# UFR 4-11 Best Practice Advice

# Simple room flow

Underlying Flow Regime 4-11 © copyright ERCOFTAC 2004

# Best Practice Advice

## Best Practice Advice for the UFR

### 7.1 Key Physics

Forced ventilation flow patterns in simple rooms or enclosures generated by modern air terminal devices typically involve a jet which forces a room-size re-circulation vortex. Near the source, there are high velocities and turbulence levels, but within most of the room (i.e. the occupied zone) mean velocities and turbulence levels are low.

The overall flow pattern and the jet velocity decay can be predicted by the standard k-ε model with an acceptable degree of realism, in the absence of thermal or buoyancy effects. The overall mean flow field is well predicted, with good qualitative predictions and quantitative agreement within a factor of 2 in most of the domain. Nonetheless there are errors in the detail of the predictions, particularly within the occupied zone where velocities are low.

### 7.2 Numerical modelling issues

**Discretisation method**

A discretisation scheme comparison was not carried out in this study; the second order ('self-filtered central differencing') SFCD scheme was used throughout.

**Grids and grid resolution**

A regular, structured mesh should be adequate, provided that the inlets, outlets, jets and obstructions are sufficiently well resolved. The effect of progressive mesh refinement on the solution was demonstrated by the using an objective measure of goodness of fit for the flow field prediction, for a series of progressively finer meshes. This showed that the solution changed as the mesh resolution improved, but that around 50,000-100,000 cells were required, before mesh dependence began to diminish, even for this simple flow.

**Boundary conditions and computational domain**

*Inlets* Diffuser inlets are generally complex, and the way in which they are modelled will affect the local detail of the flow. Inlets that have geometrical features that are sufficiently large should be modelled explicitly as part of the computational mesh geometry. Otherwise, a sub-grid modelling representation can be used, provided that appropriate source terms are added. It was found that treating such jet inlets as an equivalent source of mass, momentum and turbulence kinetic energy provides a realistic representation of the flow. In the vicinity of forced ventilation inlets, a fine mesh resolution is needed to capture the large gradients of mean velocity and turbulence. Too coarse a mesh may result in numerical smearing of the plume or jet, with incorrect dilution and flow development away from the source region.

*Outlets* It is important to ensure that outlet conditions are placed well away from regions of high gradients if zero gradient conditions are to be applied. The outlet boundary can be shifted away from the actual wall outlet locations (where flow acceleration and shear zones may be present), with the use of elongated ‘outlet ducts’ of computational cells extruded outwards from the outlet location; placing the outlet boundary at the other end of the duct ensures that the outflow does not have any stream-wise variation.

### 7.3 Physical modelling

**Turbulence modelling and near wall treatment**

Calculations for internal flow problems are usually carried out using the standard k‑ε model, with standard wall functions. The k-ε model deals with the near wall layer by assuming 'wall functions', which are a valid approximation provided that the distance of the closest grid node from the wall (y+ values) is within an appropriate range, and the flow is of sufficiently high Re number.

In practice, satisfying the y+ criterion is not always straightforward since this limit will depend upon local flow velocity, and will therefore vary as the solution progresses, particularly when used in transient mode. It is necessary therefore to check the range of local y+ values to ensure that the values of y+ remain within acceptable limits throughout the solution domain. This lower limit on the distance between the lowest grid node and the wall will constrain the degree to which the mesh can be refined near the wall, and any attempt to achieve mesh independent results.

To deal with low Reynolds number effects at the wall where the mean flow velocity in the 'free stream' is very low, a ‘two-layer’ modelling approach can be used. The bulk of the flow is modelled using the standard k-ε model but near the walls, the boundary layer is resolved with a very fine mesh and with the use of the k-l model. The two-layer approach was found to improve the near-wall results, particularly in the region in which there is a strong 'wall' jet (ceiling jet) from the inlet diffuser. Some of the commercial industrial CFD codes now include an automatic wall treatment, known as ‘scalable wall functions’, whereby a low Re (two-layer) model approach for stagnant near-wall regions is mixed with standard wall functions in regions where the Re number is sufficiently high.

The Renormalisation Group analysis (RNG) variant of the k-ε model is claimed by its proponents to be more general and accurate than the standard model. Differences between the RNG and standard k-ε model are effectively due to the effect of an additional term in the ε equation (which represents the effect of mean flow distortion on ε), and to differences in the values assigned to the empirical turbulence model coefficients, e.g. C_{μ}, σ_{k}, σ_{ε} (Computational Dynamics, 1999). In the context of the simple room flow problem, the use of the RNG model brought no discernible improvement to the results.

### 7.4 Application uncertainties

This CFD validation study is based on a well-constructed, simple test case, which was carried out in the context of a recognised international comparison exercise for the purpose of CFD validation. The main application uncertainty is in the representation of the inlet diffuser in the CFD model; the diffuser geometry detail could not be modelled directly but had to be represented by an equivalent, simplified inlet boundary. Nonetheless, this uncertainty is relatively low since the selection of an appropriate inlet boundary was supported by the results of several measurements and CFD simulations by several Annex 20 participants (e.g. Chen and Moser (1991), Ewert *et al.* (1991), Skovgaard (1991) and Heikkinen (1991b)).

### 7.5 Recommendations for Future Work

Although the k-ε model provided a reasonable agreement with experimental data for the simple flow investigated in this study, both low Reynolds number flows and turbulence anisotropy could be identified as possible causes of the artificially high levels of turbulent mixing exhibited by some of the predictions. The use of ‘scalable wall functions’ to deal with low Reynolds number effects at wall regions merits further consideration, as does the use of a Reynolds Stress turbulence model or the latest available models (Spalart-Allmaras, Menter SST or Durbin V2F).

© copyright ERCOFTAC 2004

Contributors: Steve Gilham; Athena Scaperdas - Atkins