Eindhoven University of Technology
MASTER
Punching shear failure on welded rectangular hollow section joints in aluminum
Manders, W.W.J.
Award date:
2018
Link to publication
Punching Shear Failure on welded Rectangular Hollow Section Joints in Aluminum
W.w.j. Manders 0767971 w.w.j.manders@student.tue.nl w.w.j.manders@gmail.com +31-610055050 5 April 2018 A-2018.213 Version: 1.0 Supervisors:
Prof. Dr. Ir. J. (Johan) Maljaars Prof. Dr. Ir. A.S.J. (Akke) Suiker B. (Bruno) Belin
Abstract
Hollow section joints are widely used in the aluminum build environment. In general, the strength and stability of aluminum structures are designed with formulas from the design standard for aluminum, in Europe being Eurocode 9. Eurocode 9 does not provide design rules for welded aluminum hollow section joints. Some preliminary design models have been developed and are available in literature. Previous research from Soetens and De Jongh provides experimental data and a new set of design rules for welded aluminum hollow section joints. The failure mode punching shear will be investigated in this research by experimental and numerical research. The focus will be on the capture of the instance of fracture in a finite element model and determining the ultimate resistance.
Experimental research performed by Soetens in 1987 covered two failure modes, namely weld failure and chord side wall failure. In this research experimental tests are performed on the failure mode punching shear. The experimental data is used as validation for the finite element model. Two full scale X-joints are tested in the Pieter van Musschenbroek laboratory at the Technical University of Eindhoven. Adjacent to these tests dog bone specimens were tested from two other specimens made from the same batch of material. One series of dog bone tests of the parent metal needed as input for the finite element simulation. Another series to validate the material input for the HAZ.
To capture the instance of fracture in the finite element model a material damage model is used. At first the elements in the simulation follow the stress-strain diagram of the material that was used as input. When an element reaches the damage initiation point, the damage evolution process begins. The damage initiation point in this research is defined with the fracture locus in the fracture strain – stress triaxiality space. For different stress triaxialities different fracture strains are valid. After damage initiation the stress – strain curve can no long accurately determine the materials behavior. Therefore, a stress-displacement response is used based on Hillerborg’s fracture energy proposal. This results in a linear relationship between the stress and the equivalent plastic displacement. The area of the graph plotted by the stress versus equivalent plastic displacement is denoted as the fracture energy of the material.
The results presented in this research are valid for the given values of fracture locus and fracture energy. The design equation is based on the experimental research values and the results from finite element simulations.
Index
1 INTRODUCTION TO HOLLOW SECTION JOINTS ... 1
1.1 STRESS DISTRIBUTION ... 1
1.2 DESIGN RULES AND FAILURE MODES ... 2
1.3 PROBLEM AND AIM ... 3
2 LITERATURE REVIEW ... 4
2.1 PREVIOUS RESEARCH ON ALUMINUM HOLLOW SECTION JOINTS ... 4
2.2 FRACTURE LOCUS ... 5
3 EXPERIMENTAL RESEARCH ... 8
3.1 PUNCHING SHEAR ... 8
3.2 DOG BONE PARENT METAL ... 14
3.3 DOG BONE HAZ ... 17
4 NUMERICAL RESEARCH ... 21
4.1 GEOMETRY... 21
4.2 MATERIAL ... 22
4.3 DAMAGE AND FAILURE ... 25
4.4 ELEMENTS... 28
4.5 MESH ... 28
4.6 BOUNDARY CONDITIONS AND LOADING ... 31
4.7 VALIDATION ... 31
4.8 PARAMETER STUDY ... 38
5 DESIGN EQUATION ... 47
6 CONCLUSIONS AND RECOMMENDATIONS ... 49
7 REFERENCES ... 50 A ANNEX A ... A1 B ANNEX B ... B1
List of Symbols
N1= Axial load in brace member a = Throat thickness of the weld apen= Penetration length of the weld
q1 = Angle between the brace and the chord gMw = Material factor of the filler metal gM2 = Safety factor
fw = Yield strength of the filler metal
f0,haz;0 = 0.2% proof strength of the heat affected zone of the chord fu,haz;0 = Ultimate strength of the heat affected zone of the chord f0,haz;1 = 0.2% proof strength of the heat affected zone of the brace fu,haz;1 = Ultimate strength of the heat affected zone of the brace f0.2 = 0.2% proof strength
fu = Ultimate strength
E = Young’s modulus
!" = Fracture strain
# = Ramberg Osgood exponent h = Stress triaxiality
s$ = Hydrostatic stress s% = Equivalent stress
be,p = Effective width of the brace for punching shear failure beff = Effective width of the brace
leff = Effective width
Cf,ps = Calibration factor for punishing shear Cf,bs = Calibration factor for brace failure h0 = Height of chord
h1 = Height of brace b0 = Width of the chord b1 = Width of the brace
t0 = Wall thickness of the chord t1 = Wall thickness of the brace
1 Introduction to hollow section joints
Figure 1.1 shows a typical hollow section joint. The chord is the horizontal hollow section and the braces are the vertical hollow sections welded on top and at the bottom of the chord. The braces can be welded on the chord in different angles (q1). The width is indicated by b0 and b1, the height by h0 and h1. And the thicknesses with t0
and t1, where the indices 1 and 0 correspond to brace and chord. The chord faces are the top- and bottom-wall of the chord where the braces are connected. The chord walls are the remaining walls in the height of the chord.
The load is applied at the top of the brace indicated by N1.
Figure 1.1; Hollow section joint
1.1 Stress distribution
The stress distribution in the braces will not be uniform across the width of the braces due to the deformation of the chord faces (Figure 1.2). The shape of the curve in Figure 1.2 depends on the ratio of stiffness’s between the chord wall and chord faces. This results in a failure forces which depends on the effective area of the brace.
This force can be calculated with:
& = ( )
*+ ,
-./ Eq. 1.1
The stress at failure depends on the ductility of the material. Ductility is the ability of a material to deform under (tensile) stresses. The more ductile the material the higher the strain at rupture of the material. With a higher strain at rupture there is more room for deformation and redistribution which results in a higher resisting force.
