Basics of OpenFOAM : Open source CFD Solver

by
Post Views: 12,752

What is the basic structure of Open Source CFD Solver?

By Dr. Sharad N. Pachpute

 

Introduction to OpenFOAM

  • Open FOAM is an open-source CFD software that has a C++ library for more than 80 applications of CFD modeling. This solver has a large number of interlinked libraries of solvers and utilities covering a broad range of problems related to fluid flow
  • The meaning of OpenFOAM is Open Field Operations and Manipulation for numerical simulation of physical problems in the form of differential equations
  • Any equation as a function of field variables like a scalar, vector, and tensors can be coded there in the Open FOAM framework. Hence, this solver has been popular in academia and industries.
  •  Mathematical operations and customized open-source libraries are interlinked 

 

  • OpenFOAM solves the Partial Differential Equations (PDEs) numerically using the finite volumes method (FVM)
  • Customized Multiphysics CFD solver for complex fluid flows
  • Provides numerical solutions for 3D geometries
  • Open-source software developed in C++ (object-oriented programming)
  • It can be freely downloaded  at www.openfoam.com
  • Designed as a toolbox that is easily customizable
  • Parallel computation is implemented and users can use unlimited cores on high performance computing  (HPC) machine
  • Can be installed on Windows and Linux operating systems. It needs a C++compiler for running the simulation, hence Linux is preferred.

OpenFOAM has pre-and post-processing environments. The interface to the pre and post-processing are called ads utilities. These things ensure that all variables are in OpenFOAM environments. The overall structure of the open-source CFD solver, OpenFOAM is shown below.

Advantage of OpenFOAM

  • No licensing fees
  • Easy to use CFD solvers on any HPC with unlimited cores for complex problems (LES, DNS)
  • Direct access to source codes to customize CFD solvers
  • additional code-to-code for benchmarks,
  • Users get regular updates
  • More than 80 different solvers and various tutorials
  • Ease to implement and program for any equations in partial differential equations
  • Active academic and professional communities by forum, conference, training schools

Disadvantage of OpenFOAM

  • Require more time to learn initially
  • Lack of complete user guide or direct CFD support
  • No integrated graphical user interface (GUI) for pre-processing, solver setting, and monitoring the simulations
  • More suitable for the Linux platform
  • CFD users must know Unix command lines and C++ programming

Essential Subject for OpenFOAM 

To understand the numerical algorithms with programs in Open FOAM. CFD users need to understand the following subjecting details

  1. Governing equations: various equations for  transport of scalar,  vector, tenor need understand for fluid mechanics, heat transfer, turbulence, Multiphase flow, combustion, and turbo-machinery
  2. Numerical methods and modeling of various terms
  3. Programming in C++
  4. Experience on Linux
  5. Parallel computing and shell programming

Installation of OpenFOAM

  • You should have a programming environment for C++.
  • It can be created  by installing Linux (Ubuntu Version) or  windows 10
  • The details of OpenFOAM installation are given on the CFD guide page

Parts of CFD Simulations in Open FOAM

Pre-processing

    • Utilities: these are provided to create or read the mesh model and boundary conditions for simulations and manipulation of input data
    • Meshing platforms: blockMesh, snappyHexMesh
    • Mesh conversion utilities: ANSYS, Salome, ideas, CFX, Star-CCM, Gmsh etc
    • Example: blockMesh, CheckMesh, runTime

Solvers

      • To numerically solve a specific problem based on continuum mechanics for fluid flows
      • Different applications are coded in OpenFOAM for CFD simulations: incompressible or compressible flow , heat transfer, multiphase flow, combustion, electro-magnetism, turbulence modelling (DNS, RANS, LES) and solid mechanics, etc.
      • Example: icoFoam, rhoSonicFoam etc.

Post-processing

        • After simulation, CFD results can be analzed  in ParaView
        • The data from OpenFoam can be converted to other data files for other post-processing tools (FoamToTecplot)

 

OpenFOAM Directory

After installation of OpenFOAM, we can see many subdirectories like applications, source code (src), tutorials, dictionary files, other supporting installation and compilation file.

