Sample generation with CST

This section explains how to use AirfoilCST module for generating samples. There are typically three main steps involved in the process: setting up options and initializing the module, adding design variables and generating samples.

Setting up options

First step involves creating options dictionary which is used for initializating the module. The airfoilFile and numCST are the two mandatory options, rest all are optional, please refer options section for more details. Following snippet of the code shows an example:

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

solverOptions = {
    # Common Parameters
    "monitorvariables": ["cl", "cd", "cmz", "yplus"],
    "writeTecplotSurfaceSolution": True,
    "writeSurfaceSolution": False,
    "writeVolumeSolution": False,
    # Physics Parameters
    "equationType": "RANS",
    "smoother": "DADI",
    "MGCycle": "sg",
    "nsubiterturb": 10,
    "nCycles": 7000,
    # ANK Solver Parameters
    "useANKSolver": True,
    "ANKSubspaceSize": 400,
    "ANKASMOverlap": 3,
    "ANKPCILUFill": 4,
    "ANKJacobianLag": 5,
    "ANKOuterPreconIts": 3,
    "ANKInnerPreconIts": 3,
    # NK Solver Parameters
    "useNKSolver": True,
    "NKSwitchTol": 1e-6,
    "NKSubspaceSize": 400,
    "NKASMOverlap": 3,
    "NKPCILUFill": 4,
    "NKJacobianLag": 5,
    "NKOuterPreconIts": 3,
    "NKInnerPreconIts": 3,
    # Termination Criteria
    "L2Convergence": 1e-14
}

meshingOptions = {
    # ---------------------------
    #        Input Parameters
    # ---------------------------
    "unattachedEdgesAreSymmetry": False,
    "outerFaceBC": "farfield",
    "autoConnect": True,
    "BC": {1: {"jLow": "zSymm", "jHigh": "zSymm"}},
    "families": "wall",
    # ---------------------------
    #        Grid Parameters
    # ---------------------------
    "N": 129,
    "s0": 1e-6,
    "marchDist": 100.0,
}

# Creating aeroproblem for adflow
ap = AeroProblem(
    name="ap", alpha=2.0, mach=0.734, reynolds=6.5e6, reynoldsLength=1.0, T=288.15,
    areaRef=1.0, chordRef=1.0, evalFuncs=["cl", "cd", "cmz"], xRef = 0.25, yRef = 0.0, zRef = 0.0
)

# Options for blackbox
options = {
    "solverOptions": solverOptions,
    "noOfProcessors": 8,
    "aeroProblem": ap,
    "airfoilFile": "rae2822.dat",
    "numCST": [6, 6],
    "meshingOptions": meshingOptions,
    "writeAirfoilCoordinates": True,
    "plotAirfoil": True,
    "writeSliceFile": True,
    "samplingCriterion": "ese"
}

airfoil = AirfoilCST(options=options)

Firstly, required packages and modules are imported. Then, solverOptions and meshingOptions are created which determine the solver and meshing settings, refer ADflow and pyHyp options 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. Finally, the AirfoilCST module is initialized using the options dictionary.

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:

    • upper: CST coefficients of upper surface. The number of variables will be equal to first entry in numCST list in options dictionary.

    • lower: CST coefficients of lower surface. The number of variables will be equal to second entry in numCST list in options dictionary.

    • N1: First class shape variable for both upper and lower surface. Adds only variable for both surfaces.

    • N2: Second class shape variable for both upper and lower surface. Adds only variable for both surfaces.

    • 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 upper or lower variable are to be added, the lower and upper bound should be a 1D numpy array of the same size as the number of CST coefficients for that particular surface mentioned in the options dictionary. For other cases, lower and upper bound should be float.

Following code adds alpha, upper and lower as design variables:

airfoil.addDV("alpha", 2.0, 3.0)

# Adding upper surface CST coeffs as DV
coeff = airfoil.DVGeo.defaultDV["upper"] # get the fitted CST coeff
lb = coeff - np.sign(coeff)*0.3*coeff
ub = coeff + np.sign(coeff)*0.3*coeff

airfoil.addDV("upper", lowerBound=lb, upperBound=ub)

# Adding lower surface CST coeffs as DV
coeff = airfoil.DVGeo.defaultDV["lower"] # get the fitted CST coeff
lb = coeff - np.sign(coeff)*0.3*coeff
ub = coeff + np.sign(coeff)*0.3*coeff

airfoil.addDV("lower", lowerBound=lb, upperBound=ub)

Here, the upper and lower bound for lower and upper variable are +30% and -30% of the fitted CST coefficients. You can also remove a design variable using removeDV method. It takes only one input which is the name of the variable.

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 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 and run the analysis. 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 10 samples:

airfoil.generateSamples(numSamples=10)

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 and meshing 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. Then, lower and upper surface CST coefficients are added. Thus, first value in each row will be alpha, next 6 values will be upper surface CST coefficients and last 6 will be lower surface CST coefficients.

    • Output variables: There are two kinds of output variables - mandatory and user specificed. The evalFuncs argument in the aero problem decides the user desired variables. Along with these variables, area of the airfoil is the mandatory objective.

    Following snippet shows how to access the data.mat file. In this tutorial, evalFuncs argument contains cl, cd, cmz. So, data.mat will contain these variables, along with area:

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

x = data["x"]
cl = data["cl"]
cd = data["cd"]
cmz = data["cmz"]
area = data["area"]

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