1

APPLICATION OF MSC.Marc TO THE PREDICTION

OF WELDED RESIDUAL STRESSES

Reference: 2001-60

Crown Copyright 2001/DERA

QinetiQ+

Farnborough, Hampshire, GU14 6TD, UK 1G.P. Campsie, 2A.C. Ramsay and 1J.D. McVee

1QinetiQ Future Systems Technology Division, Centre for Marine Technology,

South Arm, Rosyth Royal Dockyard, Dunfermline, Fife KY11 2XR, Scotland, UK

Phone: +(44) (0) 1383 435230, E-mail: gpcampsie@qinetiq.com & jdmcvee@qinetiq.com 2MSC.Software Ltd, MSC House, Lyon Way, Frimley, Camberley, Surrey GU16 5ER, UK

Phone: +(44) (0) 1908 606070, E-mail: alex.ramsay@mscsoftware.com

Abstract Fatigue crack growth in fusion welded steel structures is driven by tensile residual stress locked in during welding. Current knowledge of fatigue crack growth rate is primarily based on model tests and on fracture mechanics predictions, which use experimental measurement of residual stress. This experimental data base indicates that the fatigue crack growth associated with current fabrication practice is acceptably low; but it does not allow rapid assessment of the consequences of any change to the fabrication route. This paper describes the development of a numerical method, using MSC.Marc 2000, to predict residual stresses in thick welded structures containing multi-pass welds. Coupled thermo-mechanical finite element analyses have been carried out to evaluate the magnitude and distribution of residual stresses induced at a bulkhead to cylinder T -butt full penetration weld. Multi-pass welding has been simulated, with thermal loading applied to the models on a pass by pass basis. An attempt has been made to follow the complex temperature history experienced by the structure during welding. A pragmatic approach has been adopted whereby the phase transformations that occur in the base material on cooling are ignored in order to obtain the general characteristics of the structure after welding simulation. Comparisons with experimental results for longitudinal residual stresses acting through the plating thickness have shown reasonable correlation. This suggests that continued development and application of validated numerical modelling techniques, for prediction of welding residual stresses, will allow the quality of advice offered in relation to fatigue crack growth to improve significantly. 1.0 Introduction Fatigue in fusion welded steel submersible hulls occurs due to the interaction of external applied compressive stresses with the tensile residual stresses set up during welding. + Formerly a part of the UK Defence Evaluation and Research Agency (DERA).

2

Consider a scenario (1) whereby the welding residual stress is of yield stress magnitude in tension, such that σ r = σy, and the nominal applied stress cycle is -σ2 to +σ 1. The total stress range is thus (σ 1 + σ 2) and the total stress cycle varies between σ y and σ y - (σ1 + σ2), implying that the fatigue behaviour of an as-welded joint can be expressed in terms of stress range alone. For a fusion welded steel submersible hull under zero - compression applied loadin g, the total stress cycle varies between σr and σr - σ2. Thus if σ 2 < σ r, the stress remains tensile throughout the cycle, but for σ2 > σr, total stress is compressive for a proportion of the cycle, so that the damaging proportion of the cycle is the stress range σr to 0. The fatigue life is independent of σ2, unless σ2 is sufficiently large to cause yielding in compression, so that stress cycles which are partly or wholly compressive are equally as damaging as cycles of the same stress range which are wholly tensile. Under such circumstances, cracks may propagate under an external pressure loading and a driving force of residual stresses. The most likely initiation site for a fatigue crack is at the junction of the internal circumferential stiffeners with the hull. QinetiQ Rosyth has used model tests to obtain a direct indication of fatigue crack growth rates at the toe of an internal stiffener in externally pressurised cylinders. The models have near full thickness submersible hull plate, but at very much reduced diameter compared to a real submersible hull. Experimental measurements exist to show that the use of a reduced diameter induces high locked in residual stresses (restraint stress) compared to a full diameter submersible. Fatigue crack growth rates in the models are thus expected to be more rapid than in the real structure. The restraint stress at the toe of the weld takes the form of a bending moment. This is currently estimated by an extrapolation of data from strain gauges mounted on the hull during fabrication. The extrapolation is based on elastic shell theory. The detailed distribution of residual stress through the hull thickness is not known, but it is assumed that the residual stress level peaks at yield at the toe of the weld. T his estimate is used to set a through thickness residual stress distribution which has the same net bending moment as that deduced from extrapolation of the elastic strain gauge data. Once the restraint stress through thickness distribution has been established it is used to calculate elastic stress intensity factors, K r, for full circumferential defects of various depths. Similar calculations are made to obtain the (negative) stress intensity from the applied compressive stress distribution. This enables the cyclic stress intensity, ∆K, to be estimated for use in the fracture mechanics formula:

