close

Вход

Забыли?

вход по аккаунту

?

Kuntz M Menter F R Simulation Of Fluid-Structure Interactions In Aeronautical Applications (Cfx-C

код для вставкиСкачать
European Congress on Computational Methods in Applied Sciences and Engineering ECCOMAS 2004 P. Neittaanmäki, T. Rossi, S. Korotov, E. Oñate, J. Périaux, and D. Knörzer (eds.) Jyväskylä, 24—28 July 2004 1 SIMULATION OF FLUID-STRUCTURE INTERACTIONS IN AERONAUTICAL APPLICATIONS M. Kuntz
*
, F.R. Menter
*
*
ANSYS – CFX Staudenfeldweg 12, 83624 Otterfing, Germany e-mail: Martin.Kuntz@ansys.com
web page: http://www-waterloo.ansys.com/cfx
Key words: Aeronautics, CFD Simulation, Fluid-Structure Interaction, CFD-FEM code coupling, Abstract. A challenge in engineering computational technology is the simulation of multi-
physics applications where different physical phenomena are involved such as fluid-structure interactions. A simulation strategy is to solve each part with an existing software package and to couple both processes by a data interface between the software codes. The advantage of using existing software packages is that one can benefit from their advanced features, as demonstrated in the current paper using the commercial software packages ANSYS for the structural analysis and CFX of ANSYS Inc. for the flow simulation. The performance of CFX and the coupling procedure between ANSYS and CFX is demonstrated for different aerodynamic applications. M. Kuntz and F.R. Menter 2 1 INTRODUCTION Computational Fluid Dynamics (CFD) has developed into a reliable tool for analyzing external and internal flows of industrial devices. A new challenge is the computation of multi-
physics applications involving different physical phenomena. An important example is the interaction of a fluid flow with the surrounding solid structure. The interaction can be either mechanical by coupling the fluid forces with the deformation of the solid or thermal by coupling the temperature and the heat flux at the interface between the solid and the fluid. A typical example for a mechanically coupled system is wing or blade flutter simulations. In order to solve such technical relevant cases, a coupled simulation is required that allows for a simultaneous detailed analysis of both physical processes: the complex flow field including heat and mass transfer combined with the stress, deformation, and temperature distribution of the solid structure. One strategy is to simulate both processes with a single solution method, by solving all governing equations with either a finite volume or a finite element formulation. The advantage of this procedure is a uniform data structure and a single solution method, which allows for a strong coupling of the problem and avoids complex data transfer [1]. A disadvantage of this approach is that one has to reformulate and re-implement all the physics of the secondary physical process, e.g. fluid analysis, into a code, which was originally designed and optimized for the solution of the primary process, e.g. stress analysis. Experience shows that very often these codes have severe weaknesses in terms of computational efficiency and accuracy when used for the solution of the secondary process. Another promising simulation strategy is to solve each part with existing sophisticated software packages and to couple both processes by a data interface between the software codes. The advantage of using existing software packages is that one can benefit from their advanced features, in particular in solving efficiently the governing equations and using complex numerical sub-models and boundary conditions. In the present study ANSYS and CFX-5, both software packages of ANSYS Inc. are applied for a mechanical coupling of structural and fluid parts. ANSYS is a multi-purpose non-linear finite element solver for structural and non-structural (e.g. electrostatics, electromagnetics, acoustics) [2]. CFX-5 is a general purpose CFD code that is well known for its robust and accurate numerical methods for fluid dynamics [3], advanced turbulence [4] and multi-phase models [5]. In a previous study [6] a coupling between CFX-5 and ANSYS was performed for analyzing the fluid-structure interaction of