The present work has been performed in framework of the research program between Gruppo di Ricerca Nucleare San Piero a Grado of the University of Pisa and Nuclear and Indusrtial Engineering srl. The research aimed at the design and construction of a test facility for the experimental investigation of Critical Heat Flux phenomena at the same conditions as the reference PWR. THe present thesis is related to the structural analysis of the test facility, having the purpose of otimizing the facility layout and designing the support structure in compliance with the applicable regulations. Reference was made ASME VIII-Boiler and Pressure Vessel Code, adopted both for pipilines and for vessels. The analysis were performed by means of Finite Element Method using ANSYS APDL MECHANICAL release 15.0 and ANSYS WORKBENCH release 15.0 codes

MARTINI, ROBERTO

Electronic Thesis and Dissertation Archive - Università di Pisa

 Università di Pisa   Facoltà di Ingegneria  Corso di Laurea Magistrale in Ingegneria Nucleare      Tesi di Laurea    FEM Structural Analysis  Of Critical Heat Flux Test Facility                         Relatore                                                                           Candidato   Prof. Francesco D’Auria                                                                Roberto Martini Prof. Leonardo Bertini                                                                                                       PhD. Fulvio Terzuoli  Anno Accademico 2015/2016 FEM Analisys of CriticalHeat Flux Test Facility0.1 IntroductionThe present work has been performed in the context of the research programbetween Gruppo di Ricerca Nucleare San Piero a Grado of the University ofPisa and Nuclear and Indusrtial Engineering srl. This research aims at thedesign and construction of a test facility for the experimental investigation ofCritical Heat Flux phenomena at the same conditions as the reference PWR.The present thesis is related to the structural analysis of the test facility, havingthe purpose of optimizing the facility layout and design the support structurein compliance with the applicable regulations. Reference was made ASME VIIIBoiler and Pressure Vessel Code, adopted both for pipilines and for vessels. Theanalysis were performed with the aid of Finite Element Method using ANSYSAPDL MECHANICAL release 15.0 and ANSYS WORKBENCH release 15.0codes.0.2 CHF Phenomena in NPPIn a nuclear reactor system the critical heat ﬂux (CHF) is the heat ﬂux at whicha boiling crisis occurs causing an abrupt rise of the fuel rod surface temperatureand, subsequently, a failure of the cladding material. It is agreed that experi-mental investigations on CHF have to be performed for each speciﬁc design ofnuclear reactors. Nowadays a huge number of experimental data are availablewhich were obtained in diﬀerent ﬂow channel geometries and in diﬀerent ﬂuids.In addition, a large number of empirical correlations have been developed forthe CHF data base obtained from particular ﬂow channel geometries and par-ticular parameter ranges. The purpose of the development of the correlationsand of the studies on test facilities is to have less uncertainty and reduce thevalue of MCHFR, deﬁned as the minimum ratio between the critical heat ﬂuxand the operative heat ﬂux, increasing the performances of the nuclear fuel anddecreasing the cost.230.3 Existing CHF Test FacilitiesBecause knowledge of the phenomena that governs the CHF is critical to thecore project, other similar facilities were built around the world:1. KATHY(Karlstein thermal hydraulic test loop), AREVA, Germany2. HANARO (High-ﬂux Advanced Neutron Application Reactor), KAE, SouthKorea3. ODEN, Westinghouse, Sweden4. STAF, ENEA, Italy5. HPCHF(High Pressure Critical Heat Flux ), Oregon State University, USA6. HTRF (Heat Transfer Research Facility), Columbia University, USA0.4 CHF-TF LayoutFigure 1: CHF-TSThe Critical Heat Flux Test Facility Project has been built to make a seriesof experiments about the inﬂuence of a particular type of spacer grids on theCHF phenomena, on a facility that simulate the conditions occurring in a realpressurized nuclear power reactor. The radioactive fuel bundles are simulatedby nine electrical heating rods, positioned into a test section in a square array.Before arriving in the test section the water pass through the Pre-Heaters, usedfor the ﬁne regulation of the ﬂuid temperature just before the Test Section inlet.The steam condenser is placed at the exit of the test section, in order to condensethe vapor produced in test section. After the condenser ﬂuid goes into primarycirculation pump and restarts the loop. Pump, pre-heaters, test section andsteam condenser composed the test section loop, but the primary circuit iscomposed by other two loop:• Heat-exchanger loop4• heat-exchanger by pass loop.This two loops have the purpose to feed the injection system of the steamcondenser. The pressure in the primary circuit is controlled by the pressurizer,designed in the same way of those that equip a standard Pressurized WaterReactor.All primary circuit's piping is composed by 2 pipe all made in ASTM SA 312TP 304L stainless steel, while the surge line is 1 stainless steel pipe. The vesselof the Test Section and the pre-heater are made starting from a 4 pipe, whilethe steam condenser has nominal dimension of 5, and all are made in ASTMSA 312 TP 304L. All ﬁttings are projected according to speciﬁcations given byASME B16.5 and so do not need veriﬁcation.The Maximum Allowable Stress Value for the material is taken from ASMEBPVC sec. II sub. D, Table 1A. Stainless steel used for pipes is isotropic andit has linear elastic behaviour. It has the following material properties:Poisson's Modulus: 0.3Density: 8030 kgm3Young's Modulus and