Figure 1.2; Non-uniform stress distribution
Figure 1.3; Non-Linear stress distribution after σelastic,1
F
σelastic,1 F
If the material of the brace and chord member are ductile enough to allow redistribution of the stresses as depicted in Figure 1.3, the connection becomes more efficient and can resist a higher force. With this stress distribution, the connection will give enough warning before failure occurs. If the material has low ductility, redistribution is expected to be limited and cracking can occur relatively sudden and is therefore undesirable.
With this low ductility, the resisting force of the cross section is expected to be limited as well.
1.2 Design rules and failure modes
Connections in aluminum can be made in various ways. For example, by bolting or welding. Eurocode 9 [1] and the American equivalent ADM [2] provides rules to design with aluminum structures. There are some others but less wide spread. None of these standards provide design rules for welded connections of hollow sections.
Eurocode 3 (design code for steel) [3] does provide in design rules for steel welded connections in hollow sections, for example, T-, X- and Y-Joints. (Figure 1.4).
In order to add rules for connections with welded hollow sections to the revised Eurocode for Aluminum, design rules have to be developed. The design rules for hollow section joints in steel provide different failure modes.
These failure modes are expected to be valid for aluminum joints as well. In addition, due to different combinations of filler metal and alloy, weld failure can also occur in aluminum. Hence, 5 failure modes can be distinguished: Weld Failure (Figure 1.5), Chord face failure (Figure 1.6), Chord side wall failure (Figure 1.7), Punching shear failure (Figure 1.8) and Brace failure (Figure 1.9).
Figure 1.5; Weld failure Figure 1.6; Chord face failure Figure 1.4; T-, X- and Y-Joints in Eurocode 3 [3].
Figure 1.9; Brace failure
1.3 Problem and aim
There are no design rules for aluminum welded connections of hollow sections. In order to develop formulas that can be used in practice to calculate this kind of connections research is done. Previous research focused on all failure modes. This previous research recommended to look at the failure mode with a multiaxial stress state, problems were encountered with the cut-off criteria and the mesh dependence of the finite element simulation.
This research focuses on the failure mode with the multiaxial stress state, namely the punching shear failure mode. In order to find the ultimate force in finite element analyses, fracture of the connection needs to be modeled. The following two questions will be answered in this research:
Can the instance of fracture be captured in a finite element model?
If so, can the resistance of RHS connections be determined?
Only rectangular hollow sections of aluminum alloy 6005A-T6 are used during this research. Experimental tests have been performed (Chapter 3). These experiments are used to validate the finite element model (Chapter 4).
After the validation of the model the ultimate resistance of the connections can be determined with finite element simulation. An analytical solution will be presented that can be used in practice for determining the resistance of connection of welded hollow sections failing on punching shear (Chapter 5).
2 Literature review
2.1 Previous research on aluminum hollow section joints
In 1987 F. Soetens conducted the research ‘welded connection in aluminum alloy structures’ [4]. Next to an extended research on mechanical properties and fillet welds, research is performed on aluminum hollow section joints. Experimental tests were performed on two types of connection with different kinds of loading (Figure 2.1). Two types of alloy are used for the connections, namely 6063-T5 and 7020-T6, and one type of filler metal, namely 5356. Two combinations of sections are used, first a chord of 100x100x4 [mm] with a brace of 80x80x4 [mm] and second a chord section of 100x100x3 [mm] and a brace section of 50x50x4 [mm]. All specimens are welded with a fillet weld with a throat thickness of 4mm. For the X-joint specimens tested by F. Soetens two types of failure modes can be distinguished, namely weld failure and chord side wall failure.
Figure 2.1; Experimental program hollow section connection. Source: [4]
In [5] research has been conducted on welded hollow section joints in aluminum. This research contains numerical simulations and analytical analyses on all failure modes. The numerical simulations are validated with experimental tests performed on steel welded hollow section joints from the past. With the numerical data and analytical analyses, the following design rules were proposed for aluminum. Although there were problems with the finite element simulations for punching shear failure, simulations were made in order to propose a design rule.
2.1.1 Weld Failure
0/=
4 34 + 46789 :7;;ℎ/ =>
g?>
3√3 :7;;− √3:7;;sinq/+ √32 ℎ/9 sinq/ Eq. 2.1
GHIℎ: :7;;= 2 K7;;+ 2 ℎ/ sinq/ 2.1.2 Chord face Failure
0/=
2 =L,NOP,,I,Q
R1 −K/ K,T sinq/
U ℎ/ K,
sinq/+ 2V1 −K/ K,W X
Eq. 2.2
2.1.4 Punching Shear Failure
0/=
=",NOP;,I,
√3 sin q/
Y2, 75 ℎ/ sinq/ [ X?Q
Eq. 2.4
2.1.5 Brace Failure
0/==",NOP,/4678 (2ℎ/− 44678+ 2K7;;)
X?Q Eq. 2.5
GHIℎ: K7;;= 6 K,
I, a
=",NOP;,I,
=",NOP;/I/K/
2.2 Fracture locus
The fracture strain is an important variable in the determination of the ultimate strength of a welded joint with hollow sections. Due to the different failure modes different stress states are applicable. For example, for punching shear failure, there is a multiaxial stress condition. Stress triaxiality is a variable to describe the multiaxial stress state. Stress triaxiality (Eq. 2.6) depends on the hydrostatic stress sH (Eq. 2.7) and equivalent stress s% (Eq. 2.8). With s1, s2 and s3 as the principal stresses.
h = Ys$
s%[ GHIℎ: Eq. 2.6
s$=(s/+sQ+sb) 3
Eq. 2.7
s% = c1
2((s/−sQ)Q+ (sQ−sb)Q+ (sb−s/)Q)
Eq. 2.8
When −/b< e < 0 the material is in a combination of compression and shear, e = 0 represents the material under pure shear stress. For 0 < e < 0.4 there is a combined loading of shear and tension. And for e > 0.4 the material is in tension (Figure 2.2).
Figure 2.2; Equivalent fracture strain as function of the stress triaxiality for Alloy 2024-T351. Source: [6]
i
The fracture strain depends on the stress triaxiality [7].The relation between the fracture strain and the stress triaxiality can be describe by a fracture model. Different fracture models are available and evaluated in literature.
