# Unsteady Analysis of Separated Aerodynamic Flows Using an Unstructured Multigrid Algorithm

**ABSTRACT** An implicit method for the computation of unsteady flows on unstructured grids is presented. The resulting nonlinear system of equations is solved at each time step using an agglomeration multigrid procedure. The method allows for arbitrarily large time steps and is efficient in terms of computational effort and storage. Validation of the code using a one-equation turbulence model is performed for the well-known case of flow over a cylinder. A Detached Eddy Simulation model is also implemented and its performance compared to the one equation Spalart-Allmaras Reynolds Averaged Navier-Stokes (RANS) turbulence model. Validation cases using DES and RANS include flow over a sphere and flow over a NACA 0012 wing including massive stall regimes. The project was driven by the ultimate goal of computing separated flows of aerodynamic interest, such as massive stall or flows over complex non-streamlined geometries.

**0**Bookmarks

**·**

**149**Views

- [Show abstract] [Hide abstract]

**ABSTRACT:**An overview of the current status of time dependent algorithms is presented. Special attention is given to algorithms used to predict fluid actuator flows, as well as other active and passive flow control devices. Capabilities for the next decade are predicted, and principal impediments to the progress of time-dependent algorithms are identified.02/2002; - SourceAvailable from: dtic.mil[Show abstract] [Hide abstract]

**ABSTRACT:**This work is concerned with the development of an efficient parallel Large Eddy Simulation (LES) and Detached Eddy Simulation (DES) capability using unstructured meshes. The advantages of unstructured meshes include flexible modeling of complex geometries, adaptive meshing capabilities, and homogeneous data structures well suited for massively parallel computer architectures. On the other hand, unstructured mesh techniques require additional computer resources as compared to cartesian or structured mesh methods, and the achievable accuracy of the particular unstructured mesh discretization must be carefully considered. The approach developed in this work is based on an existing steady-state unstructured mesh solver which relies on agglomeration multigrid for rapid convergence and has been shown to scale well on inexpensive personal computer (PC) clusters as well as on massively parallel supercomputers using thousands of processors1.07/2001;

Page 1

1

Unsteady Analysis of Separated Aerodynamic Flows using an

Unstructured Multigrid Algorithm

Juan Pelaez

Old Dominion University

Hampton, Virginia

Dimitri Mavriplis

ICASE

NASA Langley Research Center, Hampton, Virginia

Osama Kandil

Old Dominion University

Hampton, Virginia

Abstract

An implicit method for the computation of

unsteadyflowson

presented. The resulting nonlinear system of

equations is solved at each time step using an

agglomeration multigrid procedure. The method

allows for arbitrarily large time steps and is

efficient in terms of computational effort and

storage. Validation of the code using a one-

equation turbulence model is performed for the

well-known case of flow over a cylinder. A

Detached Eddy Simulation model [1] is also

implemented and its performance compared to

the one equation Spalart-Allmaras Reynolds-

AveragedNavier-Stokes

model [2]. Validation cases using DES and

RANS include flow over a sphere and flow over

a NACA 0012 wing including massive stall

regimes. The project was driven by the ultimate

goal ofcomputing

aerodynamic interest, such as massive stall or

flows over complex non-streamlined geometries.

unstructuredgridsis

(RANS) turbulence

separatedflows of

1.Introduction

The use of time-dependent simulations for flows

of practical interest is much less widespread than

the use of steady-state flow simulations, due to

limitations related to computational time and

computational resources. However, many flows

are inherently unsteady, particularly when large

amounts of separation are present, and must be

simulated as such in order to obtain meaningful

results.

Copyright c 2001 by AIAA, Inc. All Rights Reserved.

Transient flow simulations can either be based

on explicit or implicit time-stepping schemes.

Stabilityconstraints

allowable time step size of an explicit scheme,

which is proportional to the smallest cell size in

the entire computational mesh. Explicit schemes

are well suited for unsteady applications in

which the time scale of interest is comparable to

the spatial scales. In these cases the mesh should

be clustered only in regions of interest where it is

absolutely necessary or the explicit time step can

become unnecessarily small.

limitthemaximum

Explicit time steps may become too restrictive

for cases characterized by larger time scales or in

cases where there is a wide variation in the grid

resolution. In these cases it is desirable to

develop a fully implicit method in which the

time step is only determined by the physics of

the flow and not by the cell size. At each time

step the unsteady residual must be driven to zero

and this is usually done using inner iterations.

