Docs

Buoyant Flow: Natural convection between heated plates

Overview

The aim of this test case is to validate the following parameters of steady-state natural convection between two plates maintained at different temperatures. The incompressible, turbulent case is validated with the experimental results of Betts and Bokhari [1] as archived in the ERCOFTAC database [2]. The following parameters have been analysed:

  • Velocity Profiles
  • Temperature Profiles

The geometry is uploaded on to the SimScale platform and meshed using the snappyHexMesh tool.

This project could be imported from the library upon request.

Geometry

The geometry is constructed based on the reference case [1], as shown in Fig.1. Its dimensions are \(2.18\ m \times 0.076\ m \times 0.52\ m\), and the face details have been given in Table 1.

BuoyantFlow-geometry

Fig.1. Geometry used in the study

Table 1: Domain Details
Face Type
ABCD Bottom
EFGG Top
ABFE Hot Wall
DCGH Cold Wall
BCGF Front
ADHE Back

Analysis type and Domain

The snappyHexMesh tool was used to generate a uniform mesh (see Fig.2. and Table 2.).

A typical property of the generated mesh is the \(y^+\) (“y-plus”) value, which is defined as the non-dimensionalized distance to the wall; it is given by \(y^+ = u^*y/\nu\). A \(y^+\) value of 1 would correspond to the upper limit of the laminar sub-layer.

  • Explicit resolution of the near-wall region: The first cell lies at most at the boundary of the laminar sub-layer and no further. Here, \(y^+\) value is 1 or below.
  • Use of wall-functions to resolve the near-wall region: There is no need to place cells very close to the laminar sub-layer, and typically \(30 \leqslant y^+ \leqslant 300\).

A \(y^+\) value of 30 was used for the inflation layer. The \(k-\omega\) SST turbulence model was chosen, with wall functions for near-wall treatment of the flow.

Tool Type : OPENFOAM®

Analysis Type : buoyantSimpleFoam

Mesh and Element types :

Table 2: Mesh Metrics
Mesh type Number of volumes Type
snappyHexMesh \(5.95 \times 10^6\) 3D hex
BuoyantFlow-mesh

Fig.2. Mesh used for the SimScale case

Simulation Setup

Fluid:

Table 3 encapsulates the properties of fluids used in the subsonic and supersonic case simulations.

Table 3: Fluid Properties
\(m\) \(g/mol\) \(c_p\) \(J/kgK\) \(mu\) \(N/ms\) \(Pr\)
\(28.9\) \(1005\) \(1.831\times 10^{-5}\) \(0.705\)

The boundary conditions for the simulation are shown in Table 4. Note: FFP stands for Fixed Flux Pressure.

Boundary Conditions:

Table 4: Boundary Conditions for Ahmed Body simulation
Parameter Top and Bottom Front and Back Hot Wall Cold Wall
Velocity \(0.0\ ms^{-1}\) \(0.0\ ms^{-1}\) \(0.0\ ms^{-1}\) \(0.0\ ms^{-1}\)
Modified Pressure FFP ( \(10^5\) Pa) FFP ( \(10^5\) Pa) FFP ( \(10^5\) Pa) FFP (\(10^5\) Pa)
Temperature Zero Gradient Zero Gradient \(307.85\) K \(288.25\) K
\(k\) Wall Function Wall Function Wall Function Wall Function
\(\omega\) Wall Function Wall Function Wall Function Wall Function
\(\alpha _t\) Wall Function Wall Function Wall Function Wall Function
\(\mu _t\) Wall Function Wall Function Wall Function Wall Function

Results

Velocity Profiles

Shown below are comparisons of velocity profile between the two plates from SimScale simulation results with the reference [1] at different heights. The reference lines are located at the mid-plane normal to the z-direction.

BuoyantFlow-results-V-y872

Fig.3.a. Velocity profile at \(h = 872\ mm\)

BuoyantFlow-results-V-y872

Fig.3.b. Velocity profile at \(h = 218\ mm\)

BuoyantFlow-results-V-y109

Fig.3.c. Velocity profile at \(h = 109\ mm\)

Temperature Profiles

Shown below is the comparison of the temperature profile between the two plates from SimScale simulation results with the reference [1] at a height of \(109\ mm\). The reference line is located at the mid-plane normal to the z-direction.

BuoyantFlow-results-T-y109

Fig.4. Temperature profile at \(h = 872\ mm\)

Disclaimer

This offering is not approved or endorsed by OpenCFD Limited, producer and distributor of the OpenFOAM software and owner of the OPENFOAM® and OpenCFD® trade marks. OPENFOAM® is a registered trade mark of OpenCFD Limited, producer and distributor of the OpenFOAM software.