For the evaluation of a fracture model, experimental tests are performed by Bao and Wierzbicki [8], in a wide range of stress triaxialities. The stress triaxiality is determined by numerical test parallel to the experimental tests in [8]. The equivalent strain to fracture is determined by the experimental tests. Table 2.1 shows the test results of Bao and Wierzbicki on aluminum alloy 2024-T351.
Table 2.1; Experimental program alloy 2024-T351. Source: [8]
Notice from Table 2.1 the wide range of stress triaxialities tested. There also is a wide range of fracture strains for the different stress triaxialities. For the prediction of these experimental results different fracture models are available [8]. The fracture model used during this research has a good correlation with the test results of Bao and Wierzbicki and there is only one calibration point needed for the calibration of the fracture criteria. The fracture locus of the Maximum Shear stress criteria is constructed from Eq. 2.9 and Eq. 2.10 where e = Y√b/[ (j + 1)/3√1 + j + jQ9 and nhard is the hardening exponent.
!̅;= m n√1 + j + jQ 2 + j o
/a8pqrs
&tu = −1
2< j < 1 tu 1
3< e <2 3
Eq. 2.9
!̅;= m n√1 + j + jQ 1 − j o
/a8pqrs
&tu = −2 < j < −1 2 tu −1
3< e <1 3
Eq. 2.10
To construct the fracture locus of alloy 2024-T351 with the equations above, calibration of the model is needed.
The pure shear test number 10 is used for calibration of the model. Putting e = 0 4#- j = −1 into the equation the calibration constant becomes m = 0.21. Figure 2.2 shows the result of the fracture locus and the experimental results. There is almost a perfect correlation between the experimental results and the maximum shear stress fracture locus.
be calculated from the measured relative displacement. After necking, the equivalent stress and strain could be determined from a continuous measurement of the diameter of the neck. Such a technique was not available in the lab. Instead, the true stress–strain curve was determined through an iterative procedure based on a detail numerical simulation of the necking process. This technique was described in a number of previous publications, see for example [1–3]. The true
ARTICLE IN PRESS
Table 2
Summary of the experimental program
Test number Specimen description ¯!f Zav xav !¯!f
1 Round, smooth 0.46 0.40 1.0 0.45
2 Round, large notch 0.28 0.63 1.0 0.3
3 Round, small notch 0.17 0.93 1.0 0.21
4 Flat-grooved 0.21 0.61 0.097 0.21
5 Cylinder ðd0=h0¼ 0:5Þ 0.45 % 0.278 % 0.91
6 Cylinder ðd0=h0¼ 0:8Þ 0.38 % 0.234 % 0.81
7 Cylinder ðd0=h0¼ 1:0Þ 0.356 % -0.233 % 0.82
8 Cylinder ðd0=h0¼ 1:5Þ 0.341 % 0.224 % 0.80
9 Round notched (compression) 0.62 % 0.248 % 0.84
10 Flat dog-bone tensile 0.21 0.0124 0.055
11 Flat 0.26 0.117 0.50
12 Plate with a circular hole 0.31 0.343 1.0
13 Dog-bone 0.48 0.357 0.979
14 Pipe 0.33 0.356 0.984
15 Solid bar 0.36 0.369 1.0 0.29
Note that ¯!!f is the average cross-section strain evaluated from the measured area reduction according to Eq. (25).
Fig. 6. Tests on unnotched round bar#1; two notched bars #2 and 3, and flat grooved specimens used for calibration of seven fracture models.
T. Wierzbicki et al. / International Journal of Mechanical Sciences 47 (2005) 719–743 728
Figure 2.3; Maximum shear stress fracture locus. Source: [8]
i
3 Experimental Research
For welded connections of hollow sections, experimental research is done in [4] but did not cover all failure modes. In order to validate the numerical part of this research, new tests are performed. The following failure modes are tested: brace failure, weld failure and punching shear failure. The numerical part of this research focuses on punching shear failure. Therefore, only the punching shear experiments for a full X-joint are described here. Additional tests have been performed for other failure modes. These are listed in Annex A. The results of these tests, however, have not been used in the current research. Adjacent to the experiments on the full X- joint, dog bone specimens are tested in order to find the stress strain relationship of the material used.
3.1 Punching Shear
In order to validate the finite element model for punching shear failure two experiments on full X-Joints are performed. The tests are performed in the Pieter van Musschenbroek Laboratory on the Technical University of Eindhoven.
3.1.1 Geometry
The geometry of the specimens is determined with previous research [5]. The chord is made of a hollow section with a width of 120mm a height of 80mm and a thickness of 4mm. The brace is a square hollow section with a width and height of 70mm and a thickness of 4mm. The brace has a length of 350mm. Both sections are made from alloy 6005A-T6. The throat of the weld has a height of 6mm and is of filler metal 5456. The specimens are checked for dimensional tolerances. The punching shear failure specimens are numbered 09 and 10. Figure 3.1 shows the dimensions of sample 09 and Figure 3.2 shows the dimensions of sample 10.
3.1.2 Loading
The loading of the specimen is applied at the top and is deformation controlled. In order to introduce the loading into the specimen a special method is developed. Welding is not possible, this would decrease the ultimate strength of the cross section at the top of the brace. Therefore, at the top and bottom of the brace, bolts under pretension are used in order to introduce the load into the joint. Because of the lack of stiffness of the brace, to withstand the forces introduced by the bolts an aluminum block is fabricated that fits exactly into the brace (Figure 3.3). To get an evenly distributed pretension on the walls of the brace, aluminum plates are added on the side. The aluminum block is fabricated so that the clamping device of the testing machine can be attached (Figure 3.4). The connection is calculated in Annex B. The load of the specimen is introduced by the aluminum block into the brace by friction. In order to get a reasonably high friction coefficient, the outside of the aluminum block and the inside of the brace are roughened.
Figure 3.3; Drawing loading device [mm] Figure 3.4; Loading device in practice 3.1.3 Measurement
To validate the numerical simulations, measurements are taken of the load and displacement of the specimens.