cardio-vascular applications. In this case, data files have been used for the communication between the two codes. Using data files between two codes has the disadvantages that continuous maintenance of the interface is required and that the parallel performance on multiprocessor computers may deteriorate. In order to have a more flexible link, the coupling library MpCCI [7] was used here to connect CFX-5 and ANSYS. The new method allows for an exchange of data at different levels of the individual solver procedures. Hence, depending on the problem a stronger or weaker coupling for mechanical or thermal analysis can be realized. In the frame of the present study the application area of fluid-structure interaction is described with a focus on fluid dynamics. First the performance of CFX-5 for unsteady M. Kuntz and F.R. Menter 3 aerodynamics is demonstrated. Furthermore the coupling procedure is explained for a mechanical benchmark coupling case. Finally a flutter testcase shows the coupling of fluid dynamics and structural analysis for an aerodynamic application. 2 COUPLING SOFTWARE 2.1 CFX The governing equations for turbulent flow are the Reynolds-Averaged Navier-Stokes (RANS) equations. In CFX-5 these equations are discretised using a finite volume method, which is conservative and time-implicit [3],[8],[9]. The computational hybrid and unstructured mesh can consist of different element types such as hexahedrals, prisms, wedges, and tetrahedrals. A control volume is constructed around each nodal point of the mesh and the fluxes are computed at the integration points located at the subfaces between two control volumes. The discrete equations are evaluated using a bounded high-resolution advection scheme similar to that of Barth and Jesperson [10]. The mass flow is evaluated such that a pressure-velocity coupling is achieved by the Rhie and Chow [11] algorithm. The discrete systems of equations are solved by a coupled algebraic multi-grid method developed by Raw [2]. The numerical effort of this method scales linearly with the number of grid nodes, which is selected to resolve the computational domain. Steady state applications are computed by time step iteration until a user defined convergence level is reached. For a transient computation an iterative procedure updates the non-linear coefficients within each time step (coefficient loop) while the outer loop advances the solution in time. The Reynolds stresses in the momentum equations are computed by using the BSL or SST two-equation turbulence model [4] and an automatic wall treatment [12]. The mechanical coupling of the fluid domain with the connected solid leads to a movement of the interface between both domains. Therefore, the discretized equations have to be extended to allow for moving grids (non-zero grid velocity) and deforming grids (non-constant control volume). This extension is performed according the Space Conservation Law given by Demirdzic and Peric [13]. The volume conservation equation is included in the governing equations to obtain implicitly the volumetric source without the need to solve additional equations. The implementation in CFX-5 is described by Hawkins and Wilkes [14]. The movement of the interface grid nodes at the wall requires the re-computation of the location of the interior grid nodes of the CFD grid. This is carried out by solving a Laplacian equation for the grid deformation, i.e. a grid smoothing is performed. It is a simplification of the classical elasto-dynamic equation for a dynamic grid movement. If the grid is strongly distorted, the smoothing procedure is not adequate to provide a grid with a good quality. In this case, a new grid with a different topology must be created. As a subsequent step the solution variables are interpolated on the grid nodes of the new grid by using a second order interpolation method. M. Kuntz and F.R. Menter 4 2.2 ANSYS ANSYS offers a full complement of nonlinear and linear elements, material laws ranging from metal to rubber, and the most comprehensive set of solvers available. It can handle complex assemblies-especially those involving highly nonlinear contact with and without friction. ANSYS includes matrix coupled-field (or multiphysics) studies involving acoustic, piezoelectric, thermal/structural and thermal/electric analysis. ANSYS Multiphysics integrates direct (matrix) and sequential (load vector) coupling to combine the appropriate "physical fields" required for accurate, reliable simulation results in applications ranging from cooling systems, power generation, to biotechnology and MEMS. The software allows the simulation of complex thermal-mechanical, fluid-structural and electrostatic-structural interactions, and includes the complete range of ANSYS iterative, direct and eigenvalue matrix solvers [2]. 