This paper considers a composite cylindrical structure, with low-enriched uranium (LEU) foil enclosed between two aluminum 6061-T6 cylinders. A recess is cut all around the outer circumference of the inner tube to accommodate the LEU foil of open-cross section. To obtain perfect contact at the interfaces of the foil and the tubes, an internal pressure is applied to the inner tube, thereby plastically and elastically deforming it. The residual stresses resulting from the assembly process are used along with a thermal stress model to predict the stress margins in the cladding during irradiation. The whole process was simulated as a steady-state two-dimensional problem using the commercial finite element code Abaqus FEA. The irradiation behavior of the annular target has been presented, and the effect of the assembly residual stresses has been discussed.
The majority of the molybdenum-99 (Mo-99) produced internationally is extracted from high-enriched uranium (HEU) dispersion targets that have been irradiated. Mo-99 is the parent isotope of the radioactive tracer, technetium-99 m, which is used in medical imaging procedures. The high concentration U-235 in HEU-based targets makes them potential items of interest for rogue individuals. To alleviate the potential of proliferation issues, low-enriched uranium (LEU) targets are being mandated. Unfortunately the conversion of HEU- to LEU- based dispersion targets is accompanied by a reduction in Mo-99 production given today’s dispersion target technology. An increase in the density of uranium is needed in LEU-based targets in order to recover the loss in Mo-99 production per target [
The function of the target is to contain the fission products and to effectively dissipate the generated fission heat to the reactor coolant. For dispersion target designs there is generally little concern about heat getting dissipated to the coolant as the target structure offers little resistance to heat transfer. However, for the disassemble-able LEU foil target; there is a potential of the cladding to separate from the LEU foil and significantly increase the thermal resistance between the LEU and cladding. The increase in thermal resistance could lead to a rise in LEU temperature that might exceed the limits set forth by the reactor. An analysis needs to be conducted on this target structure to ensure safe usage both during assembly and irradiation.
The target is assembled by wrapping a thin nickel foil (~15
Exploded view of the target assembly.
An internal pressure is applied to the inner surface of the inner tube to close the gap between the foil and the outer tube. The internal pressure can be applied by either a draw plug or by using a pressurized hydraulic fluid [
By design, the assembly process leaves residual stresses in the aluminum cladding. Previous thermal-mechanical analysis on annular targets with zero residual stresses has shown that there is a tendency for a gap to open up between the foil and the outer tube [
A numerical model of the annular target assembly was created using the commercial finite element code Abaqus FEA [
The finite element mesh used in the analysis, consisting of 16000 elements and 51221 nodes with 10 elements through the thickness of each assembly component, is illustrated in Figure
Finite element mesh used in the three-step analysis.
The development of the assembly model follows directly from the Argonne National Lab (ANL) target design [
Drawing of the geometry used for the assembly model in the first analysis step.
As the model is based on the ANL target, all the tube dimensions are precisely those described by the technical drawing of that target. Again, because the cross-section occurs at a length along the target that includes the uranium foil, the dimensions of the inner tube correspond to the ANL foil relief specifications. In addition, it should be noted that the foil is assumed to be in perfect initial contact with the inner tube. While this is not necessarily the case with physical specimens, it is an essential simplification to the model. The assembled stress state of a target is important as it can either aid or hinder the disassembly process. In order to achieve a stress state that encourages the target to open after being cut longitudinally, the inner tube must be plastically deformed and the outer tube must be only elastically deformed. To simulate plastic deformation, a plastic material model must be defined within Abaqus. This data must be given in the form of true stress and plastic strain. In some cases, it may be necessary to convert engineering stress and strain to true stress and plastic strain. However, as the tube material being investigated at the University of Missouri-Columbia is Al 6061-T6, the true stress and plastic strain data for aluminum 6061-T6 was obtained from [
True stress and plastic strain data for aluminum 6061-T6 and uranium.
