Implementation of a Hybrid Navier-Stokes/Vortex Panel Method for ...

2008 International 

ANSYS Conference 

Implementation of a Hybrid Navier- 

Stokes / Vortex Panel Method for Wind 

Turbine Aerodynamic Analyses in CFX 

Mark E. Braaten 1 , Kevin Standish 2 , Slawomir Kolasa 3 , 

Emad Gharaibah 4 

1 GE Global Research, Schenectady, NY 

2 GE Energy, Greenville, SC 

3 GE Polska, Warsaw, Poland 

4 GE Global Research, Munich, Germany 

© 2008 GE. All rights reserved. 1

Outline of Talk 

• Overview of hybrid CFD method 

• Implementation in CFX 

• Validation 

• Sensitivity Studies 

• Concluding Remarks 

© 2008 GE All rights reserved. 2

Hybrid CFD for Wind Turbine Aero 

• Conventional CFD methods based on Navier-Stokes have 

serious shortcomings for wind turbine analyses 

– Very large domain required to enforce far-field boundary conditions 

sufficiently far from blade 

• Inlet and outlet conditions imposed many blade radii upstream 

and downstream 

• Periodicity requires large sector (120° for 3 blades) to be 

modeled 

– Results in very large meshes (> 10M nodes), long run times, difficult 

post-processing 

• Prevents use of fine enough mesh near blade needed to capture 

turbulence transition effects 

• Unsteady CFD simply not practical on such large meshes 

– Wake behind blade dissipates too quickly due to numerical 

dissipation 

• Prior studies have shown need to resolve wake as far as 10-20 

blade radii downstream for accurate power predictions 


Full Domain CFD 

Outlet 

50 m 

Inlet 


Hybrid CFD (cont’d) 

• Hybrid Navier-Stokes/Vortex Panel method proposed by 

Schmitz, Chattot (UC Davis) looks very promising 

– Small Navier-Stokes region (~1 - 5 M nodes) around the blade 

computes near field 

– Vortex Panel method computes far field using Biot-Savart law 

• Effect of blade on far field represented by lifting line, 

helicoidal paths from prescribed wake 

Small Navier- 

Stokes domain 

Prescribed 

wake shape 


Hybrid CFD (cont’d) 

• Coupling between near and far fields 

– Navier-Stokes code computes circulation on polylines about 

spanwise blade sections needed by Vortex panel solver 

– Vortex panel method computes induced velocities on boundaries 

of NS region computed from Biot-Savart law 

– Effect of blade on far field represented by lifting line, helicoidal 

paths from prescribed wake 

– These provide coupling between Navier Stokes and Vortex Panel 

solvers 


Goals for Hybrid CFD for Wind 

Turbine Aero Design 

• Goal is to develop design system using hybrid 

methodology that can be routinely used by GE engineers 

to design wind turbine blades for optimum aero 

performance 

– Scripting of meshing, pre- and post-processing is essential 

– Hybrid CFD analysis in CFX must be no more difficult to set up 

and run than conventional analysis 

– Best practices established and embedded in process 


Implementation of Hybrid CFD in 

CFX 

• The hybrid method requires: 

– The computation of the circulation on closed loops that 

include all of the sources of vorticity 

– The calculation of the induced velocities and their imposition 

on the boundaries 

• These calculations are now done as part of a single 

CFX solver run, instead of requiring a separate 

program to be run between successive runs of CFX 

• The vortex panel solver is implemented in CFX User 

Fortran (CFX Version 11.0 and up) 


User Fortran Routines 

CFX provides two types of User Fortran routines: 

• Junction Box routines, which are User Fortran routines that are 

called and executed at particular times during a CFX run. 

• CEL routines 

– These evaluate a function in a similar fashion to CFX expression 

language 

• We basically need routines to: 

– Read the user defined loops upon which to compute the circulation, and 

save these in the CFX MMS (memory management system) for later 

use by the solver 

– Compute the helicoidal wake paths 

– Compute the circulation on the polylines at the start of each CFX 

iteration 

– Impose the induced velocities on the outer boundary as a prescribed 

velocity opening boundary condition 


Basic Hybrid CFD Flow Chart 

Initial Setup 

Read user input 

data files 

Generate polylines 

Compute helix 

Compute circulation 

Compute induced velocities 

Solve equations 

Output results file 

© 2008 GE All rights reserved. 10 

Iteration Loop 

Note 

User Fortran routines 

shown in yellow

Computing Circulation in CFX 

• The circulation is computed on closed loops (polylines) that 

include all of the sources of vorticity 

– The circulation calculation is made for a number of spanwise 

positions along the blade 

• This calculation is updated every iteration using the current 

values of the velocity field 

• Polyline points are mapped to the closest mesh points 

– Velocity vector and gradient returned at mapped points 

• User Fortran provides capability to recover gradient operator 

– Use Taylor expansion to interpolate solution from mapped point (mp) 

to polyline point (pp) 

V pp = V mp + ∇V * dr 

• Circulation calculation requires parallel implementation 

– Simplest parallel implementation is sufficient, as the line integrals are 

1D calculations: 

– Routines use CFX Flow Parallel message passing calls for parallel 

communication (as does rest of CFX solver) 