The number of inner iterations needed for each

time step is related to the problem being solved

and the size of the physical time step used.

To develop an unsteady solver that can provide

an accurate description in time of the flow is the

first requirement to address before attempting to

solve flows with massively separated regions

that are inherently unsteady. On the other hand,

it is also important to review the different

techniques available to compute turbulence,

which is at the core of separated flows, and will

be a key parameter to determine how well the

numerical scheme captures all the physical

aspects of the flow. In this sense, numerical

solutions of turbulent flow cases can be achieved

Page 2

2

using different levels of approximation. The

most widespreadmethod

ReynoldsaveragedNavier-Stokes

(RANS). In the RANS equations, the turbulent

fluctuations appear in the Reynolds stress term

that must be modeled using any of the turbulence

models available in the literature. However, a

common limitation of these models is their lack

of generality since the model coefficients are

usually set using simple well-documented flows.

In this sense, current RANS solvers are fairly

successful at predicting mostly attached flows,

such as a wing in cruise condition, but fail to

capture a range of different off-design situations

as post-stallregimes,

configurations, and non-streamlined bodies. In

general, in the cases in which the RANS

approach fails, the flow is characterized by large

amounts of separation in which a very wide

range of scales is present in the flow. While the

small scales tend to be universal in nature, the

larger scales are affected by the boundary

conditions. This is the main cause of the lack of

generality of turbulence models, as it is difficult

to model the effect of the large scales in the same

way for many different types of flows.

istosolve

equations

the

certain high-lift

The failure to develop a universally valid

turbulence model has led to alternate approaches

such as Direct Numerical Simulation (DNS) and

Large Eddy Simulation (LES). DNS is the most

straightforward approach to the problem. DNS

consists in solving the governing equations on a

mesh fine enough to capture the smallest scales

contained in the flow with a scheme designed to

minimizethe numerical

dissipation. The drawback is extremely high cost

of the DNS computation, which is proportional

to at least Re3. For these reasons, DNS is

generally limited to very simple flows and low

Reynolds Numbers.

dispersion and

The flow limitations of RANS and the difficulty

of using DNS for realistic applied engineering

problems have generated a great interest in the

Large Eddy Simulation approach (LES) for

computingflowswith

separation. Large Eddy Simulation is a technique

between Direct Numerical

Reynolds Averaged Navier-Stokes [3]. In LES

the contribution of the large scales is computed

exactly and only the smallest scales in the flow

are modeled. However, a major difficulty of

LES,particularlyfor

flows, is that near solid surfaces all the eddies

are small and the “large” and “small” eddies tend

largeamounts of

Simulationand

externalaerodynamic

to overlap. Therefore the required grid spacing

and time step gradually fall towards DNS as the

solid boundary is approached [4 ].

Using LES to resolve near wall streaks would

bring an immense penalty at industrial Reynolds

numbers. In this line of reasoning the Detached

Eddy Simulation (DES) approach was conceived

with the idea of combining the strengths of

Reynolds Averaged methods near the solid

boundaries and of Large Eddy Simulation

elsewhere [1,4,5].

The ultimate goal of this work is to develop a

large eddy simulation capability based on an

existing unstructured grid Navier-Stokes solver

[6] to be able to perform detached eddy

simulations combing RANS near the walls and

LES in massive separated regions in a non zonal

manner and to compare the solutions obtained

using this approach to the solutions obtained

using a classical RANS approach with a Spalart-

Allmaras one equation turbulence model [6].

2.Unsteady Reynolds Averaged Navier-

Stokes Solver

2.1 Steady solver description

The Reynolds averaged Navier-Stokes equations

are discretized by a finite volume technique on

meshes of mixed elements, including tetrahedra,

pyramids, prisms and hexahedra. In general,

prismatic elements are used in the boundary

layerregions,while

elsewhere.

tetrahedraare used

Flow variables are stored at the grid vertices and

a single unifying edge-based data-structure is

used to handle all elements of the grid.

