Best Practice Advice AC6-06

Jump to navigation Jump to search

Front Page


Test Data

CFD Simulations


Best Practice Advice

Gas Turbine nozzle cascade

Application Challenge 6-06 © copyright ERCOFTAC 2004

Best Practice Advice for the AC

Key Fluid Physics

The test case is an high pressure turbine nozzle guide vane with heat transfer The blade shape is optimised for a downstream nominal Mach number equal to 0.9 and the flow field in this reference condition is transonic with a shock on the SS. The tested Mach number range from 0.7 to 1.1 and the intensity and position of this recompression shock strongly depends on the working condition while the tested turbulence levels range from 1.0 to 6.0. The boundary layer presents laminar or turbulent features, depending on the free stream levels and the Mach number. On the pressure side the boundary layer is mostly in a laminar state in quite all the tested condition. On the SS the boundary layer development is strongly related to the Re and Mach numbers and free stream turbulence levels. For the higher levels of free stream turbulence and Reynolds numbers a transitional boundary layer is detected. For lowest Mach Numbers the transition onset on the SS is mainly dependent from the free stream turbulence levels, while for the highest Mach numbers the transition clearly starts from the shock position. The presence of transitional flow field and shock-boundary layer interaction has a large impact on the heat transfer coefficient. The transition onset can be clearly located for different free-stream turbulence levels, when the experimental heat transfer coefficient on the blade suction side suddenly grows. Heat transfer and efficiency are the global parameters to assess the performance of the blade profile.

For the deeper understanding of the physical phenomena involved in this AC the analysis of some simpler flow regimes could be helpful. The most important are represented by the UFR3-03, UFR3-04, UFR3-05, and UFR3-19.


From the experimental data it is evident that also for the lower tested Mach numbers the flow on SS shows a recompression zone towards the TE of the blade. In this region the boundary layer experience an adverse pressure gradient. For some working conditions the deceleration imposed by the positive gradient cannot be sustained in the near wall flow and separation can occur.

For a more complete description of this particular aspect of the flow in the NGV the UFR3-03 can be useful. In this section the essential behaviour of a 2D flow under adverse pressure gradients in different flow regimes is analysed. The effects of flow separation such as deviation of the inner scaling from the logarithmic profile, the presence of separation bubbles and induced unsteadiness due to reversal flow and reattachment are described. The main controlling parameters are investigated (turbulence level which can increase resistance to flow separation) and different test cases are reported.


The experimental evidence clearly indicate that SS boundary layer is subject to transition and relaminarization depending on a number of parameters among which the local pressure gradient (Ma-number), the local streamline curvature, the Reynolds number the turbulence level.

Transition can occur with three different mechanisms: natural, by-pass, and separated flow (or mechanical).

By-pass transition is due to the turbulence diffusion inside the boundary layer from the flow core when the free stream turbulence levels are high. This is the prevailing mechanism in this test case and is in general the most likely to occur in turbines blades. This complex mechanism requires an accurate prediction of both the inner flow layer in the immediate proximity to the solid walls, but also of the flow core from which the turbulence stems into the boundary layer. The UFR3-04 can provide some detailed insight about this specific aspect of the flow.


The transonic mach number conditions in the turbine blade causes shock waves and shock boundary layer interactions. The presence of the typical recompression due to the shock waves requires an accurate modelling of the boundary layers behaviour in the presence of adverse pressure gradients. On the aeronautic field this is a relevant problem and great experimental and numerical activity has been devoted to the understanding of the effect of shocks on boundary layer separation. The flow field around the airfoils usually experiences severe fluid dynamic conditions with strong shock-boundary layers interaction, separation downstream the shock and re-attachment ahead of the trailing edge.UFR3-05 analyses this particular aspect for the external flows typical of aeronautical applications, but most of the physics can represent an useful guideline for the better understanding and modeling of confined flows.


This test case is fundamental for the set up and tuning of turbulence and transition models in simpler geometrical applications as well as for the basic understanding of the steps leading to bypass mechanism. A wide range of experimental and numerical tests have been performed in this field and the mechanism of bypass transition has been explained in different ways.

Ø The simplest transition model (concentrated breakdown model) places the start of transition of a laminar boundary layer to a turbulent one when the first appearance of turbulent spots is detected. The subsequent growth of the spots dictates the length of the transition region prior to a fully turbulent boundary layer being achieved.

