Skip to content

Rotating machinery

Fan(MRF)

Download mesh

Download simulation

Introduction

Mesh and velocity

This is a steady-state incompressible flow analysis example. The problem is to predict the flow using multiple reference frames (MRFs) as the impeller rotates inside a fan.

The computational conditions are as follows

  • solver : buoyantSimpleNFoam
  • turbulence model : \(Standard\) \(k-\epsilon\) model
  • density : 1.225 \(kg/m^3\)
  • viscosity : 1.79e-5 \(kg/ms\)
  • Rotation velocity : 1,000 RPM
  • flow condition : 10 \(m/s\) at inelt

Start BaramFlow and load mesh

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


Use the given polyMesh folder. In the top tab, click [File]-[Load Mesh]-[OpenFOAM] in that order and select the polyMesh folder.

General

For this example, we'll use default conditions.

Models

For this example, we'll use default conditions.


Materials

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

Cell zone Conditions

Cell Zone Conditions allow you to set MRF, Sliding Mesh, Source, and more. In this example, we are using a Multiple Reference Frame, MRF condition for the 'rotating' Cell Zone.

Select Multiple Reference Frame, MRF and set values as follows

  • Multiple Reference Frame, MRF
    • Rotating Speed : 1000(RPM)
    • Rotation-Axis Origin : (0 0 0)
    • Rotation-Axis Direction : (0 0 1)
    • Static Boundary : casing


Boundary Conditions

Each boundary condition is set as follows

  • blade, casing
    • Velocity Condition : No Slip


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


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


Numerical Conditions

In this example, we'll change the settings as shown below.

  • Pressure-Velocity Coupling Scheme : SIMPLE

  • Discretization Scheme

    • Pressure : Linear
    • Momentum : Second Order Upwind
    • Turbulence : Second Order Upwind

  • Under-Relaxation Factors

    • Pressure : 0.3
    • Momentum : 0.5
    • Turbulence : 0.7

  • Convergence Criteria

    • Pressure : 0.001
    • Momentum : 0.001
    • Turbulence : 0.001

Initialization

Use default vaues.

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 Iterations : 1000
  • Save Interval : 100
  • Retain Only the Most Recent Files, 1
  • Data Write Format : Binary
  • Selct [Parallel]-[Environment] in menu. Set Number of Cores as you want and select [Local Machine] for [Parallel Type].


When the calculation is started, you'll see a graph of Residuals and Force monitor as shown below.

|residual|

Post-processing

Draw the pressure distribution in the fan.

Click the parview button in [External tools] to open the paraview.

Change the [Case Type] to [Decomposed Case].


Use the [Slice] function to cut a cross-section inside the domain.

Click the Z-normal button and enter 0.01 for the z value in Origin.



Mixer(MRF)

Download mesh

Download simulation

Introduction

This example is an MRF simulation of a mixer with a simple geometry. The MRF model enables steady-state calculations and allows the use of rotational periodic conditions based on one impeller blade, which can significantly reduce the computational cost.

The simulation conditions are as follows

  • solver : buoyantSimpleNFoam
  • turbulence model : \(Standard\) \(k-\epsilon\) model
  • density : 1000 \(kg/m^3\)
  • viscosity : 0.001 \(kg/ms\)
  • rotation velocity : 100 RPM

Start BaramFlow and load mesh

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


Use the given polyMesh folder. In the top tab, click [File]-[Load Mesh]-[OpenFOAM] in that order and select the polyMesh folder.

General

For this example, we'll use default conditions.

Models

For this example, we'll use default conditions.

Materials

Change the Name to water and enter a Density of 1000 and a viscosity of 0.001.

Cell zone Conditions

Select [Multiple Reference Frame, MRF] at [Cell Zone Conditions] and set values as follows

  • Multiple Reference Frame
    • Rotating Speed : 100(RPM)
    • Rotation-Axis Origin : (0 0 0)
    • Rotation-Axis Direction : (0 0 1)
    • Static Boundary : periodic1, periodic2


Boundary Conditions

Each boundary condition is set as follows

  • periodic1, periodic2 : Interface - Rotational Periodic
    • periodic1 : Change to Rotational Periodic, then select periodic2 as [Coupled Boundary]
    • Set [Rotation-Axis Origin] as (0 0 0), [Rotation-Axis Direction] as (0 0 1)


  • impeller, impeller_slave : Thermo-Coupled Wall

    • impeller : Change to Thermo-Coupled Wall, then, select impeller_slave as [Coupled Boundary]

  • wall, hub, hub_rot : Wall

    • Velocity Condition : noSlip

  • top : symmetry

Numerical Conditions

For this example, we'll use default conditions.

Initialization

For this example, we'll use default conditions.

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

Run

Change [Number of Iteration] as 3000 and click [Start Calculation] button.


Sirocco Fan(Sliding mesh)

Download mesh

Download simulation

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.


Cell zone Conditions

Change rotating cell zone to [Sliding Mesh]. Setting of [Static Boundary] disappears.

Boundary Conditions

Change the boundary conditions for the moving wall to the following

  • axis-r, blades : Wall
    • Velocity Condition : Moving Wall


Numerical Conditions

For this example, we'll use default conditions.