Convective and viscous fluxes are discretized

along edges using a central difference finite

volumetechniquewith

dissipation.

addedartificial

The non-dimensional steady conservative form

of the full Navier-Stokes equations can be

written as:

0)(

=

wR

(1)

where w represents the solution vector of

conserved variables and R represents the spatial

discretizationoperator,

vanishes at the steady state.

orresidual,which

Page 3

3

An implicit solution procedure for solving

equation (1) begins with the linearization of the

residual about the current time step or iteration

level:

0)(

=∆⋅

∂

∂

++

∂

∂

w

w

R

wR

w

τ

n

(2)

which can be solved as:

{} )(

1

n

wR

w

RI

τ

w

−⋅

ÿÿ

ÿ

ÿÿ

ÿ

∂

∂

+

∆

=∆

−

(3)

where ÿ is a pseudo-time used to advance the

solution, and ∆w represents the new correction to

be applied to the solution. Rather than inverting

the large Jacobian in equation (3), a reduced

Jacobian which is simpler to invert is employed.

In regions of isotropic grid cells, only the block

diagonals of the Jacobian are retained, leading to

a block-Jacobi or point-implicit scheme. In the

boundarylayerregions,

stretching is present, lines are constructed in the

direction normal to the solid wall boundary and

the Jacobians along these lines are inverted,

using a block tridiagonal solution algorithm.

This procedure relieves the stiffness associated

with high grid stretching in these regions, thus

providing more rapid convergence [7 ].

wherehigh grid

This locally implicit scheme is used as the

smoother on all levels of an agglomeration

multigrid algorithm. The multigrid algorithm

constructs coarse level grids automatically by

fusing together neighboring fine grid control

volumes to form a smaller number of large

coarse grid control volumes.

acceleration is achieved by cycling back and

forth between the fine and coarse grid levels of

the multigrid sequence, using the locally implicit

solution procedure as a solver on each grid level

[7 ].

Convergence

The unstructured multigrid solver is parallelized

by partitioning the domain using a standard

graph partitioner[8]

between the various grid partitions running on

individual processors using the MPI message-

passing library [9]. The solver can be run on

distributedor shared

including clusters of personal computers.

andcommunicating

memorymachines,

2.2 Unsteady term implementation

The unsteady form of the governing equations is

obtained by adding the time derivative to

equation (1):

0)(

=+

∂

∂

wR

t

w

(4)

where R(w) denotes the discretization of the

spatial derivative terms, as previously.

Making use of a second-order accurate three

point backward approximation for the time

derivative and evaluating R(w) at time level

(n+1), we obtain [10,11,12]:

0)(

2

1

⋅

2

∆

2

3

⋅

111

=+⋅

∆

+⋅−⋅

∆

+−+

nnnn

wRw

t

w

t

w

t

(5)

We may now define and unsteady residual as:

3

)(

+

∆⋅

t

with

2

),(

∆

),()(

2

1*

−

−=

nnwwSwRwR

(6)

11

2

1

⋅

−−

⋅

∆

−⋅=

nnnn

w

t

w

t

wwS

(7)

where wn+1is the approximation to w and the

source term S(wn,wn-1) remains fixed throughout

the solution procedure at each time step. In this

form, the non-linear problem to be solved at each

time-step reduces to R*(w) = 0.

redefinition of the residual, the same iterative

multigrid procedure employed to solve the

steady-state problem can be used to solve the

non-linear unsteady residual at each physical

time step [10,11,12].

Using this

The solution procedure consists of an outer loop

over the physical time steps, used to advance the

problem in time, and an inner (multigrid) loop

over pseudo-time used to drive the unsteady

residual to zero at each time level. While the

maximum size of the physical time step is only

determined by the physics of the problem, the

convergence of the inner sub-iterations for each

time step varies inversely with the size of the

physical time step.

3. Unsteady solver validation

The flow around a circular cylinder is a well-

known case, which has been widely studied

computationally and experimentally. This case is

used as the basis for validation of the unsteady

RANS solver, and for assessing grid resolution

Page 4

4

and

predicting

observed in the cylinder flow. Two different

meshes of 252,000 and 631,000 grid points and

three different time steps of 0.5, 0.25 and 0.1

were used. The time is non-dimensionalized as t

= to/(d/U∞) where d is diameter of the cylinder

and U∞is the freestream velocity.

timestep

the

requirements

vortex

foraccurately

frequencyshedding

Figure 1: 3D View of cylinder and lateral walls

The one equation Spalart-Allmaras turbulence

model [2] was used for all calculations in fully

turbulent mode. In all cases the agglomeration

multigrid strategy was used with four levels. The

Mach number is 0.2 and the Reynolds number is

1200 for this case. All runs were performed in

parallel using 16 processors of a Pentium PC

cluster at ICASE.

