User:Standingford.bae
Shock/Boundary Layer Interaction
Underlying Flow Regime 3-05
Abstract
Understanding the underlying flow regime of a jet in cross flow documented here is basic to solving several problems of considerable practical importance in aeronautics, civil engineering, environmental engineering and turbomachinery. This flow regime has been systematically studied since the first half of the twentieth century. In 1993 the Advisory Group for Aerospace Research and Development (AGARD) organized a conference with the title ‘Computational and Experimental Assessment of Jets in Cross Flow’. Thirty seven papers were presented, showing the vigour of this subject as a field of research. Margason (1993) gives a list of the main applications of knowledge about jets in cross flow:
Plume dispersion from smoke stacks and volcanos: This is a pollution problem where smoke concentration is of interest. The smoke leaves either the stack or the volcano with an upward momentum due to buoyancy into a stagnation air mass or into a cross wind. So it is usual to make the analysis of the motion caused by buyancy until it becomes negligible and then to consider a diffusion formulation.
Effluent dispersal into streams: This is also a pollution problem where the focus of research is diffusion of the jet into a lake or a river. The goal is the identification of the polluted region and the estimation of the concentration of pollutant. This analysis often happens in the design of sewage treatment and disposal systems.
Turbomachinery cooling and fuel injection: In cooling, the problem is to protect the components of the combustor or the turbine against very high temperatures, adopted for purposes of efficiency. The optimum design of a cooling system will protect the components using as little cooling medium as possible and affecting the efficiency of the component as little as possible. In fuel injection, the designer wishes to achieve the best possible quality of mix of fuel and air.
Control jets: On underwater vehicles and on aircraft, control jets are used to produce control moments. Interest here is on the interaction between different flows and their effect on the control moment.
Vertical and/or Short Take Off and Landing aircraft (V/STOL): This has probably been the most important application of the study of jets in cross flow. The problem is to minimise the loss in lifting force and the nose-up pitching moment caused by the jet. Objectives also include the minimisation of ground damage, of modification of aerodynamic forces and moments and of ingestion of hot, exhausted gases in engine inlets.
The Physics of a Jet in Cross Flow: The physical phenomenon is described by several authors. However, some differences of interest imply different descriptions of the fundamental aspects of the flow regime. So, those who are interested in V/STOL, describe a system where we have a jet, a cross flow and a wall, normal to the jet exit. We will concentrate our attention on a flow system that is of interest to turbomachinery and environmental engineers.
A jet exhausting into a cross flow follows a curved path downstream while its cross section changes (see Fig. 1.1). For the case of a circular jet (Margason (1993)), the pressure distribution due to potential flow around a rigid circular cylinder can be considered. The pressure coefficient is given by . At and there are stagnation points and Cp=1. At the lateral edges, whereand , the pressures reach a minimum and Cp=-3. The flow then spreads laterally into an oval shape. At the same time the cross flow shears the jet fluid along the lateral edges downstream to form a kidney-shaped cross section. At increasing distances from the jet exit, the shearing folds the downstream face over itself to form a vortex pair. Fig. 1.1 also shows the secondary vortices: the horseshoe vortex and the wake vortex street.
The ratio R = (jet velocity / cross flow velocity) is of particular importance. When R is high (6, 8, 10 or more - see for example Keffer and Baines 1962), the jet penetrates far across the main flow. If R is low, the jet tends to bow at a short distance from the orifice. Fig. 1.2 (a), from Andreopoulos and Rodi (1984) shows the case of R=0.5. The jet bends immediately after leaving the orifice. The main flow is slightly distorted by the jet and, downstream the orifice, it looks like a ‘cover’, under which the fluid of the jet flows. Fig. 1.2 (b) (same authors) shows the case of R=2. With a higher velocity, the jet penetrates into the cross stream before being bent over. The jet is weakly affected near the exit. In both cases, wakes with complex flow patterns are formed downstream the jet. Close to the wall, a region of reverse flow forms. Cross stream fluid that enters this region moves upstream, is lifted by the jet and then moves downstream with the fluid of the jet. As the jet is bent, its cross section is distorted by two counter rotating vortices, taking the shape of a kidney, as mentioned above. This secondary motion decays in the downstream direction under the action of turbulent stresses. The approaching boundary layer has negative vorticity, which is increased as the jet is bent. In the pipe, near the exit, the counter-rotating vorticity is formed by the coss stream moving around the jet.
