I’m building a wind turbine and as you might imagine, the blades are *Ye Royale Paine In Me Buttocks*. Too big for a CNC, too exposed for a 3D print, too complicated to be made by hand. I decided to make blades from pipes. This simplifies the build but now how do I know how to cut them?

I want to cut them so that they will produce as much torque in given wind conditions as possible. Now I know the question – the search for an answer may commence!

## My Approach

There is a bunch of theory on blade aerodynamics but none of it covers my case. Since *assumption is the mother of all f***ups*, I decided to make none and just test a huge number of freely adjustable designs to find the best one.

Of course I have no intention to produce a *huge number of simulations* by hand. I’ll make virtual experiments with a CFD model and even those I will automate. The whole optimization process with be governed by an external tool. *For the impatient, it’s called DAKOTA – but we’re not dealing with it just yet. First, we must prepare a black-box script that DAKOTA will run – the topic of this post. *

The algorithm of choice will choose input parameters and pass them to a black-box script. It runs a simulation from given parameters. After it’s done, it passes results back to optimization program which in turn decides which parameters to pass to the next iteration. DAKOTA doesn’t give a wet slap about what’s going on in my script. I myself must prepare it so that it does the job.

## The Black-Box Script

Here’s what it does:

- Parses the parameters given by an external optimization program
- Generates a CFD model of the geometry
*It is based on passed parameters and it changes every iteration*. - Creates a mesh
*That includes the air around a single blade and a lot of air up- and downstream of the rotor. I assume the other two blades behave the same – therefore I can copy them with a ‘cyclic’ boundary condition.* - Sets up a CFD simulation
- Runs the simulation
- Post-processes the results
*In this case, we want to know what torque the blade produces . The script reads this value and returns it to the caller.*

## Geometry Definition

A blade’s geometry (how I decided to do it, anyway) is very simple. It is completely described by a few words – the following parameters:

- pipe diameter and wall thickness
- inner angle and span (
`β`

,_{inner}`α`

)_{inner} - outer angle and span (
`β`

,_{outer}`α`

)_{outer} - rotor inner and outer radius

If that’s not enough words for you to imagine, here’s a thousand more:

Inside an optimization iteration, we *know* these parameters. That means we can readily build the model.

## CFD Model

With CFD we’re interested in what’s happening *around* our object. We don’t need a model of the object itself. We need a model of everything that object isn’t – its surrounding fluid.

A CFD model of a blade is simple and can easily be generated using `blockMesh`

. But using that alonethe surrounding domain can’t possibly be created . This could heavily complicate the situation but fear not! I’ll still use blocks but with a plot twist from this blog post. Long story short, I’ll (ab)use `blockMesh`

only to get the precious STL surfaces. `snappyHexMesh`

will then come to the rescue.

To generate `blockMeshDict`

s I’ll utilize my Grand Invention: `classy_blocks`

.

### classy_blocks: Blade

As I mentioned earlier, blade is made from a round pipe cut at the specified angles. This geometry is generated by several `Loft`

operations between pre-calculated `Face`

s. A `Face`

is just a circular arc of specified thickness, starting at angle `β`

and span angle `α`

.

Creating such a face with `classy_blocks`

is easy. Take two points on x-axis, namely `(r`

and _{inner}, 0, 0)`(r`

. The face is defined by two pairs of these two points, first rotated by _{outer}, 0, 0)`β`

, then by `α`

. To generate a circular edge, another pair of points has to be specified: the same two initial points, rotated by `(β+α)/2`

.

Put in code, a Face is generated like this:

```
import numpy as np
import parameters as p # (parameters parser)
from util import geometry as g
from operations.base import Face
def rot(point, angle):
# rotates a 'point' by an 'angle' around z-axis
return g.arbitrary_rotation(point, [0, 0, 1], angle, [0, 0, 0])
def circular_face(r, beta, arc):
# creates a circular Face on specified 'r',
# starting from angle 'beta' and spanning 'arc' angle
# r - radial location of the created face
internal_vertex = np.array([p.pipe_diameter/2 - p.pipe_thickness, 0, r])
external_vertex = np.array([p.pipe_diameter/2, 0, r])
inner_vertices = [
rot(internal_vertex, beta),
rot(internal_vertex, beta + arc),
rot(external_vertex, beta + arc),
rot(external_vertex, beta)
]
# add a single point so that blockMesh will generate a circular edge
inner_edges = [
rot(internal_vertex, beta + arc/2), None,
rot(external_vertex, beta + arc/2), None
]
return Face(inner_vertices, inner_edges)
```