the thermal expansion coeﬃcient aren't take as a con-stant, but they change in a linear way in function of temperature.0.5 Finite Method AnalisysThe ﬁnite element method (FEM) is a numerical technique for ﬁnding approx-imate solutions to boundary value problems for partial diﬀerential equations.FEM subdivides a large problem into smaller, simpler, parts, called ﬁnite ele-ments. The simple equations that model these ﬁnite elements are then assembledinto a larger system of equations that models the entire problem.The analysis is run with the Piping Commands of ANSYS, a special group ofcommands that enable you to model piping systems and their loads in terms ofconventional piping input data, instead of in terms of standard ANSYS direct-generation modeling operations. As you input piping commands, the programinternally converts your piping data to direct-generation model data, and storesthe converted information in the database. Piping command uses PIPE16 andPIPE 18 elements.• PIPE 16PIPE 16 is a uniaxial element with tension-compression, torsion, andbending capabilities. The element has six degrees of freedom at two nodes:translations in the nodal x, y, and z directions and rotations about thenodal x, y, and z axes. This element is based on the three-dimensionalbeam element, and includes simpliﬁcations due to its symmetry and stan-dard pipe geometry.• PIPE 18PIPE18 is a circularly uniaxial element with tension, compression, tor-sion, and bending capabilities. The element has six degrees of freedom ateach node: translations in the nodal x, y, and z directions and rotationsabout the nodal x, y, and z axis.5In this analysis is considered the mass load, considering steel's density equal to8030 kg/m3 and a ﬂuid's density equal to 727 kg/m3, at 350 C and 15.5 MPa,and an operative pressure of 15.5 MPa.Pipes are thermally isolated with a material of density 126 kg/m3, consideredin the analysis.For the temperature distribution, from the experiment's matrix we have chosenthe situation that gives saturation conditions at the exit of the test section,because in this condition greater thermal gradients arise, higher temperature inthe plant is reached, and condensation occurs more tumultuously.The ﬂuid exits from the pump at 310 C, it arrives inside the pre-heater at 315C and at this temperature enters in the test section, where it reaches the satu-ration's temperature at 15.5 MPa of 345 C.At this point vapor is condensated and exits from the steam-condenser at 310C.The ﬁrst step injects at 310 C from by-pass line, while the second step comingfrom the heat exchanger injects at 77 C.Figure 2:0.6 Analysis of Results and Design OptimizationThe goal of my work is to project a constraining system to design the skid onwhich the pipes are ﬁxed.The research of the deﬁnite constraining system was done by an iterative pipestress analysis, starting by a preliminary hypothetical system, based on simpleconsiderations. After each analysis, the critical issues was analysed and imple-mented in the new one.The main purpose of the process is to limit the stress on pipes due to inter-nal and external loads due to pressure and to thermal gradient under 94 MPa(conservative assumption), the maximum allowable stress value for the materialon the design temperature. To do this it is necessary to minimize the reactionvalues applied by constraints on the structures, paying attention that deforma-tions are not so big as to create an intensiﬁcation of the stress or compromisethe functionality of the facility.6• Preliminary SystemFirst I have bonded only the pump, the pressurizer and the heat-exchangeras perfect joints (because their rigidity is much greater than the rest ofthe structure) and test section, to see where the inﬂection is greater andso where the supports need to be placed. This analysis is performed atambient temperature and ambient pressure, considering only the weightof steel and water.Figure 3:• Supports LayoutTo prevent the vertical displacement of the pipes, we place a series ofvertical supports, all bilaterals. The supports are placed under the con-nection pipe, the pre-heater and the condenser, plus one after the pumpinlet to download the load on the pump's joint.7Figure 4:• Working ConditionsFrom this layout, we analyze how the system responds to applied loadsof pressure and temperature. We can see an important displacement inthe direction of the pump axis. This deformation is not dangerous for theintegrity and the functionality of the system, but moreover it allows todecrease the stress favoring the thermal dilatations.Figure 5:The immages show that with a rigid system of constraint we have twomain problems: we can see that at the end of condenser there's an in-tensiﬁcations of the stress over the limit, becouse the vertical pipe havea behavior as a beam with double joint. Furthermore some supports areloaded with a very high stress, that could break themselves.8Figure 6: Equivalent Stress• Elastic SupportsIt's necessary to change the supports more solicited with elastic supportsmade with springs, both to decrease their load, both to give greater ﬂexi-bility to the structure. We replaced the perfect supports on the condenserwith elastic supports able to absorb the vertical loads caused by the ther-mal expansion. This supports are made using LINK 11 elements. In thisway we reduce the reactions on those supports by two order of magnitude.With an initial value of the load of 2559.8 N, we choose spring MEFAFH1-3000, with an elastic constant of 117.9 N/mm.Auxiliary Support System for the PumpA critical point is the stress over the pump junctures, because acooordingto the manual the values of the pipework load have to be very strict to assurethe perfect operation without damage for the pump. We chose to