proceeding of fifteenth abaqus user group2000p17

1、LIMIT LOADS FOR AXIALLY LOADED CYLINDERS HAVING FULL CIRCUMFERENTIAL CRACKS: EXPERIMENTAL, ANALYTICAL AND NUMERICAL STUDIESM. A. Lynch*, D. N. Moreton+ and D. G. Moffat+*NNC Ltd, Knutsford, Cheshire, UK.+The University of Liverpool, Department of Engineering, Liverpool, UK.ABSTRACTThe limit load of

2、an axially loaded cylinder, containing a fully circumferential part-penetrating crack, has been established using stress analysis to find a lower bound to the limit load. Details of a finite element (FE) study, which confirms the analytical predictions, are presented for a cylinder with D/t=15 with

3、a range of crack depths. In addition, an experimental programme is presented for precision made specimens with extensive strain gauging. The experimental response is compared with the corresponding full non-linear FE analysis, for one of the crack depths considered.1a D DIDo E FE FLRlig tnsy2NOTATIO

4、NCrack depth Mean diameter Inside diameter Outside diameter Youngs modulus Finite element Limit loadLigament mean radius Wall thickness Poissons ratio Material yield stressINTRODUCTIONA previous study of cracked piping elbows 1 has shown that it is possible to over-estimate the limit load using stan

5、dard FE meshing techniques, particularly for components with long, deep cracks. That study demonstrated that it was possible to decrease the limit load for a piping elbow having a long deep crack and subjected to opening bending by increasing the concentration of the mesh through the crack ligament.

6、 The objective here is to step back from the relative complexity of piping elbows and to study a cylinder with a fully circumferential internal defect subjected to2001 ABAQUS UK Users Group Conference1tensile axial loading as illustrated by figure 1. The terminology (limit load, plastic load etc.) u

7、sed here follows the recommendations of Gerdeen 2.The work reported here was intended to provide an understanding of the type of FE mesh that is required to successfully model the limit load of such a cracked component. In this instance, a limit load solution is available from conventional stress an

8、alysis 3 and in addition, an experimental programme has included tests on four cylinders containing cracks of differing depthsas well as one uncracked cylinder.This has permitted comparison of several FEmeshing meshingtechniques with analytical and experimental data in order that the techniques coul

9、d be assessed.valueofthosetaFCrack FaceF1.Section through Cracked CylinderIt may be considered adequate to calculate the limit load of a cylinder, such as that depicted by figure 1, using the net-section of the remaining ligament. Calculation of the ligament stress and equating to the material yield

10、 stress gives:FL = sy 2pRlig (t - a)(1)The notation used within equation (1) is defined by figure 2 and in particular, Rlig represents the mean radius of the ligament. However, this approach neglects the possibility of a hoop stress in the region of the crack. By recognising this possibility and fol

11、lowing the principle of the lower bound limit theorem (see e.g. Calladine 4) a solution which gives a limit load that is greater than that suggested by equation (1) can be obtained.22001 ABAQUS UK Users Group Conference21LaRligt2.Notation for Cracked AreaThis solution is detailed in 3 and requires t

12、he following assumptions:The loading of the cylinder is purely axial.A fully circumferential part-penetrating crack, of zero width, exists in the inside wall of the cylinder.The material of the cylinder is elastic/perfectly-plastic and obeys the maximum shear strain energy (von Mises) theory of yiel

13、d.The radial stress is zero.The resulting solution is:2tF =s 2pR(t - a)a (2)Lylig(1 +33 ) 2 a1 - 3 at 2(t - a)FL = 2pR(t - a)s+a (3)ligy4 t - a (1 +3)2001 ABAQUS UK Users Group Conference3These relationships for the limit loads, normalised to the nominal yield load for the ligament are plotted in fi

14、gure 3, as a function of the crack depth to thickness (a/t) ratio.1.161.121.081.041.0000.250.5a/t0.7513.Limit Load Defect Depth Relationship3FE MESH CONVERGENCE STUDYThis mesh convergence study concentrated on three crack depth to thickness (a/t) ratios. These were 0.25, 0.5 and 0.75. The FE models

15、were generated using PATRAN 5 and analysed using ABAQUS standard 6. The material properties were, at this stage, chosen to be elastic/perfectly- plastic and consistent with the mild steel elbow study reported in 1. These and the cylinder dimensions chosen were:Do = 34.29mmE = 210 GN/m2Di = 30.00mm =

16、 0.285D/t = 15y = 308 MN/m2Two types of mesh were used for this study:A Standard limit load mesh, with nodes released to simulate a crack and,A Focused mesh, similar to a fracture mechanics mesh design.42001 ABAQUS UK Users Group ConferenceFL/sy2pRlig(t-a)Globally, the mesh structure for each case r

17、emained the same. However, the standard mesh may not make any particular allowance for the position of the crack tip, although the element mesh may be biased towards the crack tip. Conversely, the focused mesh, as the name suggests, focuses the elements towards the crack tip. These two mesh techniqu