Ø More recently the concentrated breakdown model has been replaced by a “distributed breakdown” model in which spots are initiated at different stream wise locations. In the pre-transitional boundary layer velocity fluctuations near wall are induced primarily by pressure fluctuations associated with the free-stream turbulence. The growth of these fluctuations is approximately linear in the stream wise direction. When the amplitude reaches some critical level the streamline no longer has an equilibrium position and an instability occurs. A certain number of turbulent spots are induced and transition commences.

In UFR3-19 some more details are provided and result are reported which can be used for the set up of transition modelling.

Application Uncertainties

For this application challenge the main uncertainty to assemble a high fidelity CFD model is represented by the uncertainty on inlet turbulent flow conditions. The proper implementation of the inlet boundary conditions for the turbulent variables should be based on the experimental length scale which is not available from experimental data set. In our experience, for the classical two equations turbulence models this parameter is important for the evaluation of the turbulence decay and the turbulence level before the LE of the blade. Bypass transition, which is the main transition mechanism in this test case is strongly dependent on the free stream turbulence intensity and thus the uncertainty on the length scale could influence the transition onset and length. The numerical distribution of the heat transfer profile could be different according to the adopted length scale. The k-ω model with the realizability correction proposed by Durbin (Medic and Durbin,2000) showed a certain independence from this parameter but the results obtained by other two equations approaches could be influenced by the chosen inlet condition. The independence of the turbulence level on the chosen condition should be preliminarily checked.

Computational Domain and Boundary Conditions


At the stator inlet plane the nominal total pressure and total temperature profiles as also the inlet flow angle should be imposed based on the experimental data. Pressure and density are extrapolated from the inner field.

The proper inlet boundary conditions for the turbulent variables should be implemented through the imposition of the turbulence level (Tu) and the length scale (L) from the experimental data. The kinetic energy and or should be computed according to the following relations:

For this test case as well as for typical turbomachinery application the length scale is not available from experimental data in view of the complexity of the measurements. Usually when two consecutive values of the kinetic energy are known (ie. Tu) for the incoming flow then L could be estimated assuming steady homogeneous decay:

In all other situations the length scale has to be guessed according to previous experiences. Usually L is selected in the range between 1-0.1% of a representative dimension of the problem at the inlet. For this present application the chosen value is 0.5%.


In the exit plane, usually the experimental static pressure is imposed. A fully developed flow field is further assumed neglecting all axial derivatives of the fluid dynamics variables.

Ø If a constant static pressure is imposed in the outlet section a remarkable displacement of the outlet boundary downstream the TE of the blade row is strongly suggested (usually about 1-1.5 pitch distance). In this way the reflection of sonic lines detaching from the suction side can be avoided and the assumption of a perfectly uniform distribution of the pressure and velocity profiles seems more realistic. With insufficient distances the constant pitch-wise pressure field imposed in the outlet section can be inconsistent with the tangential pressure field in the vane and influence the upstream flow field.

Ø A better method for the implementation of less reflective boundary condition is maybe represented by the imposition of an integral outlet pressure field instead of a local pitch wise averaged pressure value. A not reflective outlet boundary condition could be accomplished by the imposition of an integral outlet pressure field instead of a local pitch wise averaged pressure value. To clarify consider the red line indicated in Figure 2. The constant experimental pressure is Pext. The pressure profile extracted from the inner field (red line in the graph) is not constant and has a different mean value. The final pressure distribution, that should be used as a new boundary condition for the outlet section, is obtained scaling this profile so that the mean average coming from the pitch wise radial equilibrium is attained.

D34 image40.jpg

Figure2 -Outlet average pressure condition


On the wall the no slip condition and zero pressure gradient normal to the solid surface are imposed. The experimental temperature is also imposed, ranging from 299K to 302 depending on the test case.

For turbulent equations the boundary conditions to be applied may be summarised as:

When a k-ω model is applied, the boundary condition for the specific dissipation ω poses the problem of the numerical handling of infinite values. This can be solved imposing the following value to the first node from the wall:

Here Δy1 is the normal distance of the first computed cell.

Discretisation and Grid Resolution


The experience gained in the numerical computations of this test case as well as other turbomachinery applications with different solvers allows drawing some general conclusions about the spatial discretization methods:

Ø The FVM, used in combination with unstructured approaches can cope with a wider range of applications and problems, but the numerical cost is usually higher. Structured FVM schemes are also used with little differences from FDM approaches. FVM methods should be preferred since inherently conservative.

