CFD Modeling of Wind Tunnel Flow

over a Rotating Cylinder

John Middendorf

Student Number 3049731

Computation Fluid Dynamics

Professors Tracie Barber/Eddie Leonardi

May 30, 2003

I hereby certify that this is my own and original work,

and that all references have been cited.

signed

John Middendorf

Flow over a Rotating Cylinder

Background

Viscous flow over a rotating cylinder is an interesting problem in fluid dynamics. The rotation of a

no-slip cylinder wall creates a pressure gradient which in turn creates lift. The pressure gradient can be

explained simply by Bernoulli’s principle, in which pressure and velocity are inversely proportional.

The phenomena of a rotating cylinder’s lift is know as the Magnus effect, named after a 19

th

century

German engineer, and is related to the circulation around an object in a flow field. Rayleigh studied

the lift of a rotating cylinder for an inviscid (“frictionless”) fluid, and related lift to the circulation of a

rotating cylinder by the following formula:

in which the circulation, , is given by:

, therefore,

The relationship between lift and circulation is known as the Kutta Joukowsky relationship and applies

to all shapes, particularly to the aerodynamic shapes such as an airplane wing.

In a viscous fluid, like air, the cylinder is subjected to both pressure and viscous forces, and the

explanation is more complex. Studies (Smith, 1979) indicate that the circulation does not result from the

common explanation of the air set into an opposing rotation by the friction of a no-slip wall, as this only

occurs in a very thin boundary layer next to the surface. But this motion of the fluid in the boundary

layer does affect the manner in which the flow separates from the cylinder. Boundary layer separation is

moved back on the side of the cylinder that is moving with the fluid, and is moved forward on the side

opposing the main stream. The wake then shifts to the side moving against the main stream causing

the flow to be deflected on that side, and the resulting change in free stream flow creates a force on the

spinning cylinder.

Problem Statement and Parameters.

A cylinder 0.66m in diameter (R=0.33) is modeled as a wind tunnel test. Two parameters for the wall

boundaries were modeled in the different grids created, one with walls at 6R above and below the wheel

boundaries, giving a total height of the wind tunnel as 4.62 meters, and the other (for some of the later

CFD models) using a height of 6R from the center, giving a total height of the wind tunnel at 4 meters.

Using Fluent, the problem was analyzed in two dimensions, which in effect models an infinite width

cylinder. The cylinder is rotating at 168 radians/sec, and the windspeed flow in the wind tunnel is 200

km/hr (55.6m/s). There are two Reynolds Numbers of interest: one is the Re of the cylinder, which is:

The other Reynolds Number of interest, used for turbulence parameters is the free stream Reynolds

number, given by the characteristic length of the wind tunnel (using the 4 meter wind tunnel height

parameter):

Boundary Conditions of Wind Tunnel

It is important to accurately represent in the computational model the free stream flow in the wind tunnel

by the choice of an appropriate length. Since CFD is driven by boundary conditions, where the property

values of all the elements inside the BCs are essentially “filled in” to attain an equilibrium solution, the

placement of the inlet and outflow affects the solution. The inlet boundary is set far enough in front

of the cylinder so as to represent fully developed flow by the time the flow reaches the cylinder (since

the inlet will be set at a initial velocity, constant for all values). The modeled developed flow when

it reaches the cylinder will vary from the inlet boundary conditions because the no-slip wind tunnel

walls will slow the velocity near the wall boundaries, affecting also the modeled turbulence as the flow

approaches the cylinder. Ten times the diameter of the circle was chosen as a minimum inlet distance in

the CFD models.

The outlet boundaries also need to be far away from the point of interest, but for additional reasons

related to the assumptions of the solution process. CFD models have two main types of free flow

outlet boundary settings: outflow, and pressure outlet (generally constant pressure). Pressure outlet

boundaries are used to define the static pressure at the outlet, and are recommended with compressible

flow problems. Outflow boundary conditions are used when details of the flow velocity and pressure

are unknown prior to solution of the flow problem, and assume a zero gradient for all variables except

pressure. Outflow BCs are only appropriate when exit flow is in a fully developed condition. For

this to occur after a turbulent wake, at least ten times the diameter of the object causing the wake is

recommended (Versteeg and Malalasekera, 1995). The outflow BC was used, and values of at least

twenty times the diameter of the circle was chosen for the outlet boundaries.