create anauxiliary system that downloads the load over the principal skid, and is givenonly a normal reaction along the pipe axis over the ﬂange, absorbed by anexternal structure.Figure 7:Some loads exceed the reference values, but for FY this does not represent aproblem because we suppose to absorbe this forces along the pipe axis with an9external structure able to download the loads on the earth. MY values is greaterthan the maximum value, but we suppose that dowloading FY, also reduces MYunder the limit.Test SectionIt's important to prevent rotation and torsion to guarantee the integrity of theheaters and to prevent their rupture. Test section could only be dilated axially,and to absorb the thermal dilatation of the structure test section is whipped ona slide that permits the movement along the pump axis direction.Buckling AnalysisBuckling analysis gives a safety factor among instability of one order ofmagnitude.Modal AnalysisIn modal Analysis we chose the pump's frequency of 50Hz as exciters fre-quencies, the frequency coused by movement of ﬂuid between 0 and 0.5 Hz, anda value for condenstation phenomena of the order of kHz. The own frequenciesof the structure are in the order of Hz, but they are very close, and so at highfrequencies resonance problems are possible. In this case it's necessary to inserta dumping system in the most solicited parts.0.7 3D FEM Analysis of Sealing Flange of TestSectionThe most diﬃcult and delicate part of the plant is the design of the sealingﬂange that close below the test section. Through the ﬂange pass the heatingrods, and it must support itself and, at the same time, it's important to ensurethe system is properly sealed from the outside. Wills Rings are metal O-Ringsfor static face-sealing applications that give reliable performance over a largetemperature range for gases and liquids. Extreme high pressures and vacuumscan be sealed with Wills Rings. We start from a standardized ﬂange 4 ASMEB16.5 cl.2500, on which we are going to perform mechanical process to generaterods supports, and the cavity for wills rings and for the blockage system. Rodspass through nine hole of two diﬀerent diameters, to make a support for therods, and this parts are sealed by a second ﬂange maintained in position by fourcaptive bolts, which deform the Wills Rings.In this situation it's important to ﬁnd a compromise between the ﬂuid-dynamicsand structural requirements. From a ﬂuid-dynamics point of view the goal is toobtain a high heat exchange, because this part of the plant isn't cooled by theﬂuid and the high temperatures could damage the rods. It's necessary to min-imize the thickness of the ﬂange to obtain this, and eventually make a centralhole to increase the capability of cooled systems. An external cooling systemcould be necessary.We have performed a 3D FEM Analysis using Ansys Workbench, to comparevarious solutions diﬀerentiated in dimensions and processing. The results showthat the stress caused by the pressure on the rod's supports is incompatible witha normal stainless steel use for mechanical construction: more attention needsto be placed on high resistance alloy based on Vanadium instead, which is able10to resist up to 100MPa.0.8 ConclusionsThis process has been done to project and design a skid able to support thepipes and the vessels of the system, to guarantee the dimensional and structuralintegrity of the plant. Furthermore the analysis allow to design correctly thesupports themselves, so that they don't yield under the loads caused by thereactions. The results combly with the ASME Boiler and Pressure Vessel Code.The main purpose was to keep all the stress under 94 MPa, that rapresent thelimit for the primary strees. This value represent a conservative limit, becausewe haven't done a strict Pipe Strees Analysis, but we have considered the pro-tection against primary stress caused by mechanical loads, that represent lowerstress limit. If S is the Maximum Allowable Stress Value, the limit against bend-ing stress, secondary stress, thermal stress and peak stress are equal to αS withα > 1.5. Furthermore the structure does not undergo at fatigue, because thenumber of cycles of heating are limited, and after the ﬁrst heating the variationsof temperature are low.We have a margin of 6% compared to the limit, but the maximum value onthe structure is limited in a small region, where the greatest contributions aregiven by bending loads, so it is possible to compare this value of 89.4 Mpa with1.5S=142,5 MPa, and so the margin increases to 40%. The rest of the structurehas a margin of 60%, and is therefore in safety conditions. The download ofthe pump is not completed, so the necessity to keep attention at the load arisesand in case improve the isolation. In modal analysis we have considered onlythe lower own frequencies, because at high frequencies damping phenomena arepresent.Currently the criticality of the project is represented by the sealing system oftest section. I have analized one of the possible solutions, and concluded that inorder to keep the Wills Rings conﬁguration, further attention should be focusedon high performances steel containing vanadium, which is able to resist up to1000MPa, but unfortunately reference codes are not more detailed for this ma-terial.After the construction of the plant this project could be enriched with a moni-toring system able to obtain real forces and real reactions on the pipes and onthe supports, and also capable of measuring the real vibrations, to study theresponse of the structure to the induce loads, and the accuracy of the model.

FEM Structural Analysis of Critical Heat Flux Test Facility

Abstract

Similar works

Full text

Available Versions

Electronic Thesis and Dissertation Archive - Università di Pisa