The influence of modelling variables in FEM evaluation of fillet welded structures

The influence of modelling variables in FEM evaluation of fillet welded structures

Modelleringvariablers inverkan p˚ a FEM-utv¨ ardering av k¨ alsvetsade konstruktioner

Marko Cordasic

Faculty of Health, Science and Technology

Degree Project for Master of Science in Engineering, Mechanical Engineering Points: 30

Supervisor: Mohamed Sadek

Examiner: Jens Bergstr¨ om

Date: 2020-07-01

Abstract

Valmet is a world leading company in the pulp-, paper- and energy industry and is a manufacturer of e.g. paper machines. These paper machines are largely composed of steel frames for which beams and plates are often joined by welding. In order to evaluate the structural integrity of welded components both static and cyclic evaluations of these components are performed. At Valmet the stress in the weld can be determined in different ways, usually an Excel program is used which determines the stresses in the weld by analytical means. For a more complicated geometry a FEA approach is more suitable. The FEA modelling can be done in several ways, the geometry of the structure can be divided into several or one body. Dividing the geometry into separate bodies simplifies the meshing procedure, but the separate bodies have to be joined using contacts. Different boundary conditions can also be considered during modelling e.g. placing a fixed support at the plate face or at the face of the screw holes in the plate.

For structures affected by static loads the stress is determined in the smallest nominal area of the weld i.e. the weld throat. For fillet welds, crack propagation mainly occurs at the weld toe or the weld root. The geometry of the weld imposes problems for determining the stress due to the stress concentration present, but methods have been developed to solve this problem. The hot spot method and the effective notch method are two of these methods.

By the use of fatigue classes and calculated stresses the fatigue life of the component can be determined. Two different models have been developed in order to perform static and fatigue analysis for which stress and fatigue life has been determined for different modelling variables and evaluation methods.

The results from the static FEA show lower stresses compared to the analytical values.

Different types of supports did not show a significant influence, but a slight increase in the stress near fixed screw holes was observed. Modelling using separate bodies did not show a large effect on the results except when using the MPC contact formulation for which stresses were slightly larger compared to the reference model.

Evaluating using the effective notch method yielded longer fatigue life compared to the hot spot method. When the weld was not explicitly modelled significantly longer fatigue lives were observed, this is not recommended since this most likely overestimates the fatigue life.

Similarly in this case the MPC formulation generally showed a some what larger stress and

therefor the shortest fatigue life. It was however observed that in this test the compression

only support did yield a significantly larger fatigue life.

Sammanfattning

Valmet ¨ ar ett v¨ arldsledande f¨ oretag inom massa-, pappers- och energiindustrin och tillverkar bl.a. pappersmaskiner. Konstruktionen av dessa pappersmaskiner best˚ ar till stor del av en st˚ alkonstruktion d¨ ar pl˚ atar och balkar ofta fogas med hj¨ alp av svetsning. F¨ or att f¨ ors¨ akra sig om att svetsade konstruktioner h˚ aller s˚ a utf¨ ors utv¨ ardering av sp¨ anningar i svetsen, b˚ ade f¨ or statiska och cykliska laster. Sp¨ anningen i svetsen ber¨ aknas p˚ a Valmet p˚ a olika s¨ att, ofta anv¨ ands ett Excel-program som ber¨ aknar sp¨ anningar utifr˚ an analytiska metoder. Men f¨ or en mer komplicerad geometri s˚ a kan det vara mer l¨ ampligt att utf¨ ora en FEM-analys. Modelleringen f¨ or FEM-analysen kan utf¨ oras p˚ a olika s¨ att, t.ex. s˚ a kan konstruktionen best˚ a av en kropp med en kontinuerlig mesh eller s˚ a kan geometrin delas upp i separata kroppar d¨ ar varje kropp meshas var f¨ or sig. N¨ ar geometrin delas upp i flera kroppar s˚ a underl¨ attas meshingen, men kropparna m˚ aste s¨ attas ihop med kontakter. Vid modelleringen kan ¨ aven olika val av randvillkor g¨ oras, t.ex. kan man v¨ alja fast insp¨ anning i pl˚ atytan eller i h˚ al d¨ ar skruvar ska sitta.

F¨ or statiskt belastade konstruktioner ber¨ aknas sp¨ anningen i svetesens minsta nominella tv¨ arsnittsarea, ¨ aven kallat a-m˚ att. Spricktillv¨ axt i k¨ alsvetsar sker huvudsakligen p˚ a tv˚ a st¨ allen i svetsen, antigen svetsroten eller svetst˚ an. D˚ a geometrin av svets˚ an ger upphov till sp¨ anningskoncentrationer s˚ a m˚ aste s¨ arskilda metoder till¨ ampas f¨ or att utv¨ ardera svetsen.

Tv˚ a av dessa metoder ¨ ar hot spot metoden och effective notch metoden. Utifr˚ an ber¨ aknade sp¨ anningar s˚ a kan man med hj¨ alp av f¨ orbandsklasser uppskatta konstruktionens livsl¨ angd.

Tv˚ a olika modeller har tagits fram f¨ or att g¨ ora statisk och cyklisk utv¨ ardering d¨ ar sp¨ anning och livsl¨ angd har ber¨ aknats f¨ or olika modelleringsvariabler och utv¨ arderingsmetoder.

Resultaten fr˚ an den statiska FEM-analysen visade n˚ agot l¨ agre sp¨ anningar j¨ amf¨ ort med analytiska v¨ arden. Olika typer av insp¨ anningar visade sig inte ha n˚ agon st¨ orre p˚ averkan f¨ orutom att en n˚ agorlunda ¨ okning av sp¨ anningen observerats i svetsen i n¨ arheten av insp¨ anda skruvh˚ al. Att modellera geometrin med flera kroppar verkade inte heller ha en stor effekt p˚ a resultatet f¨ orutom med MPC formuleringen som visade n˚ agot h¨ ogre sp¨ anningar j¨ amf¨ ort med referensmodellen.