The basic feature of Jet in Cross Flow is the mutual deflection of jet and cross flow. The jet is bent over by the cross stream, near the wall if R is low and far from the wall if R is high. The cross stream is deflected as if it had hit a rigid obstacle. The vortices form when the wall boundary layer encounters an adverse pressure gradient at the front of the jet and separates.
Contributors: Flavio Franco - ABB ALSTOM Power UK Ltd
UNDERLYING FLOW REGIME DOCUMENTATION SHOCK/BOUNDARY LAYER INTERACTION
1. INTRODUCTION
2. REVIEW OF UFR STUDIES AND CHOICE OF TEST CASE
Experimental investigations of shock/boundary layer interactions have been made for laminar and turbulent boundary layers as well as laminar boundary layers undergoing transition to turbulence following the shock/bounday-layer interaction. Most interest in CFD comparison exercises has been focussed on interactions with fully turbulent boundary layers although interactions with laminar boundary layers and boundary layers undergoing transition are also relevant to aerodynamic applications.
Comparison between CFD simulations for fully laminar boundary-layers and boundary layers induced to undergo transition were made in the ERCOFTAC workshop on shock/boundary layer interactions held at UMIST in 1997 [1]. The fully laminar test case was the experiment of Bristeau et al [2] involving flow through a double throated nozzle. Following an initial pressure induced separation, a smaller shock induced separation results from the impingement of an oblique shock on the boundary layer. Relatively small differences between the CFD solutions obtained by workshop participants for this test case were attributable to differences in the numerical schemes employed. The transition test case was Skebe’s case D in which an oblique shock impinges on laminar boundary layer flow over a flat plate [3]. The problem of correctly predicting the transition made this a difficult test case in which to achieve good agreement with experiment.
In fully turbulent test cases the focus is on the performance of the turbulence model employed in the CFD simulation. Amongst turbulent boundary layer investigations the two-dimensional bump flow experiments of Delery have been widely used as test cases in CFD simulations. Delery [4] performed three experiments known as cases A, B and C. In each of these flow is accelarated from subsonic to supersonic conditions through a constriction in a tunnel of rectangular cross section. In cases A and B the constriction is formed by a symmetric configuration of bumps mounted on the floor and ceiling of the tunnel whilst in case C a bump is mounted only on the floor. In each case a shock is formed in the divergent region of the flow and interacts with the turbulent boundary layer on the rearward facing side of the bump. In case A this results in an incipient separation whilst in case B there is an extended region of separation. In case C the separation is strongest and of greatest extent. In all three cases measurements were made of surface pressures along the mid-span line. Velocity turbulent kinetic energy and shear stress profiles were also measured at a number of mid span, streamwise locations.
Delery’s bumps A and C were used as test cases in the EUROVAL collaborative programme to validate turbulence models [5]. More recently, case C was adopted as the fully turbulent test cases in the ERCOFTAC workshop on shock/boundary-layer interactions mentioned earlier. A shortcoming of using these test cases in these comparison exercises is the relatively close confinement of the flow in the spanwise direction resulting in 3d effects. The entrance to the test section has a width of only 120mm compared to a height of 100mm. Consequently non-negligible spanwise gradients of flow variables are observed casting doubt on the validity of comparisons with the 2d CFD simulations in EUROVAL and elsewhere. Whilst not really qualifying as 2d test cases these flows are not ideal as 3d test cases either due to the lack of relevant measurements for comparison with a 3d simulation.