The initial inlet flow of the wind tunnel is not known completely, but it was assumed that there pre-

exists a specific amount of turbulence in the flow field. The computational algorithm uses parameters

that are related to the creation and dissipation of turbulence. Some, like the Intensity and Length scale

parameters, are based on the assumption that the characteristic velocity and the characteristic length of

the larger turbulent eddies in the solution are of the same order as the velocity and length scale of the

mean flow, a major assumption of CFD turbulence models. Wind tunnel flows vary in their turbulence

characteristics, with turbulence intensity factors being as low as 0.05%. Intensity and length scales can

be based on fully developed duct flow by the formula and approximate relationship below:

which gives values of k and e of:

The choice of these turbulence parameters are used for the inlet BC’s and will change as the model

solves. The converged solution should be independent of the initial values, yet it is important to start

with reasonable values for the k and e, as it affects the downstream flow. Other turbulence factors can

be derived from these numbers, including the Modified Turbulent Viscosity and the Specific Dissipation

Rate (used for K-omega models).

Another, separate, parameter used to define the turbulence in CFD models in the Turbulent Viscosity

ratio. This ratio is directly proportional to the turbulent Reynolds number, which is defined in terms of

the turbulent kinetic energy, the dissipation rate and the viscosity, and is usually in the range of a value

between one and ten.

Each one of the turbulent initial boundary conditions has assumptions which relate one to another, and is

a source of error. Some, like the relationship between the turbulent dissipation rate and the length scale

are based on empirical constants. To accurately model a wind tunnel situation these initial turbulence

values would need to be calculated from empirical data to obtain accurate results. Fluent recommends

for wind tunnel situation in which the model is mounted in a test section downstream of a mesh screen

of using a value of e based on the decaying turbulence in the length of the wind tunnel. If we assume

that turbulence decay (for the main flow) to be 10% in a 20 meter wind tunnel, we get an approximate

value for e to be:

which eliminates the need for the length scale assumption based on the hydraulic diameter. Using this

method, it is important to check turbulent viscosity ratios to ensure they are not out of range. Another

way is to specify the initial guess for e so that the resulting eddy viscosity

is sufficiently large

in comparison to the molecular viscosity, and base the value for e on the rule of thumb that the turbulent

viscosity is roughly two orders of magnitude greater than the molecular viscosity. As can be seen, the

range in which the initial turbulence values vary, based on assumptions, is considerable. It is possible

that the turbulent initial conditions should be set at the scale of the cylinder, in which case the length

scale would be on the order of 0.66m x 0.07. Initial runs, were, in fact run with this figure.

The effect of the wind tunnel walls.

The wind tunnel walls were models as the standard no-slip WALL type boundary in Fluent. They were

quite close to the cylinder, computationally speaking, and have an effect on the solution both because of

the way the solution computes, as well as the differences between bounded and unbounded flow. Since

out model is modeling bounded wind tunnel flow, is important to model the wind tunnel walls quite

carefully with enough grid points to accurately model a boundary condition that reflects a no-slip wall

velocity profile. In my earlier grid models, this was not done to the precision required for this problem

and is likely a major source of error. Checking the effects of the walls is done by changing the boundary

condition for the top and bottom walls from WALL to OUTFLOW, and can be seen in the last part of the

results.