Ø The FDMs require a structured computational domain. These schemes are in most cases faster to execute and easier to manage. Their use is particularly suited for problems where the geometry is simply enough to allow a regular structured grid. The relative simplicity of geometry of LS89 test case allowed accurate results with structured approaches.

Ø Both for FV and FD methods the accuracy of the results requires at least a second order discretization scheme. Higher order schemes usually can cause instability and a special treatment is needed to provide monotonic solutions. This problem is particularly felt working with unstructured approaches where higher complexity is needed to handle the grid topology. The robustness of a first order scheme may be useful at the beginning when the disturbances of the initial guessed solution are still relevant.

Ø From the computations performed on various test cases it can be concluded that all the most widespread discretization schemes are capable of providing comparable and accurate results: an optimal FV and FD method based on cell vertex, cell centred, vertex centred… scheme did not emerge clearly.

Convection dominated problems (eg. the compressible Navier-Stokes equations) require the use of some kind of artificial dissipation to improve the stability and accuracy of the solver in the presence of sharp discontinuities and strong gradients.

Ø A widely known approach to provide artificial dissipation is to include in the spatial derivatives 2nd and 4th order artificial dissipation terms. These terms are scaled with the pressure gradients of the solution to improve the stability of the method. Artificial dissipation scheme are usually straightforward with structured schemes. The proposed extensions for unstructured approaches are usually complex and not clearly posed.

o The use of artificial dissipation is simple, efficient and stable, but in some cases can introduce excessive diffusion in the computed flow and reduce the accuracy of the solution. Some tuning empirical parameters and special corrections (such as eigenvalues scaling to provide the required anisotropy in wall boundary layers) can constitute useful tools to improve both the solution quality and stability.

Ø The use of flux upwind represents another quite common way to enforce a monotonic computed solution. Upwind schemes try to follow the dominating behaviour of the characteristics of convective terms and may be applied equally to FDM or FVM schemes for structured or unstructured solvers.

o Several proposals for the flux up winding of convective terms are available. From the experience gained by the Florence University the Roe’s method and the AUSM+ first order scheme proved the better performance in terms of accuracy and stability of the solution.

o Higher order upwind schemes can be obtained using a linear reconstruction of the computed solution inside the grid cells. In this case a monotonic solution is ensured using slope or flux limiting in conjunction with flux up winding. TVD schemes can be different depending on the structured or unstructured approach. For structured schemes the Superbee or Van Leer limiters should be preferred (R. LeVeque, 1992). Unstructured solvers should implement the Barths’s limiter in the improved version suggested by Venkatakrishnan (1995).

o The absence of tuning parameters represents a positive feature with respect to the artificial dissipation approaches.

Ø Past experience showed that both artificial dissipation approach and upwind methods showed good capabilities to ensure a monotonic solution if properly applied so there I not an optimal choice between the two approaches

An important aspect related to the CFD simulation is represented by the computation of the flow gradients used for the high order reconstruction in upwind fluxes or the viscous terms in the Navier-Stokes equations.

Ø For the linear reconstruction used for second order up winding, the most adequate schemes for the computation of the solution gradients (more details can be found in Martelli and Adami, 2001) are represented by the Gauss-Green formula and the least squares approach.

o The Gauss-Green method is easy to implement and requires less computational demand. Unfortunately it gives exact gradients for linear functions on tetrahedral elements only and therefore does not ensure the same accuracy level throughout the field when using skewed structured or mixed hybrid grids. This is a serious drawback since prismatic layers are used to represent the viscous boundary layers near solid walls. Here the accurate computation of the solution gradients is relevant especially when the heat transfer prediction is required or a sophisticate turbulence closure is used.

o The linear least squares reconstruction avoids the above pitfall and allows the same degree of accuracy in the gradient estimate throughout the mesh. More precisely the method is exact for linear functions regardless the cell type. This feature is quite important for stretched structured grids or mixed grids and therefore should be preferred as a default scheme. The least-squares reconstruction is based on a first order Taylor series for the approximation of the solution on each grid cell-centre (more details are available in Martelli and Adami, 2001).

Ø For the computation of viscous stresses the cell centred gradients of the solution, computed in the linear reconstruction can lead to an unstable solution or the decoupling of adjacent nodes.

o The gradients should be computed by a finite difference formula at the midpoint location of every element face. This approach does not involve any reconstruction phase. The fluxes can be obtained by the same quadrature formula (ie. as for the numerical scheme used for convective fluxes) provided that the viscous stresses and conduction heat are computed on the face mid-point. For the viscous terms of Navier-Stokes equations this “staggered” scheme ensures a more stable discretization giving at the same time a simple and accurate representation of the flow.