The load is measured by a 250kN load cell situated at the top of the testing machine. The load cell is calibrated regularly in order to maintain accurate test result. The displacement is measured on global scale. In order to do this LVDT’s (Linear Variable Differential Transformer) are placed on the specimen. The LVDT’s are placed on both sides of the specimen. The LVDT’s measure between two points 400mm apart. The points are placed 190mm from the top and from the bottom of the specimen (Figure 3.5).
In order to measure the local strain near the weld, strain gauges are placed on the brace. For sample 10 six strain gauges are placed at the top brace, two at the middle of the width (b1), gauges 00 (Figure 3.6) and 04 (Figure 3.7). Two gauges are placed at the corner, gauge 01 at the side of the width (b1) and gauge 02 at the side of the height (h1) (Figure 3.6). The reaming two gauges at the top are placed at the middle of the height (h1), gauges 03 (Figure 3.6) and 05 (Figure 3.7). At the bottom of the brace two strain gauges are placed in the middle of the width of the brace (b1). Gauge 06 is on the opposite side of gauge 00 and gauge 07 on the opposite side of 04, with the chord as mirror.
Figure 3.6; Strain gauges 00 till 03 Figure 3.7; Strain gauges 04 till 05 3.1.4 Test Setup
The tests are performed on an Instron 250KN testing machine. The specimen is clamped at the top and at the bottom. The tests are deformation controlled with a crosshead speed of 2mm/min. To see where the first crack appears cameras are setup around the specimen. One camera is filming the back side of the specimen. Another camera is taking pictures at the front side of the specimen (Figure 3.8).
3.1.5 Results
Figure 3.9 shows the force displacement graph of the experimental tests. The graph shows that there is a good correlation between sample 09 and sample 10, until a load of around 50 kN there is a perfect correlation between the two samples. As of that point they start to deviate. The failure load of sample 10 (68,31 kN) is 9% higher than the failure load of sample 09 (62,57 kN). There is also a difference between the displacement where failure occurs. For sample 09 the displacement is 23mm and for sample 10 the displacement at failure is 26mm. This is a difference of 13%. During testing, and with video footage after testing, it is determined that sample 09 failed due to weld failure. Therefore, sample 09 has a lower ultimate load.
Figure 3.9; Load- Displacement graph
The first crack is located at the bottom side of specimen 10. Figure 3.10 shows a picture of the crack of the specimen. A nice clean punching shear cut along the length of height of the brace (h1). On the left side the welding of the specimen was not sufficient and separated from the chord. From other images taken of the experiment during testing can be concluded that the weld on the left side was already separated before the punching shear failure occurred. Along the height of the brace (h1) the weld is sufficiently welded to the chord therefore it is not assumed that this phenomenon influenced the ultimate failure load and displacement significantly.
Figure 3.10; First crack of sample 10 0
10 20 30 40 50 60 70
0 5 10 15 20 25 30 35
Load (kN)
Displacement (mm)
Sample 09 Sample 10
Figure 3.11 depicts the force-strain graph for the strain gauges placed in the middle of the brace (b1). Gauge 00 and gauge 06 are placed opposite of each other, gauge 04 and 07 also. Till around 40 kN all the strain gauges measure a negative strain. This means that the width of the brace is not yet participating in restraining the load.
From there on a positive strain is measured and the width of the brace is activated. As seen in the graph there is a scatter of the strain at the failure load. This means that not every part of the brace is equally effective. Looking at the failure strain of pair 00 and 06 it is clear that there is big difference in the strain. Pair 05 and 07 are more equal.
Figure 3.11; Load-Strain graph strain gauges 00, 04, 06 and 07 for Sample 10
Figure 3.12 shows the force-strain graph for the strain gauges on the height of the brace (h1). There is a difference in strain at failure. This means that one side of the sample took more load into account than the other side.
Gauge 03 was at the side where the first crack appeared and is also showing the largest strain at the failure load.
0 10 20 30 40 50 60 70
-0,5 0 0,5 1 1,5 2 2,5
Load (kN)
Strain (mm/m)
SG8-00 SG8-04 SG8-06 SG8-07
Figure 3.12; Load-Strain graph strain gauges 03 and 05 for Sample 10
The last two gauges are placed on the corner. Gauge 01 at the width (b1) side and gauge 02 at the height (h1) side of the brace. As expected from the graphs above the width of the brace take less load than the height of the brace. This is clearly shown by Figure 3.13. There is a large deviation between the strain at failure of gauge 01 and gauge 02.
Figure 3.13; Load-Strain graph strain gauges 03 and 05 for Sample 10 0
10 20 30 40 50 60 70
0 5 10 15 20 25
Load (kN])
Strain (mm/m)
SG8-03 SG8-05
0 10 20 30 40 50 60 70
0 2 4 6 8 10 12 14 16 18 20
Load (kN)
Strain (mm/m)
SG8-01 SG8-02
3.2 Dog bone parent metal
In order to obtain a constitutive relationship of the material, for the numerical part of this research, dog bone specimens are taken form the brace of sample 09. As the major part of the brace remains in the elastic part during the test, dog bones can be cut from this part of the specimen after the punching shear tests. In total a number of eight specimens are tested.
3.2.1 Geometry
The geometry used for the dog bone specimens is reported in ISO 6892-1 Metallic materials tensile testing section D.2.3.2 [9]. Figure 3.14 illustrates the geometry of the doge bone specimen. The specimens are cut with a precision cutting machine at the Pieter van Musschenbroek laboratory with the following dimensions.
Table 3.1; Dimensions dog bone specimen
L0 80 mm
Lc 90 mm
Lt 300 mm
b0 20 mm
a0 4 mm
Figure 3.14; Geometry dog bone specimen 3.2.2 Loading
The loading is applied at the top of the specimens and is deformation controlled. The crosshead speed is 1.35 mm/min.
3.2.3 Measurement
The load and displacement of the specimen is measured. The displacement is measured with the tensile testing machine. The machine is equipped with a camera that can measure the displacement of two points. The two points are eighty millimeters apart and are placed in center over the specimen, as denoted by L0 in Figure 3.14 and depicted in Figure 3.15. The load is measured by a 250kN load cell at the top of the testing machine.