nKCdNda

∆=

where: da/dN is the crack growth rate in mm/cycle; C and N are material constants; ∆K is the cyclic stress intensity in MPa√m. The cyclic stress intensity ∆K is given by: (Kr – Ka) when IK rI > IK aI;

3

Kr when IK aI >IK rI. In other words, only the positive component of ∆K is taken into account in calculating the fatigue crack growth rate. This approach has been used to predict fatigue crack growth rates in both model tests and in full scale submersible hulls. The objective of current work is to improve the analytical tools for making a fatigue assessment and in particular, to develop the capability to make rapid estimates of the restraint stress magnitude and residual stress distribution resulting from any given welding process. The major thrust is thus aimed at improving the estimate of residual stress distribution at the weld toe by detailed numerical modelling. Initial attempts to do this are summarised in section 2. Section 3 describes further improvements to the numerical residual stress modelling technique. Section 4 demonstrates the use of the technique to estimate residual stress distributions for a QinetiQ Rosyth fatigue model. 2.0 Overview of Previous Studies 2.1 Structural Details Previous attempts by QinetiQ Rosyth to improve the estimate of residual stress distribution at the weld toe by numerical modelling focused on a structure with mean radius of 473.5mm and plating thickness of 19mm, fabricated from BS 4360 Grade 50D steel plate. Eight weld passes were used at the internal circumferential stiffener to plate T-butt fillet weld. This structure was of simplified arrangement and reduced plating thickness when compared with QinetiQ Rosyth fatigue models. However, the structure was deemed suitable for investigation as the joint configuration, weld pass sequence and welding parameters were well documented. Further an experimentally determined residual stress distribution at the weld toe, obtained using the Block Removal, Splitting and Layering (BRSL) technique was available for validation of the proposed numerical modelling methodology (2). 2.2 Numerical Modelling Methodology Two approaches to determining the residual stress distribution at the weld toe by numerical modelling were considered (3). To summarise the latter, and more successful, approach, a full cylinder length 2-D axi-symmetric representation of the structure was created from CAD geometry using the MSC.Marc finite element pre -processor MSC.MENTAT (4). Every attempt was made to provide an accurate representation of the joint configuration and weld cross section. After creation of a suitably discretised 2-D axi-symmetric mesh, the individual weld passe s were merged, or ‘lumped’ together, and an idealised fusion profile was explicitly defined, extending both into the cylinder plating and the stiffener. Nodal temperatures of 1550°C and 120°C were prescribed as initial conditions to the idealised fusion profile with ‘lumped’ weld pass and the bulk of the structure respectively. Kinematic constraints were also applied between the idealised fusion zone and the bulk of the structure to permit adequate heat flow across the boundary. A film coefficient was prescribed to all external surfaces and the temperature of the surrounding air was taken to be 30°C to account for connective boundary conditions. A coupled thermo-mechanical analysis of the model described above was then carried out using MSC.Marc (5). This was achieved by generation of an associated heat transfer element with coupled behaviour for every stress element defined in the finite element mesh. A staggered solution procedure allowed a transient heat transfer analysis to be performed