A grid sensitivity of the solution from the discretization scheme and grid refinement should be always performed. To tackle the additional cost of such test, a fist good indication could be obtained from the comparison of the first and second order solution computed for the same problem. This estimate should be done considering the effect produced by the discretization scheme on some relevant and meaningful parameters such as the DOAPs blade load, the efficiency, the pressure or Nusselt distribution on the blade profile.


For the proper discretization of the physical domain of this test case two kinds of advise should be given. The first concerns general grid recommendations in the field of turbomachinery application, the second pertains to the specific requirements of this particular application.

General grid recommendations

In general two basic grid topologies can be used to represent the geometrical domain in the numerical simulation: structured and unstructured grids.

Ø The structured grids are more easily generated especially for simpler geometries. Different structured grid arrangements are usually employed in turbomachinery application: the most important are H, C, or O-type grids. The O-grid is probably the best arrangement for the near wall regions. This node distribution allows a finer discretization in the leading and trailing edge regions and guarantees orthogonal grid lines near the wall surfaces. For an accurate discretization of the flow field in all the computational domain, generally the O-grid requires a patched approach and the coupling with other grid types (H or C).

Ø The unstructured grids allow a more flexible assembly of elements and a more efficient and flexible local refinement of the mesh. Besides no continuity of grid lines through the whole domain is required. For these reasons unstructured grids are usually indicated in the discretisation of complex domains. The best arrangement for turbomachinery applications is the hybrid arrangement in which quadrilateral elements are used close to the solid surfaces (to solve boundary layers features) and triangular elements are used in the core flow (Fig 1-c).

The accuracy of a CFD simulation increases with the increasing number of grid cells. The global element number is an important parameter to assess the accuracy of the CFD simulation. Anyway the spatial accuracy may be lost for complex geometries due to the high distortion and irregularity of the elements. The following requirements should be verified:

Ø The grid lines for structured approaches should not present discontinuities and guarantee as much as possible the mutual perpendicularity in the whole computational domain. The grid lines should be orthogonal to the solid boundaries.

Ø For unstructured approaches highly skewed elements should be avoided. For the tetrahedral elements the internal angles should be equal (Fig 1-d) while for quadrilaterals the edges should be almost the same (Fig 1-b).

Ø The grid elements size should vary regularly across the domain. The stretching ratio of adjacent element sides should be in the range between 1.1 to 1.6 for tetrahedral and triangles. In case of quadrilaterals the stretching ratio inside the boundary layers (the growing law) should range from 1.1 to 1.5.

Specific requirements:

For the accurate simulation of this high pressure turbine nozzle guide vane some specific requirements should be fulfilled:

Ø If a structured approach is used an efficient practice is the H-O-H type patched grid.(figure 1a). This solution represents a good compromise for improving grid flexibility and accuracy and combines the more suitable characteristics of O and H grid types in different regions of the field.

Ø A different solution is represented the I-type grid in which the blade is placed inside the computational domain by blocking a number of grid nodes. An example is reported in Figure 1b. This grid structure is potentially able to provide strong grid clustering near the blade surface and the LE and TE of the blade. Although the blocked grid nodes represent a computational overhead and the continuity of grid lines is hardly guaranteed.

D34 image026.gif D34 image028.gif

Figure 1a: Structured HOH grid Figure 1b: Structured I grid

D34 image030.jpg D34 image032.jpg

Figure 1c: Unstructured grid Figure 1d: BL Grid features

Ø A remarkable grid clustering is required near solid boundaries to integrate the turbulent equations down to the wall surface. This usually requires enough grid cells across the boundary-layer thickness to reach y+ values lower than 10 for the first node. Besides for an accurate boundary layer description 5 or more grid cells are required between the wall and y+ of 20.

Ø In case of heat transfer computations the grid requirements are further tightened and the distance of the first node from the wall should ensure y+@ 1.

Ø For this application, y+ values around 1.0 should be ensured posing the first node from the wall at a distance of about 1.0e-5mm in order.

Ø A common error done trying to enforce a very close first cell to the wall may consist in the generation of an excessively stretched grid with badly shaped elements and poor aspect ratios. An evenly refined should be guaranteed when reducing y+ for the first node. The suggested range for the stretching ratio is about 1.15-1.25. This range is a good compromise between the need to lessen the number of elements inside the boundary layers and a regular variation of the grid height between neighboring elements.