ISO 6892-1:2009(E)
a) Before testing
b) After testing
Key
ao original thickness of a flat test piece or wall thickness of a tube bo original width of the parallel length of a flat test piece Lc parallel length
Lo original gauge length Lt total length of test piece Lu final gauge length after fracture
So original cross-sectional area of the parallel length 1 gripped ends
NOTE The shape of the test-piece heads is only given as a guide.
Figure 11 — Machined test pieces of rectangular cross-section (see Annexes B and D)
White displacement dots
3.2.4 Test Setup
The tests are performed on a Instron 250KN testing machine. The specimen is clamped at the top and at the bottom.
Figure 3.16; Test setup 3.2.5 Results
Figure 3.17 reports the test results of the dog bone specimens on parent metal. At the elastic part, there is a perfect correlation between all the experiments. Small deviations are noticeable in the plastic part of the stress strain relationship. The average fracture strain is 0,12 with a standard deviation of 0.004. The average ultimate tensile stress is 275,64 N/mm2 with a standard deviation of 4.13 N/mm2. The average 0.2% proof stress is 259.46 N/mm2 with a standard deviation of 3.76 N/mm2.
Figure 3.17; Experimental results 0
50 100 150 200 250 300
0,00 0,02 0,04 0,06 0,08 0,10 0,12 0,14
Stress (N/mm2)
Strain
9.8 9.7 9.6 9.5 9.4 9.3 9.2 9.1
The average properties are used as input for the numerical simulations (Table 3.2 and Figure 3.18).
Table 3.2; Material parameters
Alloy 6005A
vw.x 259.46 0/yyQ
vz 275.64 0/yyQ
{ 67463 0/yyQ
|z 0.12
} 67
Figure 3.18; Average Experimental Results 0
50 100 150 200 250 300
0,00 0,02 0,04 0,06 0,08 0,10 0,12 0,14
Stress( N/mm2)
Strain
Average
3.3 Dog bone HAZ
To check the constitutive relationship of the HAZ material discussed in section 4.2, dog bone specimens are taken from one of the remaining samples that have not been tested. The samples are taken from the top face of the chord. In total two dog bone specimens are tested.
3.3.1 Geometry
Figure 3.19 illustrates the geometry of the doge bone specimen. The specimens are cut with a precision cutting machine at the Pieter van Musschenbroek laboratory with dimensions in Table 3.3.
Figure 3.19; Geometry dog bone specimen
Table 3.3; Dimensions dog bone specimen HAZ
L0 50 mm
Lc 58.5 mm Lt 222.5 mm
b0 20 mm
a0 4 mm
The weld is in the center of the specimen as depicted in Figure 3.20 and Figure 3.21.
Figure 3.20; Drawing Sample Figure 3.21; Sample in practice
ISO 6892-1:2009(E)
28 © ISO 2009 – All rights reserved
a) Before testing
b) After testing
Key
ao original thickness of a flat test piece or wall thickness of a tube bo original width of the parallel length of a flat test piece Lc parallel length
Lo original gauge length Lt total length of test piece Lu final gauge length after fracture
So original cross-sectional area of the parallel length 1 gripped ends
NOTE The shape of the test-piece heads is only given as a guide.
Figure 11 — Machined test pieces of rectangular cross-section (see Annexes B and D)
Dit document is door NEN onder licentie verstrekt aan: / This document has been supplied under license by NEN to:
TNO Bouw en Ondergrond Informatie en Documentatie 4/29/2010 4:34:51 PM
Weld 222.5
20
To get an evenly distributed stress along the cross section of the sample, the sample is flattened as shown in Figure 3.22.
Figure 3.22; Flattend samples 3.3.2 Loading
The loading is applied at the top of the specimens and is deformation controlled. The crosshead speed is 1.35 mm/min.
3.3.3 Measurement
The load and displacement of the specimen is measured on global scale. The displacement is measured with the tensile testing machine. The machine is equipped with a camera that can measure the displacement of two points. The two points are fifty millimeters apart and are placed in center over the specimen, as denoted by L0 in Figure 3.19 and depicted in Figure 3.23. The load is measured by a 250kN load cell at the top of the testing machine.
Figure 3.23; Displacement dots
White displacement dots
3.3.4 Test Setup
The tests are performed on a Instron 250KN testing machine. The specimen is clamped at the top and bottom.
Figure 3.24; Test setup 3.3.5 Results
Figure 3.25 reports the test results of the dog bone specimens with HAZ material. At the elastic part, there is a perfect correlation between the two experiments. Deviations are noticed in the plastic part of the curve. There is a difference between the ultimate stress and strain. After the ultimate stress of the experiment a damage evolution path is observed, this is the necking region. The average fracture strain is 0.09 with a standard deviation of 0.01. The average ultimate tensile stress is 163.67 N/mm2 with a standard deviation of 15.06 N/mm2. The average 0.2% proof stress is 145.71 N/mm2 with a standard deviation of 4.43 N/mm2. The ultimate stress of specimen 12.1 is reached at a strain of 0.03. The ultimate stress of 12.2 is reached at a strain of 0.05.
Figure 3.25; Experimental results 0
20 40 60 80 100 120 140 160 180
0 0,02 0,04 0,06 0,08 0,1 0,12
Stress (N/mm2)
Strain
12.1 12.2
Table 3.4; Average material parameters
Alloy 6005A HAZ
vw.x 145.71 0/yyQ
vz 163.67 0/yyQ
{ 68702 0/yyQ
|z 0.09
} 33
An important difference between the samples is the location of failure. Figure 3.26 depicts the failed samples.
Sample 12.1 failed just below the center of the specimen here it is assumed the HAZ determines the material properties. At sample 12.2 the failure is further away from the weld and here the material can be in transition from HAZ material properties to parent metal. This could be the cause of the difference in ultimate tensile strength of the samples.
Figure 3.26; Failed samples
4 Numerical Research
This part of the research focuses on the finite element simulations made of the experimental specimens discussed in section 3.1. The finite element simulations are performed in the commercial program ABAQUS version 6.14.
4.1 Geometry
The geometry of the specimen is symmetric on three planes. Due to this symmetry only one eight of the specimen is modeled (Figure 4.1 and Figure 4.2).