4

prior to the stress analysis, with intimate coupling of load and time step control. In terms of achieving a satisfactory output from the analysis described above, it was shown that the approach could predict a through thickness longitudinal residual stress distribution of similar magnitude and reversed ‘S’ shape to experimental results. Further, the deformed shape of the finite element model correctly displayed a characteristic ‘tourniquet’ effect, or hoop-wise shrinkage, at the welded joint. 2.3 Limitations Analytically, three parameters may be used to define the behaviour of the welded joint in terms of a restraint moment and shear force (6). These are the wrap-up parameter, the tendon force parameter and the radial shrinkage parameter. The proportion of each parameter contributing to the value of the restraint moment and shear force is influenced by the size and shape of a ‘zone of influence’, which is analogous to the idealised fusion profile discussed earlier. In terms of applying the initial numerical modelling methodology to any future finite element model, tendon force, wrap up and radial shrinkage effects at the welded joint may potentially be in error due to an explicitly defined but arbitrary idealised fusion profile. This would then throw considerable doubt on the accuracy of the through thickness residual stress distribution obtained. Further limitations with the initial numerical modelling methodology include the ‘lumping’ together of individual weld passes and the general non-applicability of the appro ach to 3-D finite element representations of the multi-pass welding process. Collectively, these limitations preclude an examination of resulting strains, stresses and deformations as each weld pass progresses. To resolve the issues highlighted above and to allow creation and analysis of 3-D finite element representations of the multi-pass welding process, a number of improvements were identified. These were implemented in years 2 and 3 of the project and are discussed below. 3 Overview of Current Studies 3.1 Material Properties To obtain a realistic prediction of the residual stresses from a finite element idealisation of the welding process requires acquisition and input of accurate physical and mechanical material property data. Where possible, physical and mechanical material property data should be acquired and input for temperatures ranging from ambient up to a nominal solidus. The experimental determination of physical and mechanical material property data for a specific material requires significant technical effort and financial expenditure. However, it must also be accepted that a shortfall in such data will limit the applicability of the model and may reduce the confidence placed in the output from the analysis. The following physical and mechanical material property data was thus obtained. Physical (a) A single curve showing the variation of specific heat capacity with increasing

temperature; (b) A single curve showing the variation of coefficient of thermal expansion with

increasing temperature; (c) A single curve showing the variation of thermal conductivity with increasing

temperature; (d) A single curve showing the variation of density with increasing temperature;

5

(e) The latent heat of fusion. Mechanical (f) A single curve showing the variation of Poisson’s ratio with increasing temperature; (g) A single curve showing the variation of elastic modulus with increasing temperature; (h) A series of stress-strain flow curves obtained for different temperatures and then

repeated for different strain rates. No strategy has been developed to account for the phase transformations that occur in steel during heating and cooling from the solidus temperature. Changes of phase within the material would give rise to changes in the volume and material properties and could potentially have a marked influence on the mechanical response of the model. However, it is the local plastic ‘shrinkage’ strains accumulated during the final stages of cooling that largely determine the residual stresses and distortion within the model. A pragmatic approach has therefore been adopted where the phase transformations are ignored in order to obtain the general characteristics of the structure after welding. 3.2 Thermal Analysis In work to date, the fusion profile has been defined explicitly. To somewhat crudely simulate the welding process, the fusion profile, plus ‘lumped’ weld pass, has been allowed to cool from 1500°C to ambient, with an associated diffusion of heat into a 2-D axi-symmetric representation of the structure. The resultant mechanical behaviour is due to thermal strains induced by using temperature as a loading condition. In 3-D, it would be necessary to account for the pre-heating effect of the welding process on material surfaces located ahead of the welding torch. It is reasonable to assume that the temperatures of material surfaces close to the weld prior to imminent deposition are raised towards the solidus temperature. Material surfaces are thus softened locally prior to a sequence of filler material deposition, fusion and cooling. Given the above considerations, a more sophisticated approach to the thermal simulation of the welding process has been sought. A number of favoured approaches in the open literature make use of empirically derived heat input models, such as the “double ellipsoid” moving heat source model of Goldak. In conjunction with MSC.Software Ltd., a tool based on standard MSC.Marc user subroutines has been developed to more accurately represent the deposition of heat into the structure. Development has focused on the input of power to the weld region by definition of a heat flux based on the current position of a welding torch and an assumed 3-D elliptical distribution of flux around that position, moving at known speed in a pre -determined path. A number of functions are inherent within the tool to implement the time and spatial variation of the heat flux due to a progressing weld pass. These include: (a) control of the heat input, i.e., the proportion of heat directed at weld and parent plate,

and specifically the amount of flux to assign to element integration points; (b) a moving heat flux; (c) control of filler material element activation. User definable inputs to the tool exist to permit the simulation of multi-pass welding.

