한국어

Simple incompressible flow examples

Mixing Pipe

Download mesh
Downlaod simulation
Link to youtube video

Introduction

This is Steady incompressible flow example. Predict the mixing of the flow inside a circular pipe with two inlets and one outlet.

Simulation conditions are as follows.

solver : buoyantSimpleNFoam
turbulence model : Standard \(k-\epsilon\) model
density : 1.225 \(kg/m^3\)
viscosity : 1.79e-5 \(kg/ms\)
flow condition : velocity of large inlet(in-1) is 5 m/s, small inlet(in-2) is 10 m/s, outlet pressure is 0

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

※ Note: When reading OpenFOAM mesh, select the “polyMesh” or “constant” folder. OpenFOAM's mesh is a folder named polyMesh under the constant folder for a single region, or multiple polyMesh folders under the constant folder for multiple regions.

General

For this example, we'll use default conditions.

Models

For this example, we'll use Standard \(k-\epsilon\) model for turbulence.

Materials

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

Boundary Conditions

You can set boundary values for multiple boundaries. Each boundary will turn red when selected.

Right-clicking on a boundary allows you to change the boundary type, and double-clicking or clicking the 'Edit' button below opens a window where you can set the value.

Each boundary condition is set as follows

in-1 : Velocity Inlet
- Velocity Magnitude : 5 (m/s)
- Turbulent Intensity : 1 (%)
- Turbulent Viscosity Ratio : 10
in-2 : Velocity Inlet
- Velocity Magnitude : 10 (m/s)
- Turbulent Intensity : 1 (%)
- Turbulent Viscosity Ratio : 10
out : Pressure Outlet
- Pressure : 0 (Pa)
wall
- Velocity Condition : No Slip

Numerical Conditions

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

Pressure-Velocity Coupling Scheme : SIMPLEC
Discretization Scheme
- Pressure : Momentum Weighted Reconstruct
- Momentum : Second Order Upwind
- Turbulence : Second Order Upwind
Under-Relaxation Factors
- Pressure, Momentum, Turbulence : 0.9
Convergence Criteria
- Pressure : 0.0001
- Momentum : 0.001
- Turbulence : 0.001

Monitor

Monitor the pressure at the location (0, 0, 1).

Select [Solution]-[Monitors] and click [Add]-[Points] at the bottom of the window to set it up as shown below.

Point Monitor
- Write Interval : 1
- Field : Pressure
- Coordinate : (0, 0, 1)

Initialization

Initial Condition allows you to enter the velocity and pressure in x, y, and z as initial values.

If you are using a turbulence model, you can enter the Velocity Scale, Turbulent Intensity, and Viscosity Ratio values, and the \(k\) and \(\epsilon\) values will be calculated and used.

Velocity
- X-Velocity : 0 (m/s)
- Y-Velocity : 0 (m/s)
- Z-Velocity : 0 (m/s)
Pressure
- 0 (Pa)
Turbulence
- Scale of Velocity : 5 (m/s)
- Turbulent Intensity : 1 (%)
- Turbulent Viscosity Ratio : 10

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

Run

For this example, we'll use default values.

Click [Run]-[Start Calculation] button.

residual & monitoring graph

Post-processing

BARAM uses ParaView for post-processing. To start post-processing, click the ParaView button in [External tools].

When running ParaView, the following features are required

Skip Zero Time: Shows the results excluding the initial value.
Case Type: Set according to the number of CPUs.
- Reconstructed Case: Single core simulation
- Decomposed Case : Parallel simulation case
Mesh Regions: You can set the internal mesh, boundary surface, etc. you want to see.
Cell Arrays: You can set the physical quantities you want to see.

Scalar distribution at boundary

Plot the pressure distribution on the wall. The initial settings are as follows.

Skip Zero Time: Disabled
Mesh Regions: internalMesh - enabled
Rest : Default

\(p_{rgh}\) is the pressure minus the term due to gravity (\(\rho gh\)), which is the same as the pressure when gravity is not considered, such as in this problem. \(p_{rgh}\) is the relative pressure relative to the operating pressure and \(p\) is the absolute pressure.

Axial cross-sectional Scalar distributions

Check the pressure distribution inside the pipe. Click the slice button and change the orientation to Y-normal to see the pressure inside the pipe.

Cantilever Beam

Download mesh

Introduction

This example is a steady-state incompressible flow analysis example. This is a 1-way Fluid Structure Interaction(FSI) example to determine how a cantilever beam is deformed by air entering from the inlet region.

The cantilever beam is 5 mm thick, 50 mm long, and 150 mm high. We model only half of it and impose a symmetry boundary condition.

The geometry and mesh are shown in the figure below.