Ø In view of the previous point the proper resolution of thermal boundary layer requires at least 30-40 prismatic layers in the O-grid around the NGV blade surface (in Fig-1d 50 layers have been used).

Ø A regular grid distance of the first cells from the solid wall should be imposed. In our experience for the accurate heat transfer prediction a smooth variation of the y+ values along the surface may be even more important than a very low value.

Ø The elements aspect ratio (ratio of two adjacent sides) needs also to be limited. This is especially the case away from solid boundaries. The suggested maximum should be less than 20 in the main flow, while higher values may be tolerated inside the boundary layers (100-200). Considering the short distance between the first node from the wall and the wall a relevant number of grid nodes is also required along the blade surface (Fig 1-d). The grid refinement along the blade profile is useful in order to capture the boundary layer development and the transition onset: around 100 grid nodes should be employed for the transitional boundary layer on the SS; on the PS a reduced number of around 60 elements should be sufficient in view of the reduced length and the laminar boundary layer.

Physical Modelling

In this application the main challenge is represented by the proper modeling of the turbulence and transition features of the boundary layers. The actual mechanism of natural transition, the incipience and growth of perturbations in laminar flows, the development and amplification of local instabilities and their break out, is beyond the capability of Reynolds-averaged Navier–Stokes (RANS). In this test case most of the previous stages in the natural transition mechanism are bypassed for presence of strong forced disturbances represented by diffusion of turbulence into a boundary layer which cause bypass transition. In this situation RANS models can give quite accurate results and different approaches have been already used to compute the transitional flow field. Some results have been reported in the AC description file. The main advantages and drawbacks of the different approaches will be briefly underlined here.


Algebraic models: are based on simple assumptions on the laws of wall from the boundary layer theory. The degree of empiricism of these models is high. They may give satisfactory results for well-tested applications involving simple shear layers and attached flows for which they have been calibrated and tuned. They are generally inadequate in the present case in view of the presence of strong adverse pressure gradients, separated zones and transitional flows.

Two-equation models: represent a widely accepted approach for turbulent flows in turbomachinery environments. The two-equation closures represent a more accurate approach for the Reynolds stresses with respect to the algebraic models but they are based on a linear constitutive law, (the Bousinnesq assumption). Generally these models give poor predictions when the non linearity of the flow field is remarkable such as for strong curvature flows, strongly not isotropic field and in the presence of flow separations and reattachment. Other limitations are revealed in the investigation of the transition problem. Amongst them the wrong location of the transition onset, under-prediction of transition length, excessive sensitivity from initial conditions and a certain dependency from the Mach number.

Ø The most documented versions are the k-ε and k-ω models should be applied in view of their experienced advantages and limitations.

Ø With k-ε and k-ω models the realizability correction proposed by Durbin shouldbe implemented. This constraint has been based on a mathematical basis and it has proved to improve both accuracy and stability of the numerical computation. The latest version of this correction can be found in Medic and Durbin (2000).

Ø In this AC curvature effects are relevant in the LE area and some correction accounting for curvature effects should be implemented. Unfortunately the curvature corrections available in literature have been developed for a special class of flows and can not be extended or assumed as a general improvement to be recommended in this application challenge.

Ø Curvature and anisotropy could be better accounted using non-linear extensions of two-equation models. Basically the governing equations retain the same features and terms, but the Reynolds stress constitutive law is modified including terms with higher powers of k/ε. These non-linear terms include a dependency from quadratic and cubic products of the strain and rotation tensors as well. The most accredited non-linear model are the Craft-Launder cubic model and the Gatzki-Speziale. Our opinion and experience is that the advantages offered by these models are often limited so that the computational effort added may not be always justified. More specifically these models result to be very unstable with a difficult convergence.