An investigation of an intentionally 3d shock boundary layer interaction was made in the experiment of Pot, Delery and Quelin [6]. This was similar to the transonic bump flows described above and was performed in the same test section. The difference in this case was that the bump was inclined at an angle of 60 degrees to the flow direction resulting in strongly three-dimensional flow. The shock generated over the backward facing surface of the bump was sufficiently strong to provoke flow separation. Surface pressures were measured on all four walls and velocity and shear stress profiles were measured at a number of locations. This flow has a highly complex structure making it difficult to visualise and understand. This complexity makes it an unsuitable choice as a test case for the shock-boundary layer UFR.
An alternative to the complexity of fully 3d flow and the uncertainties associated with 2d planar flow is axisymmetric flow such as that in the bump flow experiment of Bachalo and Johnson[7]. This experiment consists of flow over an annular bump mounted on a cylinder aligned with the flow direction. A shock above the rearward facing surface of the bump promotes flow separation. Measurements of surface pressures were made together with profiles of mean velocity, turbulent kinetic energy, shear and normal stresses. The axisymmetric character of the flow enables 2d numerical simulations to be performed in polar coordinates or 3d simulations on a thin wedge with appropriate symmetry conditions. This aspect together with the detailed high quality experimental data determined that this experiment should be selected as a fundamental test case within a collaborative research programme between UK universities and industry known as VoTMATA (Validation of Turbulence Models for Aerospace and Turbomachinery Applications). This programme sought to validate turbulence models and achieve some basic understanding of their strengths and failings. The uncomplicated character of the experiment together with the careful comparison with CFD available from VoTMATA has resulted in this being selected as the test case for the UFR.
The VoTMATA database
The Bachalo Johnson test case within the database can be accessed here The data contained comprises:
• Code for generating a mesh • Boundary conditions and set up instructions • Experimental results in ASCII format • All CFD computational results at specified locations in ASCII format. 3. BRIEF DESCRIPTION OF THE STUDY TEST CASE
Figure 1: Experimental configuration of the Bachalo Johnson axisymmetric bump
The model for this experiment [7] consisted of an annular circular-arc bump (chord length c=0.2032m, height 0.237c) attached to a circular cylinder (radius 0.375c) aligned with the flow direction (see figure 1). The leading edge of the bump was faired into the cylinder surface in an arc of radius 1.008c while the trailing cylinder surface junction was unsmoothed. The circular cylinder extended 61 cm (approximately 3 chord lengths) upstream of the bump leading-edge. Inlet from the tunnel was at a total temperature and pressure of 302K and 0.95x105N/m2 respectively. The test was conducted at a free-stream Mach number of 0.875 and a Reynolds number of 13.6x106/m. Under these conditions acceleration to supersonic flow over the first part of the bump was followed by a shock at a distance of about x/c=0.66 from the bump leading edge. This lead to a shock-induced separation at x/c=0.7 and a reattachment downstream of the bump at x/c=1.1.
Experimental measurements were made with two component LDV to give profiles of mean velocity and turbulent normal and shear stresses at various streamwise stations. Surface static pressures were also measured.
4. TEST CASE EXPERIMENTS
The experiment was conducted at the NASA Ames Research Center 2x2ft Transonic Wind Tunnel. This is a closed-return, variable density, continuous running facility with 21% open porous slotted upper and lower walls.
In contrast to planar two-dimensional bump experiment the axisymmetric character of this configuration meant it was relatively free of sidewall interference. Also, the shock in this experiment terminated before reaching the tunnel wall thus, the unsteadiness that arises in planar experiments from the interaction between the shock and the tunnel wall was absent here. Good axial symmetry was confirmed through oil flow visualisation on the surface of the bump and a holographic interferogram in the inviscid region of the flow.
In order to facilitate CFD calculations, experimental data profiles at X/C = -0.25 are available for comparison. CFD inflow conditions should then be adjusted in order to match the experimental profiles at this location (See section 5 for specific advice).