Figure 4.1; Model view 1 Figure 4.2; Model view 2
The dimensions of the model are determined by the experimental specimen. By taking a close look to the experiments it is noticed that cracking is first observed at the side of the specimen that has the smallest chord face thickness. The corresponding face thickness is 3.84mm. The thickness of the chord wall at the side of the first crack is 3.88 mm. The height and width of the chord have the values of experimental sample 10. For the brace average values are used for the thickness as well as for the height and width (Figure 4.3)
Figure 4.3; Dimensions [mm]
4.2 Material
Four different materials are used in the finite element simulation, being Alloy 6005A for the blue parts in Figure 4.4 and Figure 4.5 and Alloy 6005A HAZ for the blue parts in Figure 4.6 and Figure 4.7. For the considered plate thickness and weld process, Eurocode 9 specifies an extent of the HAZ of 20 mm, measured from the root of the weld. This extent has been adopted in the model. A specific constitutive relationship, introduced later, is implemented in order to simulate material damage, eventually accumulating in fracture. In order to reduce the computational time of the simulation the damage material model for Alloy 6005A HAZ is implemented only in the HAZ at the edge of the weld as indicated by the purple parts in Figure 4.6 and Figure 4.7. The weld has the material properties of filler metal 5456.
Figure 4.4; Alloy 6005A View 1 Figure 4.5; Alloy 6005A View 2
Figure 4.6; Alloy 6005A HAZ View 1 Figure 4.7; Alloy 6005A HAZ View 2 bHAZ
bHAZ
bHAZ
bHAZ
bHAZ bHAZ
bHAZ
HAZ is partly obtained by the dog bone tests of the parent metal and partly by Eurocode 9. The ultimate tensile strength and 0.2% proof stress of alloy 6005A are multiplied by reduction factors (indicating the ratio between the HAZ and the parent metal strength). The ultimate tensile strength of the parent metal is multiplied by 0.65 to obtain the ultimate tensile strength for the HAZ and the 0.2% proof stress is multiplied by 0.53. The fracture strain of the HAZ is calculated with Eq. 4.3. Table 4.1 specifies the material parameters. The stress strain curve for the HAZ is then obtained by using the Ramberg-Osgood relation (Eq. 4.3) specified in Eurocode 9 [1].
! =)
Å+ !,.QR )
=,.QT8
GHIℎ: # =ln Y!,.Q
!"[ ln R=,.Q
="T
4#- !"= 0.30 − 0.02 =,.Q 400
Eq. 4.3
Table 4.1; Material Paramaters
Alloy 6005A Reduction Alloy 6005A HAZ
vw.x 259.46 0/yyQ Çw.x 0.53 vw.x 137.51 0/yyQ
vz 275.64 0/yyQ Çz 0.65 vz 179.16 0/yyQ
{ 67463 0/yyQ { 67463 0/yyQ
|z 0.12 |z 0.22
} 67 } 18
The stress strain curve used for the filler metal is entirely constructed with values of Eurocode 9 using the Ramberg-Osgood relation.
Table 4.2; Material Paramaters Weld
Filler Metal 5356
vw.x 126 0/yyQ
vz 180 0/yyQ
{ 68000 0/yyQ
|z 0.23
} 12,31
Figure 4.8; Stress-Strain curves material model 0
50 100 150 200 250 300 350
0 0,05 0,1 0,15 0,2 0,25
Stress (N/mm2)
Strain
6005A 6005A True 6005A HAZ 6005A HAZ True
4.3 Damage and Failure
The material failure mechanism is represented in three different parts as shown in Figure 4.9. The undamaged material response from 0 to )É, (Yield stress at onset of damage). A damage initiation criterion at )É, (Damage
=0). And a damage evolution part from )É, (Damage =0) until !̅;6Ñ(Ultimate Failure Strain) (Damage=1) is reached.
)Ö is the undamaged material response and !̅,6Ñ is the strain at damage initiation point.
Figure 4.9; Stress-strain curve with damage evolution 4.3.1 Damage initiation criterion
The damage initiation point (D=0) is determined by the fracture strain. When !̅,6Ñ is reached the damage evolution process is started. As described in section 2.2 the fracture strain depends on the stress triaxiality. The fracture locus of Alloy 6005A HAZ needs to be determined from Eq. 2.9 and Eq. 2.10. The fracture strain of the HAZ is 0.22 as mentioned in section 4.2. The corresponding stress triaxiality for a dog bone specimen is 0.357 according to [6]. The fracture strain is calculated with Eurocode 9, and therefore a variable that is not fixed in this research.
In order to see the influence of the fracture strain a parameter study is conducted in section 4.8.2. The hardening exponent is calculated with the power law expression (Eq. 4.4), where the K value is the stress which corresponds with a strain of 1. Plotting the true stress-strain curve on logarithmic scale the plastic part of the curve should be a straight line according to [10]. Figure 4.10 indicates that the engineering stress-strain curve follows the linear relationship mentioned, but not the true stress-strain relationship. Therefore, four options are examined. In the first option, the value of the strain hardening exponent n is calculated from the engineering stress-strain relationship because it shows a linear stress-strain relationship on logarithmic scale, the strain hardening exponent then is 0.06. In the second option, the line between the circle and the triangle in Figure 4.10 is used for calculating the strain hardening exponent. This results in a value of 0.07. With the third option the hardening exponent is calculated with the line between the triangle and the square. The hardening exponent becomes 0.09.
With the last option the line between the square and cross is used for the calculation. This results in a value of 0.15.
# =ln )~"7− ln Ü ln !~"7
Eq. 4.4 )
)É,
á)Ö
)Ö
!
!̅;6Ñ (D=1)
!̅,6Ñ (D=0)
E E
Figure 4.10; Stress-Strain diagram of HAZ on logarithmic scale.
With four strain hardening exponents the damage initiation criteria need to be calibrated four times. This results in four fracture loci. Figure 4.11 shows the four fracture loci of the different hardening exponents, with on the horizontal axes the stress triaxiality and on the vertical axes the fracture strain. During the simulation the stress triaxiality of every element is evaluated for every time step and the strain of that element is compared to the fracture strain in the fracture locus. When the fracture strain is reached the damage evolution process is started.