6

These include: (a) the number of weld passes; (b) definition of weld pass start locations; (c) definition of weld paths in cartesian or cylindrical co-ordinates; (d) variation of power input per weld pass; (e) variation of welding torch travel speed per weld pass; (f) radius of the weld pass; (g) radius of the hot zone per weld pass (simplistically assumed proportional to 6). 3.3 Introduction of Filler Material Methods for introducing filler material into a 3-D finite element representation of the multi-pass welding process have been a topic of study. Three methods have been considered, as summarised below. Method 1 – The elements defining the filler material are present at commencement of the analysis and are simply melted, together with elements within an idealised fusion profile, by the application of an appropriate heat flux. In 3-D however, the constraint induced by cold, stiff, filler material elements located ahead of the welding torch will be significant for the calculation of heat diffusion and the mechanical solution. Method 2 – The elements defining the filler material are introduced as a set of contact bodies but are inactive prior to being reached by the welding ‘torch’. However, difficulties exist in limiting the artificial constraint ca used by attachment of the contact bodies after deformation due to thermal strains in preceding steps. Method 3 – The elements defining the filler material are present at commencement of the analysis but are inactive prior to being reached by the welding ‘torch’. These elements are activated at the correct melt temperature and the heat flux is corrected to allow for the specific heat capacity thus introduced. Inactive elements take up a configuration based on the current location of nodes attached to activated elements and the original configuration of nodes attached only to further inactive elements. Method 3 has been incorporated into the newly developed tool. The automation of filler material element activation through use of the tool permits a reduced modelling and analysis time. 3.4 Numerical Modelling Methodology for Multi-Pass Welding The improvements described above have been implemented to provide a new numerical modelling methodology that is applicable to multi-pass welding. A generic approach to a multi-pass welding simulation is subsequently proposed. A 3-D mesh is first created in MSC.MENTAT, to include the parent plate and weld passes. Elements defining each weld pass must be grouped separately. Where available, weld history sheets or macro-graphs will provide information to allow an accurate specification of the weld profile and weld pass sequence. An MSC.Marc analysis is then commenced with the parent plate cold or in a suitable pre -heated condition. All filler material must be in a de-activated state. For load-case 1, the temperature of the parent plate in a 3 -D elliptical zone ahead of the first weld pass is first raised automatically. The rate of heating is dependent on user defined

7

inputs to the sub-routine based tool. At a suitable time step, initial filler material elements for the first weld pass are activated, as liquid at an appropriate temperature, mechanically attached to the parent plate. With continued time -stepping, additional filler material elements for the first weld pass are activated. All filler material elements for the first weld pass will eventually be activated, dependent upon the user defined inputs of travel speed and weld path length to the sub-routine based tool. Load-case 2 allows the ‘composite’ structure to cool, and shrink, after all filler material elements for the weld pass have been activated. Load-cases 1 and 2 are then sequentially repeated for further weld passes. A typical application for the improved numerical modelling methodology is described in the following section. 4.0 Residual stresses for a QinetiQ Rosyth fatigue model 4.1 Structural Details QinetiQ Rosyth fatigue models are typically simple cylinders with R/t ratios of approximately 18 and a parallel length L > 1.25R, constructed from submersible hull steel plate. Centrally located internal bulkheads with central ‘manholes’ are welded to the cylinders using a full penetration T-butt weld. Prior to the attachment of hemispherical domes at each end for the purposes of static pressure testing and fatigue cycling, a QinetiQ Rosyth fatigue model would have had a general arrangement as shown in Figure 1. Figure 1 therefore provides the initial geometrical details for the creation of a 3 -D solid finite element model to predict the welding residual stress distribution induced at the weld toe.