Grid

Gambit was the preprocessor used to create the geometry and the grid. Both triangular and quad

meshes were created, in total over 15 grids of varying dimensions and element types. Problems became

immediately apparent with a poor grid, namely immediate high y+ values at the boundaries. In the

results following, it was clear from the high y+ values (on the order of 1500-3500) that even my finest

grid was too coarse in the boundary layers. The aspect ratio can be a source of error when the longer

side of an element is facing the direction of flow; it is preferable to have elements with a large aspect

ratio with the short side facing the flow. The other factors that are important to consider when creating

a grid are the skew, and the gradient from one element to another. For proper turbulence modeling,

opinions differ, but a gradient of 5% (change in size from one element to the next) should be adequate.

More comments regarding grid types and geometry can be found in the results. It was helpful to check

the grid in Fluent, and reordering the domain sped things up significantly, especially for the models

which had multiple faces. The ideal quad grid for this problem has very fine resolution at the circle and

fine resolution at the wind tunnel wall boundaries. Spacing of mesh points in between the wall and the

circle can be larger. Similarly, to minimize excessive grid points, the spacing of mesh seeds behind

the circle could grow to create elements with very long aspect ratio which, aligned with the flow, should

solve adequately.

Grid Convergence.

It is possible to use the results from successively finer grids to calculate the error resulting from the

grid. Grid convergence calculations on a sequence of grids based on results pages 16 and following are

presented here:

Grid

Number of Nodes

Functional (-) Functional

Medium

31368

Lift=1024.7

Drag=960.1

Fine

47095

Lift=1179.2

Drag=930.2

“SuperFine”

97096

Lift =1278.5

Drag=908.0

The refinement ratio between the grids is given by

and the relative errors:

The grid convergence indexes using the fine and the medium grids are:

The grid convergence indexes using the fine and superfine grids are:

Using these estimate we can estimate the error in our solutions due from the grid, we find the value for

lift for the superfine grid is in about 18% error due to grid parameters.

CFD MODELING AND PARAMETERS

General

CFD models solve fluid problems with five basic equations of state:

•

Mass conservation (continuity)

•

x,y,z momentum equations

•

Energy equations

Among the unknowns are density, pressure, temperature, and internal energy. Additional relationships

among the variables are derived from the Navier-Stokes equations, in which the viscous stress

components are integrated with the momentum equations. For the rotating cylinder problem, we assume

that the fluid (air) is behaving as an incompressible fluid at constant temperature (since the Mach

number is low), and therefore do not need the energy equation. The results following only use the mass

conservation and momentum equations of state.

For turbulent modeling, additional transport equations are used to account for time averaged fluctuations

in the local fluid velocities that occur with turbulence, which give rise to additional stress on the fluid,

the Reynolds stresses. Reynolds stresses create 6 more unknowns in the equations (three additional

unknowns for 2D problems), and are accounted for by additional approximated equations, depending on

the model.

Discretization

The solution process depends on solving partial differential equations. CFD uses a control volume

technique to convert the PDE’s into algebraic equations that can be solved numerically, resulting in a

solution which satisfies the governing equations in every element in the grid. Fluent uses a upwind/

central differencing scheme, in which the convection terms are solved using upwinding, and the

diffusion terms are centrally differenced. First order upwind schemes assume that the cell center values

of the variables represent the cell-average value and the face values of the control volume have the

same value. Second order schemes include the second order term of a Taylor series expansion of the

PDE’s, and are more accurate. Fluent also offers the QUICK Scheme which are based on averaging the

second order upwind and central differences of a variable. The QUICK scheme is recommended for

structured quad grids which are aligned with the flow direction.

Convergence and Under Relaxation

The model is considered solved mathematically when the values in the entire grid are “converged” and

do not change significantly from one iteration to the next. The change in value is known as the residual.

Depending on the model chosen, the necessary residual levels for convergence varies. First order

schemes generally converged adequately when the residual level was set at 0.001, while the second

order schemes required a lower residual value, not necessarily at 0.0001 but somewhere in between.

There are no hard and fast rules relating convergence to the residuals; for example, if the initial

conditions are initialized at the values close to the final solution, there will be small residuals; likewise,

if the initialization is very different from the final solution, there will be a larger drop in residuals.