Due to the four different fracture loci a study is done to see what the influences are of the different fracture loci in section 4.8.1. These fracture loci are calibrated with a fracture strain of 0.22. With a change of fracture strain also the fracture loci changes.
0,00 0,01 0,10 1,00
Stress on logaritmic scale
Strain on logaritmic scale
0,05 0,10 0,15 0,20 0,25 0,30 0,35
Fracture Strain
0.06 0.07 0.09 0.15
4.3.2 Damage evolution
When the damage initiation criteria is reached the damage evolution process starts. The stress-strain relationship can no longer accurately represent the behavior of the material during damage. Therefore, a stress-displacement response is used after damage initiation based on Hillerborg’s fracture energy proposal [11]. Figure 4.12 on the left shows the stress-displacement response, with )É, at the damage initiation point, àÖ6Ñ= â!̅6Ñ as the equivalent plastic displacement, L as the characteristic length defined by the square root of the integration point element area according to [12], and ä; as the fracture energy. ä; can be computed according to Eq. 4.5, with on the right side of Figure 4.21 the linear relation between the plastic displacement and the damage parameter.
ä;= ( â)É,-!̅6Ñ
ãÖåçé
ãÖèçé = ( )É,-àÖ6Ñ
"%åçé ,
Eq. 4.5
Figure 4.12; Linear damage evolution
The linear damage evolution can be described by Eq. 4.6 and Eq. 4.7. The equivalent plastic stress at any given increment during the damage process can be computed by Eq. 4.8, with ) as the true stress variable and )Ö as the effective or undamaged stress. Figure 4.9 illustrates Eq. 4.8.
á =â!̅6Ñ àÖ;6Ñ =àÖ6Ñ
àÖ;6Ñ GHIℎ: Eq. 4.6
àÖ;6Ñ=2ä;
)É, Eq. 4.7
) = (1 − á))Ö Eq. 4.8
The fracture energy parameter for alloy 6005A HAZ is unknown. Therefore, a study is done in section 4.8.3, in order to see the influence of the energy parameter on the failure force of finite element simulation.
àÖ;6Ñ àÖ6Ñ )É,
)É
ä;
àÖ6Ñ D
D=1
àÖ;6Ñ
4.4 Elements
The model is constructed with one type of element, namely element C3D8R. This brick element has eight nodes and one integration point. The difference of the behavior of the elements containing the damage evolution function is specified in the material model as mentioned before.
4.5 Mesh
The mesh of the model is divided into different parts. Failure is expected close to the weld so the mesh here needs to be denser than the mesh of the overall model. The walls of the brace and the chord are meshed with four elements along the thicknesses t0 and t1 (Figure 4.13). Along the leg of the weld 10 elements are placed (Figure 4.13). From here on the size of the elements along the leg of the weld is called MeshWeld. To ensure a good connection between the weld, brace and chord the adjacent parts of the brace and chord are also meshed with MeshWeld.
Figure 4.13; Mesh Close Up Weld 1 Figure 4.14; Mesh Close Up Weld 2
Figure 4.15 shows the front side of the model, the width of the brace is meshed with MeshWeld. The height of the brace is divided into different sections. Starting at the top of the brace going down to half of the length (.5*l1) of the brace. From half the length the mesh is refined to three times MeshWeld until the HAZ of the brace. From the HAZ till the weld the mesh is refined two times MeshWeld. The length (l0) of the chord is divided into three parts. From the right side till half of the length (.5*l0) of the chord the mesh size is six times MeshWeld. From half of the chord till the edge of the HAZ of the chord the mesh size is refined till three times MeshWeld. The remaining part of the chord is meshed with mesh weld. The width of the chord (b0) and the corner of the chord are both meshed with MeshWeld (Figure 4.16). The height of the chord (h0) is meshed with six times MeshWeld.
10 10
4
MeshWeld
Figure 4.15; Mesh view 1 Figure 4.16; Mesh view 2
The MeshWeld size above is selected based on a mesh sensitivity study. First a sensitivity study is conducted without damage parameters. The load at a displacement of 10mm of the experiment is compared to the force at the same displacement of the finite element simulation. Figure 4.17 shows the force – mesh size curve. It is demonstrated that, by increasing the number of elements along the leg of the weld the force converges. The grey line indicates the force of the experiment. It is observed that the simulation under predicts the oad of the experiment with a sufficiently dense mesh.
42 43 44 45 46 47 48 49 50
6 7 8 9 10 11 12 13 14
Load at displacement of 10mm (kN)
Number of elements along leg weld
3xx
2x MeshWeld
6x MeshWeld
MeshWeld
MeshWeld
3x MeshWeld
MeshWeld
6x MeshWeld
MeshWeld
6x MeshWeld MeshWeld
To see if the mesh is also sufficient for the model with the damage another mesh sensitivity study is conducted.
The model with the damage evolution criteria is used for this study, with a fracture strain of 0.17, Strain hardening exponent of 0.07 and a fracture energy of 48 N/mm. First the load at a displacement of 20mm is evaluated in Figure 4.18. There is a minimum of the load with eight elements along the leg of the weld.
Figure 4.18; Load-Meshsize curve 20mm
Second the load at a displacement of 25mm is evaluated. Around this displacement the experiments specimens failed. Figure 4.19 shows that the load is scattered. There is a minimum at a number of elements of eight. By introducing damage, a mesh dependency was expected. By increasing the number of elements from 8 till 14 a difference in force is measured of 6.27%.
60,00 61,00 62,00 63,00 64,00 65,00 66,00 67,00 68,00
6 7 8 9 10 11 12 13 14
Force at displacement of 20mm (kN)
Number of elements along leg weld
67,00 68,00 69,00 70,00 71,00 72,00 73,00 74,00
Force at displacement of 25mm (kN)
4.6 Boundary Conditions and Loading
The model uses three symmetry planes. Figure 4.20 indicates the location of the symmetry axes and the loading plane. The loading is applied by a uniform distributed displacement at the top of the brace of the specimen.