Two component laser Doppler velocimeter (LDV) measurements were made at a number of vertical sections from just upstream of separation to downstream of reattachment. The curved surface of the model had the advantage of reducing diffuse reflection of the laser beams from the surface. This allowed measurements to be made very close to the wall. 5. CFD METHODS The experiment of Bachalo and Johnson formed one of the fundamental test cases of the VoTMATA collaborative investigation of turbulence model performance. This is described in detail in the paper of Hasan and McGuirk [8]. An important feature of VoTMATA compared to previous such collaborative exercises is that strenuous efforts were made to eliminate sources of differences between the various partners computations when using a common turbulence model before turbulence model differences were investigated. The test case was computed by three partners; Loughborough University, UMIST and Aircraft Research Association (ARA). Loughborough and UMIST used cell centered finite volume codes where as ARA’s code was a cell vertex scheme. The convection schemes were all second order TVD. UMIST used a pressure based algorithm while the other partners used a density based algorithm. UMIST also solved the test case in 2D using cylindrical coordinates while the other partners solved for a 3D sector with appropriate symmetry conditions on the azimuthal boundaing surfaces.
In order to check whether code differences were resulting in any differences in results the partners all computed the flow with the high Reynolds number k- model and compared their results in detail. No significant differences were found in stress components, separation length or skin friction coefficient. The primary grid used for low Reynolds computations consisted of 221x101 grid points (221 stream-wise). A high Reynolds number mesh was formed by amalgamating the 20 cells nearest to the wall. The values of y+ for the first grid point from the wall were 1 and 70 for low and high Reynolds number computations respectively. The computational domain extended in the stream-wise direction from x/c=-4.0 to x/c=4.5 and in the radial direction to 4.5c above the surface of the cylinder.
Boundary conditions for momentum variables were no slip on the wall, extrapolation of variables at outflow, and an Euler condition on the upper boundary. Constant velocity and temperature profiles were imposed at inlet which yielded a velocity profile in good agreement with experiment at x/c=-0.25. Turbulence energy was set to 0.1% of the mean kinetic energy at inlet. Sensitivity studies showed that varying this in the range 0.01%-0.2% had little influence on the flow development in the separation region. A grid sensitivity was conducted for the high Reynolds number k- model using a grid with 377x161 points. Only very small changes in the solution resulted from the refinement.
Computations were performed with three classes of turbulence models. The simplest class was that of tensorially linear models. In addition to the standard high Reynolds number k- model with wall functions this included the Launder Sharma low Reynolds number k- model [9], the Wilkox k- model [10] and the Menter SST (k-) model [11]. The next class was that of tensorially non-linear models. This included the Speziale model [12] with wall functions, the cubic Suga model [13] and the cubic Apsley-Leschziner model [14]. The final class was that of Reynolds stress transport models. This included the Gibson Launder model [15] with wall functions, the Hanjalic et al model [16] and the Wilcox multi-scale model [17]. Intercode comparisons similar to that for the standard k- model were made between pairs of partners for the k- model, the quadratic Speziale model and the Wilcox multiscale model. They all revealed only small differences between codes.
6. COMPARISON OF CFD CALCULATIONS WITH EXPERIMENTS
A detailed comparison of CFD and experimental results can be found in the paper of Hassan and McGuirk [8]. This includes cross plots of surface pressure coefficients and skin frictions together with profiles of the streamwise velocity component, the shear stress, the turbulence kinetic energy and the streamwise and radial normal stress components. The main findings of Hassan and McGuirk with respect to pressure and skin friction coefficients are summarised here and illustrated with cross plots of these coefficients taken from their paper. For more discussion of differences in profiles of flow quantities and their relation to the observed differences in surface pressure and skin friction the reader is referred to [8]. These results can be compared by consulting the CFD data here.