Generally convergence level was monitored by the slope of the residual plot, and by looking at the

change of a functional. When the functional value stabilized to a certain value, then convergence was

likely. This can be monitored visually by turning on the plot forces charts.

Sometimes models converge very slowly, in this case, it is possible to change the under relaxation

factors of the solution process. This needed to be done somewhat carefully, as the solution could

seemingly converge quicker with higher under relaxation factors. For some models, like the Reynold’s

Stress Model, Fluent recommends lowing the under relaxation numbers dramatically, from the defaults

(on the order of 0.7) to 0.2 or 0.3. Fluent also recommends using residual levels of 0.0001 for the RSM.

Near wall treatments and boundary layer approximations for turbulence models.

In free stream flow, where Reynolds numbers are high (on the order of 100,000 to 10,000,000), the

inertia forces in the fluid are much greater than the viscous forces, and the equations are solved on

the basis of small viscous components. However, at wall boundaries, where velocities approach zero,

the viscous forces will be equal in order of magnitude of the inertia forces, or even larger. Therefore,

a separate calculation is required for such regions which include the effect of the viscous forces. A

boundary layer can be sub divided into 3 parts:

Viscous sublayer: the layer closest to the wall where viscous effects dominate and the flow is laminar (as

turbulent eddying motions must stop in layers where there is no velocity).

Transition layer: where both viscous and inertia effects are considered.

Outer layer: where inertia forces are dominant and the flow is turbulent.

In CFD models, the measurement which determines the layer region (and thus the specific calculations

that are performed) is the value known as y+, which is a dimensionless value based on the values of

density, viscosity, shear stresses due to velocity, and the distance from the wall (

).

For low values of y+ (y+<11.225 in Fluent), the flow is modeled as laminar. For the transition layer,

with mid range values of y+ (30 < y+ < 60), the flow is modeled as turbulent where viscous forces

are included in the calculations. Shear stresses are assumed constant in this region and equal to the

wall shear stress. The outer, turbulent layer is modeled with inertia forces as dominant in the CFD

calculations, and direct viscous effects are ignored.

Fluent uses two equations to calculate the wall shear stress based on the value of y+. If the value of y+

in the cell adjacent to the wall is within 11.225, Fluent uses the laminar stress strain relationship:

If the value of y+ is greater than 11.225, then fluent uses the Law of the Wall equation to solve the flow

for the cell adjacent to the wall boundary:

where k and E are constants based on empirical data. E is related to wall roughness.

In modeling with CFD, it is important to ensure that the grid is fine enough at the wall boundaries

to ensure that the y+ values are not too high, as it is in this region where the CFD programs include

viscous shear stresses in the calculations. The y+ values at the wall boundaries is marginally affected

by the choice of model (which may vary in their calculations of turbulent viscosity), but the main factor

that affects the y+ values is the mesh. Generally, the first thing to do after running a model is to plot

y+ values at the boundary to check to see the range of values. If the y+ values of the cells adjoining

the wall surface are greater than 500 (at best), the results there will be in error, as the program will be

including viscous effects in regions of the model that are outside the transition boundary layer. A finer

mesh is required in such cases. y+ values of 60 or less are desired, but note that the maximum allowable

y+ value, where the values of the log of y+ plotted against u+ are linearly related, increases as the

Reynolds number increases.

Fluent uses two main choices for modeling the wall. The Enhanced Wall Treatment is the preferred

model, as it includes reasonable equations for all points in the mesh. It is chosen as an option in fluent,

which is somewhat deceiving, since one would assume that solving as accurately as possible with the

equations of state and the turbulent equations in every cell would be the default. Fluent recommends

having a mesh which results in y+ values between 1 and 5 in the mesh points adjoining the wall

boundary as a minimum, something I did not see as being possible in a mesh of less that 300,000 nodes

for our problem. However, Fluent uses a two layer approach which includes a blending term which

allows coarser meshes to solve even if the mesh elements adjacent to a wall are not within the inner

boundary layers. If the Enhanced Wall Model is used, there is an option to include pressure gradient

effects.

