The created CFD domain is now read into the CFD package of interest to setup the CFD simulation. It should be noted that the current tutorial has a significant difference compared to other available CFD tutorials online! This tutorial is structured and developed based on a generic and methodological approach to set up a CFD simulation. The first principals and reasonings for each setting is discussed at each step. Potential alterations and modifications to perform similar analysis for different flow conditions are also addressed and discussed. Hence, in the end user will have the capability of applying potential modifications, improvements or extending the application of the current CFD simulation to a more complex problem of interest, rather than having a one time successful run of a specific simulation with specific and strictly pre-defined boundary conditions.
In simple words: Current tutorial teaches users to fish, rather than giving them a fish.
0. Import the CFD Domain into Solver:
The previously generated CFD domain, fully explained in the Domain section, will be imported properly into the CFD solver.
1. Setup Model/s:
According to the physics of the flow field user will select required model/s to simulate the flow.
2. Setup Working Fluid/s & Solid/s:
User will define the physical and thermodynamical properties of the working fluid/s and solid/s in the problem.
3. Setup Boundary & Zone Conditions:
Solving the governing equations of the flow (i.e. system of partial differential equations) requires well-defined boundary conditions within the CFD domain. These conditions are selected and defined in this step.
4. Setup Solution Methods:
In CFD simulations the governing equations of the flow are solve numerically. Based on the physics of the problem appropriate numerical schemes and solution methods are selected at this step.
In the following section the details for the above-mentioned four steps of the CFD simulation setup process for the case study of 2D Laminar Flow Over a Flat plate are explained in great details. As a general guideline, to setup a CFD simulation in OpenFoam it is recommended to start with files from one of the provided default tutorials in OpenFoam located in OpenFoam/run/tutorials. Users should find appropriate tutorial such that the general physics of the chosen tutorial is close to the problem of interest of users. This way, the majority of the required physical settings are pre-set and the others can be changed/modified accordingly. For example for the problem of 2D Laminar Flow Over a Flat plate the tutorial of 2D over an airfoil located at OpenFoam/run/tutorials/incompressible/simpleFoam/airFoil2D is used. Using the previously developed file, the above-mentioned four steps for CFD simulation development is done via editing the corresponding files, where the settings are defined and are located in the main working directory.
0. Importing the Created CFD Domain into Solver:
The official mesh generator for OpenFoam is called blockMesh. This is a command base mesher software. Users write/edit the desired settings to generate and discretize the geometry of CFD domain in a dictionary file (i.e. a text file) named blockMeshDict located at \constant\\polyMesh inside the main working directory. In simple words the file is the dictionary, where the geometry and discretization process of it are fully defined. Once edits of blockMeshDict file are completed then it is compiled via the command blockMesh. This will generate multiple required files, that include the details of the discretized CFD domain for the use of OpenFoam solver in the directory of the blockMeshDict file. Readers can read more about the blockMesh utility here.
Alternatively, OpenFoam has various built-in commands that allow it's users to convert their previously generated CFD domain in different mesher packages into the readable format for the OpenFoam. A list of these commands can be found here. In this tutorial this alternative approach is used to convert the previously generated CFD domain with .msh format to the readable format in OpenFoam. In order to perform this process users put the .msh file of the previously generated CFD domain in the main working directory and use the command fluentMeshToFoam with the name of the mesh file after the command to perform the mesh conversion process (i.e. fluentMeshtoFoam [file name]. msh). This will generate multiple required files, that include the details of the discretized CFD domain for the use of OpenFoam in the working directory. Users should make sure that the generated report contains no error or problem. The details of the previously generated CFD domain in * .msh format are fully explained in the Domain (see Common_Files -> Domain) part of this tutorial.
1. Setup Model/s:
The main assumption in the classical problem of a two dimensional flow over a flat plate is that the free stream flow is uniform and steady. Therefore, the steady model is chosen to develop this CFD simulation. This along with other numerical schemes settings are set in a dictionary file called "fvSchemes" located at \system folder. To set the solver to be steady users define steadyState for the ddtSchemes and the rest of the settings will remain unchanged:
ddtSchemes
{
default steadyState;
}
In cases where the flow properties rapidly changes with respect to time the Transient model should be chosen in this step. Various available time schemes along with other implementable option within "fvSchemes" dictionary file in OpenFoam can be found here.
In the current problem the focus is to investigate laminar flow and boundary layer behavior when a uniform flow passes over a flat plate. The appropriate model for this problem is set in a dictionary file called RASPropertise (RAS stands for Reynolds Averages Stress) located at \constant folder:
RASModel laminar;
turbulence off;
printCoeffs off;
It is important to note that the critical Reynolds number for flows over flat plate is about 1.24E+6. In cases that the Reynolds number, based on flat plate length (as the length scale), is greater than this critical value the model the appropriate turbulent model should be selected at this step. Various available turbulence models along with other options within RASPropertise dictionary file in OpenFoam can be found here.
2. Setup Working Fluid/s & Solid/s:
The choice of working fluid is problem dependent. In the absence of obligations to define a specific working fluid such as air or water, it is suggested that the users define the working fluid such that the important non-dimensional groups of interest, such as Reynolds number in this problem, is matched the desired flow conditions. This strategy removes the uncertainty in the choice of the working fluid and will solidify the bases for expected physical observations. The material properties in OpenFoam can be defined in a dictionary file transportPropertise located in constant folder. In this file the material is set to be Newtonian fluid with a defined kinematic viscosity \nu. It should be noted that the numbers in the [] set the dimension of the flow field variable of interest and the other number sets it's value:
transportModel Newtonian;
nu nu [ 0 2 -1 0 0 0 0 ] 0.01;
Considering that the flat plate length in 1 [m] and user will define a unit constant uniform velocity (1 [m/s]), the value of \nu will be defined as the inverse of Reynolds number. Therefore, changing this value would set the nominal Reynolds number of the flow based on the flat plate length. For other cases users should define the working fluid via this process. Various available transport models along with other options within transportPropertise dictionary file in OpenFoam can be found here.