Run

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

  • Time Stepping Method : Fixed
  • Time Step Size : 0.0001
  • End Time : 0.3


When the calculation is started, you'll see a graph of Residuals and Force monitor as shown below.


Post-processing

Draw the pressure distribution in the fan.

Click the parview button in [External tools] to open the paraview.

Change the [Case Type] to [Decomposed Case].


Use the [Slice] function to cut a cross-section inside the domain.

Click the Z-normal button and enter values as follow

  • Origin : (0.06 -0.017 0.05)
  • Normal : (0 0 1)



Propeller

Download simulation

Introduction

This is an example of the propeller from the pimpleFoam tutorial of OpenFOAM. This is to predict the flow over the rotation of a propeller using the sliding mesh.

The simulation conditions are as follows

  • solver : buoyantPimpleNFoam
  • turbulence model : \(Realizable\) \(k-\epsilon\) model
  • density : 1000 \(kg/m^3\)
  • viscosity : 0.001 \(kg/ms\)
  • rotating velocity : 1432 \(RPM\)
  • flow condition : 5 \(m/s\) at inlet

Start BaramFlow and load mesh

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


Use the given constant/polyMesh folder of [Download simulation] file. In the top tab, click [File]-[Load Mesh]-[OpenFOAM] in that order and select the constant/polyMesh folder.

General

Change Time to Transient.


Models

For turbulence, use \(Realizable\) \(k-\epsilon\) model and [Enhanced Wall Treatment].


Materials

Change the Name to water and enter a Density of 1000 and a viscosity of 0.001.

Cell zone Conditions

Select [Sliding Mesh] at [Cell Zone Conditions] and set values as follows

  • Rotating Speed : 1432(RPM)
  • Rotation-Axis Origin : (0 0 0)
  • Rotation-Axis Direction : (-1 0 0)


Boundary Conditions

Set the boundary type and values as shown below.

  • cellZone_surface, cellZone_surface_slave : Interface - Internal Interface
    • cellZone_surface : Change to Internal Interface, then select cellZone_surface_slave as [Coupled Boundary]


  • propeller, propellerStem : Wall

    • Velocity Condition : Moving Wall

  • far_surface : Wall

    • Velocity Condition : Slip

  • inlet : Velocity Inlet

    • Velocity Specification Method : Magnitudde, Normal to Boundary
    • Profile Type : Constant
    • Velocity Magnitude : 5 (m/s)
    • Turbulent Intensity : 1 (%)
    • Turbulent Viscosity Ratio : 10


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


Numerical Conditions

Change [Max Iterations per Time Step] to 20, [Number of Correctors] to 2. Use default value for the rest.

Initialization

Set [X-Velocity] as 5, [Scale of Velocity] as 5.

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

Run

In Run Conditions, set the following settings and proceed with the calculation.

  • Time Stepping Method : Fixed
  • Time Step Size : 1e-5
  • End Time : 0.1
  • Save Interval : 0.001
  • Data Write Format : Binary
  • Selct [Parallel]-[Environment] in menu. Set Number of Cores as you want and select [Local Machine] for [Parallel Type].

Fan in Room

Introduction


This is an example of a simulation using a sliding mesh.

It is a simple problem with a fan rotating at 100 RPM in a room with air flowing through a window.

The simulation conditions are as follows

  • solver : buoyantSimpleNFoam
  • turbulence model : \(Standard\) \(k-\epsilon\)
  • rotating velocity : 100 RPM

Start BaramFlow and load mesh

Run the program and select 'Open' from the launcher.

Select the folder created from BaramMesh tutorial.

Then select Pressure-based for 'Solver Type' and None for 'Multiphase Model'.

General

For this example, we'll use default conditions.

Models

For this example, we'll use default conditions.


turbulence model

Materials

Material properties of air is as follows

Cell zone Conditions

Double-click AMI in the [Cell Zone Conditions] to open a new window. Select [Sliding Mesh] and enter the values below.

  • Rotating Speed : 100
  • Rotation Axis Origin : (-3 2 2.6)
  • Rotation Axis Direction : (0 0 1)


Cell Zone setup

Boundary Conditions

Set the boundary type and values as shown below.

  • desk_surface_0, door, room : Wall - No Slip

  • fan_surface_0 : Wall - Moving Wall

  • outlet : Pressure Outlet - Total Pressure = 0

  • AMI_surface_0, AMI_surface_0_slave : interface - Internal Interface


boundary condition setup

Numerical Conditions

In this example, we'll change the settings as shown below.

  • Pressure-Velocity Coupling Scheme : SIMPLE

  • Use Momentum Predictor : On

  • Discretization Schemes

    • Time : First Order Implicit
    • Pressure : Linear
    • Momentum : Second Order Upwind
    • Turbulence : First Order Upwind

  • Under-Relaxation Factors : 1 for all

  • Max Iteration per Time Step : 3

  • Number of Correctors : 1


Numerical conditions setup

Initialization

For this example, we'll use default values.

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.

  • Time Stepping Method : Adaptive
  • Couraant Number : 1
  • EndTime : 1
  • Save Interval : 0.02


Residual plot