Introduction
Boiling is one of most effective heat transfer mechanisms. The ability to accurately predict such phase change phenomenon is of great importance in process and power generation industries. Although most commonly used, boiling in water flow represents a significant challenge due to large density difference between both phases (i.e. liquid water and steam) and latent heat of vaporisation.
Boiling is usually induced by a heated wall where vapour bubble creation and their departure are governed by processes that cannot be resolved by a numerical grid. For that reason, additional mathematical models are necessary to capture this important heat transfer phenomenon.

Objectives
The wall boiling flow test case examines the capability of the modelling software to predict phase change phenomena with large density changes and especially the wall boiling. Significant buoyancy forces and heat transfer associated with vaporisation and condensation in the surrounding, subcooled environment may represent an additional challenge.
CFD simulations of water flow in an annulus shall be conducted for selected, specific experimental conditions [1 & 2] where the heat flux is high enough to produce substantial vaporisation with the local vapour volume fraction reaching 30%.
The CFD simulation results shall be used to calculate radial distribution of void fraction (i.e. vapour volume fraction), vapour and liquid velocities at a specified axial location, where the experimental data was collected [1 & 2]. Such radial profiles tend to be more selective than the flow variable axial distributions.

Geometry

• Radius of heating element (R_i) is 9.5 mm.
• Tube external radius (R_o) is 18.75 mm.
• Length of the heating element (L_h) is 1.67 m.
• Length of the upsteam section (L_pre) is 0.28 m.
• Length of the downstream section (L_post) is 0.30 m.
• Elevation of the measuring plane (L_m) is 1.61 m.

Using axisymmetry, the simulation domain can be a two-dimensional tangential slice of the annular geometry. Poor convergence due to restrained entrainment may force the user to simulate a wider tangential section.

Loading
The fluid motion is induced by the prescribed water inlet mass flux `G_(i\n)`. A constant heat flux `q_w` is assigned along the vertical inner wall of the annulus. Two cases are analysed:
1)   `G_(i\n) = 474` `"kg"//"m"^2 s`, `q_w = 152.3` `"kW"//"m"^2`
2)   `G_(i\n) = 1059.2` `"kg"//"m"^2 s`, `q_w = 251.5` `"kW"//"m"^2`

Material properties
Water-vapour mixture properties based on IAPWS IF97 steam tables [3] (or equivalent) shall be used in the modelling analysis.
They should cover the pressure range between 100 and 200 kPa, and the temperature range between the 30°C of subcooling and the saturation conditions.

Meshing
Hexahedral grid elements are used in the both simulated cases. In the radial direction, the grid spacing is compressed near the inner perimeter of the annulus to 0.089 mm and then expanded in the radial direction to 0.178 mm.

In the axial direction, a uniform grid spacing of 4 mm is applied. Furthermore, 4 grid nodes are used in the tangential direction to discretise the 2° large annular section.

Initial conditions
Due to the steady-state nature of the boiling heat transfer case, initial conditions are not important. They should be used to enhance stability of the solution procedure.

Boundary conditions

• At the inlet, the following mass flux values and temperatures used in the experiments [2] shall be prescribed:
1)   `G_(i\n)=474` `"kg"//"m"^2 "s"`, `T_(i\n)=96.6^"o""C"`
2)   `G_(i\n)=1059.2` `"kg"//"m"^2 "s"`, `T_(i\n)=92.1^"o""C"`

• At the outlet, a fix pressure level should be set, which has to be adjusted to meet the requested inlet subcooling conditions:
1)   `p_(i\n)=0.142` `"MPa"`
2)   `p_(i\n)=0.143` `"MPa"`

Due to pressure dependence of the boiling location, it may be more suitable to impose fix pressure conditions at the inlet and mass flux at the outlet.

• At the section of the inner wall occupied by the heater (L_h), the following heat flux values and the no-slip boundary conditions shall be prescribed:
1)   `q_w=152.3` `"kW"//"m"^2`
2)   `q_w=251.5` `"kW"//"m"^2`

• The sections of the internal wall up- and down-stream the heater, as well as the external wall are to be kept adiabatic with no-slip boundary conditions.
• For the vertical, tangential surfaces, symmetry or equivalent conditions shall be used.

Results
The simulation results were obtained using a double precision CFD solver. For both analysed cases, the calculated radial distribution of vapour volume fraction, liquid and vapour velocities at the elevation L_m are compared with published experimental and other CFD results [1 & 2].
Case 1

Quadratic mean (or RMS) of deviation between the experimental data [1] and the current CFD simulation results is calculated for Case 1:

	RMS of deviation
vapour volume fraction	0.014
vapour axial velocity	0.092 m/s
liquid axial velocity	0.042 m/s

Case 2

Quadratic mean (or RMS) of deviation between the experimental data [1] and the current CFD simulation results is calculated for Case 2:

	RMS of deviation
vapour volume fraction	0.0061
vapour axial velocity	0.210 m/s
liquid axial velocity	0.071 m/s

Files

• Experimental data [1] for Case 1 & 2 (2016/03/21)
• CFD simulation results [2] for Case 1 & 2 (2016/03/21)