State-of-the-Art Review: Editing Turbomachinery, Internal Flow

From QNET
Jump to navigation Jump to search

Introduction

The aim of this report is to provide a reference on the state-of-the-art in quality and trust in the application of CFD, within the civil construction industry. This report has been expanded and updated over the duration of the QNET-CFD project, by members of TA4, the Thematic Area on Civil Construction and HVAC. Civil construction is associated with a very wide range of potential applications for CFD. These have been grouped into the following main areas:

1. Transport and Infrastructure

§ Tunnels (ventilation, loss coefficients and smoke control)

§ Bridges (wind loading)

2. Built environment

§ External (pedestrian level winds, wind loading, glazing loading: pollutant dispersion)

§ Internal (HVAC, prediction of natural ventilation rates, fire and smoke, thermal comfort)

3. Hydraulics

§ River sediment transport and deposition

§ Coastal engineering

Due to the diversity of physical phenomena and modeling methods involved in each of the above areas of applications, the report is divided into seven thematic subsections. TA4 members (and other members of QNET-CFD with an interest in TA4) have each contributed reports on the state-of-art of CFD in their chosen area of expertise, as follows:


Tunnel fires:


Dr Norman Rhodes and Mr Nick Waterson


MottMacdonald

Wind loading on bridge deck sections:


Dr Arnau Folch Duran


CIMNE

External Aerodynamics:


Prof Ian Castro


Univ. of Southampton


Internal ventilation:


Dr Darren Woolf and Dr Gavin Davies


Arup

Flow and sediment transport in rivers:


Prof Wolfgang Rodi



Univ. of Karlsruhe

Coastal Engineering:


Dr Alan Cooper


HR Wallingford


These contributions form the main part of the report (Section 3), which is prefaced by a brief overview on the importance of CFD as a modelling tool in the Civil Construction and HVAC industrial sectors (Section 2). © ERCOFTAC 2004 Importance of CFD for the Civil Construction and HVAC Industries

CFD is increasingly becoming an important design and analysis tool in the civil construction industry. Though viewed as an emerging technology in most areas of application, there are some applications for which it is now widely used. There is great potential in the use of CFD in the civil construction industry since it offers the following unique advantages over existing modeling methods:

• efficient and cost-effective engineering design and communication tool

• can be used in replacement or in support of physical model tests

• it is a general application analysis tool, ideally suited for innovative, non-standard designs

The extent to which CFD is used, and the confidence that can be attached to the results varies significantly between the different application areas. Civil engineering applications can be particularly challenging since they typically involve complex or large‑scale geometries and an extensive range of physical phenomena, for example:

• Tunnels: turbulent incompressible/compressible flow, dispersion, combustion, radiation, buoyancy

• Bridges: unsteady flow, fluid structure interaction

• Built environment External: atmospheric boundary layers, unsteady flow, separating bluff body flow, dispersion

• Built environment Internal: low Reynolds number flow, dispersion, combustion, radiation, buoyancy

• Hydraulics: River and coastal engineering: free surface flow, channel and wave/tidal flow and sediment transport, deposition and erosion.

Also, unlike the aerospace and turbomachinery industries which have been using CFD routinely over the last few decades, the application of CFD in the Civil Construction industry is still relatively immature, and there are much fewer examples of validation and quality evaluation initiatives.

In the wind engineering field, an increase in the use of CFD could lead to a significant expansion in the demand for wind engineering services since it could help unlock the potentially large market for studies of flow around structures, which is currently severely limited by high cost associated with such studies, typically carried out in the wind tunnel. However, wind tunnel testing is a mature and trusted experimental methodology, whereas quality and trust in the use of CFD for wind engineering applications is still a contentious issue (as discussed fully in ‘Built Environment (External Aerodynamics)’). External flow prediction is less accurate, and wind tunnels testing still the preferred or the only route to obtain data, e.g. for extreme wind loading measurements. Nonetheless, although the use of CFD does not remove the need for wind tunnel tests, in some cases this does reduce the amount of testing required and enables a range of potential design solutions to be examined rapidly.

For internal ventilation problems, CFD is now becoming an important part of the building design cycle, particularly with projects having non-typical geometry and mechanical systems. Although comparisons with full-scale measurements can be problematic, there is an increased acceptance of CFD results, for a wide range of application areas and issues, as discussed further in ‘Built environment (internal ventilation)’.

Bridge aerodynamic problems, are commonly addressed using wind tunnel tests but there are a number of areas emerging where CFD is applied: deck leading edge design, local flows, vehicle cross winds (see ‘Wind loading on bridge deck sections’). There is therefore considerable scope in the use of CFD as a ‘virtual’ wind tunnel or other laboratory facility. Furthermore, there are certain applications for which CFD is the de facto preferred modelling tool, simply because constructing a physical model is too difficult or sensitive to scale effects (e.g. fires, river and coastal modelling).

The design of tunnel ventilation systems for fire safety is an important example (see ‘CFD modelling of tunnel fires’). Here CFD is used to examine the effectiveness of different ventilation schemes in controlling smoke flow in the event of a fire – a factor critical for the safe operation of tunnels. The flows arising in a fire in a tunnel are three-dimensional and are driven by buoyancy, turbulence, combustion, and convection and radiation heat transfer processes; CFD models can provide a framework for including all of these phenomena in a calculation. However, some of the physical processes are not completely understood and they are represented by approximate models. The more models that are used in a simulation, the more care is required to ensure that they are appropriately applied (verification) and that they adequately represent the underlying physical phenomena (validation).

The calculation of flow and sediment transport is one of the most important tasks in river and coastal engineering (‘CFD for calculating flow and sediment transport in rivers’). This is particularly difficult because of the many complex and interacting phenomena involved, like irregular geometry which can vary with time causing complex flow patterns, turbulence, suspended and bed-load transport with deposition and erosion causing bed deformation. Considerable uncertainties are introduced through the boundary conditions such as roughness, properties and inflow of the sediments and the still rather crude empirical sediment formulae employed. Also, validation of the sediment transport models is difficult because reliable and extensive data are scarce; there is a great need for the development of more reliable sediment transport models and extensive testing of these under realistic conditions. © ERCOFTAC 2004 Tunnel Fires

INTRODUCTION

A fire in a tunnel gives rise to complex three-dimensional flows driven by buoyancy forces created by the energy release of the fire [11, 14]. The behaviour is modified by heat transfer and turbulence, and these factors are in turn influenced by the geometrical nature of the tunnel and any ventilation system which may be in operation. Computational Fluid Dynamics (CFD) techniques are increasingly used to study and understand smoke behaviour in tunnels. It is important, therefore, to understand how CFD is applied, the approximations used and the factors which influence the accuracy of the simulation.

PHYSICAL PHENOMENA AND MODELLING APPROACHES

The flows arising in a fire in a tunnel are three-dimensional and are influenced by buoyancy effects. In addition, the flow velocities and length scales are sufficiently high that the flow is generally turbulent. At the fire a combustion process takes place and so there are chemical reactions going on, providing soot particles and combustion products at high temperatures. Some of the heat will be transferred by radiation, and some by convection, to the tunnel walls.

CFD models can provide a framework for including all of these phenomena in a calculation. However, some of the physical processes are not completely understood and they are represented by approximate models. The more models that are used in a simulation, the more care is required to ensure that they are appropriately applied. Wherever possible, some validation of the simulations should be made.

General-purpose CFD codes are now widely used as a basis for simulating fires in tunnels. They facilitate the rapid development of simulations and embody many of the physical models that are needed for such simulations e.g. turbulence models, buoyancy source terms and combustion models. Their application involves a number of steps at which decisions are made which can affect the quality of the simulation. This short review is a guide to the more important considerations.

Geometry and boundary conditions

The geometry and boundary conditions are first established for the problem. It is necessary to consider how much of the system detail to include and where to apply the various boundary assumptions, e.g. what length of tunnel is it appropriate to model in order to obtain the information sought?

With regard to the geometry of the tunnel, it is possible to model a regular cross section without difficulty. If the cross section is not regular, for example an unlined tunnel driven through rock, then an assessment of the cross sectional variation is required and a determination of what adjustments should be made, if any, to allow for such variations. The length of the tunnel section to be modelled will be decided by the overall length of the tunnel and the region of influence of the fire. In a long tunnel, a shorter section might be modelled. In a short tunnel, or one where a fire is deemed to occur near a portal, then the stratified smoke layer may well reach the portal and the consequent effects will need to be accounted for in the model. If there is doubt about the physical process in a particular region, then it is better to rely on the numerical solution in this region and extend the geometrical boundary to a point where the boundary values are more certain or can be shown to be less influential.

The boundary conditions for the simulation include all the literal boundaries, for example, walls and portals, and also symmetry planes and any sources and sinks which might be included in the equations. Whether or not a symmetry plane exists in the problem depends on the scenario. Many experiments utilise a pool fire in the middle of the tunnel as the source of heat. Given a regular geometry, therefore, it might be reasonable to assume symmetry on either side, and therefore model one half of the tunnel, with a corresponding economy in the computation required.

The boundary conditions will specify the assumptions made at portals and ventilation shafts. The pressure, velocity or mass flow may be prescribed. If a boundary is at a portal then two modelling approaches are possible. The calculation can be extended outside of the tunnel and pressure boundaries set at some distance, so that the behaviour of air and smoke flowing in and out of the portal are calculated by the model. Alternatively, an empirical loss factor might be included at the portal to allow for boundary effects in a more approximate way.

Two other physical considerations relate to the wall friction and wall heat transfer. Conventionally, a wall function would be applied which supplies the shear stress and near-wall turbulence, and the heat transfer coefficient. The wall temperature may be assumed constant during the transient, or further modelling into the tunnel wall carried out to predict the temperature rise at the surface.

The initial velocities of the air in the tunnel, as might be caused by ventilation systems or traffic movements, are also important. These values would be obtained from another calculation method or design assumptions. The wall temperature may cause a flow due to buoyancy if the tunnel has a gradient and the atmospheric air temperature is different. Initial movements of air may well affect the initial smoke behaviour until buoyancy forces arising from the heat source of the fire begin to dominate. If this was found to be an important factor, then parametric studies should be undertaken to assess behaviour for different combinations of wall and atmospheric air temperature.

Modelling the fire

The fire itself can be represented as a heat source in the model; its position, growth rate and maximum size require consideration. The technical approach to modelling the fire might influence or be influenced by such considerations.

In general, there are a number of approaches to describing the fire and smoke source in a CFD model. If the source of the fire is known, for example a pool fire where a particular form of fuel is used, then it is possible to utilise a combustion model to represent these processes in some detail [6, 7, 8]. This is an approach that might be used when simulating a fire experiment for model validation. In the simulation of the combustion, additional transport equations would be used to represent the fuel, oxidant and combustion products. However, it should be noted that this approach may introduce additional uncertainties in respect of the ability of the combustion model to correctly predict the process. A common failure appears to be the inability to predict the combustion efficiency, resulting in temperatures which are too high. Several combustion models might be available in the CFD code and they are unlikely to give identical results. It would be inappropriate, therefore, to use such an approach without some previous study of the capabilities of such models.

When simulating a traffic-related fire, say for a ventilation design, the fire source is much more complicated since the details of the vehicle combustion are unlikely to be known, nor the overall calorific value. One approach is to assess the range of combustibility of typical traffic types in different fire ignition scenarios and estimate a reasonable fire development time and fire size.

It is self-evident that any or all of these boundary conditions may vary and it is very important to consider the sensitivity of simulation results to different boundary values. For example, in a ventilation design exercise the fire size and growth rate might be varied to determine the best operation of the system for evacuation and fire fighting.

Radiation effects

Of the heat released in a fire, about 30% can be transferred to neighbouring walls by radiation. Heat can also be re-distributed within the smoke-filled region. Radiation models enable such effects to be taken into account [12]. There is then a need to prescribe absorption coefficients, which are of uncertain value. Increasing the complexity of the model produces a higher fidelity in terms of the physical processes but requires further empirical information. A simpler approach is to enhance wall heat transfer, or simply reduce the fire output, at least to account for radiative losses at the fire source. Given the uncertainty of potential fire sizes, this approach is reasonable for preliminary design work. As with other assumptions, however, it needs to be justified and if there is uncertainty about the effect of particular assumptions, then comparative calculations should be made to determine sensitivity.

CFD VALIDATION AND EVALUATION INITIATIVES

The importance of tunnel fires and the complexity of the physical phenomena involved mean that a number of experimental studies have been undertaken both in the laboratory and at full scale. Laboratory experiments commonly use either helium-air mixtures or aqueous solutions with varying salinity to represent the buoyancy effects and can be used to understand some of the fundamental phenomena involved [17]. Where possible however full-scale experimental data should be used for model validation and a number of such test have been carried over the last 40 years, though the data obtained are not always ideal for CFD validation purposes. Early tests were carried out in the Ofennegg tunnel in 1965 [8] and the Zwenberg tunnel in 1976 [5]. In the early 1990s very extensive tests were carried out in the United States in the abandoned Memorial road tunnel in West Virginia [1] as part of the preparation for the Boston Central Artery project. These examined a variety of fire sizes and ventilation regimes and produced a very extensive data set including air velocities, temperatures and opacities. More recently tests were carried out in the Benelux tunnel in the Netherlands [3] and as part of the Eureka Firetun project [4].

CFD simulations of tunnel fires have been carried out for many years, with some of the earliest being those of Kumar and Cox [7, 8]. Since then a large number of validation studies have been published focusing mainly on Reynolds-averaged approaches using simple turbulence models, both with and without combustion models, some examples being [2, 6, 13-16, 18]. More recently some studies have started to appear using large eddy simulation. It has been demonstrated that it is possible to carry out meaningful simulations even with quite simple models though much work remains to be done to gain further confidence.

CONCLUSIONS

CFD techniques are now routinely used in the assessment of the effects of tunnel fires and their control using forced ventilation systems, however the complexity of the physical processes involved and uncertainty concerning boundary conditions, in particular the details of the fire source, mean that all such simulations should be used with care. A number of validation studies have however shown that even quite simple models can give results of engineering accuracy when applied appropriately. There remains nonetheless the need to carry out further experimental and validation studies to improve the understanding of the phenomena involved and the accuracy and reliability of the predictions.

REFERENCES

1. Bechtel/Parsons Brinckerhoff: Memorial Tunnel Fire Ventilation Test Program, Comprehensive Test Report, prepared for Massachussetts Highway Department, November 1995.

2. Biollay, H, and Chassé, P: Validating and optimising 2D and 3D computer simulations of tunnel fires, 8th International Conference on the Aerodynamics and Ventilation of Vehicle Tunnels, 357-382, 1994.

3. Bouwdienst Rijkswaterstaat: Project ‘Safety Proef’- Rapportage Brandproeven, The Netherlands, August 2002.

4. EUREKA: Fire protection in traffic tunnels - findings from large scale tests within the EUREKA project EU 499 Firetun, Final Techical Report, 1995.

5. Fiezlmayer, A H, Brandversuche in einem Tunnel, Bundesministerium für Bauten and Technik, Heft 50, Vienna, Austria, 1976.

6. Fletcher, D F, Kent, J H, Apte, V B, Green, A R: Numerical simulations of smoke movement from a pool fire in a ventilated tunnel, Fire Safety Journal 23, 305-325, 1994.

7. Goussebaille, J and Viollet, P L, On the modelling of turbulent flow under strong buoyant effects in cavities with curved boundaries, Proc. Symp. Refined Modelling of Flows, Paris, 1982.

8. Kommission für Sicherheitsmassnahmen in Strassentunneln : Schlussbericht der Versuche im Ofeneggtunnel vom 17. bis 31. Mai 1965, Report in German, Bern, Switzerland,1965.

9. Kumar, S, and Cox, G: Mathematical modelling of fires in road tunnels, 5th International Conference on the Aerodynamics and Ventilation of Vehicle Tunnels, Lille, France, May 1985.

10. Kumar, S, and Cox, G: Radiant and surface roughness effects in the numerical modelling of tunnel fires, 6th International Conference on the Aerodynamics and Ventilation of Vehicle Tunnels, Durham, England, September 1988.

11. Lacroix, D, The Mont Blanc Tunnel Fire: what happened and what has been learned, 4th International Conference on Safety in Road and Rail Tunnels, Madrid, 2 – 4 April 2001.

12. Lockwood, F C, and Shah, N G : A new radiation solution method for incorporation in general combustion prediction procedures, Proc. 18th International Symposium on Combustion, Combustion Institute, 1405-1414, 1981.

13. Owczarek, E, Chassé, P, Bollay, H: CFD validation for tunnel fires under longitudinal ventilation and application to the study of the critical velocity, Proceedings of the 3rd International Conference on Safety in Road and Rail Tunnels, Nice, France, March 1998.

14. Rhodes, N: Review of tunnel fire and smoke simulations, 8th International Conference on the Aerodynamics and Ventilation of Vehicle Tunnels, 471-486, 1994.

15. Rhodes, N: CFD Modelling of Tunnel Fires, Rhodes N, PIARC World Road Congress, Kuala Lumpur, 1999.

16. Ribot, B, Chassé, P, Gay, B, Rhodes, N: Numerical Simulation of Smoke Extraction by Roof Vents in a Tunnel: Comparison with experimental tests and Analysis of physical phenomena, Proceedings of the 1st International Conference on Tunnel Fires and One-day Seminar on Escape from Tunnels, Lyons, France, pp169-179, May 1999.

17. Viot, J, Vauquelin, O, Rhodes, N: Characterisation of the plug-holing phenomenon for the exhaust of a low density layer of gas, 14th Australian Fluid Mechanics Conference, Adelaide University, December 2001.

18. Woodburn, P, CFD simulations of fire-generated flows in tunnels and corridors, PhD Thesis, Cambridge University, UK, 1995. © ERCOFTAC 2004 Wind Loading on Bridge Deck Sections

INTRODUCTION

Numerical modelling of aerodynamic behavior of long-span bridge decks has become, during the last decade, a subject of increasing accuracy and efficiency to complement in a cost-effective manner the traditional wind-tunnel experiments due to the rapid increase in computer capacity and development of new powerful CFD techniques.

PHYSICAL PHENOMENA INVOLVED AND MODELLING METHODS USED

The main goal of a CFD evaluation of aerodynamic behavior of long-span bridge decks is the correct prediction of drag, lift and momentum coefficients. They are parameters of major importance in the design and construction of long span suspended bridges and they expensive to measure in wind tunnel experiments.

The main question to be answered is how the wind affects the bridge structure so that correctness of its structural design can be judged. Undesired phenomena may appear if the structural main oscillation frequencies coincide with those induced by the fluid motion. They include vortices and buffering which give raise to low amplitude vibrations and those that induce aerodynamic instabilities with divergent oscillations that may lead to an structural collapse including torsional divergence and fluttering.

The influence of all these phenomena is fully taken into account in the coefficients mentioned before which determine the wind influence on the structure. Thus the success of a numerical simulation is their right prediction.

Usually, the flow over a bridge is characterized by a turbulent regime, with Reynolds numbers as high as 107, so modeling methods to be used should take turbulence into account.

CFD VALIDATION AND EVALUATION INITIATIVES

First approaches were restricted to the simulation of smooth flows (without turbulence models) around basic-shaped decks without considering the effect of the equipment. [e.g. Kuroda, 1996; Onyemelukwe et al., 1997]. Kuroda [1998] used a finite difference method to solve the 2D incompressible Navier-Stokes equations around the Great Belt East Bridge suspended span considering a Reynolds number of 3´105. Good agreement with experimental data was found for the drag and lift coefficients.


Other numerical procedures included the discrete vortex method [Larsen and Walther, 1997; Larsen 1998] or finite element procedures. Of them finite element models are preferred because they are more accurate than finite difference for a given grid and require less time and computer storage than gridless methods such as discrete vortex. Despite its simplifications, these initial approaches gave insights into the potentiality of numerical techniques in wind engineering. More realistic computation of flows around bridges should be able to overcome several numerical difficulties such as particular requirements to deal with high Reynolds numbers (»107), the high turbulence of the atmospheric boundary layer which requires the use of turbulence models, the quantification of the effect of the items of equipment (side railings, crash barriers, etc.) that the bridge deck carries or the fluid-structure interaction.

Recent advances try to incorporate some of these aspects to the previous models. Thus, among other authors, Selvam [1998] investigated the Great Belt East Bridge using 2D and 3D large eddy simulations using an implicit finite element method. Bruno et al. [1999] simulated the case of a two-dimensional, steady, incompressible, turbulent flow around a deck section of the Normandy cable-stayed bridge and took into account the effect of several items of equipment of the section such as central barriers, side railings and sidewalks. After testing different turbulence models, the authors concluded that the standard model associated with standard wall functions is unable to reproduce the non-equilibrium phenomena that often occur around the deck, whereas the RNG model coupled with non-equilibrium wall functions correctly simulate the interaction between boundary layer and shear layers.

Fluid-structure interaction has been also contemplated recently. Jenssen and Kvamsdal [1999] worked with a finite volume method on moving grids with large eddy simulations. Enevoldsen [1999] used a finite element method with multiblock mesh generation. Frandsen and McRobie [1999] used also a finite element procedure to solve the Arbitrary Lagrangian-Eulerian two-dimensional Navier-Stokes equations assuming a no-turbulence model. At the present, simulations are not more accurate than wind tunnel testing, but the fast developments of computer simulations are expected to facilitate, in a near future, more reliable wind load predictions.

CONCLUSIONS

Good agreement with experimental drag and lift coefficients can be found even by solving the Navier Stokes equations in 2D simplified situations. The use of some kind of turbulence modeling is the first improvement to be considered. In order to obtain more precise results, very fine grids together with more advanced turbulence models should be used.

REFERENCES

Bruno, L., S. Khris, and J. Marcillat, Contribution of numerical simulation to evaluating the effect of section details on the aerodynamic behaviour of a long-span bridge deck, In: wind engineering into the 21st century, Larose&Livesey eds., vol. 2, 1229-1236, Rotterdam, 1999.

Enevoldsen, I., S. O. Hansen, T. Kvamsdal, C. Pedersen, and L. T. Thorbek, Computational wind simulations for cable-supported bridges, In: 10th International Conference on Wind Engineering, Copenhagen, Denmark.

Frandsen, J. B., and F. A. McRobie, Computational aerolastic modelling to guide long-span bridge cross-section design, In: wind engineering into the 21st century, Larose&Livesey eds., vol. 2, 1277-1284, Rotterdam, 1999.

Jenssen, C. B., and T. Kvamsdal, Computational methods for fsi-simulations of slender bridges on high performance computers, In: Computational methods for fluid-structure interaction, T. Kvamsdal Eds., Tapir Forlag, Trondheim, Norway, 1999.

Kuroda, S., Numerical simulation of flow around bridge, Engineering Review, 29 (2), 59-66, 1996.

Kuroda, S., An application of Navier-Stokes simulation on bridge aerodynamics, In: Bridge aerodynamics, Larsen & Esdahl (eds.), 337-347, Balkema, Rotterdam, 1998.

Larsen, A., Advances in aerolastic analysis of suspension and cable-stayed bridges, J. Wind Engrg. and Industrial Aerodynamics, 74, 73-90, 1998.

Larsen, A. and J. H. Walther, Aerolastic analysis of bridge grider sections base don discrete vortex simulations, In: 2nd International Conference on Computational Wind engineering, Colorado State University, 1997.

Onyemelukwe, O. U., M. A. M. Torkamani, and H. R. Bosch, Numerical simulation of wind induced forces on bridge deck sections of long-span bridges, Computer and Structures, 62 (4), 667-679, 1997.

Selvam, P., Computational procedures in grid based computational bridge aerodynamics, In: Bridge aerodynamics, Larsen & Esdahl (eds.), 327-336, Balkema, Rotterdam, 1998.

© ERCOFTAC 2004 Built Environment (External Aerodynamics)

INTRODUCTION

In this brief contribution the use of CFD for the prediction of surface pressures and local wind environment around buildings is discussed. Such use has increased steadily over the last 15-20 years or so and there are now numerous practitioners, whether in academia, government departments or industry, using various CFD tools – often commercial packages – to study Wind Engineering problems of this kind. Although it could be argued that only modest progress has been made in terms of the ability to make such predictions with acceptable accuracy (accuracy that is ‘fit-for-purpose’), many lessons have been learnt. We seek to encapsulate the more important ones in this document.

PHYSICAL PHENOMENA INVOLVED AND MODELLING METHODS USED

There are a number of separate issues which arise when considering the physical phenomena involved in external aerodynamics applications. First, it is worth emphasising that wind loading or pedestrian (i.e. surface level) wind events are usually most serious from a practical perspective in conditions of neutral atmospheric stability, corresponding to relatively high ambient wind speeds. The effects of density stratification on the flow around buildings are generally weak [1], except insofar as they affect the character of the upstream flow [2]. This is a distinct advantage; turbulence modelling for density stratified flows is an even more uncertain process (at least in this context) than for neutral flows, so being able sensibly to restrict attention to neutral flows is useful. Secondly, it is well-known that surface pressures and local wind fields depend crucially on the characteristics of the upstream flow, so it is important that this is simulated adequately. Thirdly, it should be noted that if interest is also restricted to the immediate vicinity of the building(s) (as required for the more important pedestrian wind questions) a computation which leads to adequate results for the mean surface pressure field on the building is likely also to yield adequate data for the mean flow field around it. Fourthly, however, it is often the fluctuating loads, or wind gusts, which have the greatest practical consequences so that adequate computation of mean values may not be sufficient. This implies that in many cases unsteady computations will be required. Finally, the case of an isolated building is a practical rarity. Any site of interest generally contains a number of structures or, at least, has others not too far away from the one of interest and certainly within the expected range of influence (fluid mechanically). Adequacy of a computation for an isolated building does not necessarily imply adequacy of similar computations for multiple buildings. In the following paragraphs we discuss these last four points in turn, with reference to the recent literature.

The upstream flow

The atmospheric boundary layer develops over a rough surface. Proper computational approaches for rough walls remain contentious. Current commercial codes tend to employ simple alternatives to the classical smooth-wall log-law, which are arguably incorrect even outside separated regions but are certainly quite wrong in the immediate vicinity of the obstacle. It is well-known that standard log-law behaviour does not apply in such regions [3] and nor, of course, is it likely to apply over most of the surface of the obstacle itself. However, it seems that the precise nature of the applied boundary conditions around and on the obstacle are not too crucial; significant changes to near-wall modelling parameters in those regions do not generally affect the qualitative nature of the computed flow and, furthermore, have only minor effects on the quantitative results – at least for steady calculations which yield only mean statistics [e.g. 4]. This must be largely because the pressure and flow fields are dominated by the large-scale motions created by the obstacle.

However, it is important to simulate the (inlet) upstream boundary layer properly and this requires a careful match between the turbulence model parameters and the rough surface boundary conditions. Initial computations without the obstacle in place are crucial to check that this is being done adequately; most published comparisons between computations and laboratory (or field) experiments do not describe such checks. Of course, if unsteady methods are being used (LES and unsteady RANS, for example – see §5) this problem is particularly acute. Various techniques are being developed ([5,6]) but some of them are not easy to apply in a genuinely external flow (rather than, say, a channel).

Mean surface pressures and velocities

Early work in this field showed that the standard k-ε turbulence model, widely used in industry, is totally inadequate for flows around bluff bodies, always giving too much generation of turbulence kinetic energy just upstream of impingement regions and thus usually showing, inter alia, a complete absence or a much too restricted size of the separation region on the top of the body [e.g. 7-9]. This results in inaccurate levels of surface pressure, particularly near the leading edges where it is well known from experimental work that very low suction levels can exist. Significant improvements can be obtained either by using appropriate ‘fix-ups’ to the k-e model or by using differential stress (or other more sophisticated) turbulence models [10,11] but it remains unclear to what extent the very strong suctions at leading edges and corners can be simulated. Much of the validation work has been done in the context of a single cube mounted on one surface of a smooth-wall turbulent channel flow. This case is rather easier than the corresponding external, rough-wall case and is also easier than cases in which the approach flow is not normal to the upstream cube face. It does seem possible, however, to produce data for the mean surface pressures and the near wake flow which are in reasonable agreement with experiment in most places, for cases of isolated (even non-cuboid) obstacles on a homogeneous surface [12], although it is clear that really adequate results even for mean flow quantities can only be obtained using LES or, at least, unsteady RANS (see below).

It should be noted that the use of more sophisticated turbulence models, whilst certainly necessary, generally requires the use of significantly finer grids and/or more accurate numerical schemes [13]. This issue seems generally not to have been addressed carefully enough in comparison (validation) exercises and it could be argued that a large majority of published computations have not been shown to be grid (or numerical scheme) independent [14].

Unsteady flow features

Recognising the inherent unsteadiness of these flows, many workers are agreed that genuinely unsteady computations are the only sensible way to proceed. The simplest approach is to use unsteady versions of the usual Reynolds-averaged methods, which implicitly assumes that there is a fair degree of scale separation between the large unsteady flow features which dominate the nature of the unsteady pressures (and gusts at pedestrian level) and the genuine turbulence. Such approaches have had some success in predicting the flow around single bodies and the best of them seem as successful as good large-eddy simulation (LES) methods [15], but there will often be doubts about the degree of scale separation. Recent LES computations have generally been shown to perform significantly better than RANS (or most unsteady RANS) methods for isolated obstacles. They yield much better prediction of the mean flow (and thus surface pressures) [6, 11, 16, 17], for various prismatic obstacles, but based on the limited comparisons made thus far do not necessarily give good agreement with rms values [18]. Their efficacy for capturing, for example, the very low instantaneous pressure suction peaks near leading edges has not yet been demonstrated. Nonetheless, it is clear that although the use of LES ‘does not guarantee success’ [6], it is inherently the least sophisticated turbulence model likely to achieve any degree of generality and usefulness for bluff body flows.

Multiple Bodies

There have been relatively few detailed CFD studies of flow around multiple surface-mounted obstacles which contain sufficient information to assess the extent of their adequacy. Generally, such studies are undertaken not in order to predict surface pressures on a particular building (although note a recent exception provided by [19]) but rather to identify any likely dominant flow features, like channelling between buildings or strong downdrafts near small buildings generated by the close juxtaposition of (say) tall ones [20, 21], or perhaps to assess dispersion characteristics of effluents emitted within the building complex [4]. It must be said that the production of quantifiably accurate computed flow fields for such cases remains a dream. There is no doubt that as the level of complexity increases (in this Built Environment field) the level of agreement between laboratory and numerical experiments reduces.

CFD VALIDATION AND EVALUATION INITIATIVES

There have been hardly any major validation exercises for this class of flows. However, in the case of a single, surface-mounted body the geometrically simple case of sheared, turbulent flow over a cube has been the subject of some evaluations. The most comprehensive is that reported by Rodi et al [16]. This workshop compared both RANS and LES computations of the cube-in-a-channel flow studied by Martinuzzi & Tropea [23], chosen under the QNET programme as an Underlying Flow Regime (UFR) and thus discussed in the appropriate D32 document.

Multiple bodies were considered in an EU-funded project on modelling uncertainty and reported by Hall [24]. This concentrated more on dispersion issues and, in all of the fourteen test cases (each computed separately by the four project partners, using standard RANS) there were scalar or buoyant sources injected from the buildings. An important conclusion was that the sometimes quite large solution variability was a result of human factors (e.g. user errors) and variations in mesh design and numerics, quite apart from uncertainties caused by inadequacies in turbulence models. Some detailed results have been published (e.g. Cowan et al [25], Castro et al [4]) and specific conclusions included the fact that whilst some quantities of industrial importance - in the context, dispersion hazard ranges, for example - could be adequately computed, the degree of agreement between CFD and laboratory experiment inevitable falls as the geometrical complexity rises. A number of the test cases included multiple buildings and it was clear that solution variability was then often a result of differences in user choices other than the turbulence model and was often no smaller than the difference between an individual solution and the experimental data.

CONCLUSIONS

Despite considerable effort over the last two decades, there is no agreed modelling approach which will automatically yield accurate results for the surface pressure field on and/or the flow field around buildings in the wind. The industry standard turbulence model (k-e) can only fortuitously lead to adequate results even for the mean pressures and velocities. More sophisticated methods can give results which may often be ‘fit-for-purpose’, except perhaps for the very strong suction effects that typically occur near building corners or eaves, but cannot normally be expected to yield any useful fluctuating data. Their use requires very careful attention to the numerical details (e.g. grid design, differencing schemes, etc) and to the appropriate surface boundary and inlet conditions [22]. Only LES techniques genuinely have the potential to yield adequate mean and fluctuating data, but these have yet to be fully developed for complex bluff body flows like those in question here. There remains much work to be done and, meanwhile, great caution is necessary, particularly in any claims made.

REFERENCES

1. Snyder WH (1994) Some observations of the influence of stratification on diffusion in building wakes. In Stably Stratified Flows, eds. Castro IP & Rockliff NJ, OUP, pp301-324.

2. Steggel N & Castro IP (1999) Effects of stable stratification on flow and dispersion around a cube. In Wind Engineering into the 21st Century, Ed. Larson A, Larose GL & Livesey FM, Balkema, pp 1725-1730.

3. Simpson RL (1996) Aspects of turbulent boundary-layer separation. Prog.Aerosp.Sci. 32, 457-521.

4. Castro IP, Cowan IR & Robins AG (1999) Simulations of flow and dispersion around buildings. J.Aerospace.Eng., 12, 145-160.

5. Kondo K, Mochida A, Murakami S & Tsuchiya M (2000) Generation of inflow turbulent boundary layer for LES computation. Proc. of 3rd Int. Conf. On Computational Wind Engineering (CWE2000), pp83-86 in ISBN 1-902996-02-X.

6. Shah KB & Ferziger JH (1997) A fluid mechanician’s view of wind engineering: large eddy simulation of flow past a cubical obstacle. J.Wind Eng. Ind.Aero., 67/68, 211-224.

7. Paterson DA & Apelt CJ (1986) Computation of wind flows over three-dimensional buildings. J.Wind Eng. Ind. Aero., 24, 193-213.

8. Baetke F, Werner H & Wengle H (1990) Numerical simulation of turbulent flow over surface-mounted obstacles with sharp edges and corners. J.Wind Eng. Ind. Aero., 35, 129-147.

9. Murakami S (1993) Comparison of various turbulence models applied to a bluff body. J.Wind Eng. Ind. Aero., 46/47, 21-36.

10. Murakami S (1997) Current status and future trends in computational wind engineering. J.Wind Eng. Ind. Aero., 67/68, 3-34.

11. Murakami S (1999)Past, present and future of CWE: the view from 1999. In Wind Engineering into the 21st Century, Ed. Larson A, Larose GL & Livesey FM, Balkema, pp 91-104.

12. Stathopoulos T (1999) Computational wind engineering: past achievements and future challenges. J.Wind Eng. Ind. Aero., 67/68, 509-532.

13. Leschziner MA (1993) Computational modelling of complex turbulent flow – expectations, reality and prospects. J.Wind Eng. Ind. Aero., 46/47, 37-51.

14. Castro IP & Graham JMR (1999) Numerical wind engineering: the way ahead? Proc. Instn.Civ.Engrs. Structs. & Bldgs. 134, 275-277.

15. Iaccarino G & Durbin P (2000) Unsteady RANS simulations using the v2-f model. Annual research Briefs- 2000, Centre for Turbulence Research, California.

16. Rodi W, Ferziger JH, Breuer M & Pourquie (1997) Current status of large eddy simulation: results of a workshop. ASME J.Fluids Eng.119, 248-262.

17. He J & Song CCS (1997) A numerical study of wind flow around the TTU building and the roof corner vortex. J.Wind Eng. Ind. Aero., 67/68, 547-558.

18. Yu D & Kareem A (1997) Numerical simulation of flow around rectangular prisms. J.Wind Eng. Ind. Aero., 67/68, 195-208.

19. Rehm RG, McGrattan KB, Baum HR & Simiu E (2000) large eddy simulation of flow over a building complex. Proc. of 3rd Int. Conf. On Computational Wind Engineering (CWE2000), pp125-128 in ISBN 1-902996-02-X.

20. Ferreira AD, Viegas DX & Sousa ACM (1999) Numerical and experimental study of the wind flow around a group of low-rise pavilions. In Wind Engineering into the 21st Century, Ed. Larson A, Larose GL & Livesey FM, Balkema, pp 1271-1276.

21. Takakura S, Suyama Y & Aoyama M (1993) Numerical simulation of flow field around buildings in an urban area. J.Wind Eng. Ind. Aero., 46/47, 765-771.

22. Cowan IR, Castro IP & Robins AG (1997) Numerical considerations for simulation of flow and dispersion around buildings. J.Wind Eng. Ind. Aero., 67/68, 535-545.

23. Martinuzzi R & Tropea C (1993) The flow around a surface-mounted prismatic obstacle placed in a fully-developed channel flow. J. Fluids Eng., 115, 85-92.

24. Hall RC (1997) Evaluating modelling uncertainty. Proj. EMU Final Rep. Under EU Contract EV5V-CT94-0531, European Union, Brussels.

25. Cowan IR, Castro IP & Robins AG (1997). Numerical considerations for simulations of flow and dispersion around buildings. J. Wind Eng. Ind. Aero., 67/68, 535-545 © ERCOFTAC 2004 Built Environment (Internal Ventilation)

INTRODUCTION

CFD is applied to vast range of building types and ventilation strategies throughout the design process, from feasibility or concept through to detailed design and even post-occupancy. Although CFD is traditionally thought of as a specialist application, its use is becoming more widespread and mainstream throughout the building industry opening up to non-expert and expert users alike.

PHYSICAL PHENOMENA INVOLVED AND MODELLING METHODS USED

In this short review some of the main application areas and issues together with implications for CFD are shown in Table 1. One conventional application is to the office environment where consideration may be for the interaction of the office furniture and internal heat gain sources with the HVAC system and the ability of the façade to cope with high solar gains in summer and down draughts in winter. In many cases, the purpose of a CFD analysis is to assess the likely comfort conditions (1), particularly in relation to high air flow speeds and excessive mean radiant and air dry-bulb temperatures.

The office environment is generally characterized by low flow speeds and low turbulence. Higher Reynolds numbers are found close to the air supply units and in regions where local buoyancy effects are important, such as in the plumes above heat sources or close to exterior glazed surfaces (which may be warm in summer and cool in winter). Building ventilation can be characterized into two principle types, mixing ventilation and displacement ventilation. These two types lead to different flow regimes within spaces. Mixing is historically the most common method for ventilation of an air conditioned office. Air is provided in reasonably high volumes into the space, with high momentum flux. The intention of such a system is to mix the air in the space to a uniform condition (e.g. temperature and humidity).

Displacement systems are becoming quite common with air supplied through floor-mounted swirl diffusers or through “dustbin” type diffusers. Displacement flows are quite different from mixing flows as the intention is to provide cool air directly to “feed” the heat sources within the space. This air is then heated and rises to form a stably stratified hot layer above the occupants.

In other applications, such as large volume spaces, large inlets with high flow rates may generate large mixing circulation flows dominating local surface effects. Other application areas for the internal built environment include the prediction of moisture and air pollutant distributions as well as movement of smoke during a fire. Smoke movement is not discussed here.

The challenges of using CFD to predict air flows in internal spaces are significant as there are frequently several different flow regimes within the single space. Overviews of CFD (and other) modeling can be found in [2,3,4,5].


Application


Issues


CFD implications

Office environment


Performance prediction and design optimisation of HVAC and natural ventilation systems for peak or typical summer and winter conditions.

Effect of internal heat gains (e.g. occupants, small power, lights).



Solve for short- and long- wave radiant field through complex façade (sometimes including fixed shading and blinds). Sometimes use supplemental software based on a thermal network, e.g. dynamic thermal model (DTM).

Represent mechanical air supply through grilles usually with simplified surface mesh. Represent natural ventilation openings using effective areas with/without wind pressure (still day often assumed for design condition).

Input convective component of heat load as volume or surface heat fluxes. Calculate increased surface temperatures due to radiative component of heat load using DTM.

Large volume spaces such as atria and airport termini


Jet throw and trajectory for nozzle system.

Down draughts from large areas of glazing.

Condensation risk analysis for glazing.


Tie in CFD predicted throw to manufacturer’s data making adjustments to inlet boundaries if necessary.

Use sol-air temperature with fabric resistances to represent heat losses to outside including radiation losses to the sky.

Representation of moisture gains from water features.

Museum environment


Moisture content and relative humidity (RH) distribution.


Use scalar concentrations for occupant latent heat gains and inlet condition. Passive scalar derivation for RH distribution.

Underground car park facilities


Air pollutant distribution.


Exhaust emissions distribution representing all exhaust gases and scalar concentration (e.g. CO) for idling, accelerating and decelerating vehicles.

Fire strategy


Relationship between smoke layer propagation and means of escape.


Transient heat and scalar concentration model with appropriate growth applied. Ensure that fire source is representative and heat losses to surfaces accounted for.

Comfort criteria


Understanding combined radiant and convective field.


Calculate view factor from each cell to surfaces at applied or calculated surface temperature to derive mean radiant temperature (MRT). Then combine MRT with air dry bulb temperature distribution and other factors if required.

Heavy-weight structures


Representation of thermal capacity and diurnal climatic variations.


CPU limitations for 24-hour CFD necessitates the use of supplemental DTM software to generate surface temperatures at the time of the design scenario.

Table 1: CFD applications, issues and implications for the internal built environment


Architectural design is becoming increasingly complex in terms of enclosed volume and space function. There are therefore a number of projects requiring an unstructured body-fitted grid approach utilizing automatic meshing software.

Automatic meshing software in recent years has become more powerful and sophisticated than early versions enabling quality tetrahedral meshes to fill the flow domain with prisms at the surfaces for appropriate y+ and wall function representation. Hexahedral meshes are regarded as more computing efficient, though, with methods including cell “machining” at the edges with polyhedral cells at the interface between the surface prisms and bulk hexahedral fluid. Future developments in meshing technology include general polyhedra throughout the flow domain and overlapping meshes.

Use of a standard high Reynolds number k-ε turbulence model is the common approach for many applications due to the relatively low computing cost although it is understood that other models may be more suitable and accurate for certain applications. Sometimes a multi-stage solution approach is required initially solving isothermally and then restarting solving for temperature with all or part of the heat load. Additional pressure under-relaxation may be required for natural ventilation cases. Papers on accuracy include [6,7].

CFD VALIDATION AND EVALUATION INITIATIVES

Validation of air flow prediction in buildings using CFD is inherently difficult. The work is usually completed long before the building is constructed, making in situ comparisons between measured data and modelling extremely rare. Unless there is an air flow problem with a completed building, the client is usually unwilling to pay for measurements facilitating comparisons with a CFD model. This challenge is further compounded by the differences between the input assumptions used in the modelling and the real operation of the building, e.g. variations in temperature boundary conditions, internal heat gains, building operation and control.

However, comparisons between air flows measured in test chambers and other experimental facilities and CFD have been made. These studies range in complexity from flows driven by a point heat source to models with thermal manikins.

CONCLUSIONS

CFD for the built environment (internal) is used for a wide range of application areas and issues but cannot currently practically answer all the questions posed. Supplemental software may be required to solve for solar radiation through a complex façade, for example, and the effects of diurnal climatic variations. Nevertheless, CFD is an important part of the building design cycle, particularly with projects having non-typical geometry and mechanical systems. Although comparisons with measurements are problematic, there is an increased acceptance of the results with architects and clients alike.

REFERENCES

[1] Fanger, P.O. (1970). Thermal comfort – analysis and application in environmental engineering. pp244 McGraw Hill

[2] Murakami, S. (1992) Prediction, analysis and design for indoor climate in large enclosures, Proc. 3rd International Conference on Air Distribution in Rooms (ROOMVENT ’92), Vol. 1, pp. 1-30, Aalborg, Denmark

[3] Leschziner, M. A. (1992) Turbulence modeling challenges posed by complex flows, Proc. 3rd International Conference on Air Distribution in Rooms (ROOMVENT ’92), Vol. 1, pp. 31-58, Aalborg, Denmark.

[4] Li, Y and Heiselberg, P (2003) “Analysis methods for natural and hybrid ventilation – a critical literature review and recent developments”, International Journal of Ventilation, Vol 1 Special Edition Feb 2003, pp3-20

[5] Emmerich, S.J. (1997) “Use of Computational Fluid Dynamics to analyze indoor air quality issues”, NISTIR 5997, 48pp.

[6] Roache, P. J. (1994) Perspective: A method for uniform reporting of grid refinement studies, J. Fluids Engg, 116, 405-413.

[7] Roache, P. J. (1997) Quantification of uncertainty in computational fluid dynamics, Annu. Rev. Fluid Mech., 29, 123-160. © ERCOFTAC 2004 Flow and Sediment Transport in Rivers

INTRODUCTION

Flood protection, keeeping rivers navigable, securing household and irrigation water supply and providing the conditions for hydropower generation are the prime tasks of river engineers. For this, not only economical and technical considerations are important, but increasingly also ecological ones and the impact of any human measures on the environment. For planning such measures, the engineers need to be able to predict the consequences of these. In the past, such predictions were mainly based on integrated programmes of field and hydraulic model studies, but these are very costly and time-consuming. With the rapid increase in computer power and the advancement of numerical methods, more and more computer models are used, and the prime task of such models is to predict the flow and sediment transport in rivers and the impact of human measures.

PHYSICAL PHENOMENA INVOLVED AND MODELLING METHODS USED

The prediction flow and sediment transport in rivers is a difficult task because of the many complex and interacting phenomena involved, like irregular geometry which can vary with time causing complex flow patterns involving separation and secondary motions, turbulence, suspended and bed-load transport with deposition and erosion causing bed deformation.

Different levels of idealisations and empirical input have been used in computer modelling. 1D models are widely used in practice and can be applied to long river stretches. With these only cross-sectional average quantities and long term morphological developments can be calculated while details cannot be resolved and many influences require an empirical treatment. Typical 1D codes are HEC-6 [1], SEDICOUP [2] and MIKE-11 [3]. 2D depth-average models resolve horizontal variations and provide many more details like the influence of changing cross-sections and irregular side boundaries which may cause separation and dead-water zones. These models cannot account directly for secondary motions, which are particularly strong in bends, as well as for vertical motions around structures. They solve the depth-averaged continuity and momentum equations. Turbulence effects are treated through simple models like relating the eddy viscosity to the local depth and bed-friction velocity or by using a depth-averaged version of the k-ε model. An important input is the bottom friction which is related to the depth-averaged velocity through a quadratic friction law with the friction coefficient generally obtained from the Manning’s roughness coefficient which has to be specified. Efficient and flexible finite-element and finite-volume methods have been developed which allow also to account for falling dry and flooding of parts of the calculation domain. These methods are also used already for solving practical problems, albeit only for shorter river stretches.

3D models are the most powerful ones as they can calculate secondary motions directly. Some models solve the full 3D equations [4 – 6] while others make the assumption of hydrostatic pressure distribution [7, 8] (and hence are not so suitable in the case of stronger vertical accelerations). Generally, turbulence effects are simulated with the k-ε model, but some codes use this only for the vertical exchange. Large-scale boundary irregularities are resolved while smaller-scale ones and in particular roughness are treated with the aid of wall functions, typically employing the log law for the velocity. The roughness height appearing in this has to be specified by empirical formulae. Again, efficient and flexible finite-element and finite-volume methods are available.

The calculation of sediment transport with erosion and deposition is similar in 2D and 3D models. Usually bed load and suspended load are treated by separate models (in some applications only one of these modes is important) and a model is necessary for the interaction between the 2 modes of transport. The bed deformation is calculated from an Exner equation which is a sediment mass balance equation. As bed-load transport is a 2D phenomenon, the same treatment is basically used in both 2D and 3D models. In general the bed load is calculated from one of the many empirical formulae for equilibrium bed load, but an equation for non-equilibrium bed load transport is also sometimes used [6]. Suspended sediment transport is calculated by solving a convection-diffusion equation for concentration, either a 3D one or a depth-averaged one in 2D models, involving a settling velocity and a turbulent exchange term which is generally related to the eddy viscosity. For the boundary condition at the bed and for determining the net erosion or deposition flux, a near-bed value of the (equilibrium) concentration has to be prescribed empirically. Further, in 2D models the effect of secondary currents is sometimes accounted for by special empirical models. Some models are only for uniform sediment material, while others account for graded sediment transport. Altogether, sediment transport modelling involves a high degree of empiricism.

A summary of the 2D and 3D models developed and applied in the author´s group is given in [9]. Examples of other 2D models can be found in references [8, 10, 11] and an overview and comparison of commercial codes in [15]. Examples of 3D models are given in references [4 - 8].

Research is under way on the development of large-eddy simulation methods for open-channel flows [12 – 14], but this method is certainly still far away from practical applicability and has not been used for sediment transport calculations.

CFD VALIDATION AND EVALUATION INITIATIVES

Some of the 2D and 3D models cited above have been verified first by application to relatively simple, well controlled laboratory experiments and by comparison of the calculation results with the measurements (e.g. [6, 16]). Validation of the models was performed by application to various natural rivers like streches of the river Rhine [9], Elbe [9], Mississippi [7], Columbia [4], Yangtze [9] and by comparison sometimes with laboratory studies for those rivers or with some field data, which are however scarce. Quite satisfactory results have been obtained in many cases, but considerable uncertainties prevail. The author does not know of any evaluation exercises in which different models for calculating the flow and sediment transport in rivers have been applied to the same test case, i.e. comparative test-case studies are not available in this field. Rather, the performance of the models can only be judged from the application to different river sites as reported in individual papers and laboratory reports.

CONCLUSIONS

1D and 2D depth-average models are used in routine calculations by river engineers while 3D models are still more the subject of research. The 2D and especially the 3D models can deal with the complex situations occurring in real rivers, but considerable uncertainties are introduced through the boundary conditions such as roughness, properties and inflow of the sediments and the still rather crude empirical sediment formulae employed. Also, validation of the sediment transport models is difficult because reliable and extensive data are scarce. Certainly, there is a great need for the development of more reliable sediment transport models and extensive testing of these under realistic conditions. Comparative evaluation exercises are so far lacking and would help to increase the trust in the models available.

REFERENCES

[1] HEC. (1991): HEC-6 scour and deposition in rivers and reservoirs, Users Manual, Hydrologic Engineering Centre, US Army Corps of Engineers.

[2] LHF. (1993): SEDICOUP-1.0 methods and users guide, Laboratoire Hydraulique de France.

[3] MIKE (1989): MIKE-11, Manual I and II, Danish Hydraulic Institute.

[4] Sinha, S.K., Sotiropoulos, F., Odgaard, J. (1998): Three-dimensional numerical model for flow through natural rivers, J. Hydraulic Eng., 124, pp. 13-23.

[5] Fang, H.-W., Wang, G.-Q. (2000): Three-dimensional mathematical model of suspended sediment transport, J. Hydraulic Eng., 126, pp. 578-592.

[6] Wu, W., Rodi, W., Wenka, Th. (2000): 3D numerical modelling of flow and sediment transport in open channels, J. Hydraulic Eng., 126, pp. 4-15.

[7] Gessler, W., Hall, B., Spasojevic, M., Holly, F., Pourtaheri, H., Raphelt, M. (1999): Application of 3D mobile bed, hydrodynamic model, J. Hydraulic Eng., 125, pp. 737-749.

[8] Hervouet, J.-M., Bates, P. (eds.) (2000): The TELEMAC modelling system, special issue of Hydrological Processes, Vol. 14, issue No. 3.

[9] Rodi, W. (2000): Numerical calculation of flow and sediment transport in rivers, Proc. 8th Int. Symp. on Stochastic Hydraulics, Beijing, 25 – 28 July 2000, Balkema.

[10] Cheng, R.T., Casulli, V., Gartner, J.W. (1993): Tidal, residual, intertidal mud flat (TRIM) model and its applications to San Francisco Bay, California. Estuarine, Coastal and Shelf Science, Vol. 36.

[11] Spasojevic, M., Holly, F. (1990): 2D bed evolution in natural water resources - new simulation approach. ASCE J. of Water Way, Port, Coastal and Ocean Engineering, Vol. 116 (4).

[12] Nadaoka, K., Yagi, A. (1998): Shallow water turbulence modelling and horizontal large-eddy computation of river flow, J. Hydraulic Eng., 124, pp. 493-500.

[13] Bradbook, K.F., Lane, S.N., Richards, K.S., Biron, P.M., Roy, A.G. (2000): Large-eddy simulation of periodic flow characteristics at river channel confluences, J. of Hydraulic Research, 38, pp. 207-215.

[14] Sih, J., Thomas, T.G., Williams, J.J.R. (2000): Free surface effects in open channel flow at moderate Froude and Reynolds numbers, J. of Hydraulic Research, 38, pp. 465-474.

[15] Langendoen, E.J. (2001): Evaluation of the Effectiveness of Selected Computer Models of Depth-Averaged Free Surface Flow and Sediment Transport to Predict the Effects of Hydraulic Structures on River Morphology.

[16] Minh Duc, B. (1998): Berechnung der Strömung und des Sedimenttransports in Flüssen mit einem Tiefengemittelten numerischen Verfahren, Ph.D. thesis, University of Karlsruhe © ERCOFTAC 2004 Coastal Engineering

INTRODUCTION

This review refers to the use of CFD in the modelling of water flow, sediment transport and morphodynamic change in coastal areas. The purpose of such studies may be to assess the impact of engineering works, such as harbour construction, but not specifically beach evolution because this is conventionally treated separately. In practice the quality of the modelling, for each case study, is established by comparison with survey data.

The aspects of flow modelling and sediment transport are in many aspects the same as those described for flow and sediment transport in rivers and channels but with the extra complications that the influence of waves, including breaking waves, are often dominant.

PHYSICAL PHENOMENA INVOLVED AND MODELLING METHODS USED

A coastal area morphodynamic model comprises:

- Flow modelling. Either two-dimensional depth-integrated (2DH) or three dimensional.

- Wave modelling, including the computation of wave-breaking stresses, which cause flows (such as rip currents).

- Sediment transport modelling based on currents and waves computed above

- Morphodynamic modelling, how the bed level will rise or fall due to deposition or erosion of sediment and thus change in turn the currents and waves.

Each of the modelling tasks will be reviewed in turn, bearing in mind that there are interactions, e g between the waves and the currents. Validation data for problems of coastal flow and sediment transport modelling are available from the EU COAST3D project (Reference 1) both for a straight coast (Egmond in Netherlands) and for a complex 3D headland/estuary coast at Teignmouth in England.

Often the area to be modelled will be dominated by tidal flows. In certain cases where tides are very weak, e g in the Mediterranean Sea, the flows in the area may be most affected by winds and ocean currents. In all cases the effects of the waves in the breaker zone will be important in creating stresses which give rise to currents.

In a depth-integrated model the breaking wave stresses are readily input from the wave model. If a 3D model is used then the breaking wave stress is distributed through the vertical (Reference 2).

A flow model for this purpose will include representation of bottom friction (this may need to be enhanced to account for the wave action). Eddy viscosity is often given a specified (constant value) or it may be obtained from a k-epsilon model. In the area where waves are breaking it may be required to enhance the eddy viscosity to account for the extra turbulence caused by the waves breaking.

Models used for this purpose include TELEMAC-2D and 3D (Reference 3), MIKE21 and MIKE3 (Reference 4) and Delft3D (Reference 5). The model may be based on solution of the equations in finite difference, finite element or finite volume frameworks. Most applications make use of the hydrostatic pressure approximation, which is valid for bottom slopes less than the order of 1:10 (Reference 6).

During the COAST3D work it was found that adequate boundary conditions could not be specified from measurements alone and the use of a well-calibrated model of a larger area to provide boundary conditions for the local area was found to give the best result.

The model calibration will establish the user’s confidence in its performance and trust may be established. The flow model is usually calibrated by adjustment of the bed roughness and the eddy viscosity. These parameters must fit within a realistic band of values, but they can be adjusted within this range to give the best agreement.

A wave model, to be suitable for coastal area modelling includes the processes of refraction, shoaling and energy dissipation and possibly refraction by currents. As the waves enter water shallow enough to cause breaking the wave energy should be dissipated by breaking and a breaking wave stress (called a “radiation stress”) is computed as input to the flow modelling. Wave models used include COWADIS (from the TELEMAC system) and SWAN (Reference 7). Offshore data on waves are used as a boundary condition.

A sediment transport law is used as the basis for sediment transport modelling. The law may include the presence of different size fractions of sediment. A review of the laws that have been used is contained in Reference 8. References 9, 10, 11 and 12 describe present techniques for the bed-updating procedure.

CFD VALIDATION AND EVALUATION INITIATIVES

Several validation and evaluation initiatives have been carried out.

For the coupling of wave and current processes data have been measured in a laboratory basin (Reference 13) and those data compared with subsequent computations (References 14 and 2).

In the COAST3D project (Reference 15) five institutes were involved in the measurement of data at Teignmouth, UK and also in modelling. Objective measures of goodness of fit between model and data were also applied in this project. As part of the COAST3D study two models of waves and currents have been compared with field surveys by different institutes (Reference 1).

Seven wave-driven current models from different institutes have been intercompared (Reference 16). The test case is flow behind a shoreline parallel breakwater. The model results are compared with physical model measurements. The authors suggest that the model results give reproduction of the main elements of the wave-driven flow. However they suggest that further work should be carried out to define better the breaking wave stresses that drive the flow and the representation of bedstress (usually assumed to be co-linear with the wave-averaged current) and the turbulence modelling.

Five different models of coastal morphodynamic change have been also intercompared for the same offshore breakwater situation (Reference 8). The results were similar to one another and in line with general expectation (laboratory data are not available for the change to the bed). It was found that it is necessary in such cases to include the interactions of currents, waves and bathymetry as extrapolation of the initial pattern of changes does not predict the final state correctly.

CONCLUSIONS

In modelling coastal regions it is acknowledged that quality can be assured only by comparing the model with field data for each study area. Parameters are adjusted to yield a good agreement and then whatever engineering works that are to be built, are incorporated into the model and the effects quantified. Validation and evaluation initiatives have demonstrated that the models are capable of yielding reasonable agreement with observations although some differences in the current patterns and morphodynamic change were found between different institutes and models. Further research has also been called for to refine the computation of

- breaking wave stresses

- bed stress

- turbulence

REFERENCES

1 Walstra, D.J.R., Sutherland, J., Hall, L., Blogg, H. and van Ormondt, M., 2001. Verification and comparison of two hydrodynamic area models for an inlet system. Coastal Dynamics ‘01, proceedings of the Fourth Conference on Coastal Dynamics, Lund, Sweden. ASCE, pp433-442.

2 Improved prediction of 3D flows at structures, HR Wallingford Report SR544, July 1999.

3 Hervouet, J.-M., Hubert, J.-L., Janin, J.-M., Lepeintre, F. and Peltier, E., 1994. The computation of free surface flows with TELEMAC: an example of evolution towards hydroinformatics. J Hydraulic Res., 32 (Extra issue) 45–64.

4 DHI, MIKE3, Reference Manual, A Three-Dimensional Hydrodynamical Model, A Short Description, 1998.

5 Roelvink J.A., and Banning G.K.F.M. van. (1994)Design and development of DELFT3D- and application to coastal morphodynamics. Hydroinformatics '94, Verwey, Minns, Babovic & Maksimovic (eds), Balkema, Rotterdam, 1994, pp. 451-455.

6 StansbyPK and Zhou JG "Shallow-water flow solver with non-hydrostatic pressure:2D vertical plane problems" Int J Numer. Methods in Fluids, Vol. 28 ,1998, pp 541-563.

7 Booij, N., Holthuijsen, L.H. and R.C. Ris, 1996, The SWAN wave model for shallow water, Proc. 25th Int. Conf. Coastal Engng., Orlando, USA, Vol. 1, pp. 668-676.

8 Dynamics of marine sands, A manual for practical applications, Richard Soulsby, Thomas Telford, 1997.

9 De Vriend, H.J., Zyserman, J., Nicholson, J., Roelvink, J.A., Péchon, P., Southgate, N.H., 1993. Medium term 2DH coastal area modelling. Coastal Eng. 21, 193–224.

10 De Vriend, H.J., 1996. Mathematical modelling of coastal morphodynamics. In: Advanced Series in Ocean Engineering. World Scientific, Singapore.

11 Nicholson, J., Broker, I., Roelvink, J.A., Price, D., Tanguy, J.M., Moreno, L., 1997. Intercomparison of coastal area morphodynamic models. Coastal Eng. 31, 97–123.

12 De Vriend, H.J., 2DH Mathematical Modelling of Morphological Evolutions in Shallow Water, Coastal Engineering 11, 1 – 27 (1987).

13 Borthwick, A.G.L. and Foote, Y.L.M., 2002. Wave-induced nearshore currents at a tri-cuspate beach in the UKCRF. Proc ICE, WME, in press.

14 Park, K-Y and Borthwick, A.G.L., 2001. Quadtree grid numerical model of nearshore wave-current interaction. Coastal Engineering 42: 219-239.

15 Soulsby, R.L. 2001. Sediment transport and morphodynamics on complex coastlines - the COAST3D project. Coastal Dynamics ’01: proceedings of the 4th Conference on Coastal Dynamics, Lund, Sweden. ASCE pp92–101.

16 Pechon, P, Rivero, F., Johnson, H., Chesher, T., O’Connor, B., Tanguy, J.-M., Karambas, T., Mory, M. and Hamm, L., 1997, Intercomparison of wave-driven current models, Coastal Engineering 31: 199-215.