Case Set up in OpenFOAM

To set a case for CFD simulation, we have to create three subdirectories for numerical simulation

  • 0 :
    • All initial boundary conditions are given with different files created for pressure (P), velocity(U), temperature (T), concentration (C) and turbulent viscosity (nut) as key variables implemented in CFD solver
    • This directory is common for both steady and unsteady problems
  • Constant
    • Mesh files: files for boundary conditions, faces and nodes
    • Transport properties /Material properties
    • Selection of turbulence models like RANS/LES
  • System
    • conrtolDict: Files to control the simulation
    • decomposeParDict: files for parallel simulation on HPC
    • fvSchemes: discretization schemes for both temporal and spatial
    • fvSolution: selection of tolerance, residual and pressure-velocity coupling
  • Additional files for mesh and post-processing
  • After simulation different directories of iteration of time steps are created which have data of domain for velocity, pressure, temperature, TKE, Dissipation rate etc.

Application Utility

Applications are programmed in OpenFOAM for pre and post-processing. CFD users need to be familiar with such commands.

Preprocessing:  Meshing Utilities

  • BlockMesh: convert geometry to mesh
  • CheckMesh: To check mesh quality such as skewness and aspect ratio
  • fluentMeshToFoam: Converts fluent 2D mesh (in ASCII format)  to OpenFOAM format
  • snappyHexMesh: Generate Hex-dominant automatic mesh
  • surfaceTransformPoints: Scale, rotate, translate surface mesh vertices
  • fluent3DMeshToFoam: Converts a Fluent 3D mesh  to OpenFOAM format
  • star4toFoam: Converts the mesh file of PROSTAR v4  to OpenFOAM format

Preprocessing: Application Utilities

  • setFields: Modify internal field values using sets
  • FunkySetFields: Enhanced setFields with interpreted functions
  • mapFields: Parallel mapping of solution fields

Preprocessing:  Utilities for Parallel simulation

  • decomposePar: Decompose or split the mesh and fields for parallel execution
  • reconstructParMesh:  Merge decomposed mesh and data (simulated files from parallel processors) into a single set of files
  • reconstructPar: Merge decomposed fields (parallel run data) from parallel runs

Post-processing Utilities

  • foamToVTK:  Converts  OpenFOAM file  to  VTK format
  • foamToTecplot360: Converts OpenFOAM (mesh and data) files to Tecplot 360 format
  • foamLog: Create plottable ASCII files from solution logs
  • foamCalc: Perform mathematical operations on existing fields
  • ptot: Calculate and write the total pressure field
  • yPlusRAS:  Calculate and write the y-Plus field for RANS (Renolds averaged Navier stokes equations) models
  • yPlusLES: Calculate and write the y-Plus field for large eddy simulation (LES)
  • sample:  Sample results on points, lines, and surfaces
  • vorticity: Calculate and write the vorticity field of velocity
  • wallShearStress: Calculate and write the field of  wallShearStress  over the wall
  • wallHeatFlux: Calculate and write the field  of convective heat flux  over the wall

Solvers in OpenFOAM

  • After installation of open-foam libraries, check available source code as per physics of  CFD applications like turbulent flow, sonic flow, combustion and multiphase flow etc, $FOAM_APP/solvers or ($FOAM_SOLVERS)\
  • Find the source code for the CFD solvers arranged as follows:
    • Combustion: example: reactingFoam
    • Compressible coupled
    • Discrete methods
    • Direct Numerical Simulation (DNS)
    • Electromagnetics engine
    • Incompressible flow:  example: icoFoam, simpleFoam
    • Heat Transfer
    • Lagrangian Flow
    • Multiphase Flow: example:interFaom
    • Stress Analysis
    • surface Tracking
    • viscoelastic flow
    • Financial Application
  • Some examples of CFD solvers are listed below

 

 

Discretization schemes in OpenFOAM

  • In OpenFOAM case set up,  there is a fvSchemes dictionary in the system directory to define different numerical schemes for discretization of different terms in governing equations

Different interpolation schemes are used for various terms in equations. However, the linear interpolation is more effective in most cases

  • OpenFOAM provides enough choices to CFD users for the selection of interpolation schemes for different interpolation terms.

