Practical Application of Finite Element VII. Simplified ANSYS model ANSYS 10 or 11 ED (Education version or Academic version) will be used for modelling the structure. A disadvantage of this software is the limitation of nodes (10000 nodes) and the amount of elements (1000 elements). Therefore, the reinforced concrete is restricted to model in the range of element given. The results may be acceptable in this situation.
Figure 5 VII.1. Element types Preprocessor -> Element type -> Add/Edit/Delete -> Add Choose Concrete 65 (SOLID65)
Figure 6 Similarly to choose: BEAM -> PLASTIC 23 (BEAM23) In the OPTION of BEAM23, choose ROUND SOLID BAR at Cross-section K6 VII.2. Real Constants Preprocessor -> Real Constants -> Add/Edit/Delete -> Add - Choosing SOLID65 as SET 1 and no input data at here because the rebar will be modelled as BEAM23. In addition, SOLID65 element only supports 3 rebars however there are 4 rebars in this problems. - Similarly to choose BEAM23 as SET 2: OUTER DIAMETER OD: 0.012 VII.3. Material properties
TU T NGUYEN @00221721
1
Practical Application of Finite Element There are 2 material properties needing to be input. One is concrete, one is rebar. Preprocessor -> Material Props -> Material Models
Figure 7 + Concrete (Material Model Number 1): -
-
Structural -> Linear -> Elastics -> Isotropic: o
EX (Young’s modulus): 3E10
o
PRXY (Poisson’s ratio): 0.2
Structural -> Nonlinear -> Inelastic -> Rate Independent -> Isotropic Hardening Plasticity -> Mises Plasticity -> Multilinear
In this situation, the ratio between stress and strain must be equal to Young’s module at the first data, and then this ratio is decreased to the last data when the compressive strength increases. As the figure below shown, the cross-area is safe-area, where the reinforced concrete does not crack or crush.
Figure 8 A: Safe area, B: Starting cracking, C: Totally collapsed Strain 0.0005 0.0010 TU T NGUYEN @00221721
Stress 1.5E7 2.1E7 2
Practical Application of Finite Element 0.0015 0.0020 0.0025 0.0030 -
2.4E7 2.7E7 3.0E7 2.4E7
Structural -> Nonlinear -> Inelastic -> Non-linear Metal Plasticity -> Concrete o
Shear transfer coefficients for an open crack (ShrCf-Op): 0.5
o
Shear transfer coefficients for a closed crack (ShrCf-Cl): 0.9
o
Uniaxial tensile cracking stress (UnTensSf): 3E6
o
Uniaxial crushing stress (positive) (UnComSt): 3E7
+ Rebar (Material Properties 2): -
-
Structural -> Linear -> Elastics -> Isotropic: o
EX (Young’s modulus): 2E11
o
PRXY (Poisson’s ratio): 0.3
Structural -> Nonlinear -> Inelastic -> Rate Independent -> Isotropic Hardening Plasticity -> Mises Plasticity -> Bilinear o
Yield Stress: 460 N/mm2
o
Tang mod: 0
Figure 9 VII.4. Modelling The beam given is symmetrical geography and concentrated load, therefore, one half of the beam will be taken for simplification of computer model. L = 5.5/2 = 2.75mm D = 0.4m B = 0.25m
There are 4 rebars, the cover is 0.05m
Therefore, the model will have 780 nodes (6 nodes in Z direction, 5 nodes in Y direction, 26 nodes in X direction and have 4x5x25 = 500 elements < 1000 elements. Modelling structural form with first-six-nodes in Z direction, after that using COPY function to finish the model. Preprocessor -> Modelling -> Create -> Nodes -> In Active CS Node TU T NGUYEN @00221721
X
Y
Z 3
Practical Application of Finite Element 1
0.00
0.00
0.00
2
0.00
0.00
0.05
3
0.00
0.00
0.10
4
0.00
0.00
0.15
5
0.00
0.00
0.20
6
0.00
0.00
0.25
- These nodes need to copy to become the structural model. Co-ordinate
Distance from NODE I to NODE J
Axis X
0.11
Axis Y
0.1
Axis Z
0.05
+ Generating node in Y direction Modelling -> Create -> Copy -> Nodes -> Copy - ITEM NUMBER OF COPIES: 5 - DX (X-offset in active CS): 0 - DY (X-offset in active CS): 0.1 - DZ (X-offset in active CS): 0 + Generating node in X direction - ITEM NUMBER OF COPIES: 26 - DX (X-offset in active CS): 0.11 - DY (X-offset in active CS): 0 - DZ (X-offset in active CS): 0 VII.5. Creating element SOLID65 will be created with all nodes. The node list should be opened to simply create each element. Element Attributes of SOLID65: -
Element type of number : SOLID65
-
Material Number: 1
-
Real Constant set number: 1
Creating SOLID65 element, Command-line should be input E,1,31,32,2,7,37,38,8 because of a simple creation in three-dimension (3D). Similar way to the other SOLID65 element.