t

0.5 L

R

0.5 Lt

Figure 1 – QinetiQ Rosyth Fatigue Model

8

4.2 Welding Details For a specific QinetiQ Rosyth fatigue model, the bulkhead to cylinder full penetration T-butt weld was completed using the spray MIG process and a 1.6mm diameter AX90 welding consumable. Relevant welding parameters for input to the 3-D solid finite element model are as follows: Preheat temperature 120°C Interpass temperature 150°C Welding torch travel speed 266mm/min Heat Input 2.2KJ/mm Figure 2 details the welding procedure used. Records of the weld profiles, obtained by making casts at twelve positions around the circumference of the model were also consulted to determine an accurate weld profile for th e 3-D solid finite element model.

LONGITUDINAL SEAM WELDS 1. Inside weld completed. STBD SIDE WELD 8 PASSES PORT SIDE WELD 10 PASSES

2. Root run removed by air arc gouging

3. Outside weld completed. 5 PASSES EACH SIDE

4. Weld flushed by grinding BULKHEAD STIFFENER WELDS

All welding in down hand position 1. FIRST SIDE COMPLETELY welded [14 passes] using Back Step

Technique 2. Root run removed by air arc gouging 3. SECOND SIDE COMPLETELY welded [13 passes] using Back Step

Technique

Figure 2 – Fatigue Model Welding Procedure

9

4.3 Experimental Results Restraint forces and moments induced at the bulkhead to cylinder full penetration T-butt weld were derived experimentally, by a method of least squares, from strains measured on the surface of the cylinder before and after welding. Figure 3 shows the strain measurement positions. A nominal axi-symmetry of the restraint forces and moments was confirmed by making strain measurements at three positions around the circumference of the model.

178

127

76

CROWN

LOOKING AFT

STIFFENER

POSN. 1

GAUGES AT POSITIONS 1,3

GAUGES AT POSITION 2

FORWARD

FORWARD

178

127

76

POSN. 3

AFT

AFT

PLATING GAUGES - RIGHT ANGLED PAIRSINTERNAL AND EXTERNAL BACK TO BACK

POSN. 2

76

178

127

Figure 3 - QinetiQ fatigue model, locations for strain measurement

Strains measured on the fatigue model are therefore as provided in table 1. These strain values will be used to validate the numerical modelling methodology.

Position Distance from Edge of Stiffener [mm]

Internal Long. [µε]

Internal Circ. [µε]

External Long. [µε]

External Circ. [µε]

76 766 -1040 -163 -674 127 192 -762 271 -474

1

178 -139 -518 432 -249 76 808 -728 -153 -1190

127 83 -475 351 -928 2

178 -263 -219 550 -594 76 882 -1352 -221 -605

127 232 -968 268 -396

Forward

3

178 -93 -669 423 -222 76 587 -526 38 -1149

127 -17 -350 423 -879 Aft 2

178 -270 -137 489 -542

Table 1 – QinetiQ fatigue model, strains induced by welding

10

4.4 Structural Idealisation In keeping with previous studies, a 2 -D axi-symmetric cross section of the model geometry was first created on a CAD system as an IGES file for input to the MSC.Marc finite element pre-processor, MSC.Mentat. A representation of the joint configuration and weld cross section, as shown in figure 4, was obtained by reference to the fatigue model welding procedure and weld profile.

Figure 4 - 2-D visualisation of weld passes

After minor repairs to the imported geometry, a 2-D planar mesh was discretised in MSC.Mentat to give a high mesh density local to the bulkhead to cylinder T-butt full penetration weld, where high thermal stress gradients were anticipated. Away from the weld, a coarse mesh density was possible to reduce c omputational costs. To further reduce computational costs, a symmetry condition was imposed at the bulkhead mid-thickness and further boundary conditions were applied to constrain against rigid body motion. The structure to the aft side of the bulkhead, welded using thirteen passes, was therefore idealised. The 2-D planar axi -symmetric mesh was then rotated to give a 3-D solid mesh representing a half-length 4° segment of the structure, as shown in figure 5.