18、es were used to evaluate the limit loads for the three different crack depths.4.(a) Schematic of FE model Layout(b) Typical FE modelThe cylinders and their cracks considered herewere axisymmetric, enabling the use ofaxisymmetric elements. The elements used throughout were 8-noded, biquadratic, reduc

19、edintegration, axisymmetric solid elements (ABAQUS element: CAX8R). The use of such elements allowed modelling simply through the plane of the cylinder thickness. Additionally, only onesymmetrical axial half of the cylinder was modelled as shown in figure 4.The nodes at theligament were constrained

20、axially (i.e. in the 2 direction) to provide a symmetry face. The tensileload was applied by means of a pressure acting on the end of the cylinder in order to provide uniform loading across the thickness. The crack was modelled by allowing the nodes along the crack face to be unconstrained: the crac

21、k was thus assumed to have zero width.Three typical standard mesh designs for an a/t ratio of 0.75 are shown in figure 5. Two types of standard mesh were assessed: Element size kept constant through the thickness at the crack position - this would be the case if an existing uncracked model was alter

22、ed to create a cracked model and,2001 ABAQUS UK Users Group Conference5Refining the mesh so that the element size was biased towards the crack tip, (referred to as a non-uniform standard mesh).5.Typical Standard mesh designs for a/t=0.75Away from the crack, the number of elements through the thickne

23、ss was always two. In the region of the crack, the number of elements through the thickness was varied from four (for a standard mesh) and eight (for a non-uniform standard mesh) to 32. The degree to which the element size was biased towards the crack tip was investigated by varying the non-uniformi

24、ty ratio. This ratio is defined as the ratio of the lengths of the smallest and largest elements along the crack ligament and could be adjusted easily in PATRAN 5.The construction of the focused mesh was more complex. The mesh away from the crack position remained of the same form but the elements s

25、urrounding the crack tip were generated such that the nodes could be collapsed or focused to the crack position, forming elements, as shown in figure 6. The number of elements through the ligament, and hence the size of the focused elements, was varied but found to have very little effect on the lim

26、it load. Hence, the effect of the number of focused elements surrounding the crack tip was the main concern. The method of mesh construction in this region is illustrated by figure 7. The number of elements through the ligament was increased with increasing elements around the crack tip in order to

27、maintain reasonable element form away from the tip.62001 ABAQUS UK Users Group ConferenceyzxCrack TipCrack FaceLigamentElements Created around Crack Tip PositionLigament NodesNodes Collapsed to Crack Tip and Mid-Side Nodes Adjusted6.Focused Mesh Construction for a/t=0.752001 ABAQUS UK Users Group Co

28、nference77.Typical Focused Mesh Designs for a/t=0.754EXPERIMENTAL WORKFor this experimental programme, a total of five cylindrical specimens were tested in tension. Four of the specimens contained cracks having nominal a/t values of 0.15, 0.3, 0.5 and 0.75. A fourth specimen having no crack was test

29、ed and served also to provide the uniaxial stress-strainrelationship for the material.Further material was set aside for additional tensile test specimens.82001 ABAQUS UK Users Group Conference8.Manufacturing Specification for Cylinders1.Dimensional Survey in the Region of the DefectAll specimens we

30、re machined from the same bright, mild steel bar. The specimen design is shown in figure 8. This was manufactured by rough machining the bore and outside surfaces prior to stress relief of these blank specimens. The heat treatment used also served to introduce a clearperfectly-plastic region or lowe

31、r yield plateau, to the material behaviour. This was achieved by a one hour soak at 650C and furnace cooling to room temperature. The bore of the specimens was honed to the finished dimension allowing the specimens to be supported on a mandrel for the2001 ABAQUS UK Users Group Conference9SpecimenDi

32、min/max mmDo max/min mmDi mean mmDo mean mmt mean mmamma/tA30.01030.02534.28234.25230.01734.2672.125-B30.01830.03034.26434.26230.02434.2632.1190.330.16C30.03830.07634.27234.26530.05734.2682.1050.700.33D30.01330.03634.27234.26230.02434.2672.1211.080.51E30.03030.04034.27034.24930.03534.2592.1121.550.7

33、3machining of the outside surface. This machining, including the threads, was conducted on a CNC turning centre. A dimensional survey was conducted at this stage and is summarised, for each specimen, in Table 1.The machining of the defects, or cracks, was problematic. Previous experience suggested t

34、hat Electric Discharge Machining (EDM) using graphite electrodes was the best option. However, in this instance, the length of the cylinders, the internal location of the defect, the small defect width and the required dimensional accuracy made this process difficult to implement. In particular, it

35、was found that the erosion of the electrode material meant that several orbits, each time with a new electrode, were necessary. This was done and the finished defects were verified by making impressions of the defects and by inspecting these impressions. The result of this is summarised in figure 9

36、together with the a/t ratios actually achieved.0.16 FLAT0.270.18 FLAT0.290.18 FLAT0.290.17 FLAT0.300.320.330.340.329.Measured Crack ProfilesIn addition to the defect free cylindrical specimen, three standard tensile test specimens were machined from the same bright, mild steel bar stock. The manufac