Figure 4.20; Boundary Conditions
4.7 Validation
In order to determine if the model accurately predicts the experimental specimens, the simulation is compared with the experimental results on the following parameters. First the global load-displacement diagram of sample 10 is compared to the simulations. Second, the deformations are compared. Third, the results of the strain gauges of sample 10 are compared with the simulations. Fourth, the location and shape of the crack is compared. Fifth, the damage model is check for any inconsistencies. Finally, a simulation of dog bone samples is compared with the dog bone samples in section 3.3.
4.7.1 Load-Displacement
Figure 4.21 shows the load-displacement curves of sample 10 and the simulation. As mentioned before this simulation is only valid with a specific mesh size, but also the fracture strain, fracture energy and hardening exponent are fixed for this simulation. This simulation is only valid with a mesh size of 10 elements along the leg of the weld, a fracture strain of 0.17, a facture energy of 47 N/mm and a strain hardening exponent of 0.07. The elastic part of the simulation has a perfect fit with the experimental results. From around 25 kN a deviation is noticed the simulation is stiffer than the experiment. At around 55 kN the simulation is almost equal to the experiment but from here the simulation is stiffer until final failure. The ultimate load of the simulation is 70.79 kN which is a deviation of the experimental ultimate load of 3.6%. The ultimate displacement has a deviation of the experimental result of 0.5%. Overall the simulation is stiffer than the experimental result. Reaching the ultimate load, at increasing deformation, a sudden decrease of the load is measured in the simulations and in the experiment. The load stabilizes around 47 kN.
Figure 4.21; Load – Displacement curve
4.7.2 Deformation
The deformation of sample 10 is depicted in Figure 4.22. Figure 4.23 illustrates the deformation of the simulation.
In order to make a proper comparison between sample 10 and the simulation the model is mirrored. Due to the tensile force the walls of the chord are moving inward, so that the walls of the brace and chord are lining up. Due to this effect the wall of the chord is bulging. The face of the chord is also bulging due to the tensile force.
Figure 4.22; Deformation Sample 10 Figure 4.23; Deformation Simulation 0
10 20 30 40 50 60 70
0 5 10 15 20 25 30 35
Load (kN)
Displacement (mm)
Sample 10 Simulations
4.7.3 Strain Gauges
The strain gauges are placed to determine the strains at the centers of the brace and at one corner as explained in section 3.1.4. The simulations also provide the data of the strains at the place of the strain gauges. The data of the simulations is compared to the data of the experiments. Figure 4.24 shows the graph of the strain gauges at the middle of the brace (b1). First the simulation shows a negative strain and then at around 40kN the strain becomes positive. This is also the case for the strain gauges at sample 10. Near the ultimate load and beyond, the strain of the simulation is larger than for the sample.
Figure 4.24; Load – Strain curve gauges on b1
Figure 4.25 depicts the Load-Strain curve at the corner of the sample. Until around 30 kN there is a good correlation between the simulation and the sample. From that load onwards, the simulation predicts a too low strain. Gauges 01 has a better correlation overall then gauges 02. However, from a qualitative point of view, a correct behavior is predicted.
The Load-Strain curve for the center of the height of the brace (h1) is illustrated in Figure 4.26. At the location of the failure of the experiment are no strain gauges available. Gauge 03 was on the opposite side of the crack.
Gauge 03 is compared to the simulation of the strain gauges at the weld. During the whole simulation the strain gauge of the simulation is stiffer than the strain gauge of the experimental specimen. At a strain of 15 there is an increase in force with a constant strain. This is an indication for the failure of the specimen.
0 10 20 30 40 50 60 70
-1 -0,5 0 0,5 1 1,5 2 2,5 3 3,5
Load (kN)
Strain (mm/m)
SG8-00 SG8-04 SG8-06 SG8-07
SG8-00 Simulation
Figure 4.25; Load – Strain curve gauges at Corner 0
10 20 30 40 50 60 70
0 5 10 15 20
Load (kN)
Strain (mm/m)
SG8-01 SG8-02
SG8-01 Simulation SG8-02 Simulation
0 10 20 30 40 50 60 70
0 5 10 15 20 25
Load (kN)
Strain (mm/m)
SG8-03
SG8-03 Simulation Opposite
4.7.4 Crack
The crack of the simulation is modeled with the damage and failure model as discussed in section 4.3. The damage parameters are added to the elements with a blue color in Figure 4.28. Blue elements indicated that the damage initiation point is not yet reached. The red color indicates the damage process,s a full red color indicated complete failure of the element. As observed there is a clean cut straight along the weld, clearly pointing toward failure through punching shear. Figure 4.27 shows that the crack of the sample also has a clean cut along the weld, this is identical with the simulation (Figure 4.28).
Figure 4.27; Crack of sample 10 Figure 4.28; Crack of simulation
4.7.5 Damage model
The damage model is implemented in HAZ along the weld. Figure 4.29 depicts an element on the outside of the chord. To see if the damage model is implemented correctly the Von Misses stress is plotted to the principal strain in Figure 4.30.
Figure 4.29; Position element
Figure 4.30 clearly shows stress – strain curve of the material with damage evolution. A clear distinction is observed between the normal stress-strain curve, until a strain of 0.20, and the damage evolution curve from a strain of 0.20 till complete failure at a strain of around 0.61.
Figure 4.30; Stress – Strain Curve element on the outside of the chord
4.7.6 HAZ
The material parameters of the Dog Bone specimen in section 3.3 are not uniform across the length. This results in a strain that is the average strain over the measuring points. The Dog Bone specimen does therefore not provide a reliable constitutive relationship for the material of the HAZ. In this research the HAZ is constructed with the Ramberg Osgood relation in Eurocode 9. To see if this is a proper representation of the material behavior, a simulation is made of the Dog-Bone specimens in section 3.3. For the used plate thickness and weld process the Eurocode specifies an extent of the HAZ of 20mm (Figure 4.31). Literature however specifies that the extent of the HAZ is 10mm for alloy 6061-T6 [13], therefore also a simulation is performed with an HAZ of 10mm (Figure 4.32)
0 50 100 150 200
0 0,1 0,2 0,3 0,4 0,5 0,6 0,7
Stress (N/mm2)
Strain
Outer Element