Except for the Menter SST model all of the tensorially linear models perform badly. As can be seen from the pressure distribution, the shock is located well downstream of the experimental location and they all fail to predict the pressure plateau in the separation region indicating an insufficiently large recirculation region. The Menter SST model on the other hand gives a very much better prediction of the shock location and pressure plateau. From the skin friction distribution it is seen that the Menter SST model predicts a slightly early separation. The k- model gives a separation location close to experiment while the k- models give a much delayed separation. This is consistent with the known poor performance of k- models under conditions of strong adverse pressure gradient and the improvements that arise from using the scale determining equation.
The non-linear models perform much better overall than the linear models (excluding the Menter SST model). Of these models the Speziale model performs least well both in capturing the pressure plateau and in the predicting the separation location. The most significant difference between the Speziale model and the other two models is the lack of any strain dependence in the coefficient C . The Reynolds stress transport models appear to give best overall agreement with experiment as is to be expected although examination of velocity profiles reveals that both these models and the non-linear models lag behind experiment in the flow recovery region.
Figure 1 Cross plots of Cp (left) and Cf (right) for linear models (top row), non-linear models (middle row) and Reynolds stress transport models (bottom row).
7. BEST PRACTICE ADVICE FOR THE UFR 7.1 Key Physics For an aircraft wing operating at transonic cruise conditions, the interaction of a shock wave with a turbulent boundary layer can have a significant effect on key aerodynamic parameters such as lift and drag. Therefore, it is essential that the key physical processes of this interaction be captured with sufficient accuracy by a numerical method. The rapid change in the mean flow through a shock can cause rapid normal straining of the boundary layer. This results in thickening of the boundary layer and possible flow separation. This may be followed by flow re-attachment of the separated shear layer and flow recovery. There will generally be a time lag in the response of the turbulence structure to the rapid changes in the mean flow through the shock. That is, the flow is far from equilibrium. It is essential that the turbulence model used is able to model the effect of this non-equilibrium flow. In addition, during the flow recovery following re-attachment, the turbulence model must be able to model the interaction between the growth of the new boundary layer and the attaching shear layer. 7.2 Numerical Modelling Issues • Discretisation Method
USE a high order accurate scheme, at least second order accurate in space, with as little numerical dissipation as possible
• Grids and grid resolution
For low Reynolds number turbulence models, USE a mesh that has wall adjacent cell heights of y+ < 1. For a wall function approach, USE a mesh with wall adjacent cell heights in the range 50<y+<100 USE a mesh that has at least 10 grid points in the streamwise direction across the shock. USE a mesh that has between 5-10 grid points within a distance of y+=20 from the wall. USE a mesh that has between 30-60 grid points across the boundary layer
• Boundary conditions and computational domain
USE constant velocity and temperature profiles (i.e. plug flow) at an inlet plane 4-chord lengths upstream of the bump to give the experimental velocity profile by 0.25 chords upstream. USE extrapolation of variables at outflow. USE an inflow turbulent kinetic energy in the range 0.01%<k<0.2%
7.3 Physical modelling • Turbulence modelling
Do NOT USE standard linear models such as k- or k-. These typically result in a delayed shock position with weak or non-existent flow separation. If a linear model is to be used, USE the MENTER SST (Shear Stress Transport) model. However, note that this model tends to predict a slightly earlier separation. If a better prediction of shock location, pressure plateau and separation location is required, USE a cubic non-linear model such as the cubic k- model of Suga [13] or that of Apsley and Leschziner [14]. The Speziale variant [12] performs least well in capturing the separation location and pressure plateau and should not be used.
• Transition modelling No transition modelling has been applied as part of this UFR.
• Other modelling None
7.4 Application Uncertainties • The advice given here is not applicable to laminar boundary layers undergoing transition due to shock wave interaction. • The advice is limited to transonic flows. • None of the models considered perform particularly well in predicting velocity profiles in the flow recovery region.