 Schemes for Vector fields

For vector fields such as the gradient of scalar, various numerical schemes are used in OpenFOAM

Unsteady Terms

For transient flows, there is an unsteady term (d/dt) governing equation. This is called is the first time derivative. In OpenFoam solver, it is presented as ddtSchemes. The discretization schemes for each term can be selected from those listed below.

  • Steady State: time derivative is set with zero value
  • Euler Scheme: this time scheme is suitable for unsteady, 1st order implicit and bounded solution
  • Backward scheme: it is suitable for unsteady, 2nd order implicit and potentially unbounded problems
  • Crank Nicolson scheme: it is suitable for unsteady, 2nd order implicit and bounded problems. This scheme requires to set a coefficient of 1 for Crank Nicolson and zero for Euler scheme. For most engineering problems it is set with 0.9 to get stable solutions
  • In openfam it is written as

  • A list of time schemes available in OpenFOAM is given below

 

Gradient schemes

a) Gauss linear

  • finite volume method (FVM) discretisation of Gaussian integration which interpolate of values from cell centres to face centres
  • Linear interpolation scheme or central differencing is used
  • Its value can be specified with 1 for boundness and 0 for no boundness
  •  In some cases, cell Limited scheme used to limit the calculated gradient due to extrapolation from faces. It helps to improve boundedness and stability for velocity gradients for poor mesh quality

b) least-squares: this is a second-order scheme and calculates the least-squares distance using all neighbor cells.

c) Gauss Cubic: third-order scheme that is suitable for the direct numerical simulation (dnsFoam) on a regular mesh.

Divergence schemes for Advection and Diffusion

In governing equations such as momentum, energy or species transport there are advection and diffusion terms. These terms are treated as divSchemes in Open FOAM. The non-advective terms is generally interpolated with the Gauss integration considering a linear variation 

  • Upwind: This is a first-order bounded scheme
  • Linear: this scheme is based on second-order, unbounded.
  • Linear Upwind: second-order, upwind-biased, unbounded (but much less so than linear). For this discretization, velocity gradients need to be specified
  • LUST (Linear Upwind Stabilised Transport) : This scheme is a combination of both linear (75%) and linear Upwind (25%). For this discretization, velocity gradients need to be specified. This scheme is used for large eddy simulation (LES).
  • Limited Linear: it is a modified linear scheme that limits towards the upwind schemes in the region of a sudden change in gradients. It needs to define with a coefficient of one for upwind and zero for linear.

Application source code in OpenFOAM

  • The main code application is included in the *.C file.
  • In OpenFOAM, depending on flow application, the source code is developed in several other files
  • This file is given at the beginning of any piece of code using the class, including the class declaration code itself
  • Any piece of code in ( *.C file) can have a number of classes and which are declared in *.H files
  • The classes in these files may have other classes

  • In OpenFOAM Header files are included in the application code using # include statements: # include “otherHeader.H”
  • It is given for compiling to suspend reading from the current file to read the file specified
  • Any self-contained piece of code or custom code is put into a header file and included at the relevant location in the main code in order to improve code readability
  • For example, in most OpenFOAM applications, the code for creating or reading the field of input data is given in a file createFields.H

Structure of Application in OpenFOAM

We can consider the sonicFoam application as an example of application directory This application can be found at:

The top-level source file takes the application name with the .C extension. For any application, classes are defined on *.H files and governing equations are generally coded in *.C files

 

Compilation of Application using the wmake command 

For the compilation of a new application, the directory should have a Make subdirectory that contains 2 files: options and files. The wmake command is used to compile a modified application.

There are several files (*.C and *.H) that are given in a particular directory of applications. Do required changes as per OpenFOAM framework without any error in compilation

The OpenFoam compiler checks for the included header files in the following order. It is specified with the -I option in wmake:

 

  •  lnInclude is added as a local  directory for incompressible solver (icoFoam): $WM_PROJECT DIR/src/icoFoam/lnInclude
  • Platform dependent paths are  set in files :  $WM_PROJECT_DIR/wmake/rules/$WM_ARCH/
  • The full paths of directory to locate header files are given in the folder: “ Make/options” file using the following syntax:

EXE_INC = \ -I$(LIB_SRC)/finiteVolume/lnInclude

 

 Implementation of Governing Equations in OpenFOAM

Mass, Momentum, and Energy Equation in OpenFOAM

  • The turbulent kinetic energy equation is given as below

  • In open Foam, the above governing equations are implemented as equation representation

Here, the first term represents of the left side the unsteady term, the second term is the divergence f mass flux (phi) and K. The four term is diffusion term.