Figure 5 – Finite Element Mesh Figure 6 - 3-D visualisation of weld passes Figure 6 provides a 3-D visualisation of the thirteen weld passes. Rotational symmetry conditions were next applied.

11

Throughout the current studies, stability of the coupled thermo-mechanical analysis, model size and selection of a suitable element type have been concerns. The extent of the 3-D mesh displayed in figure 5 has been influenced accordingly. Large thermal gradients induced by the shock of filler material introduction could potentially cause divergence o f the thermal part of the solution or non-convergence of the mechanical part. Experience has dictated a requirement for three increments or constant time steps to move the welding torch through a single plane of elements to maintain stability of the analysis. Clearly, the number of increments selected to maintain the stability of the analysis has an implication for the model size. Limiting the path length, and therefore the number of elements defining the path length, minimises the total number of increme nts required to complete a weld pass. For the 3-D mesh shown in figures 5 and 6, ten elements along the weld length results in 30 time steps to complete a weld pass. It is still conceivable that the number of increments required to simulate a full multi-pass welding process could approach or exceed 1000, if accounting for the significant additional increments between weld passes required to model the cooling and shrinkage of the structure. A fundamental study paper has provided guidelines for element selection (7). To avoid high distortions in newly activated elements, lower order elements are recommended. This implies a large number of elements, and thus increased model size, for acceptable results. However, fast integration times, coupled with an iterative solver, could lead to a relatively fast solution for a large number of elements. The 3-D mesh of figure 5 therefore contains 9510 8-noded, isoparametric, arbitrary hexahedral lower order MSC.Marc type 7 elements and 11352 nodes. Finally, a nodal temperature of 120°C was prescribed as an initial condition to the parent plate to simulate electrical pre -heating conditions and a film coefficient was prescribed to all external surfaces, with the temperature of the surrounding air taken to be 30°C to account for connective boundary conditions. A coupled thermo-mechanical analysis was then carried out with the newly developed user subroutine based tool plus suitable user defined inputs. This analysis required 545 increments and 63 hours CPU time on a Hewlett Packard V-class V2200 Unix server to solve for 13 weld passes. 4.5 Predicted Results The application of the improved numerical modelling methodology to the physical model has resulted in a finite element model that behaves rationally. Figure 7 demo nstrates that in the initial stages of laying down a weld pass, e.g. weld pass 2, and immediately prior to filler material activation, there is a rapid heating of the parent plate induced by the ‘virtual’ welding torch. This heat diffuses into the parent plate material and stresses are created, as natural thermal expansion is inhibited by cooler, stiffer, surrounding parent material. Although not shown, it would be possible to chart the migration and reduction of these stresses through the parent plate and further obtain a measure of the plastic strains developed.

12

Figure 7 - Weld pass 2 pre -heating effect

Figure 8 – Weld pass 2 isotherms

In figure 8, weld pass 2 is partially completed. Filler material continues to be added at melt temperature, fully connected to the deformed parent plate. At this stage, the filler material has no strength at elevated temperature and will contract under the expansion of the parent material. Diffusion of heat also continues, due now to the combined effe cts of pre-heating ahead of the welding torch and the presence of hot filler material. Stress fields developed by the pre -heating are now being overtaken by thermal stresses due to differential cooling effects. During cooling load-cases, the natural contraction of the filler material is once again inhibited by the restraining effect of the cooler stiffer surrounding parent plate material. The residual plastic strains so developed give rise to external distortion and a system of self-equilibrating locked-in residual stresses. Figure 9 shows the deformed shape of the structure after all weld passes have been completed. The characteristic tourniquet effect, or hoop wise shrinkage at the welded joint, due to tendon force, wrap up and radial shrinkage parameters is clearly apparent.

Figure 9– Deformed shape

Figures 10 and 11 provide contour plots of the predicted elastic circumferential and longitudinal strains.

13

Figure 10 – Elastic strains 22 (circumferential)

Figure 11 – Elastic strains 33 (longitudinal)

Figures 12 and 13 show that the predicted elastic circumferential and longitudinal strains, extracted from the cylinder internal and external surfaces, are in reasonable agreement with corresponding experimentally determined elastic circumferential and longitudinal strains, as listed in table 1.