Element
Input Command-line
Concrete block 1
E,1,31,32,2,7,37,38,8
Concrete block 2
E,2,32,33,3,8,38,39,9
TU T NGUYEN @00221721
4
Practical Application of Finite Element Concrete block 3
E,3,33,34,4,9,39,40,10
Concrete block 4
E,4,34,35,5,10,40,41,11
Concrete block 5
E,5,35,36,6,11,41,42,12
Element Attributes of BEAM23: -
Element type of number : BEAM23
-
Material Number: 2
-
Real Constant set number: 2
Element
Node I
Node J
Comment on creating
Rebar 1
8
38
To simply create element in 3D, at command-line: e,8,38 for
Rebar 2
9
39
Rebar 1.
Rebar 3
10
40
Similarly to creating node, the rebar 1 should be copy to the
Rebar 4
11
41
end of the beam: ITEM NUMBER OF COPIES: 25, and NODE NUMBER INCREMENT: 30
1 ELEMENTS FEB 12 2010 11:21:44
Reinforcement
Figure 10 – Rebar created in concrete
TU T NGUYEN @00221721
5
Practical Application of Finite Element ELEMENTS FEB 12 2010 12:12:54
Y
Z
X
Reinforcement
Figure 11 – Structural Model finished
VII.6. Applying boundary condition -
Solution Type o
Solution -> Analysis Type -> New Analysis -> Choose Structural
o
Solution -> Sol’n Controls
Frequency: Write every substep (Investigation cracks start to take shape in the reinforced concrete)
-
Number of substeps: 20
Max no. of substeps: 1000000
Min no. of substeps: 20
Define loads: o
Solution -> Define Loads -> Apply -> Structural -> Displacement -> On Node UX is applied for nodes from 751 to 780 at the end of the structural model. UY and UZ is applied for nodes 1,2,3,4,5, 6.
TU T NGUYEN @00221721
6
Practical Application of Finite Element S FEB 12 2010 16:51:33
Y
Z
Su
X
ort of the beam
Figure 12 o
Solution -> Define Loads -> Apply -> Pressure -> On Elements (External load applieds for investigating cracks and crush of concrete at L/3 = 1.8666) The 500000N applies at sixteenth element on top of the reinforced concrete.
VII.7. Results To view the region of crack and crush: - General PostProc -> Read Results -> By Pick, - General PostProc -> Plot Results -> Concrete Plot -> Crack/Crush o Plot symbols are located at: Integration pts Plot crack faces for: any cracks o Time history:
TU T NGUYEN @00221721
7
Practical Application of Finite Element
Figure 13 – Time history Investigation of a cracked line is at 0.9 of time-line: CRACKS AND CRUSHING FEB 12 2010
STEP=1
15:56:05
SUB =18 TIME=.9
Y Z
X
Figure 14 – No Crack and Crush However, crack and crush start occurring in concrete block at the last step:
TU T NGUYEN @00221721
8
Practical Application of Finite Element CRACKS
AND
CRUSHING FEB 12 2010
STEP=1 SUB
16:06:37
=999999
TIME=1
Y Z
X
Figure 15 – Crack and crush with Element Centroids
1 CRACKS AND CRUSHING FEB 12 2010
STEP=1
16:11:52
SUB =999999 TIME=1
Figure 16 – View at the region of crack
TU T NGUYEN @00221721
9
Practical Application of Finite Element CRACKS AND CRUSHING FEB 12 2010
STEP=1
22:18:49
SUB =999999 TIME=1
Y Z
X
Figure 17 – Crack and Crush with Integration pts Reinforced concrete has more cracked line when the analysis of plastic criteria with 170kN 1 CRACKS AND CRUSHING FEB 12 2010
STEP=1
15:09:47
SUB =11 TIME=.002737
Region of crack and crush
Y Z
X
Figure 17 – Analysis of plastic criteria
TU T NGUYEN @00221721
10