Utv¨ ardering med effective notch metoden resulterade i l¨ angre livsl¨ angder j¨ amf¨ ort med

hot spot metoden. Att bortse fr˚ an svetsen vid FEM analysen resulterade i avsev¨ art l¨ angre

livsl¨ angder av konstruktionen och rekommenderas inte d˚ a det antagligen signifikant ¨ overskattar

livsl¨ angden. ¨ Aven f¨ or utmattningsanalysen s˚ a verkar det inte resultera i n˚ agon st¨ orre skillnad

att anv¨ anda en modell med flera kroppar. ¨ Aven i detta fall visar MPC formuleringen p˚ a

st¨ orst sp¨ anning och d¨ armed kortast livsl¨ angd. I detta test visade det sig dock att modellering

av ett ”compression only support” gav en avsev¨ art l¨ angre livsl¨ angd.

Contents

1 Introduction 2

1.1 Problem formulation . . . . 4

1.2 Aim and goal . . . . 5

2 Literature study 6 2.1 Modelling of contacts in ANSYS Mechanical . . . . 6

2.2 Evaluation of stresses (static) . . . . 9

2.3 Fatigue . . . . 11

2.3.1 Thickness factor . . . . 14

2.4 Evaluation of stresses (fatigue) . . . . 15

2.4.1 Nominal method . . . . 16

2.4.2 Hot spot method . . . . 17

2.4.3 Effective notch method . . . . 19

2.4.4 Fracture mechanics . . . . 20

2.5 Weld design, standards . . . . 20

2.5.1 Eurocode . . . . 20

2.5.2 BSK . . . . 25

3 Methods 28 3.1 Static analysis . . . . 28

3.1.1 Limit-load analysis . . . . 33

3.2 Fatigue analysis . . . . 34

3.2.1 Hot spot method . . . . 36

3.2.2 Effective notch method . . . . 38

4 Results 40 4.1 Static results . . . . 40

4.1.1 Square cross section . . . . 40

4.1.2 Rectangular cross section . . . . 46

4.1.3 Limit-load results . . . . 52

4.2 Fatigue results . . . . 53

5 Discussion 60

6 Conclusions 62

1 Introduction

Valmet is a world-leading manufacturer and distributor of technology, service and automation within the paper-, pulp-, and energy industry. The company consists of about 1500 employees with several production units in Sweden, where the largest ones are located in Gothenburg, Sundsvall and Karlstad. Valmet produces paper and board machines which have been estimated to be responsible for 40% of the total paper and board production in the world. The frame structure of the paper machine to which the components are mounted contains load bearing beams and plates which are often joined by welding. During welding the materials involved are heated to melting temperature, which is then followed by solidification, this can be done with or without the addition of a separate material [1]. Two of the most common weld types are fillet welds and butt welds, these are illustrated in figures 1 and 2.

Figure 1: Terminology and illustration of a fillet weld.

Figure 2: Terminology and illustration of a butt weld

The welding process often leads to some characteristic features which could cause a reduction in e.g. fatigue strength. Some features which are often present are sharp changes in the section of the weld, local discontinuities, large tensile residual stresses, acting as sites for crack initiation. A consequence of this is that it is very difficult to model the geometry of the weld in detail. The weld also often contains a mixture of the filler material and the base material, leading to uncertainty in the material properties.

In order to evaluate the structural integrity of components joined by welding, evaluation of the stresses and strains is performed. These stresses and strains can occur due to both static and cyclic load. A static evaluation can be performed by either calculating the stress in the weld or by determining the maximum load that the structure can carry. For complicated geometries a FEA(finite element analysis) approach using Ansys can be utilized. In the analysis, contact settings determine how the contacting bodies can move relative to each other. Today Valmet uses several methods for evaluating welded joints, the weld can e.g. be evaluated analytically by considering the forces and moments acting on the weld. For complicated geometry and where local deformation needs to be taken into account a FEA approach is more suitable. The welded structure can be modelled as a single body or as separate bodies joined by contacts.

There are different contact types for which different contact formulations can be chosen.

Some of the contact types available in Ansys are frictionless, no separation and bonded. In

order to solve the contact problem there are different contact formulations available such as

Augmented Lagrange and Pure Penalty.

1.1 Problem formulation

There are standards for the design of steel structures and particularly the design of joints.

A literature study will be performed to investigate and describe standards which are used today. Welded components can experience different types of loads such as tensile forces, bending forces, bending moments and torsional moments, see figure 3.

Figure 3: Component in a) Tensile force, b) bending force, c) bending moment and d) torsional moment

In order to determine the stresses in welds, which are affected by both cyclic and static loads, there are different techniques of modelling the weld which may affect the accuracy of the results. The model can consist of a single body, i.e. the whole geometry is meshed together and requires no modelling of contacts. This method of modelling is often impractical and time consuming in practice particularly for large structures and/or complicated geometry. By modelling the geometry as separate bodies acquiring an adequate mesh can be simplified since each body can be meshed individually, the mesh of adjacent bodies does not have to match.

When performing FEA with bodies connected by contacts, different contact formulations can be utilized, the stresses calculated may vary depending on the particular formulation chosen.

Bodies can be fixed in several ways e.g. by fixing the face of a plate or by fixing the screw

holes of the plate.

1.2 Aim and goal

In summary the thesis aims to answer the following questions:

• How can stresses in welded structures be determined?

• How is weld design performed according to common standards?

• How is the weld stress/fatigue life affected depending on the way the welded structure has been modeled?

• How is the weld stress/fatigue life affected depending on the boundary condition?

• How is the weld stress/fatigue life affected depending on the contact formulation?

• How is the estimated failure load of the welded structure affected depending on the method used?

The goal of this thesis work is to provide Valmet with a higher certainty regarding which

methods to use and how the methods used may affect the final result.