Note that blockMesh will treat all unspecified edges as straight lines. When cutting straight through a pipe at any angle (except axially) the result is always a curve. To obtain a geometry that would resemble a cut pipe, the simplest solution I could think of was simply to create a number of blocks from `r`

to _{inner}`r`

. For each block a linear interpolation between _{outer}`β`

and _{inner}`β`

is used. The same goes for _{outer}`α`

and _{inner}`α`

._{outer}

```
from classes.mesh import Mesh
from operations.operations import Loft
# generate this many blocks span-wise;
# the higher the number, the smoother the curve
n_blocks = 10
mesh = Mesh()
betas = np.linspace(beta_inner, beta_outer, num=n_blocks+1)
arcs = np.linspace(arc_inner, arc_outer, num=n_blocks+1)
radii = np.linspace(p.r_inner, p.r_outer, num=n_blocks+1)
for i in range(n_blocks):
inner_face = circular_face(radii[i], betas[i], arcs[i])
outer_face = circular_face(radii[i+1], betas[i+1], arcs[i+1])
block = Loft(outer_face, inner_face)
block.count_to_size(0, p.pipe_thickness/2)
block.set_cell_count(1, 1)
block.set_cell_count(2, 10)
mesh.add_operation(block)
```

### classy_blocks: Domain

The domain is just a third of a cylinder. Could be `Extrude`

d from a circular-sector `Face`

or a rectangle, revolved by 120°. I went for the latter. Most *work* actually went into specifying patches: `cyclicLeft`

, `cyclicRight`

, `top`

, `inlet`

, `outlet`

. The bottom patch (block’s *front* side) is missing – it’s coincident with rotation axis.

```
from operations.operations import Revolve
# extension in the direction of flow (x-axis)
x_start = np.array([-3*p.r_outer, 0, 0])
x_end = np.array([5*p.r_outer, 0, 0])
# domain is a 120 degree section of a cylinder,
# revolved around y-axis
face = Face([
x_start,
x_end,
p.outside_vertex + x_end,
p.outside_vertex + x_start
]).rotate([1, 0, 0], -p.a/2)
domain = Revolve(face, p.a, [1, 0, 0], [0, 0, 0])
domain.set_cell_count(0, 10)
domain.set_cell_count(1, 30)
domain.set_cell_count(2, 30)
domain.set_patch('bottom', 'cyclicLeft')
domain.set_patch('top', 'cyclicRight')
domain.set_patch('back', 'top')
domain.set_patch('left', 'inlet')
domain.set_patch('right', 'outlet')
```

## Case Organization

A directory in which everything happens includes the following:

`classy_blocks`

Cloned from github and with added`parameters.py`

,`generate_blade.py`

and`generate_donut.py`

scripts.`mesh`

This directory handles generation of three meshes:- blade geometry:
`system/blockMeshDict.blade`

- domain mesh:
`system/blockMeshDict.domain`

- background mesh for snappy:
`system/blockMeshDict.background`

- make_BMD.py: the script that actually generates background mesh for snappy. I talk about this very loudly in an ancient blog post about meshing shortcuts.

- blade geometry:
`case`

The actual simulation case. After the mesh has been finalized and polished, it is copied to`constant/polyMesh`

in this directory. Here, only boundary conditions and whatnot is handled.`Allrun`

script (see below).

## Allrun Script

Allrun scripts from OpenFOAM tutorials are very simple but this one is a bit more complicated. Unfortunately *with great complexity comes a great mess*. Here’s an almost but not quite entirely non-messy script with all Bash (or my) awfulness included.

Let’s go slowly and with lots and lots of apologies.

```
#!/bin/bash
# parameters:
# (Here, the code that parses parameters from optimization program
# is omitted. It belongs to another blog post.)
# constants
r_inner=0.12 # [m]
r_outer=0.75 # [m]
pipe_diameter=0.125 # [m]
pipe_thickness=0.004 # [m]
# optimization parameters (fixed for now)
beta_inner=-120
arc_inner=120
beta_outer=-40
arc_outer=40
###
### CFD MODEL GENERATION
###
. $WM_PROJECT_DIR/bin/tools/RunFunctions
. $WM_PROJECT_DIR/bin/tools/CleanFunctions
### blade: create an STL file by extracting blockMesh patches
# blockMeshDict generation
cd classy_blocks
./generate_blade.py $r_inner $r_outer $pipe_diameter $pipe_thickness \
$beta_inner $arc_inner $beta_outer $arc_outer
mv blockMeshDict.blade ../mesh/system/.
# blade surface extraction
cd ../mesh
cleanCase
runApplication -s blade blockMesh -dict system/blockMeshDict.blade
runApplication surfaceMeshExtract -constant constant/triSurface/blade.stl
```