37、ture of these specimens followed the same procedures as the cylindrical specimens, that is, rough machining, heat treatment and finish machining. These specimens were routinely tested in a uniaxial testing machine using an extensometer to measure the axial strain. The three resulting stress-strain c

38、urves were used to generate an averaged true stress-strain curve, constructed for FE modelling, using the technique described in 7. The result of this is included as figure 10.10Conference2001 ABAQUS UK Users Group0.330.10.700.11.080.11.55Specimen Ref.BCDEa/t0.160.330.510.7360050040030020010000510Tr

39、ue Strain %152010. Averaged True Stress-Strain Response used for FE AnalysisReturning to the cylindrical specimens, the primary objective was to produce load displacement plots in order that the limit load for each of the crack depths could be obtained. However, advantage was taken of the opportunit

40、y to obtain more information relating to the spread of plasticity around the cracks. To this end, a number of strain gauges were bonded to the outside surfaces of these specimens, each orientated in the axial direction.=A44551673On Reverse122Section A-AA30.033.011. Strain Gauge Positions for Uncrack

41、ed Specimen2001 ABAQUS UK Users Group Conference11True Stress N/mm2=33.00Bending GaugesSpecimen D987 6 12 3 4 5 x x3 7 6.61.02698 7 65 4 1 2 3 x x15Specimen C4Crack Centre LineChain Gauge LocationNominal Crack Width = 0.3 mm12. Strain Gauge Positions for Cracked SpecimensThe locations of the strain

42、gauges on both the uncracked specimen and the cracked specimens is shown in figures 11 and 12 respectively. As will be apparent from these illustrations, additional gauges were positioned to determine the degree of bending present in the specimens. For specimens C and D, chain (or strip) gauges were

43、 used (as shown in figure 12) in order to increase the number of measurements in the region of an anticipated high strain (45 from the crack tip (see Anderson 7).The positions of the gauges for each specimen are shown in Table 2.2.Measured Strain Gauge Positions for Cracked Specimens12Conference2001

44、 ABAQUS UK Users GroupDistance of Gauges from Crack CentrelineSpecimena/t1234567B0.160.01.592.16-2.140.01.972.60C0.330.01.882.60Chain Gauge UsedD0.510.01.252.20Chain Gauge UsedE0.730.00.451.38-0.830.00.761.63Testing Machine CrossheadUpper Universal Joint ArrangementClevis-eye ConnectorTest SpecimenL

45、ower Universal Joint ArrangementTesting Machine Base13. Experimental ArrangementFor the testing of these specimens, a 250kN servo hydraulic testing machine was employed. of universal joints was incorporated to minimise the bending induced in the specimens.A set Thisarrangement is shown in figure 13.

46、 Elastic bending checks were carried out on each specimenprior to undertaking the limit load tests and adjustments made to the universal joints (to reduce bending) if necessary.5FULL NON-LINEAR FE ANALYSISA full non-linear FE analysis of the experimental cases was undertaken. The measured geometry o

47、f the specimens and their cracks, the true stress-strain relationship for the material and the non- linear geometry option within ABAQUS were all used. The geometry of each crack was modelled using the measured profiles to provide the width and depth dimensions. A radius was included to connect the

48、flat at the bottom of the crack face. The four FE meshes are shown in figure 14. The mesh around the crack is of a slightly different form. The mesh was biased towards the crack tip2001 ABAQUS UK Users Group Conference13radius but no focused mesh was used as it was thought that this would make littl

49、e difference at a crack tip having a curved profile.14.Experimental FE Mesh Designs6RESULTS AND DISCUSSIONResults from the mesh convergence studies have been reported previously 3. However, it is useful to include here one set of data from that publication. Figure 15 shows the limit load for the cra

50、cked cylinder plotted against the number of elements used through the thickness. The limit load here is obtained using the fifteen times elastic slope criteria that has been used with several other limit load assessments at Liverpool. It is clear from figure 15 that these results confirm the stress

51、analysis reported earlier and that the models using focused elements give results that are closer to the theoretical stress analysis value than the standard mesh designs. Refining the standard mesh towards the crack tip (non-uniform standard mesh) gives limit loads closer to the stress analysis than

52、 the uniform standard mesh. Further details of the variation between these FE results and the stress analysis results may be found in 3.14Conference2001 ABAQUS UK Users Groupa/t=0.2560a/t=0.540a/t=0.7520008162432Number of Elements through Thickness15. FE Limit Load Results2001 ABAQUS UK Users Group

53、Conference15Limit Load kNStandardNon-Uniform Standard FocusedTheoretical (Section 2)For the experimental work reported here, the specimen bending was found to be minimal. Typically, the two bending strain gauge pairs at the centre of the specimen show some initial bending which reduces to less than

54、4% once a significant load had been established.The specimens were subjected to increasing tensile loads whilst recording load, strains and machine cross-head displacement. It was found that the flexibility of the testing machines frame and the universal joints was significant. This was corrected by adjusting the experimental data so that the linear region had the same slope as the corresponding