2 Literature study

2.1 Modelling of contacts in ANSYS Mechanical

Depending on the application there are a few different contact type available in Ansys. In situations e.g. where surfaces are expected to separate, nonlinear contact types should be used since these contact types perform better in terms of modelling gaps and the real contact area [2]. The linear and nonlinear contact types available are:

• Bonded

• No Separation

• Frictionless

• Rough

• Frictional

• Forced Frictional Sliding Bonded

The Bonded Contact type is used for all types of contact regions (surfaces, solids, faces, edges) by default. This contact type ”glues” the contact regions i.e. no separation or sliding between faces or edges is allowed. Since no separation is allowed the contact area does not change and the contact type can utilize linear solutions [2].

No Separation

As the name suggests this contact type does not allow separation between surfaces similarly to the bonded type. No Separation applies to face regions in the case of 3D solids and edges for 2D plates [2].

Frictionless

Frictionless contact allows for free sliding and gaps between bodies, the constant of friction is zero. This contact type models contact in one direction, if separation occurs normal pressure is set to zero. It is important that the constraints for the model are well defined when using frictionless contact [2].

Rough

This contact type is similar to that of the frictionless type, but instead of a zero coefficient of friction it is set to an infinite value, meaning that the contact allows for no sliding [2].

20

Frictional

The Frictional contact allows for sliding but only when the shear stress carried by the bodies reaches a certain value which is defined as a fraction of the contact pressure. The state before sliding occurs is called ”sticking” [2].

Forced Frictional Sliding

This type is similar to the frictional type except that in this case there is no sticking phase.

At every contact point a resisting tangent force is applied [2].

When bodies come into contact they can transfer compressive normal forces and frictional tangential forces, but usually not tensile normal forces. Nonlinearity occurs when bodies are allowed to come into contact and separate, the system stiffness depends on the status of the contact. Bodies which come into contact do not penetrate, the prevention of penetration of two encountering bodies is called ”contact compatibility”. The enforcement of contact compatibility can be done in several ways depending on the specific algorithm. The type of algorithm used in the solution will depend on the formulation chosen by the user. Depending on the contact type only some of the formulations are useful [2]. The contact formulations available in Ansys are:

• Pure Penalty

• Augmented Lagrange

• Normal Lagrange

• MPC

• Beam

Pure Penalty and Augmented Lagrange Formulation

Pure Penalty and Augmented Lagrange are both appropriate to use for nonlinear solid body contact of faces. Both of these formulations are based on penalty methods according to eq.(1):

F

= k

x

(1)

F

is the contact force, and k

is the contact stiffness which limits the penetration distance

x

, see figure 4.

Figure 4: Schematic of two bodies with a penetration distance x

For an infinite contact stiffness no penetration would occur, but this is not possible numerically using penalty methods. For a small or negligible x

, the results will be accurate.

For the augmented lagrange formulation an extra term λ is added which augments the contact force according to eq.(2):

F

= k

x

+ λ (2)

The extra term causes a decrease in the sensitivity of the contact stiffness. Both the formulations are useful for any type of contact behavior [2].

Normal Lagrange formulation

The Normal Lagrange formulation introduces an extra DOF (degree of freedom), contact pressure, in order to enforce contact compatibility. This is done instead of resolving the contact force into stiffness and penetration and the contact force/pressure is solved for as an extra DOF. This method may increase computation requirements. Sometimes contact points may oscillate between states of penetration and gap causing difficulties in convergence, this is called Normal Lagrange Chattering. By allowing some degree of penetration the convergence problem can be prevented. Normal Lagrange is useful for any type of contact behavior [2].

Multi-point Constraint

In the MPC (Multi-point constraint) formulation constraint equations are added to tie displacements between contacting surfaces. In contrast to pure penalty and augmented Lagrange the MPC formulation is not penalty based. The bonded contact regions are related directly in an efficient manner. MPC is useful for Bonded and No Separation contact [2].

Beam Contact formulation

In the beam contact formulation the contacting topologies are ”stitched” together with

massless linear beam elements. Beam contact can only be used for Bonded contact [2].

2.2 Evaluation of stresses (static)

When analyzing the stresses in a weld which can be described with simple geometry and which isn’t affected by a large number of cycles, an Excel program based on analytical solutions, is often utilized at Valmet. This is useful since the modelling of the weld is highly simplified which saves time. The weld joint connects a plate and a beam according to figure 5.

Figure 5: Weld joint and applied loads.

The program uses the reaction forces due to the loads F

, F

, F

, M

, M

, M

and the

geometry of the weld as input data. The calculated weld stress is the average stress over the

weld throat area in contrast to fatigue evaluation methods where the weld toe is assumed to

be the critical part of the weld. The stress components are σ

, τ

and τ

according to figure

6

Figure 6: Weld stress components

The weld is assumed to be linear elastic while the plate and beam are considered to be rigid meaning that no deformation of the plate or beam occurs. For an analysis where local deformations need to be taken into consideration a FE-analysis is recommended. The weld joint is divided into a number of weld elements. These weld elements are then in turn divided into N number of point areas see figure 7.

Figure 7: Weld elements and point areas.

The program calculates local forces and moments at each point area by force and moment equilibrium. Using normal and shear stresses, von Mises effective stress is calculated in each point using eq.(3):

σ

= q

σ

+ 3τ

+ 3τ

(3)

2.3 Fatigue

Components which undergo cyclic loading can weaken or eventually lead to failure of the material even if the stresses present aren’t particularly high, i.e. significantly lower than the yield stress of the material, this phenomena is commonly known as fatigue. Components which rotate at high frequencies are often exposed to fatigue to a large extent. All loads which cause fatigue i.e. all loads which are fluctuating are called fatigue actions [3]. Fluctuating loads that may potentially affect a structure includes:

• Changes in the magnitude of loads

• Changes in the location of the load

• Changes in the direction the load is applied

• Structural vibrations caused by loads and dynamic response

• Temperature transients

In order to correctly analyze the risk for fatigue, a superposition of the stresses caused by the various loads needs to be taken into consideration. When assessing fatigue it is crucial that a safe estimation of the component fatigue life is considered. Therefor it is always the upper bound estimate of the total fatigue actions which is of interest, it may also be of interest to apply partial safety factors based on characteristic load data which is specified in codes regarding structural design. Fatigue actions may originate from e.g. wind, waves, pressure and transient temperature changes [3]. The fatigue process can be divided into three main phases:

1) Crack initiation: The time before a microscopic crack is formed.