The other model Fluent uses is the Wall Functions, and is the default. Wall functions make additional

assumptions regarding the transition layer, and when wall function is selected, Fluent does not solve

directly for flow in this viscosity affected region, rather, calculations are based on assumptions arising

from the linear part of the log y+/u+ plot. Still, it is recommended to keep y+ values close to 30 when

using this model, although values up to 500 may be acceptable for high Reynold’s number flows. Above

these numbers, the wake component becomes larger (where velocities may change direction).

The non-equilibrium wall functions option is a variation to the standard wall functions which include

pressure gradient calculations, and are recommended for flows which involve separation (although the

enhanced wall treatment is more applicable in such flows).

Turbulence models

Various models were utilized to study the rotating cylinder in the wind tunnel, and varied considerable

in the results. The total number of choices and sub-choices are staggering. Excluding the variations of

the setting of initial conditions, which varied from model to model, as well excluding energy solution

parameters, the total number of turbulent model options exceeds 50, if one includes the choices of

wall treatments for each model. Without direct experience with each specific model, it is difficult to

choose the best one for our scenario. For example, it is difficult to know on what scale “swirl” is fluid

dynamically defined without seeing computational examples of it. Many models were tried, and many

failed. The basis of each turbulence model is discussed here.

Spalart-Allmaras Turbulence Models

The Spalart-Allmaras is a one-equation (in addition to the general transport equations) turbulence

model which solves for the turbulent eddy viscosity, and eliminates the need to calculate the length

scale related to local turbulence. Although designed to be used with meshes that fully resolve the inner

boundary layer (i.e, cells with y+ values of 1-11.25), in which case the enhanced wall treatment option

should be selected, it has been shown to be adequate for coarser meshes if the wall function option is

chosen. When using this model, the Strain/Vorticity based turbulence production option should probably

be used for flows which include separation, as it includes the effects of the mean strain due to rotational

velocity gradients. My runs show mixed results with the Spalart Allmaras.

K-e Turbulence Models

The K-e models are the workhorse of the CFD industry, and have been shown to be robust in a variety

of applications. K-e models use two equations to calculate turbulent Reynolds stresses, based on

calculations of turbulent kinetic energy (k), and turbulent dissipation (e). The k-e model uses additional

constants based on empirical data from a wide range of flows. However, although the turbulent kinetic

energy can be calculated quite precisely, the dissipation rate is a bit of a fudge, as there are many

unknown and unmeasurable terms in the dissipation equations. The basic assumption is that turbulent

dissipation is on the same order of the turbulent production term, and the K-e model applies mostly to

flows that are fully turbulent, where the effects of molecular viscosity are negligible. The model has

problems with flows that have curved boundary layers, as our rotating cylinder problem does, yet it was

used for many of the runs in the results because of its consistent results.

Besides the standard K-e model, two more variations are available in Fluent. The RNG model also

uses two equations for turbulence kinetic energy and dissipation, yet has different constants and

calculates the effective viscosity differently. It is considered more responsive to flows with rapidly

changing strains, and for flows with high streamline curvature. Two options are available with RNG:

“differential viscosity”, which accounts for low Reynolds number changes to turbulent viscosity, and

is only recommended for grids which are refined in the boundary layer. The other is “swirl dominated

flow”, which also affects the turbulent viscosity calculations and used for flows which have significant

swirl. When using the RNG model, it is recommended to begin with a solved solution from the standard

K-e model, although I didn’t have much luck with this technique. The third K-e model is the Realizable

model, which uses a similar equation for turbulent kinetic energy, but calculates turbulent dissipation

independent of the rate of production. This makes the model more likely to diverge with a poor model,

but is shown to produce better results for flows which include mixing layers and boundary separation.

Good results were had with the Realizable model.

