CANDU Fuel Bundle Deformation Model L.C. Walters A.F. Williams Atomic Energy of Canada Limited Abstract The CANDU (CANada Deuterium Uranium) nuclear power plant is of the pressure tube type that utilizes heavy water as a coolant and moderator. As with other thermal power plants, nuclear fuel produces heat that is subsequently converted into electrical energy. The CANFLEX fuel bundle consists of forty-three fuel elements which contain natural uranium in the form of cylindrical pellets of sintered uranium dioxide. Fission reactions in the natural uranium fuel produce heat that is removed by a flow of pressurized heavy water coolant. This heat is transferred to light water in steam generators to produce steam which drives turbines that generates electricity. A finite-element model of the CANFLEX fuel bundle was developed using ANSYS. The application of this model is the prediction of the overall geometrical deformation of the bundle as a response to a given thermal/mechanical load that may occur under accident transient conditions. This paper summarizes the finite-element fuel bundle deformation model and the testing done on components. Introduction In the CANDU reactor assembly, shown in Figure 1, several hundred fuel channels are contained in and supported by a horizontal cylindrical tank known as the calandria. The calandria is filled with heavy water moderator at low temperature and pressure. The calandria is closed and supported by end shields at each end. The fuel channels, supported by the end shields, are located on a square lattice pitch. Shown in Figure 2, the fuel channel assemblies include a zirconium-niobium alloy pressure tube, a zirconium calandria tube, and four spacers which maintain separation of the pressure tube and the calandria tube. Each pressure tube is thermally insulated from the cool, low pressure moderator, by the CO 2 filled gas annulus formed between the pressure tube and the concentric calandria tube. Under normal operating conditions the pressure in the pressure tube is 10 MPa. Each fuel channel locates and supports 12 fuel bundles in the reactor core. Figure 3 shows the placement of the fuel bundles and channels in the reactor core. CANDU is a registered trademark of Atomic Energy of Canada Limited (AECL). CANFLEX is a registered trademark of AECL and the Korean Atomic Energy Research Institute.
Figure 1. Simplified Schematic of the CANDU Reactor Design Figure 2. CANDU Fuel Channel Arrangement
Figure 3. Placement of the Fuel Channels and Fuel Bundles in the Reactor Core A schematic of a CANFLEX 43-element fuel bundle is shown in Figure 4 [1]. About thirty cylindrical UO 2 pellets are stacked end-to-end to form a fuel stack. A thin layer of graphite (CANLUB) coats the inside surface of the sheathing to reduce pellet/sheath interaction. The pellets are contained in a zirconium alloy (Zircaloy-4) sheathing closed at both ends by end caps. The end caps are resistance welded to the sheath extremities and provide effective fuel stack termination for attachment to the Zircaloy-4 end plate. The forty-three fuel elements are held together at both ends by end plates to form a fuel bundle. The desired separations at the transverse mid-plane of the bundle are maintained by spacers brazed to the fuel elements. The outer ring of fuel elements have Zircaloy bearing pads which support the bundle within the pressure tube. Figure 4. Schematic of a CANFLEX 43-Element Fuel Bundle The fission reaction in the natural uranium fuel produces heat that is removed by a flow of pressurized heavy water coolant around and through the fuel bundles in the fuel channels. This heat is transferred to light water in steam generators to produce steam which drives turbines that generates electricity.