2) Crack growth: The time in which the crack grows with every load cycle.

3) Fracture: In this state the material can no longer withstand the loads due to the large crack.

A material which has been welded will always contain flaws due to the formation of micro-cracks in the welding process, this means that the material immediately undergoes the crack growth phase. The fatigue life of the material will mostly depend on the stress range σ

which is the difference between the maximum and the minimum stress according to eq.(4):

σ

= σ

− σ

(4)

The stress state at the crack tip is described by the stress intensity factor K according to (5):

K = σY √

πa (5)

Where Y is a term which describes the geometry and a is the crack length. The stress intensity factor range ∆K is expressed in eq.(6):

∆K = K

− K

(6)

For the case of welds, the actual fatigue strength of the material will have a low impact on the fatigue life since the fatigue strength of different materials mostly depends on the time required for crack initiation and as previously mentioned cracks will always be present for welded materials [4]. The crack growth rate depends on the cyclic stress and the elasto-plastic response of the material on the crack tip area, environmental factors and some fracture criterion. The cyclic strain-hardening behavior of the material will have an effect on the plastic deformation around the tip of a fatigue crack [5].

In the context of fatigue analysis there are generally three types of stresses mentioned depending on the method of evaluation: nominal stress, geometric stress and notch stress.

The nominal stresses are defined as the global stresses in the cross section, disregarding stress concentrations. Although e.g. macroscopic changes in geometry or point forces can cause increasing local stresses which need to be taken into consideration. In simple bending cases nominal stress can be calculated using simple linear elastic beam theory according to eq.(7):

σ

= F A + M

I z (7)

where

F = Normal force

A = Cross-sectional area M = Bending moment I = Area moment of inertia z = Distance from neutral layer

Figure 8: Nominal stress in a beam.

All stress increasing effects, except the nonlinear stress peak σ

caused by the geometry of the weld (such as the radius of the weld toe), are included in the geometric stress. The geometric stress is often larger than the nominal stress since it includes stress increasing effects, but they are equal at a large distance away from local changes in the structure. The geometric stress is linearly distributed over the plate thickness and can be divided into two components: membrane stress σ

and bending stress σ

[4].

Figure 9: The geometric stress and its components.

The membrane stress is defined as the average stress over the thickness of the plate and the bending stress is the difference between the stress at the top and bottom of the plate divided by two. Generally the geometric stresses cannot be determined analytically, they are determined by either FEA or by experimental measurements. For some structures a geometric stress concentration factor K

can be used to determine the geometric stress, but it is often difficult to find a stress concentration factor which is suitable for the specific problem.

The notch stress σ

is defined as the total stress, in e.g. the weld toe or root, assuming a linear elastic material. The toe of a weld can cause a nonlinear stress distribution across the plate thickness, this stress can be divided into three components as seen in figure 10 [4].

Figure 10: The notch stress and its components

The stress components for a given stress distribution σ(x) through the thickness t of a component can be expressed analytically according to eqs.(8-10):

σ

= 1 t

Z

σ(x)dx (8)

σ

= 6 t

Z

(σ(x) − σ

)( t

2 − x)dx (9)

σ

= σ(x) − σ

− (1 − 2x

t )σ

(10)

By using data from a large number of fatigue tests for different stress ranges, so called S-N curves, or W¨ ohler-curves, can be formed. In order to obtain reliable results, at least five specimens should be tested at each stress range [6]. The results from the tests are usually plotted in a log/log-diagram. The value of the slope of the S-N curves is usually the same for all types of welded joints and is usually 1/3 in a log/log-diagram.

Over time a large number of data has been collected on fatigue tested details. A way to collect and systemize the material is by the use of ”reference libraries”. According to most norms and guidelines, the welded joints are categorized through detail categories (C). The fatigue resistance of structural details can be classified by the characteristic fatigue strength at 2*10

cycles, this is the fatigue class FAT (FATigue). For a constant stress range σ

the number of cycles can be determined from the equation of the S-N curve according to eq.(11):

N = N

 C σ



(11) C and N

are constants according to the corresponding fatigue strength in a point on the curve. When using the FAT class, N

is 2 ∗ 10

and C is the FAT-value.

2.3.1 Thickness factor

Since a larger volume of material is more likely to contain some type of defect the fatigue strength decreases with an increase in plate thickness [4]. This means that a thicker plate has a larger probability of failure and a reduced fatigue limit for a given lifetime. In order to take account for these effects, a thickness factor φ

is multiplied to the fatigue strength. The thickness factor is given by eq.(12):

φ

=  t

t



(12)

The reference thickness t

and exponent n can vary depending on the handbook used, in

Konstruktionshandboken [6] t

=15 and values for n are given in table 1.

Table 1: Table for determining the thickness factor φ

(t

= 15mm) for fillet welds [6].

t < 4mm φ

= 1.22 4 < t ≤ 15 mm n ≈ 0.15 t > 15mm n ≈ 0.25

However, according to the IIW:s (International Institute of Welding) recommendations [3] the thickness factor is only used to reduce the fatigue strength when the plate thickness is larger than the reference thickness (t

= 25mm).

2.4 Evaluation of stresses (fatigue)

Determining stresses in welds accurately is difficult. The welding operations is usually carried out manually and the actual geometry of the weld rarely matches that of the specified drawing or FEM model. FEM models of welds often contain sharp corners which result in singularities meaning that the stress at the sharp corner does not converge to a particular value, in fact the stress increases with a refinement of the mesh. For this reason, evaluation of stresses for a welded construction affected by cyclic loads can be performed in several ways.

The choice of method depends on the required accuracy of the results and the complexity of

the problem see figure 11.