Computation of Helicoidal Paths 

• Helicoidal paths are computed based on 

simple actuator disk theory 

• Paths depend on estimated power 

coefficient 

– Paths are periodically updated during 

CFX calculation based on latest 

computed power coefficient 

• Helicoidal paths computed redundantly on 

each processor using a Junction Box 

routine 

– This allows each processor to 

compute induced velocities in perfectly 

parallel fashion 

Navier-Stokes 

domain 

Wind 

direction 


Induced Velocities 

• The induced velocities are computed on the outer boundary of 

the domain, using the Biot-Savart law 

– This involves the line integration along a helicoidal path, starting out 

from each spanwise location on the trailing edge 

• Outer boundaries of Navier-Stokes domain are treated as 

openings 

– Induced velocity on boundary is defined as an expression, which is 

provided by a user CEL function 

– Influence coefficients computed at beginning of run, and stored in 

MMS 

– Subsequent updates of induced velocities use stored coefficients 

• Influence coefficients updated periodically to reflect updated 

helicoidal paths 


Equations for Induced Velocities 

Induced Velocities (Biot-Savart Law) 

Influence Coefficients 

All equations from 

Schmitz’ thesis 


Computation of Induced Velocities 

• Total storage requirement 

– (6 influence coefficients) X (nbf 

boundary faces) X (jx polylines) 

– For 100,000 boundary faces, 40 

polylines 100 MB storage 

– Typically represents about 20% 

additional storage for solver 

• Each processor needs only to 

compute influence coefficients, 

induced velocities just for its 

boundary faces 

– Naturally parallel ! 

– Storage is distributed across 

processors 


Specification of BCs in CFX 


Mesh Generation 

• The blade geometry is created in 

Unigraphics, and imported into ICEM- 

CFD for meshing 

• Restrictions on Navier-Stokes domain: 

– Needs to contain polylines for computation of 

the circulation 

– Exit plane should be orthogonal to wake path 

• A grid template with a C-H topology has 

been developed to simplify the mesh 

generation process 

– The blocking file can be imported to any 

ICEM project with the same parts and 

adapted to a new blade geometry 


Creating the polylines 

• The polylines over which the circulation is computed are 

generated using two utility programs: 

– BladeContours 

• A CFX-POST Power Syntax script file that extracts the 

contours of the blade cross sections at the spanwise locations 

where the polylines are desired 

• These blade contours are then input to 

– PolyGen 

• A program that created closed polylines that are offset from 

the blade contours 

• The polylines, and the location of the leading and trailing edge 

locations of the spanwise blade sections are written into files 

that are input files for the CFX run 


Generation of the polylines 

Screen shot from BladeContours script, 

showing spanwise blade contours 

Polylines for NREL wind turbine 

blade 


Post-processing 

• Post-processing of the results is also performed using a 

CFX-Post Power Syntax script 

– Normal and tangential directions input for each spanwise blade 

section 

– At each section, script calculates: 

• Normal and tangential forces 

• Pressure coefficients 

• Torque force 

• Same post-processing script used for full-domain and 

hybrid CFD computations to facilitate comparisons 


NREL Validation Case 

• National Renewable Energy Laboratory (NREL) performed detailed 

wind tunnel experiments on 10m diameter wind turbine in NASA Ames 

wind tunnel 

• This was the test case used by Sven Schmitz (UC Davis) to help 

develop the hybrid methodology 

• Calculated torque values, pressure distributions match experiment very 

well for low wind speeds 

– 7 & 9 [m/s] cases are attached flow 

Hybrid CFD 


Pressure distribution at 63% span 

– 7 m/s wind speed

GE46 Validation Case 

Navier-Stokes domain 

• This was the first GE blade run 

using the hybrid CFD method 

• Comparisons made to full-domain 

CFD, other analytical methods 

– Power predictions match well for 

attached flow cases 

Power Coefficient 

Tip Speed Ratio 

Pressure Coefficient (PC) Comparison 

CPU time (min) 

400 

350 

300 

250 

200 

150 

100 

50 

0 Solver time [min] 

Full CFD 366 

Hybrid CFD 

46.9 

Run Time Comparison 

(equal # iterations) 

Computed Mach Numbers (TSR=8) 


Sensitivity Study 

• Sensitivity studies are being performed to investigate the 

effects of a number of parameters, and to establish best 

practices 

• Parameters under study: 

– Size of Navier-Stokes domain 

– Grid size 

– Number of polylines 

– Location, orientation of polylines 

• Results appear to be relatively insensitive 


Example: Effect of Domain Size 

• Vary size of Navier- 

Stokes domain, from 

one chord (C=1) 

down to ¼ chord 

• Vorticity field 

starts to look 

unphysical if 

domain is made 

too small 

Vorticity at 20% Span 

(a) 

(b) 

(c) 

(d) 

Full domain CFD 

Hybrid (C=1) 

Hybrid (C=½) 

Hybrid (C=¼) 


(a) 

(c) 

(b) 

(d)

Future Work 

• Hybrid methodology allows fine enough 

grid in Navier-Stokes domain to allow 

transition to be modeled 

– Initial calculations with Langtry-Menter 

transition model look very promising 

• Reduction in run time makes transient 

simulations possible 

– Unsteady hybrid analysis capability 

currently under development (w/ UC Davis) 


Concluding Remarks 

• Hybrid CFD approach looks very promising for wind 

turbine aerodynamic analyses 

– Grid size and run times much less than full domain CFD 

– Results similar to full-domain CFD 

– Results reasonably insensitive to size of Navier-Stokes domain 

and location of polylines 

• User Fortran in CFX solver and Power Scripting in CFX- 

POST allows the development of an integrated hybrid 

CFD design system 


Impact 

Hybrid CFD – Represents a unique differentiating 

technology that will be a prime enabler for next 

generation quiet, efficient wind turbine blades 

– Hi-fidelity 3D aerodynamic design 

– Low noise design with CFD-based or direct CAA 

noise prediction 

– Aero-elastic fully-coupled design methods

Implementation of a Hybrid Navier-Stokes/Vortex Panel Method for ...

You also want an ePaper? Increase the reach of your titles

Delete template?

Save as template?