only the controls related to meshing.
  2. Double-click the Global Data Tree item to expand it.
  3. Double-click Global Mesh Attributes to open the Global Mesh Attributes detail panel.
  4. Change the Mesh size type to Absolute.
  5. Enter 0.0096 m for the Absolute mesh size.


    Figure 31.

Set Surface Mesh Parameters

Surface mesh attributes are applied to a specific surface in the model. It is a type of local meshing parameter used to create targeted mesh controls for one or more specific surfaces.

Setting local mesh attributes, such as surface mesh attributes, is not mandatory. When a local mesh attribute is not found for a component, the global attributes are used as the mesh generation control for that component. If a local mesh attribute is present, it will take precedence over the global setting.

In the next steps you will set the surface meshing attributes.

  1. Expand the Model Data Tree item.
  2. Under the Model branch, expand the Surfaces. Under Surfaces, expand the Wall_Up surface group.
  3. If necessary, check the box next to Surface Mesh Attributes to activate it. Double-click it to open the Surface Mesh Attributes detail panel.
    The detail panel should now be populated with options related to the local surface meshing controls.
  4. Change the Mesh size type to None.
  5. Switch the Boundary layer flag to On.
  6. Change the Boundary layer type to Match Outer Layer.
  7. Ensure that First element height is set to 0.001 m.
  8. Change the Growth rate to 1.2.
  9. Leave the remaining settings at their default values.


    Figure 32.

The surface groups Wall_Fan and Wall_Down will have the same settings as the Wall_Up group. In order to not to repeat the steps again, you will propagate the settings to those two groups.

  1. Under the Wall_Up surface, right-click Surface Mesh Attributes and select Propagate.
  2. In the Propagate dialog, select the surface Wall_Fan and Wall_Down, and click Propagate.


    Figure 33.

Generate the Mesh

In the next steps you will generate the mesh that will be used when computing a solution for the problem.

  1. Click on the toolbar to open the Launch AcuMeshSim dialog.
    For this case, the default settings will be used.
  2. Click Ok to begin meshing.

    During meshing an AcuTail window opens. Meshing progress is reported in this window. A summary of the meshing process indicates that the mesh has been generated.



    Figure 34.
    Note: The actual number of nodes and elements, and memory usage may vary slightly from machine to machine.
  3. Visualize the mesh in the modeling window. Turn on the display of surfaces and set the display type to solid and wire.
  4. Rotate and zoom in the model to analyze the various mesh regions.

Compute the Solution and Review the Results

Run AcuSolve

In the next steps you will launch AcuSolve to compute the solution for this case.

  1. Click on the toolbar to open the Launch AcuSolve dialog.
    For this case, the default settings will be used. AcuSolve will run using four processors (if available, higher number of processors may be specified) and AcuConsole will generate AcuSolve input files and will launch AcuSolve. AcuSolve will calculate the steady state solution for this problem.
  2. Click Ok to start the solution process.

    While computing the solution, an AcuTail window opens. Solution progress is reported in this window. A summary of the solution process indicates that the run has been completed.

    The information provided in the summary is based on the number of processors used by AcuSolve. If you use a different number of processors than indicated in this tutorial, the summary for your run may be slightly different than the summary shown.



    Figure 35.
  3. Close the AcuTail window and save the database to create a backup of your settings.

Post-Process with AcuProbe

AcuProbe can be used to monitor various variables over solution time.

  1. Open AcuProbe by clicking on the toolbar.
  2. In the Data Tree on the left, expand Residual Ratio.
  3. Right-click on Final and select Plot All.
    This will plot the residuals for the three variables - eddy viscosity, pressure and velocity in the plot area. This plot indicates the convergence of the variables with respect to timestep.
    Note: You might need to click on the toolbar in order to properly display the plot.


    Figure 36.
  4. Right-click on Final under Residual Ratio and select Plot None.
  5. Click the User Function icon from the toolbar.
  6. In the dialog, enter the Name as dP.
  7. In the Data Tree dialog, expand Surface Output > Fan_Inlet > Pressure.
  8. Right-click on pressure and select Copy name.
  9. In the Function field of the User Function dialog, type Fan_In = then paste the name you just copied.


    Figure 37.
  10. Type Fan_Out = on a new line.
  11. Under Fan_Outlet, expand Pressure then right-click on pressure and select Copy name.
  12. Paste the name in the Function field.


    Figure 38.
  13. Type value = Fan_Out - Fan_In on a new line.
    Note: The word “value” is case sensitive and should always be in lower case. If you use a capital letter, an error window appears.


    Figure 39.
  14. Click Apply.


    Figure 40.

    From the above figure, you can see the pressure rise got stabilized at around 9th iteration and remains constant with a pressure of 494.53 Pa for a given volume flow rate of 525.35 m3/hr which is very near compared to reference value of 494.91 Pa.

Summary

In this AcuSolve tutorial, you successfully set up and solved a problem involving the FAN_COMPONENT feature for an axial fan. The FAN_COMPONENT directly computes body force term to yield the pressure rise within the volume of interest. The problem simulated is the flow inside pipe with a fan placed at the middle of the pipe causing pressure rise due to fan and exits at the outlet. You started the tutorial by creating a database in AcuConsole, importing and meshing the geometry, and setting up the simulation parameters. The fluid domain is divided into three volumes – UpstreamDuct, Fan & DownstreamDuct – using the Volume Manager Dialog option. Once the case was setup, the solution was generated with AcuSolve. Results were plotted in AcuProbe by creating a user function to check for the fan pressure rise based on Fan_Inlet and Fan_Outlet pressures. New features that were introduced in this tutorial include: using Fan Component feature and explaining how the axial coefficients are calculated based on volume flow rate and fan pressure rise and using the User Function option in AcuProbe.