3 COUPLING CONCEPT The coupling of codes requires access to internal data in order to export or import variables during the coupled solution run. Different coupling strategies must be available depending on the application. In some cases it is sufficient to have a one-way coupling, other applications require a two-way coupling. The data exchange frequency can be low, if the data are exchanged only after a certain number of time steps or high, when the exchange is carried out at each time step. A stronger coupling is obtained by exchanging data during the internal coefficient loops. Furthermore, the coupled programs can run simultaneous or alternating. All these different strategies may be applied for iterating towards a steady-state solution (fluid and solid) or for a transient application. Depending on the application it may be unclear to the user in advance which coupling strategy he should select. Therefore, a flexible communication concept is applied, which allows a simple switching between the coupling algorithms. The coupled codes are extended by coupling ports controlling the import and export of data to and from the codes. The coupling is synchronized by activating / deactivating the coupling ports on both sides. Figure 1 shows the scheme for coupling of ANSYS and CFX. Coupling port 1 is used for the data exchange at the start of the computation, which is applied for synchronization of the solution at a restart. For CFX, coupling ports 2 and 3 are implemented at the start / end of the time step loop and coupling ports 4 and 5 are at the start and the end of the coefficient loop. For steady state runs, only coupling ports 2 and 3 are accessible. On ANSYS side, at the start and end of the stagger iteration data can be imported and exported at coupling ports 2 and 3. All coupling algorithms, which have been mentioned above, can be chosen by connecting the different coupling ports, as shown be the different lines with arrows in Figure 1. The global convergence status of both codes is checked and exchanged at the end of the inner loops. In case the convergence criterion is matched for both codes, the next time step is launched. The coupling ports at both codes are connected the code coupling library MpCCI [7], which controls the coupling and the data transfer and, in case of dissimilar meshes, carries out the data interpolation at the interface. M. Kuntz and F.R. Menter 5 Figure 1: Coupling concept 4 APPLICATIONS Three different examples are described in the present chapter: an uncoupled aerodynamic application, a mechanically coupled demonstration testcase and a coupled aerodynamic application. 4.1 Unsteady aerodynamics Transient aerodynamics is computed for the flow over an NACA 0012 airfoil pitching around its quarter-chord point. Experimental data is available in the AGARD report R-702 [15], Dataset 3. The pitching motion is defined by the mean angle and by the amplitude and frequency of the sinusoidal oscillation: )sin()(tt
m
(1)
The angular frequency is expressed by the reduced frequency: U
c
2
(2)
Coef. loop
Coupling
loop
CFX-5
ANSYS
1
2
4
5
3
2
3
Time
step
loop
Stagger loop
Time
step
loop
Coupling
loop
1
C
C
M. Kuntz and F.R. Menter 6 O-type grids with a distance from the airfoil to the farfield of about 15 chord lengths are used. The grid size is 192 x 64 points. The grid points are clustered in the boundary layer resulting in an average y