-1.50E-03

-1.00E-03

-5.00E-04

0.00E+00

5.00E-04

1.00E-03

1.50E-03

0 100 200 300 400 500

Distance from centre of bulkhead [mm]

Mic

rost

rain

Predicted External

Predicted Internal

Exp. Ext. (fwd)

Exp. Ext. (aft)

Exp. Int. (fwd)

Exp. Int. (aft)

Figure 12 – Elastic strains 22 (circumferential) induced on cylinder surfaces

-1.50E-03

-1.00E-03

-5.00E-04

0.00E+00

5.00E-04

1.00E-03

1.50E-03

0 100 200 300 400 500

Distance from centre of bulkhead [mm]

Mic

rost

rain

Predicted External

Predicted Internal

Exp. Ext. (fwd)

Exp. Ext. (aft)

Exp. Int. (fwd)

Exp. Int. (aft)

Figure 13 – Elastic strains 33 (longitudinal) induced on cylinder surfaces

14

Further confidence in the improved numerical modelling methodology may be gained by considering the circumferential residual stresses at the welded joint. In a cylindrical structure, circumferential residual stresses at the welded joint are analogous to longitudinal residual stresses at a plain butt joint. Intuitively therefore, the filler material and the fusion zone might be expected to have tensile yield magnitude residual stresses in the circumferential direction, with balancing compression in the parent material. Figure 14 is a contour plot that confirms this behaviour.

Figure 14 – Stress 22 (circumferential) at welded joint

Figure 15 – Stress 22 (longitudinal) at welded joint

Figure 15 is a contour plot of the longitudinal residual stresses that occur in the structure close to the welded joint on completion of welding. A tensile yielded zone is clearly evident at the toe of the weld, with a compressive zone on the outer surface of the structure. Finally, figure 16 is the extracted through thickness longitudinal residual stress distribution at the toe of the weld, as required for fatigue crack growth predictions.

-800

-600

-400

-200

0

200

400

600

800

Through Thickness, t

Com

p. 3

3 of

Stre

ss [M

Pa]

I.D. O.D.

Figure 16 – Through thickness stress 33 (longitudinal) distribution

15

5.0 Conclusions and recommendations A numerical method for the prediction of residual stresses in thick section welds has been developed and applied to the analysis of a multi-pass weld in a QinetiQ Rosyth fatigue model. The methodology developed could be used to make a rapid assessment of the consequences of any proposed changes in submersible hull welding practice on fatigue crack propagation rate. This will allow identification of submersible construction procedures that minimise both procurement and through-life costs. The methodology will also be applied to the prediction of residual stresses induced at plain butt welds and stiffener to plate butt welds during construction of surface ships. 6.0 References (1) Gurney T. R., Fatigue of Welded Structures, 2nd ed., Cambridge University Press,

Cambridge, 1979. (2) Gray-Stephens, D. “Residual Stresses in Ring Stiffened Cylinders,” Ph.D thesis,

Cambridge University Engineering Department, 1987. (3) Campsie G. P., Ramsay A., Rahim M. A., & McVee, J. D. “F.E. Predictions of

Residual Stresses in Fusion Welded Steel Pressure Vessels,” NAFEMS World Congress ’99 on Effective Engineering Analysis, Newport, Rhode Island, 1999.

(4) MSC.Marc Mentat User Manuals , Version 2000, The MacNeal Schwendler Corporation, Los Angeles, CA, 2000.

(5) MSC.Marc User Manuals, Version 2000, The MacNeal Schwendler Corporation, Los Angeles, CA, 2000.

(6) Porter-Goff D., “Welding Effects in the Fabrication of Ring Stiffened Cylinders,” Cambridge University Engineering Department, Final Report to AMTE Dunfermline – NCRE/02/1057, August 1982.

(7) Ramsay A., “A Study of Finite Element Meshing Methods to be used in Welding Simulation of Ship Structures,” IMechE Seminar S708, Recent Advances in Welding Simulation, London, 1999.