Figure 11: If accurate results are to be obtained for complex problems, usually a larger amount of work effort is required.

Various literature describes four main methods for fatigue assessment of welded structures:

nominal method, hot spot method, effective notch method and fracture mechanics [3, 4].

The assessment methods can be categorized into local and global approaches, where the global approaches are based of the acting forces and moments or alternatively of the nominal stresses assuming a constant or linear stress distribution [7]. If the assessment is however based of local stress and strain parameters they fall into the local approach category.

2.4.1 Nominal method

The nominal stress is defined as the global stress in the cross section. In this method nominal stresses are compared to reference fatigue strengths according to fatigue classes.

These classes are based on a large number of tests on e.g. fatigue specimen with different

types of weld joint. These classes consider different types of stress increasing effects due to

small structural changes, but not structural changes on the macro scale since these should be

included in the calculation of the nominal stress. The fatigue strength is given in the form

of a nominal stress range [4]. Fatigue resistance values for structural details with different

geometries and loading conditions are described in ”Recommendations for fatigue design of

welded joints and components” by A. Hobbacher with over 80 different types of details, an

example is shown in figure 12 [3].

Figure 12: Example of a structural detail and the fatigue resistance value [3].

For simple welded component basic linear elastic theories can be applied to calculate the nominal stresses. The nominal stress is the average stress in either the weld throat or in the plate near the weld toe. The nominal stress in the weld can be expressed according to eq.(13):

σ

= F

A

= F

al

(13)

Where F is the force in the weld, A

is the area of the throat section, a is the weld throat thickness and l

is the length of the weld. For more complex situations such as statically over-determined structures, or with geometries which consist of macro-geometric discontinuities, a FEA approach is required.

2.4.2 Hot spot method

The critical point in which a crack is expected to grow is called the hot spot, this is

usually around e.g. the toe of the weld (see figure 1). There are typically two types of hot

spot, type a and type b. Type a hot spots are located at the weld toe on the plate surface

while type b hot spots lie on the edge of the plate see figure 13.

Figure 13: Hot spot types.

The hot spot stress corresponds to the geometrical stress in the hot spot and the results of this method is based on these types of stresses. Stress concentrations considered in the hot spot approach are macro-geometrical effects, but also structural discontinuities due to the welded joint itself [3]. It is recommended that the hot spot stress is calculated by initially determining the stress in at least two points at a certain distance away from the weld see figure 14.

Figure 14: Extrapolation from two reference points.

The calculated stress should be a principal stress which acts approximately perpendicular

to the weld toe. The stress at the hot spot is then determined by extrapolation. The choice

of location of the points is done in such a way that the effect of the nonlinear stress peak can be considered negligible. According to A. Hobbacher [3]a distance of 0.4t away from the weld toe where t is the plate thickness avoids the effect of the nonlinear stress peak. Hobbacher also recommends that the two reference points for the nodal stresses are chosen at 0.4t and 1.0t respectively, the hot spot extrapolation is then given by eq.(14):

σ

= 1.67σ

− 0.67σ

(14)

For stresses which are strongly nonlinear towards the hot spot a quadratic extrapolation is recommended according to eq.(15):

σ

= 2.52σ

− 2.24σ

+ 0.72σ

(15) The equations above apply to type a hot spots using a fine mesh with element lengths not larger than 0.4t.

Just as in the method of nominal stress, the reference fatigue strength is evaluated by comparison of fatigue classes. For assessment of fatigue resistance based on hot spot stresses there are examples of 9 structural details in [3]. In order to perform an assessment based on the FAT classes the detail which most resembles the actual welded structure is used. The fatigue strength according to classifications is given as a geometric stress range [4].

2.4.3 Effective notch method

The effective notch method is based on the notch stresses located at local radii [4]. Instead of considering the real geometry of the weld toe it is replaced by an effective radius of 1mm see figure 15.

Figure 15: The toe and the root of a fillet weld replaced by 1mm radius.

This is done in order to consider the variation in the geometry of real life welds, but also the potential non linear behavior of the material caused by large stresses around the notch.

The introduction of a radius at the weld toe solves the problem of the stress concentration at the toe, meaning that the stress can be measured at the weld toe itself. This has been shown to give consistent results, at least for structural steels and aluminium alloys [3]. The effective notch method requires a very fine mesh around the notches in order to get accurate results.

For hexahedral mesh elements a mesh size no more than r/4 for quadratic elements and r/6 for linear elements should be used, this results in element sizes of maximum 0.25mm and 0.15mm respectively for r=1mm [8].

The effective notch stress is compared to a single fatigue resistance diagram for welded joints. The method is restricted to fatigue failure originating from either the toe or root of the weld. The method is appropriate for structures with a thickness of 5mm or thicker.

2.4.4 Fracture mechanics

The behaviour of cracks can be determined using theoretical models from fracture mechanics by considering the region around an initiated crack tip. The crack growth is controlled by the change of the stress intensity ∆K. The number of load cycles from crack initiation to failure can be determined using Paris law [4].

2.5 Weld design, standards

2.5.1 Eurocode

The way structural design should be conducted in the European Union is described by the eurocodes,”Eurocode 3: Design of steel structures” contains design guidelines for joints in steel structures. A joint is defined in the standard as the interconnected zone between two or more members. A partial safety factor γ is given in order to ensure that the member provides an adequate resistance to compression, tension, bending and shearing. The partial safety factor for resistance of welds is set to γ

= 1.0 − 1.2 depending on the severity of the consequences of potential failure. The guidelines given apply to weldable structural steels with minimum thickness of 4mm with a weld material which has similar mechanical properties to the parent material [9].

Design considerations for fillet welds and fillet weld all around are performed using one of two methods: the Directional method or the Simplified method [9].

Directional method

• The force transmitted by a unit length weld consists of a parallel and a transverse

component

• The design throat area is defined as A

= Σal

, where l

should be taken as the effective length where the weld is full size and a is the throat thickness.

• A

is assumed to be concentrated at the location of the root.