value of 7. Studies about the time step size are carried out in order to obtain a time-accurate lift and momentum coefficient independent on the time step size. An optimal value of 160 time steps per period with 5 subiterations per timestep was found. All computations are carried out with the BSL turbulence model and the high-resolution advection scheme. The test conditions summarized in Table 1 are analyzed. Testcase Mean Angle of attack Angle of attack variation Reynolds number Mach number Reduced frequency CT 5 016.0
m
51.2
0
6
105.5
755.0
M
0814.0
CT 1 89.2
m
41.2
0
6
108.4
6.0
M 0808.0
Table 1: Example of the construction of one table. Figure 2 shows the comparison of the lift and momentum coefficient for the NACA 0012 with almost symmetrical pitching movement. In Figure 3 the same comparison of lift and momentum coefficient is shown for the NACA 0012 airfoil with asymmetric pitching movement. A good agreement is found between numerical simulation and experimental data. There is a slight mismatch of the avarage slope of the lift curve and a shift of the momentum curve. This fact is also seen in other computational results [16]. The hysteresis in the lift and momentum curves is mainly an inviscid effect. Therefore, no strong influence of the turbulence model on the result is expected. Figure 2: Comparison of lift and moment coefficients for experimental data and CFX-5 simulation, NACA 0012, 0814.0,51.2,016.0,755.0
0
m
M
M. Kuntz and F.R. Menter 7 Figure 3: Comparison of lift and moment coefficients for experimental data and CFX-5 simulation, NACA 0012, 0808.0,41.2,89.2,6.0
0
m
M
4.2 Mechanical FSI coupling The coupling of ANSYS and CFX is demonstrated for a mechanically coupled simulation problem. The testcase is an elastic-walled tube with longitudinal tethering, defined as a benchmark for a coupling software for cardiovascular applications [17]. Womersley [18] published solutions indicating that the pressure wave moves along the pipe with a finite speed depending on the properties of the fluid and the tube. Theoretical investigations lead to the Moens-Korteweg equation, which relates the wave speed in a longitudinally tethered thin-walled elastic tube of thickness h and radius R, Youngs modulus E and Poissons ratio
, carrying a fluid of density and zero viscosity: )1(2
2
0
R
Eh
c
(3)
The viscosity of the fluid tends to reduce the wavespeed. The above equation is derived for a periodically varying pressure gradient. In the present study only the onset of the pressure wave is simulated, which is approximated with a prescribed linearly increasing pressure at the inlet of 1
35200
sPa
. The outlet pressure is fixed to zero. The fluid has a density of 3
1000
mkg
and a viscosity of 0.001 Pa s. The structural part is modelled with a wall stiffness in the range
PaE
6
105.0
to PaE
6
104
and a Poisson ration of 45.0
. The tube is 0.08 m long with a radius of 2.0 mm and a wall thickness of 0.12 mm. It is discretized with structured meshes of 4600 fluid nodes and 1600 solid nodes for the quarter of the domain (see Figure 4). M. Kuntz and F.R. Menter 8 Figure 4: Fluid and solid mesh (deformed shape) for flexible pipe testcase The coupled simulation is carried out by activating the coefficient loop coupling ports for CFX and the stagger iteration coupling ports in ANSYS. An identical number of coefficient iterations (CFX) and stagger iterations (ANSYS) is set. ANSYS sends at the end of each stagger iteration (coupling port 3) the mesh displacement of the interface nodes to coupling port 4 of CFX. CFX sends the traction variable (pressure and viscous tension) at the end of the iteration (coupling port 5) to coupling port 3 of ANSYS. A time step of 0.001 s is selected. The explicit coupling algorithm is unstable without any underrelaxation of the variables at the interface. Therefore underrelaxation factors of 0.5 for the displacement and 0.15 for the traction are found to be suitable to obtain a proper convergence of the variables at the interface. The inner loop is stopped in case both codes have reached their global convergence criterion and the next time step begins. In order to compare to the analytical expression of the Moens-Korteweg equation (3), the wave speed of the pressure pulse is extracted from the computational results. In Figure 5 (left) the displacement profiles along the tube are plotted for 8 different