K-omega Turbulence Model

The K-omega model also uses two equations to represent the turbulence, but instead of e, it calculates

a specific turbulence dissipation rate, which can be considered the ratio of e to k. It is recommended

for low Reynolds number flows, and does not offer the standard wall function choices in Fluent, as by

default, it uses the enhanced wall treatment methods described above; that is, it solves for near wall

treatments when the mesh is fine enough, and uses wall functions when the mesh elements are not

placed entirely within the boundary layer. The SST (Shear-Stress Transport) K-omega model takes into

account the transport of turbulent shear stress, and makes a gradual change of solution variables from the

standard K-omega model in the inner region of the boundary layer to a high Reynold’s number version

of the K-e model in the outer part of the boundary layer. The SST K-omega model is more reliable for

flows which have adverse pressure gradients, and would be the preferred model, of the two k-omega

choices,for modeling the rotating cylinder, as it includes boundary separation. Options for the K-omega

model include transitional flows (a low Reynolds number correction to turbulent viscosity), and for the

standard K-omega model, shear flow corrections.

Reynold’s Stress Equation Turbulence Models

The most advanced (requiring the most computational resources) classic turbulence model is the

Reynold’s Stress Model (RSM), which uses equations to solve directly for the Reynold’s stresses.

Five additional equations are involved in the 2D model (seven in 3D), and because it makes fewer

assumptions about the turbulent eddy formations and dissapations, it is considered the “simplest” and

most accurate of the turbulence models for fluid flows.

Recommendations

The standard K-e model with enhanced wall functions, is the model that seemed to work overall the best

for my models, despite its not being recommended for problems due to the high pressure gradients and

separated flow. There were also good runs with the K-e Realizable with enhanced wall functions. Other

possible models would include the K-omega SST with the transitional flows option, and perhaps even

the Spalart Allmaras with the Strain/Vorticity option and with standard wall functions, for the coarser

meshes. For a three dimensional model, perhaps swirl would be a consideration on the ends of the

cylinder, and would require a model like the RNG with swirl modifications. The RSM model solved

occasionally in my runs, but requires better meshwork than I was able to provide. Perhaps it too would

be the best choice for a 3D model. Second order descretization is also preferred.

Errors, Validation, Verification

Our goal here was to predict the characteristics of flow over a rotating cylinder in a wind tunnel. The

CFD model contour plots give a good indication of the general flow characteristics, however, there are

many sources of error, including the 2D assumption, the approximations made in the discretiazation

calculations, the compressibility of the flow (this model is in the subsonic range), the mesh error, the

lack of energy modeling, and the assumptions made in the boundary conditions.

Validation

The rotating cylinder problem is modeled as 2D, and assumes an infinite width cylinder, and thus does

not take into account flows around the edges that would occur in a real world test. To accurate model

the wind tunnel test, a 3D problem would need to be set up. In addition, more precise knowledge would

need to be obtained about the actual turbulence conditions in the wind tunnel. The exact temperature

and pressure of the flow would also need to be monitored and recorded. The boundary condition set at

the outflow is also an assumption (constant pressure). In addition, the cylinder walls are modeled as

smooth with default roughness variables. The exact surface characteristics and how they affected the

creation and dissipation of turbulence would also require accurate measurement to compare the CFD

model with the physical one. From my data, I was getting results which indicate a lift/drag ratio which

varied from about 1.6 to 1.1. Empirical data suggests the actual values for lift/drag of a rotating cylinder

to be on the order of 1, but perhaps this takes into account edge effects, which would lower the L/D

ratio. The theoretical inviscid solution gives lift values of around 7000, my values were on the order of

1200. This is no help in validation, but the drag coefficient of an infinitely long (non-rotating) cylinder

is available, which gives a value of approximately 0.6, which is in range of my results:

.

Verification

With the results from the CFD models, we can verify the appropriateness of the result by examining

the assumptions made in the calculations. The grid errors are discussed above, as well as the quality,

which involves the grid size, shape and type. We can also verify the assumptions made in each of the

turbulent models, related to how the actual turbulence is created, and what factors are included, as well

as the entire CFD process, which, for example, truncates all the third order and higher terms from the

Taylor and power series expansion when solving the PDE’s. CFD methodology is discussed previously.