 Implementation of Compressible Flow solver (rhoSonicFoam)

  • The conservation of equations for compressible flow in OpenFOAM are presented as

 Pressure and Velocity Coupling in OpenFOAM

 Semi-Implicit Method for Pressure-Linked Equations (SIMPLE)

    • The details of SIMPLE algorithm it is useful for most simple steady flows
    • You can find on open foam wiki website:
    • The SIMPLE  is used to couple the mass and moemtum (Navier-Stokes)  equations during  iterative procedure, which is given as below
      1. set the domain with boundary conditions
      2. Solve numerically the discretized momentum equation to calculate the intermediate velocities
      3. Calculate the mass fluxes at the cells faces.
      4. Solve the pressure corrected equation and  apply under-relaxation factors
      5. Correct the mass fluxes for all the cell faces.
      6. Correct the velocity fields based on new pressure fields
      7. Update the boundary conditions.
      8. Repeat above steps till convergence

 PISO: Pressure-Implicit with Splitting of Operators

  • This algorithm is more suitable   to solve the Navier-Stokes equations in unsteady (transient) problems of CFD modeling
  • It can support the worst mesh model

 

 PIMPLE: a combination of SIMPLE and PISO

  • This is more suitable to use adaptive steps with a fixed courant number in large-eddy simulations (LES)
  • We can fix the courant number during the transient simulation

The PISO loop in OpenFOAM

Boundary Conditions in OpenFOAM

  • Most the boundary conditions are defined based on a fixed value or fixed gradients
  • It is important to understand these values before CFD modeling
  • For details of boundary conditions: \src\finiteVolume\fields\fvPatchFields\
  • There are major types of boundary conditions:
    • Basic: calculated, fixed value, fixed gradient, zero gradient
    • Constraint: symmetry, wedge, cyclic, jump, cyclic AMI
    • Derived: slip, no-slip, fan pressure, inlet-outlet, outlet inlet, total pressure

 

Post-processing of OpenFOAM Files in Paraview and Tecplot

  •  Paraview is used for performing data analysis and visualization of OpenFOAM simulations 
  • First, convert OpenFOAM files to VTK format
  • Click here : Userguide of Paraview
  • Then read the OpenFOAM files and read the data for scalar and vector quantities

 

CFD post of OpenFOAM

  • Understand the data type of open FOAM while displaying the contours: Point data array or cell center array

  • You can filter out some data while post-processing CFD results in Paraview

 

  • Open foam data can be exported to the third parties like Tecplot, FLUENT:
  • Many CFD post tools can be used. You can find useful commands for data conversion for third-party conversion.
    • Command for foam data to Tecplot conversion: foamToTecplot360
    • Watch how to convert: watch the video

YouTube Videos

Summary

  • OpenFOAM is a finite volume method (FVM) based CFD solver. Its source code is freely available.
  • Libraries of OpenFOAM are in C++ language and can be installed in Linux or windows where compiler
  • OpenFOAM simulation comprises three parts: preprocessing, simulation using the CFD solver  (application utilities), post-processing
  • This solver is easy to customize but it takes more time for new users
  • Most CFD simulations can be carried in OpenFOAM

Reference

  1. Open FOAM downloads and details of solvers: www.openfoam.org
  2. OpenFOAM discussion forum: www.cfd-online.com/Forums/openfoam/)
  3. community-driven wiki: www.openfoamwiki.net 
  4.  Open Foam Blog by Fumiaya Nozaki: Fumiya Nozaki
  5. Customization of CFD solvers: Chalmer University tutorials on OpenFOAM

1 thought on “Basics of OpenFOAM : Open source CFD Solver”

  2. ESI-OpenCFD is pleased to announce the release of OpenFOAM v2006 (20 06) of the OpenFOAM open source CFD toolbox.

    Reply

Leave a Comment