• The stress on the throat section is assumed to be uniformly distributed with normal and shear stresses according to figure 16.

Figure 16: Stresses acting on the throat section σ

= Normal stress perpendicular to the throat σ

= Normal stress parallel to the axis of the weld.

τ

= Shear stress perpendicular to the axis of the weld.

τ

= Shear stress parallel to the axis of the weld

• σ

is not considered when verifying the weld resistance.

• It can be concluded that the resistance of the weld is sufficient if the two conditions, according to eqs.(16-17), are both fulfilled:

[σ

+ 3(τ

+ τ

)]

≤ f

/(β

γ

) (16)

σ

≤ f

/γ

(17)

f

= ultimate tensile strength of the weaker material in the joint.

β

= correlation factor depending on the steel grade of the weaker material.

Simplified method

• The design resistance of the weld is adequate if the force transmitted per unit length at every point of the weld follows the condition according to eq.(18):

F

≤ F

(18)

where

F

= the design value of the weld per unit length F

= the design weld resistance per unit length.

F

= f

a

f

is the design shear strength of the weld

• The design shear strength is given by eq.(19):

f

= f

/ √ 3

β

γ

(19)

Design resistance considering fatigue in eurocode

Assessment of fatigue resistance of welded joints is described in EN 1993-1-9. The relevant fatigue stresses are normal stresses σ

= p(σ

)

+ (τ

)

and shear stresses τ

= τ

, see figure 16.

Construction details are placed in various detail categories, see 17. The number of a detail category specifies the constant amplitude stress range (N/mm

) where the design value of the endurance is 2 ∗ 10

cycles.

Figure 17: Example of a detail category [9].

The stress range used as the design value for fatigue assessment corresponding to N

=

2 ∗ 10

cycles is denoted γ

∆σ

, where γ

is the partial factor for equivalent constant

amplitude stress ranges and ∆σ

is the equivalent constant amplitude stress range (a

simplified constant amplitude resulting in the same fatigue damage as an actual variable

amplitude) related to 2*10

cycles. The design value of the nominal stress range is given by eqs.(20-21):

γ

σ

= λ

x ∗ λ

∗ λ

∗ ... ∗ λ

∗ ∆σ(γ

Q

) (20) γ

τ

= λ

x ∗ λ

∗ λ

∗ ... ∗ λ

∗ ∆τ (γ

Q

) (21) Where σ(γ

Q

), τ (γ

Q

) is the stress range caused by fatigue loads, where Q

is the static characteristic value of the action according to [10]. λ

are the equivalent damage factors specified in EN 1993. When determining the design value of modified nominal stress ranges the right side of equation 20 is multiplied by the stress concentration factor k

.

When high stress concentration at a weld toe is present geometric stress ranges should be used. The design value of geometrical or hot spot stress range is given by eq.(22):

γ

∆σ

= k

(γ

∆σ

) (22) γ

∆σ

is the design value when considering a simplified truss model with pinned joints.

By looking at S-N curves corresponding to typical detail categories the fatigue strength for nominal stress ranges can be evaluated, for fatigue strength at 2∗10

cycles the reference values ∆σ

and ∆τ

are used to represent each detail category. See fig.18.

Figure 18: Fatiue strength curves for normal stress ranges [11]

Figure 19: Fatigue strength curves for shear stress ranges [11]

The criterion for nominal, modified nominal or geometric stress ranges due to frequent loads are given according to eqs.(23-24):

∆σ ≤ 1.5f

for normal stress ranges (23)

∆τ ≤ 1.5f

/ √

3 for shear stress ranges (24)

The criterion for fatigue loading is given according to eqs.(25-26):

γ

∆σ

∆σ

/γ

≤ 1.0 (25)

γ

∆τ

∆τ

/γ

≤ 1.0 (26)

The criterion for combined stress ranges is given according to eq.(27):

γ

∆σ

∆σ

/γ

!

+ γ

∆τ

∆τ

/γ

!

≤ 1.0 (27)

where γ

is the partial factor for fatigue strength.

2.5.2 BSK

BSK is a Swedish handbook which contains regulations for steel structures, these regulations, although still widely used, were replaced by the eurocodes in 2011.

In a full penetration welding joint the design resistance is considered in a section nearby the weld, see figure 20. If the filler material is weaker than the base material, design resistance should be considered inside the weld as well [12].

Figure 20: Examples of design sections nearby full penetration welding joints.

For a fillet weld, the sections considered should be the sections adjacent to the weld but also the section in the weld with the smallest nominal area i.e. the throat area [12].

• The section length is the effective length where the weld is full size.

• A load bearing fillet weld should have a weld length of at least 50mm or 6a for a>8mm.

• The effective length is considered to be at most 60a if the load carried in the direction of the length is assumed to be evenly distributed.

• If there is no risk of fatigue or brittle fracture, the maximum effective length considered is increased to 150a.

• The weld throat should be no less than 3mm.

• The design resistance of a section through the weld is determined according to eq.(28):

f

=



 



 

 ϕ √

f

f

1.2γ

if f

< f

ϕf

1.2γn if f

≥ f

(28)

where

f

= Ultimate tensile strength of the base material. If there are several materials, the weakest material is chosen.

f

= Ultimate tensile strength of the filler material.

γ

= Partial safety factor (=1.2) ϕ= Reduction factor (=0.9)

• The design resistance of a section adjacent to the weld is determined according to eqs.(29-30):

F

= 0.6slf

(29)

F

= slf

√ 2 + cos 2α (30)

where

s = Section height

l = Effective length of the weld

F

= Force component in the longitudinal direction

F

= Force component in a plane perpendicular to the length α = angle between F

and the design section

• In a situation where both transverse and longitudinal forces are present the criterion according to eq.(31) should be fulfilled:

( F

F

)

+ ( F

F

)

≤ 1.00 (31)

• S and R denote solicitation and resistance respectively.

