Sample generation using DAFoam

This section explains how to use WingFFD module for generating samples using DAFoam. There are typically three main steps involved in the process: setting up options and initializing the module, adding design variables and generating samples. The WingFFD module is demonstrated using a CRM wing example. This script is available in examples directory of the repository on github.

Setting up options

First step involves creating options dictionary which is used for initializating the module. There are five mandatory options: solverOptions, ffdFile, gridFile, liftIndex and aeroProblem, rest all are optional, please refer options section for more details. Following snippet of the code shows an example:

from blackbox import WingFFD
from baseclasses import AeroProblem
import numpy as np

solverOptions = {
    "designSurfaces": ["wing"],
    "solverName": "DARhoSimpleCFoam",
    "primalMinResTol": 1e-6,
    "primalMinResTolDiff": 1e2,
    "checkMeshThreshold": {
        "maxAspectRatio": 1000.0,
        "maxNonOrth": 70.0,
        "maxSkewness": 4.0,
        "maxIncorrectlyOrientedFaces": 0,
}

# Creating aeroproblem for adflow
# Chord ref is 1.0 since all the dimensions are scaled according to it
ap = AeroProblem(
    name="crm", alpha=2.0, mach=0.85, reynolds=5e6, reynoldsLength=1.0, T=298.15,
    areaRef=3.407014, chordRef=1.0, evalFuncs=["cl", "cd", "cmy"], xRef=1.2077, yRef=0.0, zRef=0.007669
)

# Options for blackbox
options = {
    "solver": "dafoam",
    "solverOptions": solverOptions,
    "openfoamDir": ".",
    "gridFile": "crm_volMesh.cgns",
    "ffdFile": "crm_ffd.xyz",
    "liftIndex": 3, # Very important
    "aeroProblem": ap,
    "noOfProcessors": 8,
    "writeDeformedFFD": True,
    "getSurfaceForces": True
}

# Initialize the class
wing = WingFFD(options=options)

Firstly, required packages and modules are imported. Then, solverOptions dictionary is created, refer DAFoam documentation for more details. Then, AeroProblem object is created which contains details about the flow conditions and the desired output variables are defined using evalFuncs argument. Then, options dictionary is created, refer options section for more details.

Note

In solver options dictionary for DAFoam, no need to mention arguments such as primalBC, function, normalizeStates, inputInfo. These options are internally set before each analysis.

In the options dictionary, you can provide the location of 0, constant, and system directories (required by openfoam) by using openfoamDir argument. This is the location where blackbox will look for these directories. The default location is "." i.e. current working directory, refer options section for more details.

Adding design variables

Next step is to add design variables based on which samples will be generated. The addDV method needs three arguments:

  • name (str): name of the design variable to add. The available design variables are:

    • shape: FFD control points which parameterize the airfoil shape

    • twist: Twist of the airfoil sections along the wing span, number of sections will be one less than the sections defined in the FFD file since root is fixed

    • alpha: Angle of attack for the analysis

    • mach: Mach number for the analysis

    • altitude: Altitude for the analysis

  • lowerBound (numpy array or float): lower bound for the variable

  • upperBound (numpy array or float): upper bound for the variable

    Note

    When shape variable is to be added, the lower and upper bound should be a 1D numpy array of the same size as the number of FFD points. The number of FFD points can be accessed via nffd attribute of the class.

    When twist variable is to be added, the lower and upper bound should be a 1D numpy array of the same size as the number of section defined in the FFD file minus one. The twist is defined in degrees. The number of twist sections can be accessed via nTwist attribute of the class.

    For other cases, lower and upper bound should be float.

Following code snippet adds alpha and mach as design variables:

# Add alpha as a design variable
wing.addDV("alpha", lowerBound=1.5, upperBound=3.5)

# Add mach as a design variable
wing.addDV("mach", lowerBound=0.7, upperBound=0.8)

Generating samples and accessing data

After adding design variables, generating samples is very easy. You just need to use generateSamples method from the initialized object. This method has two arguments:

  • numSamples (int): number of samples to generate

  • doe (numpy array): 2D numpy array in which each row represents a specific sample

Note

You can either provide numSamples or doe i.e. both of them are mutually exclusive. If both are provided, then an error will be raised.

Typically, numSamples (int) should be used for generating samples. This option will internally generate doe based on the options provided while initializating the module. In some cases, you might want to generate samples based on your own doe. In that case, you use doe (numpy array) argument. Following snippet of the code will generate 5 samples using internally generated doe:

wing.generateSamples(numSamples=5)

You can see the following output upon successful completion of sample generation process:

  • A folder with the name specificed in the directory option (or the default name - output) is created. This folder contains all the generated files/folders.

  • Within the main output folder, there will be subfolders equal to the number of samples you requested. Each of the folder corresponds to the specific analysis performed. It will contain log.txt which contains the output from mesh generation and solver. There will be other files depending on the options provided to solver and blackbox.

  • data.mat file which contains:

    • Input variable: a 2D numpy array x in which each row represents a specific sample based on which analysis is performed. The number of rows will be usually equal to the number of samples argument in the generateSamples method. But, many times few of the analysis fail. It depends a lot on the solver options, so set those options after some tuning.

      Note

      The order of values in each row is based on how you add design variables. In this tutorial, first alpha is added as design variable and then shape coefficients are added. Thus, first value in each row will be alpha, next nffd values will be FFD coefficients, and then nTwist values will be twist values.

    • Outputs: There are two kinds of outputs - mandatory and user specificed. The evalFuncs argument in the aero problem decides the user desired outputs. Along with these outputs, volume of the wing is the mandatory output. Following snippet shows how to access the data.mat file. In this tutorial, evalFuncs argument contains cl, cd, cmy. So, data.mat will contain these variables, along with volume:

      from scipy.io import loadmat
data = loadmat("data.mat") # mention the location of mat file

x = data["x"]
cl = data["cl"]
cd = data["cd"]
cmy = data["cmy"]
volume = data["volume"]

  • description.txt: contains various informations about the sample generation such as design variables, bounds, number of failed analysis, etc.

Extracting surface force data

To get forces at each surface mesh coordinate, set the option getSurfaceForces to True, refer options section for more details. This creates a surfaceForces.mat file in each corresponding analysis folder. This mat file contains two variables: forces and surfaceCoords. The forces is a 2d numpy of size Ncoords x 3, where Ncoords is the number of surface mesh points and 3 corresponds to x, y, and z component of the force vector. The surfaceCoords is also a 2d numpy array of size Ncoords x 3, containing surface mesh coordinates. These forces and surface coordinates can be extracted as shown in previous section using loadmat function from scipy.