Looking at the contours, we can verify if the results from the CFD are realistic in terms of the flow

characteristics (see discussion following). And of course, the CFD results can be verified by tests done

in a wind tunnel if the conditions can be modeled exactly. This would include studying and measuring

the boundary layer and moment of separation, pressure distribution along the cylinder walls, and

measurements for turbulence around the cylinder.

Summary

CFD is a delicate process of balancing many assumptions to predict real world fluid flows. To

accurately model a fluid flow, it is important to have a excellent understanding of the flow features prior

to creating a grid and selecting a CFD model, as different models make different assumptions which are

specific to certain types of flows. A good understanding of every process in the CFD analysis is vital to

obtaining reasonable results, and extensive experience in comparing computed results to experimental

tests would be essential for a researcher to have prior to predicting untested flows.

General Flow Features

Right: This velocity contour

shows a stagnation point at

the center front position,

and a forward upper sepa-

ration point and a delayed

lower separation point. The

wake behind the cylinder is

shifted upwards relative to a

non-rotating cylinder.

Right: zero rotation

velocity contour for

comparison

Right: The pressure con-

tour shows a high pressure

spot for front center, with

a pressure imbalance on

the top and bottom center

points. The lower pressure

area is the greater than the

lower pressure area on the

zero rotation model, below,

while the upper pressure

area on the rotating model is

higher than the zero rotation

model.

Right: Zero rotation pres-

sure plot for comparison

Above: Velocity vectors showing the

wake pattern of the region behind the

cylinder. Below: the velocity stream-

line plot shows

the stagnation

and separation

points more

clearly.

Above: Pressure distribution on the wall

of the cylinder. The forward stagnation

is the high point of the curve, while the

two low points are the top and bottom

pressure. The flat area is the wake.

Results and General Flow Features

Please see the next 20 or so pages for results. Pertinent results can be found on the last three pages, from

which produced the following plots. Cylinder is rotating counter clockwise is all runs.

Right: Zero rotation turbu-

lence plot for comparison

Right: The turbulence con-

tour plot shows high turbu-

lence along the front edge of

the cylinder, with a pocket

of lower turbulence in the

wake near the cylinder. The

displaced wake diverts the

main flow, which in turn

affects the velocity differ-

ential, affecting the pressure

imbalance which creates the

lift.

Front

Wake

top

bottom center

Above right: Contour plots of velocity, pressure,

and turbulence. The velocity shows the upper/lower

differential, while the pressure plot shows that the

gradient reaches the wind tunnel walls. Turbulence

in this model diminishes considerably after about 5

diameters of the cylinder.

RESULTS Page 1

Initial Runs with Quad Mesh and standard K e model and second order discretiation. This is where I

learned about the proper way to check for convergence.. These tests were run with my initial medium

quad mesh (12 faces), which initially had 57073 nodes (200 mesh seeds on circle).

First run converged to

.001 residuals after 140

iterations, second with

0.001 residual level at

500 iterations. Left side is

0.001 convergence, right

side is 0.0001 conver-

gence. After this I decid-

ed to check convergence

by examining the residual

plat and checking when

the residuals level off.

Turbulence, Pressure

contour, and pressure

on surface of circle

for 0.001 conver-

gence level (140

iterations)

Turbulence, Pressure

contour, and pressure

on surface of circle for

0.0001 convergence

level (>500 iterations).

Note the more devel-

oped turbulent flow

contour.

Above:

LIFT=

-1221.3

Above:

LIFT=

-1326.1

drag=

976.4

drag=

918.2

Right: velocity vectors

on the spinning (168

radians/sec) circle. Note

the spinning circle does

not have enough rotation

to counter the oncoming

flow, despite the fact that

it is a no-slip wall.. This

seemed to be indepen-

dent of the grid size, as after several boundary adaptions,

the velocity vectors still did not reverse on the surface of

the circle. Yet when the rotation was increased to 1680

radians/sec, the vectors on the top surface did reverse.