Design resistance considering fatigue in BSK

The stress range σ

is calculated as nominal stresses without considering stress variations due to geometry details. The stress components are defined in the same way as in figure 16, but with slightly different notation:

σ

= Normal stress perpendicular to the throat σ

= Normal stress parallel to the axis of the weld.

τ

= Shear stress perpendicular to the axis of the weld.

τ

= Shear stress parallel to the axis of the weld

The design criterion considering fatigue at pure normal stress is gievn according to eq.(32):

σ

≤ f

(32)

where f

= f

/(1.1γ

) where f

is the fatigue design resistance and f

is the reference fatigue strength value. If the stress range is of pure shear the design criterion is given according to eq.(33):

τ

≤ f

(33)

where f

= 0.6f

. In a multiaxial stress state with stress ranges σ

, σ

, τ

and τ

, as well as the criterion in eqs(32-33), the criterion according to eq.(34) should be fulfilled:

s σ

f

+ σ

f

+ τ

f

+ τ

f

≤ 1.10 (34)

The reference fatigue strength, f

, is calculated considering notch effects characterized by the detail category C and the design life time expressed as a number of stress cycles n

. The detail category C is the characteristic fatigue strength at 2 ∗ 10

stress cycles at a constant stress range. Detail categories for bulk material and weld joints can be found in tables, see appendix 3 in [12]. For stresses at a constant nominal stress range with less than 5 ∗ 10

stress cycles the reference fatigue strength is given by eq.(35):

f

= C 2 ∗ 10

n

!

(35)

Figure 21: The horizontal axis represents the number of stress cycles and the vertical axis

represents the reference fatigue strength (MPa)

3 Methods

3.1 Static analysis

A structure which resembles a typical load bearing component consisting of a plate and a beam connected by a weld is developed, see figure 22.

Figure 22: Component composed of a beam welded onto a plate.

Tests are performed on beams with two different cross-sections, one square and one

rectangular with dimensions 200x200mm and 200x100mm respectively both with a wall

thickness of 15mm and length 500mm. The plate is supported either by applying fixed

supports to the back face of the plate or to the holes, see figure 23. When the plate is fixed

in the holes the model is also tested by applying a ”compression only support (COS)” at the

back face of the plate to simulate some object on which the plate is mounted to.

(a) (b)

(c)

Figure 23: Figure showing the three types of support variants: a)fixed plate, b)fixed holes

and c)fixed holes and compression only support.

The simulation variables which are to be tested are summarized in the lists below:

Cross sections:

• Square100x100(mm)

• Rectangular200x100(mm) Loading conditions:

• Tensile force 30kN

• Bending force 20kN

• Bending moment 10kNm

• Torsional moment 10kNm Supports:

• Fixed support (plate)

• Fixed support (holes)

• Fixed support (holes) + compression only support (plate) Contact formulations:

• Augmented Lagrange

• Pure penalty

• Multi-point constraint

• Normal Lagrange

A reference model is produced in which the fillet weld is modelled as a triangle extrusion and

the entire component consists of a single body, the whole geometry is meshed together and

requires no modelling of contacts. In order to make sure that the force is transferred through

the weld and not directly from the beam to the plate, a small gap between the plate and

the beam is constructed. For the models which consist of multiple bodies, bonded contact

between weld-plate and weld-beam is used, see figure 24.

(a) (b)

Figure 24: Bonded contact between weld-plate and weld-beam.

All of the parts including the weld material are assigned a structural steel with isotropic elasticity according to table 2.

Table 2: Material data of structural steel

Density (Kg/m

)

Young’s Modulus (Pa)

Poisson’s Ratio

Bulk Modulus (Pa)

Shear Modulus (Pa)

7850 2 ∗ 10

0.3 1.6667∗10

7.6923∗10

In order to confirm that the models yield reasonable results the FEM stresses in the throat

section are compared to the analytical stresses calculated using the previously mentioned

Excel program. To determine the stresses along the length of the weld the weld is sliced into

a number of elements, see figure 25.

Figure 25: Figure showing the sliced weld elements

The meshing is done so that a mesh in and near the area of interest is fine, but rough far away from the weld in order to reduce the number of elements. To confirm that the mesh is adequate a convergence study is performed on the first test. For each refinement of the mesh the average von Mises stress in the weld element is calculated, see figures 26 and 27.

(a) (b)

Figure 26: The von Mises stress in the throat section of one weld element.

4 4,5 5 5,5 6 6,5 7 7,5 8 8,5 9

0 50 100 150 200 250 300 350 400 450

Number of elements

Mesh test

FEM Tension 30Kn

200x200mm von-Mises

Stress (MPa)

Figure 27: The von Mises stress plotted with the number of mesh elements at the face of one weld elements.

Although a convergence of the stress seems to occur already at about 70 elements, a refinement of 200 elements is chosen since the computation time is not significantly increased.

Efforts are made in order to produce a similar mesh for each new model so that fair comparisons can be performed. A similar procedure of determining the stress is performed for different models with the various variables. In order to minimize computation, symmetry is used when possible, e.g. when the beam is subjected to tension, with the force applied at the centre of the beam, it is enough to model one fourth of the geometry. This requires that the force applied is one fourth of the actual force in order to get the correct stress.

3.1.1 Limit-load analysis

The models used in the section 3.1 are now used in order to determine the maximum load that the structure can carry. The load is calculated using three different methods.

Analytical method

The limit-load is calculated analytically determining the load which leads to a von Mises stress, in the weld throat, which is above the yield stress.

Linear FEA

The limit-load is calculated using the results from the analysis in section 3.1 by assuming a linear relationship between load and stress. The limit-load is determined using the following equation

F

F

= σ

σ

(36)

Where F

is the limit-load, F

is the applied load, σ

is the yield stress and σ

is the maximum von Mises stress in the weld caused by the applied load F

.

non-linear FEA

A non-linear analysis is performed assuming a elastic-perfectly-plastic material model. The limit-load is the load which causes total structural instability. Structural instability is indicated in the model when an equilibrium solution cannot be obtained for a small increase in load, i.e. the solution does not converge. The limit-load is calculated by multiplying the applied force to the last step time for which a solution has been obtained, see figure 28.