time values (0.001 s to 0.008 s). For particular values of the displacement (lines A,B,C) the propagation of this disturbance along the tube is measured and a wave speed is evaluated. The obtained speed values are not identical for the different radial locations and a standard deviation is related to each value. In Figure 5 (right) the computed wave speed is plotted for different values of tube stiffness versus the analytical expression. A good agreement is obtained taking into account the uncertainty for the evaluation of the computed wave speed. M. Kuntz and F.R. Menter 9 Figure 5: Left: displacement profiles along the pipe for different time values. Right: Comparison of wave-speed of pressure pulse with analytical expression. 4.3 Aeroelastic FSI coupling As an example for aeroelastic coupling the AGARD wing 445.6 test case is analyzed. A detailed description of the experimental set-up is given in the AGARD report R-765 [19]. The wing span is 0.76 m and is swept by 45 degrees at the quarter chord line (see Figure 6). The total weight of the wing is 1.8 kg. Figure 6: Geometry of AGARD 445.6 test case The wing is disretized with 6300 solid nodes and the computational fluid domain includes about 300.000 nodes. The material of the wing is laminated mahogany. For the present investigations the so-called weakened model (with holes in the wing in order to reduce the material stiffness) is selected. The stiffness along the grain of the wood is taken from the AGARD report with a Young’s modulus of PaE
9
1025.3, a shear modulus of 0.37 m
0.76 m
0.56 m
45
0.37 m
0.76 m
0.56 m
45
0.76 m
0.56 m
45
A
B
C
M. Kuntz and F.R. Menter 10 PaG
9
10412.0
and a Poisson ration of 31.0
. No further details about the orthotropic material properties are taken into account. To verify the selection of the material properties, a modal analysis is carried out with ANSYS. The computed frequencies are too low compared to the experimental data (see Table 2). These differences are caused by the simplified assumption of the material properties, and are accepted for the following fluid-structure computations. The deformed shape of the first two modes is plotted in Figure 7. Mode 1 2 3 Experiment 9.59 Hz 38.16 Hz 48.34 Hz Computation
8.62 Hz 35.69 Hz 44.02 Hz Table 2: Modal frequencies of AGARD 445.6 wing Figure 7: First two modes (bending, torsion) of AGARD wing. As a first step, a steady CFD solution is generated (without coupling) for each operating point using the experimental data for Mach number, inlet velocity and density. Starting from this flow solution the coupled fluid-structure computation is launched with a time step of 0.001 s. At each time step, CFX sends the traction data (pressure plus viscous tension) to ANSYS and ANSYS sends back the displacements at the interface to CFX. The wing starts to oscillate with the flutter frequency. The comparison of predicted and experimental flutter frequency as function of the Mach number is shown in Figure 8 (left). The computational results are slightly below the curve of the experimental data, but this difference is consistent with the differences of experimental and computationally predicted modal frequencies of the wing. The differences almost vanish when evaluating the flutter frequency relative to the frequency of the first torsion mode (see Figure 8 right). A much better agreement of computational results and experimental data is obtained. The results are comparable to the studies of other authors summarized in [20]. M. Kuntz and F.R. Menter 11 Figure 8: Flutter frequency and flutter frequency ratio as function of Mach number for AGARD 445.6 wing 5 CONCLUSIONS The code coupling of ANSYS and CFX applied for different test cases. The analysis of a pitching airfoil demonstrates the performance of CFX for the prediction of the transient lift and momentum coefficients. Furthermore, the mechanical coupling example of an elastic-
