# Engineering of a FGM Interlayer to Reduce the Thermal Stresses Inside the PFCs
## 3 Conceptual Design of a Steel-Based PFC with a Engineered W/Steel FGM Interlayer
### Design of the Heat Sink  
Under the above mentioned assumptions, the geometry of the heat sink is independent from the interlayer, whose thickness \(\delta_{3}\) and W concentration \(C\) are yet to be defined. The design of the heat sink is carried out by satisfying the design criteria even if no interlayer and armor were joined to it. The heat sink is the structural material in these components and has to ensure the capability to manage the primary and secondary stresses even if both the PFM and FGM were to fail and detach from it. The main parameters of Figure 3 that drive the stresses in the steel plate are the thickness \(\delta_{hs}\) of the upper/lower part of the heat sink and the ratio \(\left(\frac{L}{\delta_{hs}}\right)\). The first variable impacts the secondary stresses, while the latter mainly defines the primary loads which are the one due to the pressure applied by the coolant. The determination of \(\delta_{hs}\) and \(\left(\frac{L}{\delta_{hs}}\right)\) is carried out in such a way that the design criteria [6] are satisfied. The process is explained in details in [24] and will not be reported here for brevity. Using the primary membrane plus bending stress criterion along with the membrane primary plus secondary membrane stress criterion one obtains 1 mm for the heat sink thickness and 7 for \(\left(\frac{L}{\delta_{hs}}\right)\). One must point out that for the allowable stress intensity \(S_{e}\) we used conservatively the definition of one third of the minimum ultimate tensile strength, to take into account a high neutron exposure which could lead to a minimum uniform elongation of less than two percent. For the complete geometry of the steel sub-component, only the parameter \(\delta_{side}\) is left to be determined. The impact of this quantity is mainly on the temperature field. The smaller \(\delta_{side}\) is, the lower would be the maximum temperature of the heat sink, and also the temperature field would depend more weakly on \(x\), \(T\sim T(y)\). In this work we chose arbitrarily \(\delta_{side}=2\delta_{hs}\). To check if all criteria are indeed satisfied, we then proceed by importing the computed geometry in a FEM thermomechanical model of the steel heat sink. The numerical model is carried out in ANSYS Workbench 2022 RI, using only an elementary cell which has been extruded along the \(z\) direction for a length \(L\), chosen arbitrarily equal to the channel width. The kinematic boundary conditions used for the thermomechanical model are the following:  
* No bending: the \(y\) component of the displacement is zero on the backside of the plate, which are the points \((x,y=0,z)\). * Symmetry condition: the \(x\) component of the displacement is zero on the points \((x=0,y,z)\). * Symmetry condition: the \(z\) component of the displacement is zero on the points \((x,y,z=0)\). * \(z\) direction: the \(z\) component of the displacement is constant on the points \((x,y,z=L)\). Figure 3: Sketch of the geometry of the PFC, together with a magnification of the elementary cell. The nomenclature of all the dimensional parameters is also shown. \(x\) direction: the \(x\) component of the displacement is constant on the points \((x=L+2\delta_{side},y,z)\). By applying the last two conditions, we are admittedly ignoring the boundary effects that can occur at the edges of a plate, where points of the body that were on a line perpendicular to the middle surface of the plate do not stay in such a configuration after the application of the temperature field. These effects depend on the real geometry of the whole plate and would be computed at a later stage of the design than the conceptual phase. The mesh of the model is shown in Figure 4, along with the temperature field \(T(x,y)\) inside the steel plate. Assuming a negligible heat peaking factor in the solid domain of the interlayer and the armor, which is valid for poor thermal conductors, the load has been applied directly to the heat sink. The mesh is made of 11200 SOLID186 elements, corresponding to more than 80 k nodes.