Figure 28: Figure showing displacement vs time, the last step time with a converged solution is indicated (t=0.11s).

Only the reference models are used in the limit-load analysis since the non-linear analysis is very time consuming. The models are tested using tensile and bending forces.

3.2 Fatigue analysis

For the fatigue analysis section a structure consisting of a fillet welded pipe and a flat

flange according to figure 29 is considered.

Figure 29: 1/2-symmetry of the fillet welded pipe and flange.

Similar to the static analysis the structure is evaluated in different loading conditions:

tensile force, bending force and bending moment. Note that the structure is not tested in torsion, this is because a torsional moment would not produce a significant amount of stress perpendicular to the toe. The fatigue life is evaluated using two different methods: hot spot method and effective notch method. In both of the methods the model is evaluated as a single body and as multi-body with contacts. Since the stress is not directly measured in the weld when using the hot spot method, the analysis is also performed without actually modelling the weld to see how the lifetime is affected. When significant compressive effects are present such as in the bending conditions, the structure is modelled both with and without

”compression only support” at the flange bottom. The structure is fixed at the flange holes

and loads are applied to the top of the pipe. The analysis is performed assuming a constant

pulsating stress range (R = 0), this means that the stress range is simply the maximum hot

spot or notch stress measured. Although the problem is dynamic in nature, the frequency

is assumed to be sufficiently low that a static calculation can be used without too much

error. Since the geometry is axisymmetric, symmetry conditions can be applied, e.g. when

applying simple tension, modelling only 1/8 of the geometry is sufficient for describing the

whole structure, see figure 30.

Figure 30: 1/8 of the geometry, load applied to top face of pipe and fixed support at holes.

3.2.1 Hot spot method

The stress in the hot spot method is measured a distance away from the weld and not in

the weld itself, therefore the structure is modelled both with and without including the weld

itself. Meshing is done according to the recommendations in [3]. Hexahedral (hex) elements

of size 1mm is chosen since the thickness of the plate (pipe) is 5mm and meshing elements of

less than 0.4t is recommended, see figure 31.

Figure 31: 1mm hex elements.

The stress at the surface perpendicular to the weld is plotted along a path of 0-100mm

from the weld, see figure 32.

Figure 32: Stress plotted along the path.

In order to determine the hot spot stress the stress is extrapolated according to eqs.(14-15) found in section 2.4.2. As seen in figure 32, the stress is clearly non-linear at the extrapolation points so a quadratic extrapolation according to eq.(15) is appropriate.

After calculating the hot spot stress it is then used to determine the fatigue life using equation 11 in section 2.3. The FAT-value is taken to be equivalent to that of a load-carrying fillet weld in [3] with FAT-value for steel of 90.

3.2.2 Effective notch method

As mentioned in section 2.4.3 the weld toe and root is replaced by a 1mm radius. Since the stress is measured directly at the weld toe, a very fine mesh is required at the notches.

Quadratic hex elements of 0.1mm are used in the notch regions (see figure 33), for an effective

radius r=1mm [3] recommends element sizes no larger than 0.25mm in the notch regions.

Figure 33: Meshed effective notch model.

The effective notch stress is obtained by taking the largest value of the maximum principal

stress at the notch. After calculating the effective notch stress it is then used to determine

the fatigue life using eq.(11) in section 2.3. For assessment based on the effective notch stress

there is only one FAT class which has the FAT-value 225 for steel.

4 Results

All FEM calculations were done in Ansys Mechanical using geometry created in Ansys DesignModeler.

4.1 Static results

4.1.1 Square cross section

The following results show how the von Mises stress in the weld throat changes along the length of the weld. Stress is measured along the fewest number of weld elements which sufficiently describes the behavior of the whole structure, e.g. 6 weld elements represents one eighth of the total weld length or one half of one of the sides. However, for models in bending it is necessary to plot the stresses along one fourth of the total weld length or one half of two separate sides. The stresses are always plotted starting from the edge to the middle of the weld length, see figure 34.

Figure 34: Figure showing the weld elements used to plot stresses.

Figures 35, 36, 37 and 38 show comparisons between analytically calculated stresses and

stresses calculated for the FEM-models consisting of a single body.

0 2 4 6 8 10 12

0 1 2 3 4 5 6 7

von-Mises Stress (MPa)

Weld element No Analytical vs FEM

Reference Analytical TF (30kN)

200x200mm

Figure 35: Analytical vs simulated stress along weld using the reference model (tensile force).

0 10 20 30 40 50 60

0 1 2 3 4 5 6 7

Analytical vs FEM, side 1

Analytical Reference von-Mises

stress(MPa)

BF (20kN) 200x200mm

Weld element no

(a)

0 10 20 30 40 50 60

6 7 8 9 10 11 12 13

Analytical vs FEM, side 2

Analytical Reference von-Mises

stress(MPa)

BF (20kN)

200x200mm Weld element no

(b)

Figure 36: Analytical vs simulated stress along weld using the reference model (bending

force)

0 10 20 30 40 50 60

0 1 2 3 4 5 6 7

Analytical vs FEM, side 1

Analytical Reference von Mises

Stress (MPa)

BM10kNm

200x200mm Weld element No

(a)

0 10 20 30 40 50 60

6 7 8 9 10 11 12 13

Analytical vs FEM, side 2

Analytical Reference von Mises

Stress (MPa)

BM10kNm

200x200mm Weld element No

(b)

Figure 37: Analytical vs simulated stress along weld using the reference model (bending moment)

0 5 10 15 20 25 30 35 40 45

0 1 2 3 4 5 6 7

Analytical vs FEM

Analytical Reference

von-Mises Stress (MPa)

TM (10kNm)

200x200mm Weld element no

Figure 38: Analytical vs simulated stress along weld using the reference model (torsional moment).

Figures 39, 40, 41 and 42 show comparisons between models with different types of

supports.