Numerical analyses of the heat transfer processes of a key cooling system in the ITER reactor

One challenging problem that has been successfully addressed is the quantitative characterization of the plasma thermal load on the structures and components of the EC H&CD antenna (or “launcher”).
The plasma is contained in a toroidal vacuum chamber and is kept confined by strong magnetic fields, which prevent it from coming into contact with the chamber walls (and with any materials that face the plasma through openings on these walls, such as those belonging to the launchers). Nevertheless, all plasma facing materials are exposed to intense heat radiation, the characterization of which requires solving a rather complex and computationally expensive thermal radiation problem.
Despite the simplifying hypothesis of uniform and isotropic thermal radiation from the plasma, the exposed surfaces are exposed to a heat flux that is distributed in a highly uneven manner, since it depends locally on the surface orientations, their distance from the radiation source, and on the presence of intermediate shielding elements. This type of radiation problem can be reduced to the calculation of the so-called view factors (VF) from the elemental source surfaces to the elemental target surfaces and requires appropriate numerical methods, such as the Radiosity Solution method (and particularly the embedded Hemicube Method) available in Ansys Mechanical APDL, which takes a discretization into shell elements of the entire set of source and target surfaces as input.

The VF calculation, using the Ansys method above, is a computationally intensive task, the cost of which is approximately proportionate to the square of the total number N of shell elements in the model. In fact, a VF factor is calculated for each shell element relative to every other shell element using a robust “brute force” numerical approach.
However, only a small subset of the N(N-1) VFs calculated is usually necessary (i.e., only the VFs from the source shell elements to the target shell elements) and extracting those VFs from the entire set requires additional post-processing steps that can be quite expensive in computational terms if executed by built-in APDL routines.
NINE has developed its own improved methodology that combines Ansys Radiosity Method for robust VF calculation with ad-hoc Python routines to extract the relevant VFs quickly and efficiently (i.e. with a reduction of processing time by two orders of magnitude).
Once the selected VFs are available, you can obtain the heat flux distribution for the launcher’s plasma-facing surfaces and use it as a boundary condition for subsequent heat transfer and structural assessment analyses.

Another key problem for the structural evaluation was to determine the temperature distribution over the launcher’s entire structure, which then had to be transferred to the finite element analysts as input for the thermal-structural assessment.
The geometrical configuration of the launcher’s cooling system is extraordinarily complex. The physical quantities that characterize the structure-coolant heat exchange locally (such as heat fluxes and heat transfer coefficients) are spread over very wide ranges, and thus it is not possible to resort to classical engineering correlations without introducing very large inaccuracies into the analysis. Instead, a state-of-the-art detailed analysis approach is necessary, taking advantage of the multi-physics modelling capabilities of CFD codes.
Specifically, a CFD conjugate heat transfer (CHT) analysis is needed, in which the thermal-fluid-dynamic problem (i.e., the solution of the mass, momentum and heat balance equations over the fluid domains that represent the cooling system) is numerically coupled to the problem of the heat conduction through the cooled structures. On the other hand, the use of a coarser two-step approach, involving segregated fluid and solid problems to be solved separately, would require the thermal boundary conditions to be defined (in terms of temperature, or heat flux, or heat transfer coefficient) respectively at the interfaces with solid and fluid domains; in complex cases it can be hard, if not impossible, to obtain reasonably accurate estimates of those boundary conditions, and an analyst may be tempted to make overly simplifying assumptions. In a CFD-CHT analysis those interfaces are handled in an implicit manner (by appropriate continuity and energy conservation conditions) and the distributions of temperature and heat flux are outcomes of the simulation rather than an arbitrary input provided by the user.

The first major step in the CFD-CHT analysis of the launcher was the preparation of the 3D geometrical models of the various necessary solid and fluid computational domains. The source information is constituted by the official ITER 3D CAD models, from which the relevant parts need to be exported (see, for instance, Fig. 3). As the exported geometry was incredibly detailed and not directly usable for CFD analysis purposes, it was necessary to accurately defeature and simplify all the irrelevant details and to correct several defects. Moreover, the available CAD geometry obviously includes solid parts only, so the fluid volumes had to be “extracted” from them. All these geometry manipulation tasks were efficiently performed by Ansys SpaceClaim, within an Ansys Workbench project.

The outcome consisted of several volumes representing selected “modules” of the launcher’s structure and the various sections of the cooling circuits. Those volumes are shown in Fig. 4.
The cyan-colored ones correspond to the cooling circuit for the launcher’s structures and consist mostly of channels drilled through the metal bodies and shells that constitute the launcher, which form an intricate network of flow paths.
The volumes in yellow and green correspond to the cooling circuits for the optical components: they must be included in the analysis because, in addition to removing heat from the optical components, they also provide supplementary cooling to certain parts of the launcher’s structure.
The volumes depicted in transparent pink represent part of the launcher’s solid structures, in particular those closest to the plasma (whereas the outermost ones do not play a significant role in the thermal problem and need not be considered in the analysis). The next key step consisted of the generation of computational grids (or “meshes”) for the above volumes with Ansys Meshing. Multiple versions were developed in some cases to allow grid sensitivity studies. The “production” grids, selected on the basis of a balance of accuracy and computational costs, were assembled into a global computational model that counted some tens of millions of nodes and approximately 100 million cells.

CFD-CHT test and production calculations were then setup in Ansys CFX. Thermal-hydraulic boundary conditions for coolant pressure, flow rates and inlet temperatures were obtained from interface information specified by ITER and F4E and from the results of other in-house analyses.
Thermal boundary conditions for the solid domains consisted of distributions of plasma heat flux (as obtained from the VF calculation task described previously) and of heat flux due to power dissipation from the electromagnetic beams (referred to as stray radiation).
Spatial distributions of volumetric power sources were applied over all domains, to account for the energy deposition from neutron and gamma radiation; those distributions, provided by F4E in the form of “point clouds”, were imported into user-defined functions. The Shear Stress Transport (SST) model was used to treat the turbulence. IAPWS-IF97 formulation of water properties, available in CFX libraries, was used.
For the solid materials in the model (stainless steel AISI 316 LN ITER Grade, and CuCrZr alloy) temperature-dependent thermophysical properties were imported from reference tables provided by F4E. Appropriate thermal contact conductance was applied to those solid-solid interfaces where an imperfect thermal contact takes place (e.g., at bolted connections).
Although the so-called “plasma operation” of the ITER reactor is characterized by a pulsating transient behavior, with the full power conditions being maintained only for a fraction of time in a cycle (e.g., for 600 s of an 1800 s period), the main simulations were performed as steady-state, with stationary full-power thermal loads, thus providing conservative results while maintaining acceptable computational costs.
The steady-state simulations were performed to achieve the best convergence level allowed by the available meshes and the numerical setup used, i.e., with a sufficient number of iterations to minimize the residuals and the imbalances and to stabilize the locally monitored quantities.
In particular, the thermal balances over each domain were carefully checked to verify the correct application of boundary conditions and source terms. The target results of the main simulation are the 3D distribution of temperature over all fluid and solid domains (Fig. 5), and the distribution of heat flux over all domain interfaces (both fluid-solid and solid-solid). This information was then exported for use as input for the Ansys thermo-structural models by other analysts in the work team.
Further CFD simulations were also performed to estimate the concentrated and distributed pressure losses through the cooling system, thus providing useful quantitative information to support the design and to ensure the fulfilment of the project requirements and interface specifications (such as those for total available coolant flow rate and maximum allowed total pressure loss).