Ø Different low-Re-number modifications have been proposed at different modelling levels. The main effect is the achievement of an overall damping of turbulence as the wall approaches. In many cases they claim to guarantee an accurate description of transitional boundary layers. In our experience the stand alone implementation of a low Re modification is not sufficient to give accurate results in presence of transitional flow fields. In fact in the most widespread models no distinction is made between the turbulence damping due to pure viscosity effects and the non-viscous directional wall blockage. The viscosity damping affects evenly the turbulence fluctuations in all directions. The solid wall imposes a non permeability conditions only in the normal direction. This induces a consequent eddy deformation with a damping effect which is felt mainly by velocity fluctuations normal-to-the-wall so the presence of the wall results in an increased turbulence anisotropy. Most low-Re-number models treat both effects jointly and usually relates the overall damping only to the local wall distance. Such a practice can reproduce near-wall behaviour in near-equilibrium steady flows but fails in most cases with complex wall topography, or with a significant departure from equilibrium conditions. In view of the fact that most transitional phenomena are provoked, enhanced or controlled by sudden changes in boundary or external conditions, it is obvious that such models can not reproduce a broader variety of transition phenomena.

Reynolds stresses:

Reynolds stress approaches undeniably introduce more physics in to the model. The major advantages are represented by the provision to account for anisotropy of the free-stream and of the near-wall stress field, particularly in the ability to reproduce the normal-to-the-wall velocity fluctuations. Another merit is the exact treatment of the turbulence production and of effects of streamline curvature. These features help also in handling other forms of non-equilibrium phenomena, such as separation and reattachment, which are frequently encountered with different forms of transition. The difficulty encountered in transition modelling relies most probably on the solid wall boundary condition problem. In fact, the most popular Reynolds stress models still use wall functions to bridge the boundary layer in proximity to the wall. The theoretical background of wall functions indicates that the correct prediction of transition, or the effect of pressure gradients and stagnation points, is at least debatable. Although several attempts have been made to avoid wall functions in Reynolds stress models, like those of Shi et al. or by Savill et al. (2000), the higher complexity of this modelling approach implies too large a computational effort, also on account of the extremely refined grids required to resolve the boundary layer.


Transition onset: The most commonly used approaches to determine the position of the onset of transition and the transition length are represented by integral models, two-equation models and intermittency transport models. From the experience gained in this field it seems that all the attempts to predict transitional flows by using classical models did not allow a satisfactory predicting of transition features.

Ø The transition point often in poor agreement with experiments

Ø transition length often under-predicted

Ø the sensitivity of the model to the initial profile is excessive

Ø insensitivity of the predictions to the Mach number

The best results have been obtained using conventional closure with intermittency function coupled to empirical criteria for the onset and length of transition. In this case the intermittency transport model of Steelant and Dick (1999) should be considered. For turbine blades the recommended onset correlation is that from Mayle (for Tu > 3% Reθ(transition) = 400Tu-5/8). Otherwise a more general criterion is the Abu-Ghannam and Shaw correlation for attached flows. Concerning the transition length a good result was achieved assuming that Reθ(end transition)} = 2Reθ(transition). Owing to these correlations, the intermittency function production terms may be properly conditioned as to fulfil the transition onset and length according the experiments.

Recommendations for Future Work

For the definitive assessment of the AC6-06 much work should be done to provide further elements of discussion and improve the quality of the test case. The following activities might provide very useful contributions:

Ø The curvature effects are relevant especially in the region immediately after the LE area but no correction accounting for curvature effects have been already tested.

Ø The numerical simulation of the present AC and some of the associated UFRs should be repeated using contemporary and advanced turbulence models. The research activity in the turbulence field is still proceeding and up to date approaches can include more and more physics in the modeling.

Ø For the computation of complex flows with transitional phenomena RANS methods are undeniably limited in their possibility to capture real physics in comparison with DNS or large-eddy simulations (LES). DNS and LES numerical simulations have been already performed to reproduce also the temporal growth of the instabilities inducing a transitional flow field. The use of massive computing resources (parallel architectures and clusters) is today commercially available so that the CFD computation of a more complex geometry is possible in reasonable computing times. The DNS or LES simulation of the test case could be profitably used to obtain a reference solution or a data base for the assessment of simpler turbulence and transition models.

Ø The simulation of related UFRs such as UFR3-19 concerning bypass transition on flat plate is a very interesting test case for the set up and tuning of the turbulence models implemented. In fact bypass transition is the prevailing mechanism in the determination of the transition onset. This test case is simpler and can be used to tune the transition model in absence of other phenomena such as curvature effects and shock boundary layer interaction. The comparisons of the performance of the transition models on the two different applications could provide interesting information about the accuracy of the model.

© copyright ERCOFTAC 2004

Contributors: Elisabetta Belardini, Francesco Martelli - Universita di Firenze

Site Design and Implementation: Atkins and UniS

Front Page


Test Data

CFD Simulations


Best Practice Advice