↑top

Tutorial - Calculation of axial fan with moving mesh function

Updated: August 18, 2021

In this tutorial, we will calculate a rotating axial fan with moving mesh function.

Analysis summary

We wll calculate an axial fan rotating at a speed of 120°/sec for 10 seconds. We also set the output setting to get the flow rate generated by the rotation of the axial fan.

ParaFoam velocity result Analysis result

Creating an analysis configuration file

Creating a project

Open XSim. Type "AxialFan" as Project Name and click Create button to create project.

Dialog for project creating Dialog for project creating

Importing shapes

We will use a prepared shape file in this tutorial. Please download a zipped file from next link, "tutorial-AxialFan.zip", and extract it.

Drag&Drop the extracted files "fan.stl", "inlet.stl", "outlet.stl" and "side.stl" at "Drop files" tab and load it. The loaded shape will be shown in 3D view.

Importing shapes from a file Importing shapes from a file

You can switch the 3D display to semitransparent by clicking a display-mode button'toggle display' iconunder 3D view.

Click Next button to go to Mesh page.

Mesh

  • Volume mesh settings

    Set 80000 as target number of base meshes and (0, 0, 0.5) as computational domain.

    Note: You can not set the computational domain definition point in the rotation area. It must be set on the stationary area.

  • Refinement settings

    In Refinement settings, select "Cylinder" as range type and set 0.135 m to radius, (0, 0, 0.065) m to center of top, (0, 0, -0.03) m to center of bottom. Then set 2 to refinement level. Preview the range shape by clicking preview button'Preview' icon, then click Add.

    Refinement setting (Cylinder) Refinement setting (Cylinder)
    Cylindrical area for refinement Cylindrical area for refinement
  • Layer mesh settings

    Confirm that 0.3 is set to layer thickness ratio and 3 is set to number of layers. Click "side" in Navigation view at left side of the window to select, then click Set.

    Layer mesh settings Layer mesh settings

Click Next button to go to Basic Settings page.

Basic Settings

In this section, we will set a type of analysis. Select "Transient" and set 10 seconds as end time. Then select "Rotating regions".

Basic Settings Basic Settings

Click Next button to go to Physical Property page.

Physical Property

No configuration is required because we will use default physical property. Confirm that "Water" is set as the physical property value.

Physical Property Physical Property

Click Next button to go to Initial Condition page.

Initial Condition

No configuration is required because we will use default parameters. Click Next button to go to Physical Property page.

Initial condition settings

  • Inflow boundary

    Select "Selected regions" as region and "Natural inflow/outflow" as type. Then select "inlet" on Navigation view and click Set.

    Inflow boundary condition Inflow boundary condition
  • Outflow boundary

    Select "Selected regions" as region and "Fixed static pressure" as type. Then select "outlet" on Navigation view and set 0 Pa as static pressure. After that, click Set.

    Outflow boundary condition Outflow boundary condition
  • Stationary wall boundary

    Select "Selected regions" as region and "Stationary wall" as type. Then select "side" and "fan" on Navigation view and click Set.

    Note: The stationary wall condition must be set for any wall that moves in rotation.

    Wall boundary condition Wall boundary condition

Inflow boudary and outflow boudary are displayed as arrows in 3D view.

Inflow/Outflow boundaries will be shown in 3D view Inflow/Outflow boundaries will be shown in 3D view

Click Next button to go to Rotating Region page.

Rotating Region

Select "Moving mesh" as rotating type and "Cylinder" as region type. Then set 0.12 m to radius, (0, 0, 0.05) m to center of top, (0, 0, -0.015) to center of bottom and -120 °/s to rotational velocity. Preview the rotating region and rotational direction by clicking preview button'Preview' icon, then click Set.

Rotating region settings
Rotating region settings
Preview rotating region in 3D view
Preview rotating region in 3D view

You can select "MRF" or "Moving mesh" as rotating type. Each has the following advantages and disadvantages.

  • MRF

    By adding the effect of rotational volume force (centrifugal force, Coriolis force) to the specified area, the rotation is simulated without rotating the shape.

    Advantages: It can be used for both steady and transient analysis, and is often more stable and faster than the Moving mesh calculations.

    Disadvantages: The flow must be rotational symmetry about the rotating area, otherwise (e.g. cross flow fan) the flow cannot be reproduced correctly. Also, it may be difficult to see the rotational velocity when visualizing the results because the shape does not actually rotate.

  • Moving mesh

    By actually rotating the mesh in the specified area, it reproduces the rotation of the shape.

    Advantages: It can be used for any flow. It is easy to see the rotation velocity when visualizing the results, because the shape actually rotates.

    Disadvantages: It cannot be used for steady analysis. Also, the calculation is often more unstable and slower than the MRF because the mesh is actually moved.

Calculation Settings

In this section, we set parallel number of CPU core that we use in this calculation (for example, 10).

Calculation settings Calculation settings

Click Next button to go to Output page.

Output

Because this analysis is a transient analysis, select "Each specified time" as type and set 0.33 second to interval.

出力設定 Output settings

Next, set the output for the flow rate.

Select "Region" tab and set "Selected regions" as region and "Flow rate" as type. Select "outlet" on Navigation view and click Set.

Output settings for the flow rate
Output settings for the flow rate

Click Next button to go to Export page.

Export

Finally we finished all settings. Click Export button to export the analysis setting as zipped OpenFOAM case directory "AxialFan.zip". The zip file download starts immediately.

Export Export

Running a calculation

Extract downloaded file "AxialFan.zip". There is a bash-script "Allrun " in the case directory. So run the script to make mesh and start the OpenFOAM solver by following command.

./Allrun

If the machine that calculation is running has desktop environment and gunuplot was installed, residual convergence chart will be displayed.

Chart for monitoring Chart for monitoring

Running in 10 parallel (Inter(R) Core(TM) i7-8700 CPU @ 3.20GHz 3.19GHz), it takes 10 seconds to create a mesh and about 8 minutes to analyze.

Confirming a calculation result

After the calculation, execute a following command to visualize the mesh and the calculation result.

paraFoam

Mesh is following.

We used a coarse meshes to shorten the calculation time, but if you want to make the fan shape more precisely, you can make a finer mesh.

Meshes for the fan Meshes for the fan
Meshes for fluid region Meshes for fluid region

The pressure distribution at the fan surface at the final time is as follows.

Pressure distribution at fan surface Pressure distribution at fan surface

And the flow velocity has been changing as shown in the video below.

Time change in flow velocity

The flow rate will be outputed to the text file "surfaceFieldValue.dat" in "postProcessing/flowRatePatch(name=outlet)/0" as following . The left side column is time and the right side column is flow rate.

# Region type : patch outlet
# Faces  :    2011
# Area   :    5.025579e-01
# Time        	sum(phi)
0             	0.000000e+00
0.33          	7.599636e-05
0.339429      	5.986955e-05
…………
9.977         	5.033736e-04
9.988         	5.038820e-04
9.999         	5.042866e-04