7.5 Recommendations for future work • Calculations should be submitted which evaluate the performance of other, very promising modern turbulence models such as Spalart and Allmaras [18] and Durbin’s v2f [19]. • Further work is clearly required in order to improve model performance in capturing the flow recovery following re-attachment. 8. REFERENCES 1. P. Batten, H. Loyau and M. Leschziner (eds.), “Workshop on shock-boundary-layer interaction”, UMIST, 25th-26th March 1997, UMIST report. 2. M.O. Bristeau, R. Glowinski, J. Periaux and H. Viviand (Eds), “Numerical Simulation of Compressible Navier-Stokes Flows”, In Proceedings of the 1985 GAMM Workshop, Notes on Numerical Fluid Mechanics, Vol. 18, 1985. 3. S.A. Skebe, I. Greber and W.R. Hingst, “Investigation of Two-Dimensional Shock-Wave/Boundary-Layer Interactions”, AIAA, 25(6), 1987. 4. J.M. Delery, “Investigation of strong shock-boundary layer interaction in 2-D transonic flows with emphasis on turbulence phenomena”, AIAA-81-1245. 5. W. Haase, F. Brandsma, E. Elsholz, M. Leschziner and D. Schwamborn (Eds), “EUROVAL – An European Initiative on Validation of CFD Codes”, Notes on Numerical Fluid Mechanics, Vol. 42, 1992. 6. T. Pot, J. Delery and C.Quelin, “Interaction choc-couche limite dans un canal transonique tridemensionnel – nouvells experiences en vue de la validation du code canai.” Technical Report 92/7078 Ay, ONERA, Fevrier 1991 7. W.D. Bachalo and D.A. Johnson, “ Transonic turbulent boundary layer separation generated on an axi-symmetric flow model”, AIAA Journal, Vol. 24, p. 437, 1986. 8. R.G.M. Hassan and J.J. McGuirk, “Assessment of turbulence transport models for transonic flow over an axi-symmetric bump”, The Aeronautical Journal, Paper No. 2562, January 2001. 9. B.E. Launder and B.I. Sharma, “Application of the energy-dissipation model of turbulence to the calculation of flow near a spinning disc”, Letters in Hear and Mass Transfer, 1974, Vol 1 pp 131-138. 10. D.C. Wilcox, “Reassessment of the scale determining equation for advanced turbulence models”, AIAA J. 1988, Vol 26, pp1299-1310. 11. F.R. Menter, “Two-equation eddy viscosity turbulence models for engineering applications”, AIAA Journal, Vol 32, pp1598-1605, 1994. 12. C.G Speziale “On non-linear k-l and k- models of turbulence”, J. Fluid Mech, Vol 178, pp 459-475, 1997. 13. K. Suga “Development and Application of a Non-linear Eddy-Viscosity Model Sensitised to Stress and Strain Invariants.” PhD Thesis, UMIST, 1995. 14. D.D. Apsley and M.A. Leschziner, “A new low-Re non-linear two-equation turbulence model”, Int. J. Heat and Fluid Flow, Vol 18, pp 15-28, 1997. 15. M.M Gibson and B.E. Launder, “Ground effects on pressure fluctuations in the atmospheric boundary layer”, J. Fluid Mech., Vol 86, pp 491-511, 1978. 16. K. Hanjalic and S. Jakirlic and I. Hadzic “Expanding the limits of ‘equilibrium’ second-moment turbulence closures”, Fluid Dynamics Research, Vol 20, pp 25-41, 1997. 17. D.C. Wilcox, “Multiscale model for turbulent flows”, AIAA Journal, Vol 26, pp 1311-1320, 1988. 18. P.R. Spalart and S.R. Allmaras “A One-Equation Turbulence Model for Aerodynamic Flows” , AIAA-92-0439. 19. P.A. Durbin “Near-Wall Turbulence Closure Modelling Without “Damping Functions” ” , Theoretical and Computational Fluid Dynamics, Vol. 3, pp 1-13, 1991.