The plasticity data supplied by [
The desired internal pressure for hydroforming was determined through a combined analytical and experimental approach. According to analytical plastic theory, the critical pressure which will cause yielding is given by the following as
Using the dimensions of the inner tube previously described and a typical yield stress for Al 6061-T6 of 255 MPa, the calculated critical pressure using (
Through the experiments run with the hydroforming test bench (Figure
(a) Hydroforming test rig with annular target in place. (b) Assembled hydroforming test rig.
Loading and boundary conditions for the hydroforming model in the first analysis step.
To model the irradiation behavior which takes into account the residual stresses from the assembly process, a fully coupled thermal stress step was added after the residual stress step. The loading conditions and the contact definitions from the first two steps were suppressed. A heat generation rate of 1.6 × 1010 W/m3 was applied to the foil, which corresponds to a heat flux of 100 W/cm2 incident on the outer surface of the inner tube and the inner surface of the outer tube. Water coolant flow at 323 K through the inner and along the outer tubes was simulated by defining a surface heat transfer coefficient and a sink temperature. The heat transfer coefficient of 19000 W/m2 K corresponds to a flow velocity of 0.83 m/s through the inner tube and 1.86 m/s along the outer tube. The loading and boundary conditions for the irradiation model are illustrated in Figure
Loading and boundary conditions for the irradiation model in the third analysis step.
New contact definitions had to be made for the irradiation model due to the different contact interaction property for the normal behavior. For the irradiation model it is assumed that the tubes may have a tendency to separate after they come in contact, whereas for the hydroforming part, the normal behavior does not allow any separation once the tubes are in contact. This is the main difference in the mechanical contact definition properties for the assembly and the irradiation part. Due to the composite structure of the model and the presence of interfaces, a thermal conductance had to be defined while defining the contact interaction properties. As the magnitude of the thermal conductance is unknown, an infinite conductance was specified at zero clearance, and for a clearance of 0.01 m the thermal conductance is assumed to be zero. Abaqus interpolates between these values to obtain the thermal conductance for any interfacial gap in the model. It is assumed that there is conduction through the air, and the effects of heat redistribution have not been considered in modeling the gap.
Figure
Postassembly numerical displacement contour and microscope images.
Figure
Equivalent plastic strain across the assembly radius at
One of the goals of the hydroforming process is to close the gap between the foil and the outer tube by plastically deforming the inner tube. The magnitude of the applied hydroforming pressure should be such that it should be able to close the gap between the foil and the outer tube and induce sufficient plastic deformation in the inner tube so that even during elastic recovery an interfacial bond is maintained between the foil and the outer tube. Figure
Separation at the interface of the foil and the outer tube after the various modeling steps.
Figure
Radial temperature distribution across the inner and outer cladding.
Figure
Hoop stress distribution in the inner tube through various modeling steps at
The hoop stresses in the outer tube through the three modeling steps have been illustrated in Figure
Hoop stress distribution in the outer tube through various modeling steps at
The goal of this paper was to integrate the assembly process of the annular target along with the irradiation analysis to analyze the behavior of the target and assess the effect of residual stresses. A three-step elastoplastic model was built using the commercial finite element code Abaqus FEA [
The results from the analysis show that the applied internal pressure is adequate to induce enough plastic deformation to maintain the bond at the interface of the foil and the outer tube. The residual stresses from the assembly process tend to negate and decrease the hoop stresses in the inner and outer tubes at the end of the irradiation step. This is favorable from a material standpoint as the inner and outer tubes are unlikely to fail under the applied heat generation of 1.6 × 1010 W/m3. This corresponds to a heat flux of 100 W/cm2 incident on the outer surface of the inner tube and the inner surface of the outer tube. The postirradiation compressive hoop stresses in the inner tube are greater than the stresses in the outer tube, which move from being compressive to tensile across the thickness. Hence, the inner tube is likely to dictate the failure of the target.
The authors would like to thank Charlie Allen at the University of Missouri Research Reactor (MURR), Dr. Sherif El-Gizawy at the University of Missouri, Dr. George Vandegrift at Argonne National Laboratory, and Lloyd Jollay and John Creasy at Y-12 National Security Complex for supporting this activity.