Basic flow with a stationary body

In this notebook we will simulate the flow past a stationary body.

using ViscousFlow

using Plots
using Statistics

The basic steps

From the previous notebook, we add one additional step:

Specify the problem: Set the Reynolds number, the free stream, and any other problem parameters
Discretize: Set up a solution domain, choose the grid Reynolds number and the critical time step limits
***Set up bodies***: Create the body or bodies and specify their motions, if any
Construct the system structure: Create the operators that will be used to perform the simulation
Initialize: Set the initial flow field and initialize the integrator
Solve: Solve the flow field
Examine: Examine the results

The rest of the steps are nearly the same as in the previous example.

As before, we initialize the parameters dictionary:

my_params = Dict()

Dict{Any, Any}()

Problem specification

Set the Reynolds number and free stream. We will set the free stream to be in the $x$ direction, with speed equal to 1.

my_params["Re"] = 200
my_params["freestream speed"] = 1.0
my_params["freestream angle"] = 0.0

0.0

Discretize

We set the grid Re to 4.0 here to get a quicker solution, though it is generally better to make this smaller (it defaults to 2.0).

xlim = (-1.0,5.0)
ylim = (-2.0,2.0)
my_params["grid Re"] = 4.0
g = setup_grid(xlim,ylim,my_params)

PhysicalGrid{2}((308, 208), (53, 104), 0.02, ((-1.04, 5.08), (-2.06, 2.06)), 1)

Here, we will set up a rectangle of half-height 0.5 and half-width 0.25 at 45 degrees angle of attack. We also need to supply the spacing between points. For this, we use the function surface_point_spacing

Δs = surface_point_spacing(g,my_params)
body = Rectangle(0.5,0.25,Δs)

Closed polygon with 4 vertices and 108 points
   Current position: (0.0,0.0)
   Current angle (rad): 0.0

We place the body at a desired location and orientation by creating a joint. This joint "joins" the body to the inertial coordinate system. In order to create this joint and apply it, we first need to place the joint in the inertial coordinate system with a MotionTransform.

cent = [0.0,0.0] # center of joint with respect to inertial system
α = 45π/180 # angle of joint with respect to inertial system
X = MotionTransform(cent,α)
joint = Joint(X)

Joint of dimension 2 and type FreeJoint2d
   Constrained dofs = [1, 2, 3]
   Exogenous dofs = Int64[]
   Unconstrained dofs = Int64[]

The next two steps will seem unnecessarily cumbersome, but they reveal an important aspect of how this package treats surface motion. Every problem with bodies has joints, and every joint has at least one degree of freedom, even if none of these degrees of freedom is meant to vary in time.

For this reason, we must always create a RigidBodyMotion object and a joint state vector, x, even if there is no motion. In this example, x is just a vector of 3 zeros (describing the angle, x, and y coordinates of the joint).

To set the body in place, we use update_body!(body,x,m). After the operation is applied, body is transformed to the correct location/orientation.

m = RigidBodyMotion(joint,body)
x = init_motion_state(body,m)
update_body!(body,x,m)

Closed polygon with 4 vertices and 108 points
   Current position: (0.0,0.0)
   Current angle (rad): 0.7853981633974483

Let's plot it just to make sure

plot(body,xlim=xlim,ylim=ylim)

Construct the system structure

This step is like the previous notebook, but now we also provide the body as an argument. It is important to note that we have not provided any explicit information about the boundary conditions on our shape. It therefore assumes that we want to enforce zero velocity on the shape. We will show another example later in which we change this. Note that we have to supply the RigidBodyMotion object via the motions keyword.

sys = viscousflow_system(g,body,phys_params=my_params,motions=m);

Initialize

Now, we initialize with zero vorticity. Note that we do this by calling init_sol with no argument except for sys itself.

u0 = init_sol(sys)

(Dual nodes in a (nx = 308, ny = 208) cell grid of type Float64 data
  Number of Dual nodes: (nx = 308, ny = 208), [0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0  …  0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0], [0.0, 0.0, 0.0])

and now create the integrator, with a long enough time span to hold the whole solution history:

tspan = (0.0,20.0)
integrator = init(u0,tspan,sys)

t: 0.0
u: (Dual nodes in a (nx = 308, ny = 208) cell grid of type Float64 data
  Number of Dual nodes: (nx = 308, ny = 208), [0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0  …  0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0], [0.0, 0.0, 0.0])

Solve

Now we are ready to solve the problem. Let's advance the solution to $t = 1$.

@time step!(integrator,1.0)

 13.710600 seconds (5.61 M allocations: 1.986 GiB, 0.79% gc time, 48.79% compilation time)

Examine

Let's look at the flow field at the end of this interval

plot(
plot(vorticity(integrator),sys,title="Vorticity",clim=(-15,15),levels=range(-15,15,length=30), color = :RdBu,ylim=ylim),
plot(streamfunction(integrator),sys,title="Streamlines",ylim=ylim,color = :Black),
    size=(700,300)
    )

Compute the moment and force histories

To do this, we supply the solution history sol, the system sys, and the index of the body (1).

sol = integrator.sol;
mom, fx, fy = force(sol,sys,1);

Plot the histories. Note that we are actually plotting the drag and lift coefficient histories here: $ CD = \dfrac{Fx}{\frac{1}{2}\rho U\infty^2 L}, \quad CL = \dfrac{Fy}{\frac{1}{2}\rho U\infty^2 L}, \quad Cm = \dfrac{M}{\frac{1}{2}\rho U\infty^2 L^2} $ Since the quantities in this simulation are already scaled by $\rho$, $U_\infty$, and $L$ (because $\rho$ has been scaled out of the equations, and the free stream speed is set to 1 and the height of the shape to 1), then we obtain these coefficients by simply dividing by 1/2, or equivalently, by multiplying by 2:

plot(
plot(sol.t,2*fx,xlim=(0,Inf),ylim=(0,4),xlabel="Convective time",ylabel="\$C_D\$",legend=:false),
plot(sol.t,2*fy,xlim=(0,Inf),ylim=(-4,4),xlabel="Convective time",ylabel="\$C_L\$",legend=:false),
plot(sol.t,2*mom,xlim=(0,Inf),ylim=(-4,4),xlabel="Convective time",ylabel="\$C_m\$",legend=:false),
    size=(800,350)
)

The mean drag and lift coefficients (omitting the first two steps) are

meanCD = mean(2*fx[3:end])

2.123193095975185

meanCL = mean(2*fy[3:end])

-0.7050286530831306

This page was generated using Literate.jl.