walled tube shows the flexible coupling concept between structural and fluid software. The combination of both, transient aerodynamics and flexible coupling is applied for the AGARD 445.6 wing flutter test case. A good agreement has been obtained for the comparison of the flutter frequency in a wide range of Mach numbers. The results of the present paper are preliminary and further validation studies are planned in the field of flutter computations. Different quality procedures, which are common practice in single field analysis, will to be taken into account for coupled multi-physics investigations. These procedures are e.g. parameters studies of time step size or grid density size, which allow judging more precisely the quality and accuracy of the coupled simulation results. 6 ACKNOWLEDGEMENT The authors would like to thank Justin Penrose for supporting the work of one of the testcases. M. Kuntz and F.R. Menter 12 REFERENCES [1] I. Demirdzic and S. Muzaferija. Numerical methods for coupled fluid flow, heat transfer and stress analysis using unstructured moving meshes with cells of arbitrary topology. Comput. Methods Appl. Mech. Engrg. 125, pp.235-255, 1995. [2] ANSYS 8.0 Theory Manual, ANSYS Inc., 2004. [3] M.J. Raw. Robustness of coupled algebraic multigrid for the Navier-Stokes equations. AIAA Paper 96-0297, 1996. [4] F.R. Menter and T. Esch. Elements of Industrial Heat Transfer Predictions. Presented at the 16th Brazilian Congress of Mechanical Engineering (COBEM), Nov. 2001, Uberlandia, Brazil, 2001. [5] J.P. Zwart, A.D. Burns, S. Phillipson and D. Gobby. Finite Volume Simulation of an Airlift Loop Reactor with Coupled Algebraic Multigrid. Proceedings of ASME FEDSM’02, ASME Fulids Engineering Division Summer Meeting, Montreal, Quebec, Canada, 2002. [6] J.M.T. Penrose, D.R. Hose, C.J. Staples, I.S. Hamill, I.P. Jones and D. Sweeney, D. Fluid Structure Interactions: Coupling of CFD and FE. 18. CAD-FEM Users’ Meeting, Internationale FEM-Technologietage, Sep. 20-22, 2000. [7] MpCCI Specification. Release 2.0, March 2003; MpCCI Homepage www.mpcci.org
[8] G.E. Schneider and M.J. Raw. Control volume finite-element method for heat transfer and fluid flow using colocated variables. 1. Computational procedure. Numerical Heat Transfer, 11:363-390, 1987. [9] CFX-5.7 Solver Manual. ANSYS Inc., 2004. [10] T.J. Barth and D.C. Jesperson. The design and application of upwind schemes on unstructured meshes. AIAA Paper 89-0366, 1989. [11] C.M. Rhie and W.L. Chow. Numerical study of the turbulent flow past an airfoil with trailing edge separation. AIAA Journal, 21:1525-1532, 1983. [12] H. Grotjans and F.R. Menter. Wall Functions for General Application CFD Codes. Computational Fluid Dynamics, Proceedings of the 4th Computational Fluid Dynamics conference, 7-11 Sept. 1998, Athens, Greece, Vol. 1, Part 2, ECCOMAS, Papailiou, K.D., Tsahalis, D., Periaux, J., Hirsch, C. and Pandolfi, M., John Wiley & Sons, pp. 1112-1, 1998. [13] I. Demirdzic and M. Peric. Space conservation law in finite volume calculations of fluid flow. Int. J. Num. Methods in Fluids, 8, pp1037-1050, 1998. [14] I.R. Hawkings and N.S. Wilkes. Moving Grids in Harwell-FLOW3D. AEA, InTec-0608, 1991. M. Kuntz and F.R. Menter 13 [15] R.H. Landon. NACA0012 Oscillatory and Transient Pitching, Compendium of Unsteady Aerodynamic Measurements, Data Set 3. AGARD Report R-702, Aug. 1982. [16] C. Gao, S. Luo, F. Liu and D.M. Schuster. Calculation of Unsteady Transonic Flow by and Euler Method with Small Perturbation Boundary Conditions. AIAA 03-1267, 2003. [17] J.M.T. Penrose and C.J. Staples: Implicit Fluid Structure Coupling for Simulation of Cardiovascular Problems. International Journal of Numerical Methods in Fluids, 40(2-
3), 469-480, 2002. [18] J.R. Womersley. Oscillatory flow in arteries: the constrained elastic tube as a model of arterial flow and pulse transmission. Physics in Medicine and Biology, 2, 178-87, 1957. [19] E.C. Yates. AGARD Standard Aeroelastic Configuration for Dynamic Response, I – Wing 445.6. AGARD-R-765, 1988. [20] W. Haase, V. Selmin, B. Winzell. Progress in Computational Flow-Structure Interaction. Notes on Numerical Fluid Mechanics and Multidisciplinary Design, Springer, Volume 81, 2003. 
Автор
Redmegaman
Документ
Категория
Техническая литература
Просмотров
365
Размер файла
473 Кб
Теги
kuntz, structure, Газовая динамика, simulation, interactions, menter, aeronautical, cfx, турбулентность, fluid, applications
1/--страниц
Пожаловаться на содержимое документа