3. Setup Boundary and Zone Conditions:
In OpenFoam the type of boundaries within the CFD domain are defined in the boundary file located at \constant\polyMesh. Whether the users use blockMesh or the convert command to create the CFD domain and discretize the boundary file will be created in this process. Furthermore values for the field variables, such as velocity U and pressure p, at these boundaries are set in U and p files located at 0 folder located in the working directory respectively. The 0 folder includes the values of the field variables at boundaries for the time t=0.
As discussed earlier in the CFD domain's creation and discretization section, the CFD domain has four faces as boundaries. The boundary and zone conditions settings to develop CFD simulation for 2D Laminar Flow Over a Flat plate case in OpenFoam are as follows:
Inlet: The flow enters from the inlet face of the CFD domain with constant velocity and uniform atmospheric pressure (i.e. zero gauge pressure). To set the type of this boundary edit boundary file in \constant\polyMesh. Set the type of face to patch, which is a condition that contains no geometric or
topological information about the mesh:
inlet
{
type patch;
nFaces 100;
startFace 20100;
}
Set the field variables at this boundary edit U and p files in \0 folder to a constant uniform velocity in the streamwise direction (x-direction) with zero pressure gradient:.
// In U file at 0 folder:
inlet
{
type fixedValue;
value uniform (1 0 0);
}
// In p file at 0 folder:
inlet
{
type zeroGradient;
}
Outlet and Top Surface: The flow exits the CFD domain from the outlet and top face of the domain and reach atmospheric pressure (i.e. zero gauge pressure). To set the type of this boundary edit boundary file in \constant\polyMesh and set the type of face to patch, which is a condition that contains no geometric or topological information about the mesh:
outlet
{
type patch;
nFaces 100;
startFace 19900;
}
free_surface
{
type patch;
nFaces 100;
startFace 19800;
}
Set the field variables at this boundary edit U and p files in \0 to a constant uniform atmospheric pressure with zero velocity gradient:
// In U file at 0 folder:
outlet
{
type zeroGradient;
}
// In p file at 0 folder:
outlet
{
type fixedValue;
value uniform 0;
}
// In U file at 0 folder:
free_surface
{
type zeroGradient;
}
// In p file at 0 folder:
free_surface
{
type fixedValue;
value uniform 0;
}
If in a problem of interest, there exist a specific pressure difference between the inlet and outlet or other surfaces, that magnitude can be defined in corresponding faces of the domain.
Flat Plate: The flow is bounded by the flat plate on the bottom of the CFD domain and interacts with it based on the no-slip boundary condition. To set the type of this boundary edit boundary field in \constant\polyMesh and set the type of face to wall:
flat_plate
{
type wall;
inGroups 1(wall);
nFaces 100;
startFace 20000;
}
Set the field variables at this boundary edit "U" and "p" files in \0 to a fixed value of zero velocity with zero pressure gradient, which represents the fundamental assumptions of the uniform laminar flow over a flat plate:
// In U file at 0 folder:
flat_plate
{
type fixedValue;
value uniform (0 0 0);
}
// In p file at 0 folder:
flat_plate
{
type zeroGradient;
}
If the shear forces and formed boundary layer becomes turbulent in this region user should modify this boundary conditions and provide required mesh resolution to capture the phenomena or set this boundary to free slip condition such that fluid elements would not interact with wall region. For low reynolds number flow, similar to the current problem of interest, a reasonable mesh resolution is sufficient to capture the laminar boundary layer region.
Since this problem is two dimensional the boundary type and flow field variables for the frontToBack boundary, which defines the third dimension of the flow field are set to empty:
frontAndBackPlanes
{
type empty;
inGroups 1(empty);
nFaces 20000;
startFace 20200;
}
// In U and p files at 0 folder:
frontAndBack
{
type empty;
}
For more detail on definitions and settings for defining CFD domain boundary conditions in OpenFoam readers are referred to here.
4. Setup Solution methods:
In this step, it is highly recommended to use the default/suggested solution methods set in fvSolution file located in \systems, unless based on physics of the problem the user is aware of any specific choices. Upon non-smooth convergence and potential divergence of the CFD simulation user can modify and examine various solution methods.
The fvSolution file includes the solution methods for velocity and pressure fields and the required under relaxation factors for flow field variables.
Now all boundary conditions and settings for the CFD simulation are fully defined. User can initialize the solution through an educated guess to start the iteration process. In OpenFoam the initialization of the velocity and pressure fields is set on top of the U and p files located in the 0 folder:
// In U file at 0 folder:
internalField uniform (1 0 0);
// In p file at 0 folder:
internalField uniform 0;
The solution initialization would incept the flow field variables, such as velocity and pressure, based on the defined values by user. For the current problem the CFD domain is recommended to be initialize by values of velocity and pressure at the inlet.
Iteration process for solving the flow field governing equation now shall start till converged solution is obtained. In OpenFoam the iteration can initiated by running a command line using the name of the application of choice. The name of the application and set marching time steps to solve the flow field governing equations are set in controlDict dictionary file located in \system folder:
application simpleFoam;
startFrom startTime;
startTime 0;
stopAt endTime;
endTime 10;
deltaT 0.005;
For this problem a 10 seconds time interval is set with time steps of 0.005 seconds. The outputs will be written every 1 second till either the end of time interval or set tolerances for the residual of field variables are reached. The iterations can be started by running the command simpleFoam.
In [ ]: