WSP Environment & Energy are leading consultants providing green design solutions within the Built Environment industry for the commercial and residential markets. Wilde works in close partnership with WSP, so as to better understand the airflow around the structure and also provide recommendations on design improvements. This case study provides some advice on modelling approaches and the benefits of ANSYS CFD for these applications.
Introduction
WSP Environment & Energy are leading consultants providing green design solutions within the Built Environment industry for the commercial and residential markets. Keeping in line with the company’s commitment to eco-friendly practices and innovative methodologies, Computational Fluid Dynamics (CFD) analyses have been employed to better understand the flow around urban landscapes.
In all instances, several layouts are assessed, with an objective of reducing velocity magnitudes for a given number of seasonal wind directions. Thermal gradients and particle dispersion (due to possible pollutants) are other factors that can be evaluated in such analyses.
Due to restrictions associated with computational grid size and project deadlines, the analyses tend to be steady state in definition and utilize a traditional Reynolds Averaged Navier-Stokes (RANS) model. While transient Scale Adaptive Shear Stress Transport (SAS-SST) or Large Eddy Simulation (LES) approaches are also available, these tend to very costly in time and computational effort. A comparison between steady state and transient analyses has shown that the ‘average’ solution obtained using the RANS method is sufficient for design purposes.
Wilde Analysis works in close partnership with WSP, so as to better understand the airflow around the structure and also provide recommendations on design improvements. The animation below is an example of a simulation from a recent project.
Methodologies & Assumptions
In doing a project where a potential number of layouts require investigation, setting up a parametric model is beneficial. Doing so not only provides a method for rapid response, but also ensures that the same global meshing controls and physics are applied for each consecutive design.
Besides parameterisation, it is often convenient to construct the 3D geometry in a modular fashion, such that building structures can be easily replaced or moved without the need to dismantle the entire CAD. This obviously requires some knowledge beforehand of where the revisions are most likely to occur in the CAD mode
1. Domain Shape
Typically a circular or near elliptical shaped computational domain is set up. Using these shapes tends to negate edge or vertex effects (such as local accelerations or artificial gradients) that might be present in similarly sized cubical domains. The main advantage however of using a more circular shaped domain lies in the specification of wind conditions during pre-processing; an entire array of wind directions can be setup in a single sitting, using the same CAD and mesh file.
For example if the seasonal wind direction is known to arise from bearings 50°, 230°, 290° and 230°, it therefore makes sense to divide the circumferential face and edge of the domain into 36 divisions, each arcing 10° (Fig. 3). Taking the case of wind at 50° (Fig. 4), we can specify all Inlet faces to lie between (50°-90°) to (50°+90°). As the circumferential face has already been divided into 10° segments, it is obvious that 18 faces conveniently fit into the Inlet and Outlet boundary conditions each. In other words, if we have a wind bearing of N°, the Inlet faces will span from (N°-90°) to (N°+90°), while the Outlet will be specified on all the remaining faces.
Not surprisingly, the above technique works best on circular shaped domains and provides a significant reduction in analysis set up time. The major benefit of this method lies in the fact that each wind direction does not need its own CAD (and associated mesh); all the possible Inlets and Outlets exist in this single CAD and mesh file. The user only has to assign an Inlet or Outlet condition for the different wind simulations; this is usually done using some command language or automated scripting.
2. Domain Size
While most CFD simulations on such a project are concerned with a small region of interest within an urban landscape, the effects of downwash and interference with the surroundings is equally important. Consequently, keeping the domain large enough to capture any wake effects (regardless of direction) is crucial. There are many industry guidelines on choosing the diameter and height of the domain, but in reality, the domain size is also governed by the computational cost and items of priority (i.e. investigation of wakes or local regions of recirculation). Using the tallest building (of height H) as a guide, the vertical extent of the domain should extend to at least 5H. In the lateral direction, the choice for domain width is largely dependent on some measure of wind blockage area and how tightly the buildings are packed in the landscape. Broadly speaking,
- For groups of buildings with a large net aspect ratio, (i.e. significant blockage to the wind), the effective width of the collective buildings (Leff) is taken into account. Using this value the length of the domain in the wake region is typically kept to at least 8 Leff.
- For cases where wake effects are not a high priority (region of interest is enclosed, taller structures are in immediate surrounding or more commonly where the downstream buildings are not included due to their location or size) or the buildings offer very little blockage, an effective downstream length of 3 to 4 times the collective width will suffice. In using any of the above guides, care should be taken to ensure that the domain edges are a good distance away from the outermost building, in order for the flow field to stabilize before it exits the domain.
- The size of the domain also depends on the velocity field expected within the domain. For higher velocities (which may take longer to stabilize in the wake region) a larger domain might be required.
While there are lot of guidelines for domain size based on downstream wake capture, it is important to note that the upstream velocity resolution and terrain definition are just as important. Failure to provide a stable upstream velocity can result in seriously flawed downstream flow patterns, regardless of how well defined the downstream domain is modelled. Common effects of placing the Inlet boundaries too close to the built-up areas or not adequately defining the velocity in the upstream region include:
- Artificial acceleration of fluid near building surfaces; this occurs because the fluid has to squeeze past the building and the outer edge of the domain. This squeezing effect through a small area increases the velocity in the local region.
- Vortex generation from mundane surfaces: the above effect in combination with the building being in close proximity to the domain boundary leads to artificial vortex shedding due to rapidly changing gradients in this region.
- Non-real velocities been applied at the inlet. This occurs when the stagnation pressure region (upstream of an object) interacts with the Inlet, due to their close proximity. In such cases, there is a danger that the Inlet velocity profile might end up being different to the one manually inputted by the user, due to flow interaction
For a flat terrain, the Inlet velocity gives a good indication of domain length required upstream of the built-up areas. It is important that the velocity profile between the Inlet and the building structure is stable and does not degrade with distance from the Inlet. Figure 5 shows very minor degradation of the velocity profile upstream of the buildings. On the vertical plane nearest the civil structures (call it Plane A), the contour bands appear to be slightly raised, suggesting that the effects of the buildings can be felt in this region. This hypothesis is confirmed in Figure 6 which shows that the stagnation pressure (on the windward side) extends to a similar location as Plane A. Consequently, the Inlet boundary should be placed at some location outside this high pressure region.
In this case, the Inlet is located more than twice the length of the high pressure region; this guarantees that:
- Domain edge effects are not felt in the local region and vice versa
- Upstream flow is stable before it interacts with the buildings
- There is enough domain length in the upstream direction to capture the large region of high pressure.
3. Volumetric Meshing and Boundary Layer Resolution
In contrast to transient simulations which require spatial and temporal mesh considerations, a steady state analysis mainly addresses spatial concerns only.
As with all CFD simulations, a more refined mesh is typically placed in regions of interest or large gradients (Fig. 7). In the case of Pedestrian Comfort for the Built Environment industry, the region of interest is usually all ground surfaces up to an elevation of 1.5m.
In the lateral direction (assuming a cluster of buildings with net diameter Dnet), a refined mesh on the ground for a distance of 1 Dnet away from the central buildings does generally suffice. For low speed wind velocities as in the case for this project, the refined zone on the ground surface can drop down to a distance of 0.5Dnet.
Within this region of high mesh density, the element size is kept between 0.25m to 1m, depending on the proximity to a building surface. Similar to typical CFD meshing strategies in other applications, the rate of change in element size between refined zones and the remainder of the domain is gradual and is kept at ~1.2.
The choice of element size on building surfaces is very much dependent on the geometry, areas of interest and potential velocities induced. Generally speaking, building surfaces are resolved with at least 0.5m elements, growing to a maximum element size of 1m in any direction. Note that in the vertical direction, the building surfaces have an even finer mesh near the ground, to capture the boundary layer resolution (Fig. 8).
For edges or surfaces on buildings which are smaller than 0.5m, their location is first considered. If they are not in the region of interest or directly affect the flow, such entities can be manually removed from the CAD or smoothed out using Virtual Topologies available to most meshing tools. Experience shows that such entities only increase the mesh count without having any significant effect on the solution.
Between adjacent buildings, typically 5 to 8 mesh elements are used to model flow in the street and near the buildings. For densely populated environments or structures with narrow passageways, street ‘Canyon Effect’ is captured using at least 10 elements between adjacent structures.
In order to investigate the flow near the ground surface, an appropriate boundary layer is required. Calculating the Reynolds’ Number using a characteristic building length or the net length L for a tight cluster of buildings, a target value for Y+ is adopted.
For highly turbulent flow fields, the use of Wall Functions is recommended. In such approaches, the first node should be kept at a Y+ of 30. Keeping the first node at a lower value implies the Log-Law is incorrectly applied to the inner laminar region of the boundary layer, rather than the intermediate logarithmic zone. Newer turbulence models such as Shear Stress Transport (SST) automatically switch between a low Re formulation (which solves for velocity right down to the wall) and Wall Functions (which apply the logarithmic relationship) based on the surface’s Re.
The advantage of using SST is that a fine mesh with Y+<30 can be placed within the boundary layer; the turbulence model then determines whether a low-Re model is to be used or a Wall Function instead. It is worth pointing out that as a consequence of this extra calculation, the SST model tends to solve slower than the traditional K-ε model.
Figure 9 shows a contour of Y+ on the ground surface. The values suggest that the boundary layer resolution is suitable to the flow as the contour bands fall within the realms of explicit or automatic Wall Functions. Moreover, any further grid refinement has shown that the difference in the solution is marginal. Based on this grid independence, the mesh is deemed to be adequate for the flow domain.
4. Boundary Conditions
A fully developed velocity profile with low turbulence intensity is assumed at the Inlet. Using ANSYS CFX Expression Language (CEL), inputs for the wind direction and magnitude are specified.
As pointed out earlier, the circumference of the domain is split into 36 equal faces. For each analysis where a different wind condition (magnitude or direction) is simulated, CEL calculates the appropriate velocity components (as a function of elevation) in the East-West and North-South direction (Figure 8). Eighteen faces have the Inlet condition imposed on them, while the remainder are kept as Outlets.
Stability within the solution is best achieved when a velocity inlet is used in combination with a pressure outlet. In this case, due to possible recirculation at the domain extents, an Opening condition is used instead of an Outlet. In using an Opening condition, fluid is allowed to exit the system at some velocity and pressure based on the solved flow field, but also allowed to re-enter the domain at a static pressure specified on the boundary. In contrast, an Outlet condition does not allow re-entry of fluid into the domain.
While the definitions of the lateral extents (Inlet or Outlet) and surfaces (buildings or ground) of the domain are fairly straightforward, the choice of boundary condition for the ceiling does depend largely on the size of the domain in the vertical direction. As the domain height is ~4 times the height of the tallest structure, two boundary condition options are available (in decreasing order of preference) for the ceiling:
- Free-Slip Wall condition: ideal when the ceiling is placed high enough, such that interference with any terrain or building structure is near zero or negligible.
- Inlet with tangential velocity for that given elevation: if the ceiling has to be placed closer (i.e. <2.5 times the height of the tallest structure), interference between the top of the domain and some building structure or terrain is very likely. Specifying a velocity (which accounts for elevation) at the top of the domain ensures that the resultant flow in this region has accounted for the close proximity between the ceiling and the structures.
A symmetry boundary condition is not recommended for the ceiling, as the flow on either side of this surface are rarely mirror images.
5. Post Processing and Data Reduction
The first run is usually done on a coarse mesh, so as to gauge run times and identify regions of concern within the flow field. Typically convergence criteria of 1E-4 shows that the solution is stable and can be used to assess the results.
Based on the initial results, further action that is not limited to the following may be required:
- Mesh refinement in regions of sharp gradients or separated zones
- Boundary layer mesh adjustment based on the value of Y+
- Investigation of turbulence model to match plots of Y+
- Extension of domain based on wake dissipation and interference with domain extents
Further runs should be carried out until successive mesh refinements provides a constant solution in the region of interest or downstream wake. A good example of mesh independence and stable downstream effects are shown in Figures 11 and 12. Examining the streamlines and the velocity contours, it is evident that (a) the swirling nature of the flow has settled down before reaching the domain exit (b) the downwash velocity has reverted to free-stream conditions before reaching the exit.
CFD & Built Environment Industry
Besides external aerodynamics, other applications of CFD in the industry include:
- Flow induced vibrations and aerodynamic noise
- Pollution or dispersed particle tracking
- Thermal insulation and ventilation
- Fire hazard and escape
Benefits of Using ANSYS CFD
Any user of ANSYS will testify to the software’s user friendly GUI and its ability to allow for parameterization. This ability to assess multiple designs is not just true for CAD build up, but also for mesh sensitivity studies and physics set up. Using the ANSYS Workbench project interface, not only are all simulations accounted for within a single project file, but each component of a simulation (i.e. CAD, mesh or simulation) can be traced to its origin, be it within the ANSYS suite or some third party software.
Figure 13 shows a simple project schematic that analyzes two CAD designs. The area highlighted in red shows the CFD process broken down for the first simulation of Design 1. Once this process has been established, further runs with revised boundary conditions can be duplicated as shown in green. As the runs highlighted in green do not require a new mesh, the initial mesh can be used for these analyses (as shown).
Alternatively, the entire CFD process can be combined into one component as shown in grey region. Revision to the geometry or mesh for subsequent runs can be easily done by duplicating either item in the blue-dashed area.
While we have so far concerned ourselves with pure fluid flow, there are times when a coupled field analysis is required. Most common of these is a Fluid Structural Interaction (FSI) analysis that combines fluidic pressures with a corresponding structural deformation. In such cases using the ANSYS project schematic bears a clears advantage, in that the results from one simulation can be easily transferred as initial or boundary conditions for another simulation. Such is the case in the area highlighted in the red dotted line.
The schematic show in Figure 13 is a simple example of a few design iterations. It should be noted that a specific project can constitute N simulations, meshes or CAD files independent of each other or linked together in any combination.