The computational domain in the plane normal

to the cylinder span has an aspect ratio of 1 and a

side length of 100 cylinder diameters. A span of

two cylinder diameters is employed, and inviscid

(slip velocity) boundary conditions are applied at

theend-walls.The

simulations reported herein were also compared

withtwo-dimensional

aroundacircleusing

dimensional unstructured solver [12], and found

to agree well in terms of force coefficient

histories and shedding frequency.

three-dimensional

simulations

a

offlow

two-validated

Table 1 shows the Strouhal Numbers computed

for each mesh and each time step of the three-

dimensionalsimulations.

achieved as the time step is reduced and the

mesh size increased. A second-order accuracte

convergence behavior is observed as the time-

step is reduced, validating the accuracy of the

Convergenceis

three-point backwards difference scheme used to

discretize the time step. From the smallest time

step results, the solution can be seen to be grid

converged, at least with respect to the prediction

of the vortex shedding frequency. The computed

Strouhal number compares very well to the

experimental value of St = 0.21 given by Dresher

[13,14]. Figure 2 shows the time history of the

lift coefficient, while the oscillatory pattern

corresponding to the vortex shedding is shown in

Figure 3.

Time Step

0.25 0.50.1

0.252

Million

0.631

Million

0.192490.203040.20833

Grids

0.193790.204080.20833

Table 1. Predicted Strouhal Number for Various

Grid and Time Step Sizes

Figure 2: Mach contours at two different time

states for flow over circular cylinder. Mach =

0.2, Re = 1200.

Page 5

5

.

Figure 3. Computed LiftCoefficient Time History

for Flow over Circular Cylinder using three

different time steps. Mach = 0.2, Re = 1200

Figure 4. Mean Surface Pressure Coefficient

Distribution for Flow over Circular Cylinder at

Mach = 0.2, Re = 1200, Compared with

Experimental Data at Various Reynolds

Numbers

Figure 4 shows the pressure distribution over the

surface of the cylinder. The pressure distribution

was computed by averaging results at different

times distributed along several oscillations. For

this calculation the finest mesh and the smallest

time step was used. As can be observed from

Figure 4, the computed pressure distribution

compares closely to experimental results at a

higher Reynolds number than the one used for

these computations. This is likely due to the use

of the turbulence model in fully turbulent mode,

in order to avoid the issues of transition

prediction. Similarly, the backpressure obtained

of Cpb= -1.20 compares closely to the Cpb= -

1.20 at Re=27,700 measured by Linke [13,15].

The mean value of the drag coefficient computed

is Cd=1.3 compared to Cd=1.2 as measured by

Wieselsberger [13,16] for Re=30,000.

4.Detached Eddy Simulation.

Detached Eddy Simulation (DES) is a hybrid

technique that combines RANS and LES in a

non-zonal manner. DES is based on the Spalart-

Allmaras one equation RANS model [2] in

which the length scale d, which is traditionally

taken as the nearest distance at any given point to

the closest wall, is replaced as the minimum

between the distance to the wall and a length

proportional to the local grid spacing:

dDES= min (d, CDES∆x)

where CDESrepresents a model constant which

has been taken as 0.65 in previous work [1,17].

Traditionally, on structured grids [1,17,18], ∆x is

taken as the maximum grid spacing over all three

directions. In our particular case, the definition

of ∆x has been modified for unstructured grids

by taking it as the maximum edge length

touching a given vertex. In boundary layer

regions, ∆x far exceeds the distance to the wall

d, and the standard Spalart-Allmaras RANS

turbulence model is recovered. However, away

from the boundaries d exceeds CDES∆x and the

models turns into a simple one equation sub-

grid-scale (SGS) model with the mixing length

proportional to the grid spacing. This effect is

illustrated by plotting contours of the distance or

length scale function for both the RANS and

DES models in Figure 5, where it is observed

that both models employ the same length scales