PAGE 2. Next I experimented with Adapted Grids, using both y+ and boundary adaptation. Later found

out that the boundary adaptation process could cause undue effects due to adverse mesh gradients, but

the y+ adaptation worked well (y+ adaption usually added no nodes after boundary adaption).

Above: various plots after grid adaptation.

Left: Bound-

ary Adapted

Grid.

Right: Forces

after adapting

grid.

Left: A quick check

of forces after a

run with zero rota-

tion on the circle.

Note lift force error

(should be zero)

probably due to

coarseness of grid.

LIFT = -9.027

Above: 57073 nodes to 71795 nodes

Above: LIFT = -1331.8

Side Notes

(note: I also ran other

models here, includ-

ing RNG, Reynolds,

Spalart-Allmaras, but

this was prior to my

knowing the correct

parameters for them,

so the results were

bad.

drag=

918.2

PAGE 3. Next I ran some tests with SIMPLE and first order solutions, with 0.0001 and 0.00001

residual levels. There was no difference between the residual levels. These were with the adapted

grid, and the values for the lift were lower than the second order solution.

Above: LIFT= 1109.7 (first order solution)

Side note: around this time I also tried a run with

the PISO algorithm, but it failed to converge.

drag=

1026.6

PAGE 4. Below are various other plots of the initial experimental runs with the same Medium

Quad mesh.(top four before grid adaption).

Above: skin friction before grid adaption,

Below: after adaption (nearly identical

except the zero point has changed with grid

adaption). Left: plots after adaption.

PAGE 5. Next I built and ran a fine mesh, without adaption.. This had 171,597 nodes in its 12 faces

and took a ridiculous amount of time to run. (Standard Ke).

Above: LIFT= 1112.7

Right: Even with

this excessively

dense mesh, the

y+ values on the

wall were still out

of range (peak =

1000). Clearly

there had to be

another way.

Left and

below: pres-

sure and

turbulence

contours.

Above: mesh with 400 nodes on circle, and a

bazillion elsewhere.

drag=

1020.8

PAGE 6. Next was a coarse quad mesh to do some quick test runs(14560 nodes before adaption). 100

nodes on circle.

LIFT=

-738.6

PAGE 7. Same Coarse Mesh after boundary adaption.. Again, this is before I realized that random

boundary adaption didn't solve the y+ problem.

LIFT=

-1220.4

Note how

the boundary

adaption does

not solve the

y+ value prob-

lem of being

too high (max

=1600), yet

even with the

coarse mesh lift

values improve

after boundary

adjustment.

PAGE 8. Next I ran some triangle meshes .Version 1, using a standard Ke model.

Original Gambit Mesh: 100 mesh

seeds on circle, 200 bi-exponent on

top and bottom walls, 80 front and

back walls. 20452 nodes before

boundary adaption.

LIFT=

-1005.7

After Boundary Adaption:

25904 nodes.

Below: Turbulence, Velocity and

Pressure contours.

drag=

913.3

PAGE 9. Triangle Mesh Version 2. 200 nodes on circle, 225 bi exponent nodes on sides, 75 front, back.

Standard Ke model.

LIFT=

-1005.55

Above: experiment with double boundary adaption.

Left, above and right:

Version 2 Triangular

mesh plots and contours.

Not much difference in

the visuals from the quad

mesh, though the lift is

less for the equivalent

mesh parameters.

drag=

913.5

PAGE 10. More Experiments with a new Coarse Quad mesh and standard Ke model. Again we see more

signs of a novice randomly adapting meshes using the boundary command.

Above: max y+ = 6000

Above max y+ = 3000

LIFT=

-959.68

LIFT=

-765.2

Later I did the exact same boundary adaption comparison with my final medium quad meshes. Lift went

from 1024.7 to 1314.7, maximum y+ values decreased from 3500 to 1700, and number of nodes in-

creased from 31368 to 33736. The y+ adaption proved to work better in the end.

Drag=

888.9

drag=

1027.4