If you compare `generate_blade.py`

and `generate_donut.py`

you will notice how many lines are dedicated to setting block patches in the latter but not a single is needed in the former. The whole blade is a single patch. Instead of juggling with `block.set_patch()`

where first and last block need special treatment, I can just replace the *defaultFaces* region in STL file with *blade*. That is done with `sed`

.

```
sed -i "s/defaultFaces/blade/" constant/triSurface/blade.stl
# domain surface, the same as blade
cd ../classy_blocks
./generate_donut.py $r_inner $r_outer $pipe_diameter $pipe_thickness \
$beta_inner $arc_inner $beta_outer $arc_outer
mv blockMeshDict.donut ../mesh/system/blockMeshDict.domain
cd ../mesh
runApplication -s domain blockMesh -dict system/blockMeshDict.domain
surfaceMeshExtract -constant -patches "(inlet outlet cyclicLeft cyclicRight top)" constant/triSurface/domain.stl
###
### MESHING
###
# snappyHexMesh: create background mesh first
```

Warning, what comes next is something that *escalated quickly*. In a parametric CFD model, everything is *related* (scaled) with the parameters you chose. That involves multiplication, which Bash, amazingly, refuses to do (except with integers). I had two options, to use another cryptic utility (bc) or a slightly better known tool, Python.

```
#bg_mesh_size=$(bc <<< "scale=3;$pipe_diameter/1.1") # bc
bg_mesh_size=$(python3 -c "print(${pipe_diameter}/1.1)") # python
```

Passed and calculated parameters are then fed into `make_BMD.py`

and inserted into dictionaries for `topoSet`

.

```
./make_BMD.py constant/triSurface/domain.stl $bg_mesh_size
runApplication -s background blockMesh -dict system/blockMeshDict.background
# now everything is prepared to run: snappy and all
runApplication surfaceFeatureExtract
runApplication decomposePar -force
runParallel snappyHexMesh -overwrite
runParallel checkMesh -constant
# toposet: prepare topoSetDict to extract the right MRF zone
#mrf_radius=$(bc <<< "scale=3;$r_outer*1.2")
mrf_radius=$(python3 -c "print(${r_outer}*1.2)")
cp system/topoSetDict.template system/topoSetDict
sed -i "s/{{x1}}/-${pipe_diameter}/g" system/topoSetDict
sed -i "s/{{x2}}/${pipe_diameter}/g" system/topoSetDict
sed -i "s/{{radius}}/${mrf_radius}/g" system/topoSetDict
runParallel topoSet
runParallel setsToZones -noFlipMap
runApplication reconstructParMesh -constant
```

Then, and only, then, the mesh is complete. Moving on to `../case`

directory.

```
###
### SIMULATION
###
# prepare and run the case
cd ../case
cleanCase
# copy mesh from its directory
cp -r ../mesh/constant/polyMesh constant/
runApplication createPatch -overwrite
restore0Dir
# decompose and renumber
runApplication decomposePar -force -time 0
runParallel renumberMesh -overwrite
runParallel simpleFoam
runParallel -s postProcess simpleFoam -postProcess -func yPlus -latestTime
```

The simulation is done and results are ready: what’s left is to extract the relevant data – torque on the rotor. I would like to thank StackOverflow for kindly informing me about `tail`

, `tr`

, `awk`

, `cowsay`

and other useful tools.

```
# extract results from moment.dat
torque=$(tail -n 1 postProcessing/forces_blade/0/moment.dat | tr -d '()' | awk '{print $2}')
cowsay "This design gives you a torque of $torque Mooton-meters"
```

At this point we have the `$torque`

for this iteration. And that’s all! We can go outside and play now!

Well, not exactly. This what’s left to be done:

- Read parameters from an input file
- Write torque to output file
- Set-up DAKOTA and point it to this script
- Run a gazillion of iterations to find the best design.

But we’ll do this in another blog post.

Pingback: OpenFOAM and DAKOTA: a Complete Guide | Damogran Labs

Hi, great job !

as far as possible i also use blockMesh.

but on question: sHM needs pure hex cells with asect ratio approx. 1. As your basemesh violates this criterion, due to the radial face growth, does sHM really work ? I have a similar problem and failed.

Pingback: blockMesh for External Flows - Damogran Labs