Under accident transient conditions, the fuel elements (as part of a bundle) will be subjected to a set of thermal and mechanical loads. These loads can lead to fuel element bowing and/or elongation. In order to determine the overall geometrical deformation of the fuel bundle in response to a given thermal/mechanical load that may occur under accident transient conditions a finite-element model of a CANFLEX fuel bundle has been developed using ANSYS/Mechanical Version 6.1 [2]. The framework of the bundle model focuses on three basic components: the fuel, fuel sheath (including end caps), and end plates. The pressure tube was modeled as a non-deforming boundary. The scope of the model does not include the effects of thermalhydraulics within the fuel bundle, radiation heat transfer between the fuel elements within the fuel bundle or the components beyond the pressure tube. Recognizing that there are many parameters that affect the behaviour of a bundle during a transient, the bundle model includes selected key parameters (for example, fuel and sheath temperatures, fuel thermal expansion, fuel/sheath interaction, and end-plate effects). The temperature distribution within the fuel and sheath is provided as input and the integrated mechanical response of the system is calculated based on the thermal and mechanical properties of the individual components. The Bundle Model The three-dimensional solid model of the fuel bundle was assembled from the usual ANSYS components: keypoints, lines, areas and volumes. Keypoints were placed at locations defining the boundaries of the entities in the model. Lines were created between the keypoints to define the boundaries of the areas and volumes. Volumes were used to generate the finite-element mesh for the model. The bundle model was meshed using the ANSYS SOLID5 finite element. This eight-noded hexagonal finite element has three-dimensional thermal and structural field capabilities with coupling between the fields. The nodalization of this mesh is sufficiently detailed to allow for radial, azimuthal and axial temperature distributions to be applied within each fuel element and throughout the bundle. Figure 5 shows the finiteelement mesh of the fuel-bundle model. A total of 150,000 finite elements were used in this model. Figure 5. Finite Element Mesh of the 43-Element Fuel Bundle Model
Thermal expansion, radial and axial heat transfer and mechanical response in the fuel stack and sheath are modeled by defining the respective temperature-dependent material properties for UO 2 and Zircaloy [3]. To account for the latent heat during a phase change, the enthalpy of the sheath was defined as a function of temperature. The surface-to-surface contact problem was modeled using contact pairs. The target surfaces were modeled using TARGE170 elements and the contact surfaces were modeled using CONTA174 elements. Friction, specific to each contact pair, was modeled between the fuel and the sheath and between the spacers of neighbouring fuel elements. If the friction between the surfaces is sufficiently large, the two materials will behave much like a layered composite material in which deformations in one component are matched in the other. On the other hand, if the interfacial friction is low, the two materials will not behave as a composite, but rather as two separate objects in simple contact. The coefficient of friction between the fuel and the sheath was selected to be 0.2. Between the spacers of neighbouring fuel elements the coefficient of friction was estimated to be 0.1. The modeling of the fuel was simplified to be one continuous, solid cylinder instead of thirty individual pellets stacked end-to-end inside the sheath. A detailed model of the fuel is not included, not because it is inherently difficult to model, but rather to reduce the complexity of the model. This assumption that the fuel pellets act as a monolithic fuel stack neglects the thermal resistance at the interface between the pellets and the friction/slippage between the pellets in cases of buckling and bowing. The fuel was modeled in contact with the bottom inside surface of the sheath. A gap between the top of the fuel and the sheath of 0.07 mm was assumed. The axial clearance modeled between the end of the fuel and the end caps was 2.0 mm. The end caps are modeled assuming perfect contact with the sheath. The junction between the end cap and the end plate is a continuous metal interface due to the end cap/end plate weld. Heat will flow through this as it would through normal Zircaloy, and loads will be transmitted as well. Details such as chamfers and rounded edges on the end plates have not been modeled. If calculations with the bundle model indicate that high stresses are present in the end plate, fillets will be added to the model. To model the pressure tube as a non-deforming boundary, constraints were placed on all the nodes of the bearing pads so that deformation in the radial direction would be limited to the distance between the bearing pads and the pressure tube. Boundary conditions were used to account for subchannel thermalhydraulic effects and the heat generated in the sheath as the result of radiation heat transfer and zirconium-steam reaction at high temperatures. Boundary conditions were also used to account for fission-gas pressure applied on the inside surface of the sheath and the coolant pressure applied on the outside surface of the sheath. The temperature and pressure boundary conditions were applied to the finite-element nodes via input tables. These tables (in ASCII format) can be produced by external codes. A test case using a simplified boundary condition was performed to examine, qualitatively, the behaviour of this model. In this test, the fuel bundle was constrained in the vertical direction only at the bottom bearing pads to simulate a bundle resting on a non-deforming pressure tube. A temperature profile was imposed on the bundle to simulate the response to a hypothetical accident scenario. A temperature of 300 o C was applied to the bottom fuel elements to represent the reactor coolant conditions. A temperature of 900 o C was applied to the fuel elements at the top of the bundle to represent a steam environment. Figure 6 shows that the temperature on the remaining fuel elements was linearly increased from the bottom to the top elements. Figure 7 shows the deformation of the fuel bundle as a response to this hypothetical accident scenario. The difference in rate of thermal expansion between the top and bottom elements caused the endplates to deform. The fuel elements at the top of the bundle also experience some bowing in the vertical direction since their deformation in the axial direction due to thermal expansion is limited by the stiffness of the endplate. This example has shown that under accident transient conditions, the finite element model displays fuel element elongation and bowing which leads to geometrical deformation of the fuel bundle.
