Sirocco Fan(Sliding mesh)

Introduction

This is an example of transient incompressible flow. The problem is to predict the flow inside a sirocco fan when the impeller is rotating.

First steady-state simulations is performed using the MRF method. Then using the steady results as initial condition, the transient simulation is performed using the sliding mesh.

The simulations conditions are as follows

solver : buoyantPimpleNFoam
turbulence model : $Standard$ $k-epsilon$ model
density : 1.225 $kg/m^3$
viscosity : 1.79e-5 $kg/ms$
Rotation velocity : 2,000 RPM

Start BaramFlow

Run the program and select [New Case] from the launcher. In the launcher, select [Pressure-based] for [Solver Type] and [None] for [Multiphase Model].

Mesh

Use fluent format mesh. Select [File]-[Load Mesh]-[Fluent (ASCII)] from the menu to open the file selection window. Select the downloaded siroccofan.msh file and the following window will open.

This mesh has two cell zones, fluid and rotating. These two cell zones and two regions, region1 and region2, are shown. Click the (+) icon to the right of region2 to add a region. This is an option to convert to a multi-region grid. Since this is not a multi-region problem, you can leave both cell zones as region1. You can also delete region2 by pressing the trash icon below region2.

Steady-state simulation

General

Change Time to Steady.

Models

For this example, we’ll use $Standard$ $k-epsilon$ model for turbulence.

Materials

For this example, we will use the properties of air.

Cell zone Conditions

Double-click rotating in the [Cell Zone Conditions] to open a new window. Select [MUltiple Reference Frame, MRF] and enter the values below.

Rotating Speed : 2,000(RPM)
Rotation-Axis Origin : (0, 0, 0)
Rotation-Axis Direction : (0, 0, 1)
Static Boundary : interface-rotating, interface-stat
- Select the non-rotating boundaries in the cell zone to use MRF. One of the two interface boundary is inside the cell zone and the other is outside. It is usually hard to tell which one is the case, so you can select both. It is okay to include boundary faces that are outside the cell zone.

Boundary Conditions

Each boundary condition is set as follows

interface-stat, interface-rotating : Interface – Internal Interface
- interface-stat : Change to Internal Interface, then select interface-rotating as [Coupled Boundary]

axis : Wall
- Velocity Condition : Rotational Moving Wall
- Speed : 2000 (RPM)
- Rotation-Axis Origin : 0 0 0
- Rotation-Axis Direction : 0 0 1

axis-r, blades, externalwalls, walls : Wall
- Velocity Condition : No Slip

inlet : Velocity Inlet
- Velocity Specification Method : Magnitudde, Normal to Boundary
- Profile Type : Constant
- Velocity Magnitude : 1 (m/s)
- Turbulent Intensity : 1 (%)
- Turbulent Viscosity Ratio : 10

outlet : Pressure Outlet
- Total Pressure : 0 (Pa)

Numerical Conditions

For this example, we’ll use default conditions.

Initialization

For this example, we’ll use default conditions.

Enter the value and click the Initialize button at the bottom. Then click the [File]-[Save] menu to save the case file.

Run

Change the values as shown below, and click [Start Calculation] button.

Number of Iteration : 1000
Save Interval : 100
Selct [Parallel]-[Environment] in menu. Set Number of Cores as you want and select [Local Machine] for [Parallel Type].

Because the flow is unsteady, the residual does not converge, but it is fine to use as an initial condition for the transient simulation.

Transient simulation

General

Change Time to Transient.

The following window appears. It asks if you want to use the steady-state results as initial conditions for the transient simulation. If you select Yes, the last saved data will be set as the initial condition and the calculation will start from time 0.