Figure 6. Temperature Gradient Across the Face of the Fuel Bundle in the Qualification Test Case Figure 7. Side View of the Bundle Model Showing Displacement in the Vertical Direction in the Qualification Test Case
Testing of the Single Fuel Element Model The test case described above demonstrated the feasibility of the ANSYS code and the applicability of the modeling techniques to further development of the fuel bundle deformation model. The next step in the development of the model was to verify phenomena deemed important to meet the target application of the model, i.e., the geometrical deformation of the fuel bundle to thermal/mechanical loads. In this section, thermally induced deformation in a single fuel element model is compared against experimental data. Suitable data for testing thermally induced bow, caused by a circumferential temperature distribution around a fuel element, was found in [4]. Bow is defined as the magnitude of deflection measured normal to the restraint plane. Figure 8 shows a schematic of the fuel element bow tests experimental set up. A fuel element simulator with an eccentric tungsten heater was developed and used to study the influence of major parameters affecting bow up to a maximum sheath temperature of 600 o C. The bottom sheath temperature was held constant during each test at about 300 o C (ranging from 287 o C to 312 o C) to represent the reactor coolant conditions. The transient bow in the fuel element was measured for various top-to-bottom sheath temperature differences and different bottom sheath temperatures. Figure 8. Schematic of the Fuel Element Bow Tests Experimental Set Up
Finite-element models of a single fuel element were developed using geometrical dimensions for the fuel and the sheath consistent with those used in the fuel element bow tests. Three different geometries were examined in which the fuel/sheath diametral gap was 0.004 mm, 0.02 mm and 0.082 mm. In the experiments, eighteen fuel pellets were placed end to end inside the sheath. In the single fuel element model, however, the eighteen fuel pellets were modeled as a solid monolithic cylinder 0.27 m long. The sheath, modeled as 0.29 m long (slightly longer than the fuel), was constrained in the vertical direction at two points near the ends of the sheath, 0.25 m apart. Temperature of the fuel and the sheath was input from experimental data. Results from the simulations compare well with the experimentally measured transient bow as shown in Figure 9. In the experiments with the fuel/sheath diametral gaps of 0.004 mm and 0.02 mm the eighteen fuel pellets thermally expanded across the small fuel/sheath gap into contact with the sheath, interacted with the sheath, and remained in axial contact with each other. The fuel/sheath then acted as a layered composite material, in that deformations in the fuel were matched in the sheath. Therefore, modeling the fuel as a monolithic stack accurately represented the behaviour of the fuel when the fuel/sheath diametral gap was 0.02 mm. However, when the fuel/sheath gap was larger (0.082 mm) the mechanical interaction between the fuel and sheath was low and the pellets did not come into tight contact with the sheath or remain in axial contact with each other. Instead of driving the deformation in the fuel element, the fuel pellets acted as individual weights reducing the overall transient bow. Therefore, the monolithic fuel stack was not a good approximation when the fuel/sheath diametral gap was 0.082 mm and it was necessary to model the fuel pellets as eighteen individual pellets, each 15 mm long. In Figure 9, the simulated results for fuel/sheath diametral gaps of 0.004 mm and 0.02 mm were produced using a monolithic fuel stack while for the gap of 0.082 mm the fuel was modeled using individual pellets. Figure 9. Comparison of Experimental Data from the Fuel Element Bow Tests and the Finite Element Simulations (Note: Each Data Point Represents an Individual Test) Conclusion A finite-element model of a 43-element CANFLEX fuel bundle was generated using ANSYS. The target application of this model is the prediction of the overall geometrical deformation of the bundle as a response to a given thermal/mechanical load that may occur under CANDU reactor accident transient conditions. A test case where a thermal load was applied to the model showed that the fuel bundle model
demonstrates the correct qualitative response. Simulations using a single fuel element subject to a circumferential temperature distribution were also performed. The resultant deformations in the fuel element for various circumferential temperature distributions agreed very well with experimental data. The success of these simulations encourage further development of the fuel bundle deformation model using ANSYS to ultimately develop a comprehensive model for use by safety analysts in CANDU reactor licensing activities. References 1. W.R. Inch and P. Alavi, "CANFLEX MK-IV Qualification Program and Readiness for Implementation, " Seventh International Conference on CANDU Fuel, 2001 September 23-27, Kingston, Ontario, Canada. 2. ANSYS Inc., "ANSYS Theory Reference 6.1", Canonsburg, PA, 2002 April. 3 P.E. MacDonald, "MATPRO-Version 09: A Handbook of Materials Properties for use in the Analysis of Light Water Reactor Fuel Rod Behavior", EG&G Idaho, Inc., 1976. 4. P.M. Mathew, S. Baset, J. Veeder and E. Kohn, "Quantification of Factors Affecting Thermally- Induced Bow in CANDU Fuel Element Simulator", 5th International Canadian Nuclear Society CANDU Fuel Conference, 1997, p.342.