FEA Project-Pressure Vessel & Heat Loss Analysis

ME/AE 408: Advanced Finite Element Analysis

1
Table of contents
• Introduction and Project summary
• Finite Element (FE) model development
 Procedure
 Mesh dependency and convergence results
• Equations for internal pressure and thermal load cases
• Summary and discussion
 Case 1 – Internal pressure
 Case 2 – Internal temperature
 Case 3 – Internal pressure and temperature

2
Introduction and Project summary:
This project includes the numerical modelling of a pressure vessel with internal pressure and heat
loss on the outside surface. The pressure vessel dimensions are presented below in Figure. 1. Due to
symmetry, just one-eighth of the FE model was developed in ABAQUS/CAE for analysis. This would
save the required computational time significantly for the finer mesh.
Figure 1. Pressure vessel dimensions
The material properties were specified as follows: young’s modulus, E= 207 GPa; poisson’s ratio,
ν= 0.3; mass density, ρ= 7.8×103
kg/m3
; coefficient of thermal expansion= 1.2×10-5
K-1
; thermal
conductivity= 60 W/m/K.
For this project, three different cases were analyzed. Each case and the required results are stated
below:
Case 1- The cylinder is subjected to an internal pressure of 34 MPa. Use fine mesh at the fillet and
perform the convergence study. Plot the stress and strain distribution, and find the maximum von-Mises
stress and its location.
Case 2- The inner surface of the cylinder is kept at 373.15 K, and the heat is lost on the exterior by
convection to the ambient. The convection coefficient is 179 W/m2
/K and the sink temperature is 293.15
K. Plot the temperature distribution, von-Mises stress and strain distributions.
Case 3- Consider both mechanical and thermal loadings (cases 1 and 2). Plot the von-Mises stress and
strain distributions, and find out the maximum von-Mises stress and location.

3
Finite Element (FE) model development
Procedure
A one-eighth model of pressure vessel due to symmetry was developed and analyzed in the
ABAQUS/CAE FE program. The material properties and dimensional geometry were introduced and
assigned to the model according to the problem statement. Three load cases were also considered and
applied to the numerical model as follows:
Case 1- The uniform internal pressure of 34 MPa;
Case 2- The internal temperature boundary condition of 373.15 K with a surface convection coefficient of
179 W/m2
/K and an external sink temperature of 293.15 K;
Case 3- The inclusion of both the internal pressure and the constant temperature with the heat loss du to
convection on the external surface.
The boundary condition on the model was applied to simulate the symmetry condition of the vessel, as
illustrated in Figure. 2. On the right side of the model (y-z) plane, displacement was clamped in the x-
direction. Conversely, on the left side of the model (x-y) plane, displacement was clamped in the z-
direction. At the bottom surface (x-z) plane, displacement was clamped against in the y-direction. Then,
the internal pressure (34 MPa), temperature boundary condition (373.15 K) or both cases was applied for
the applicable case.
Figure 2- Eighth model of the pressure vessel in the ABAQUS/CAE environment

4
The 8-node C3D8RT element was used to mesh the FE vessel model. The different mesh size
were used to investigate the mesh dependency of the results and acquire the accurate mesh independent
results. The finer mesh was used for the filleted corners due to the stress concentration and the
corresponding higher stress value and the coarse mesh toward the ends and parts which potentially
exhibited lesser value of stress and strain. This would allow a computationally economic FE model to
accurately predict the results. Next section provides the results on the convergence study on the results
acquired from the FE model due to mesh variations.

5
Mesh dependency and convergence results
As stated in the previous section, different mesh sizes for the filleted part and straight parts were
considered and convergence studies were implemented. Different mesh sizes including coarse, medium-
coarse, medium, medium-fine and fine were considered for the analyses, as illustrated in Fig. 3.
(Coarse) (Medium-coarse) (Medium)
(Medium-fine) (Fine)
Figure 3- Different mesh sizes considered in the convergence analysis

6
The percentage difference in the computed stresses between different cases considering different
mesh sizes (i.e., coarse, medium-coarse, medium, medium-fine and fine) were analyzed and the mesh
density at which the results started to converge was selected.
From the values specified in the Table 1 it could be noticed that the medium-fine mesh was
enough to acquire the convergency of the results in the analysis. It is also noticed that increasing mesh
density from medium-fine to fine does not significantly increase the accuracy of the results, while it
significantly increases the computational time. Subsequently, the medium-fine mesh was used for further
presentation of the results within this report.
Mesh
density
Seed size at Maximum Von-Mises stress (Pa)
Filleted
side (m)
Flat side
(m)
Case 1
(load)
Deviation
(%)
Case 2
(temp)
Deviation
(%)
Case 3 (load-
temp)
Deviation
(%)
Coarse 0.01 0.04 4.015E+08 -- 7.342E+06 -- 4.991E08 --
Medium-
coarse
0.0075 0.03 4.982E+08 24.1 9.045E+06 23.2 5.10E+08 2.18
Medium 0.005 0.02 5.011E+08 0.58 1.082E+07 19.62 5.321E+08 4.33
Medium-
fine
0.00375 0.015 5.048E+08 0.74 1.231E+07 13.77 5.551E+08 4.32
Fine 0.0025 0.01 5.102E+08 1.07 1.297E+07 5.36 5.57E+08 0.34

7
Equations for internal pressure and thermal load cases:
In this study the 3D-solid elements were used to represent the thick-walled pressure vessel. The
solution for the finite element model for a virtually small displaced body would be as follow:
1 1
2 2
3 3
x
y
z
u
u u
u
w u
w u w u
w u
δ
δ δ δ
δ
 
 
= = Ψ∆ 
 
 
= 
 
= = = =Ψ ∆ 
 = 
Where in the above Δ is for nodal values and Ψ presents the interpolation functions.
The finite element model, as stated in Reddy’s text book has the following form then:
e e e e e e
M K F Q∆ + ∆ = +
Where in the above equation, M is the mass matrix, K is the stiffness matrix, F is the element load vector,
and Q is the vector of internal forces.
The weak form of the Poisson equation for the heat transfer problem could be used as below:
( )0
e e e
x y z n
w T w T w T
k k k wg dx wTds w q T ds
dx dx dy dy dz dz
β β ∞
Ω Γ Γ
 ∂ ∂ ∂ ∂ ∂ ∂
= + + − + − + 
 
∫ ∫ ∫ 
While the finite element solution of the above equation could be stated as below:
( )
1
, ,
n
e e
j j
j
T T x y zψ
=
= ∑
Where T and Ψ in the above equation are the nodal temperature and shape (interpolation) functions,
respectively.
The finite element model then as shown in the Reddy’s textbook could be constructed as below:
e e e e
K T f Q= +

8
Summary and discussion:
The tabulated values as the summary of the numerical study on the pressure vessel for three
different cases are presented. As intuitively expected, the results for case 3 (internal pressure +
temperature) caused the largest stress and strain values when compared with case 1 (internal pressure
only) and case 2 (thermal), due to combined stresses by combined loading conditions (mechanical +
thermal). Details for each case are detailed in next sections.
Load case Maximum
Von-mises
stress (Pa)
Case 1 (internal pressure only) 5.048E+08
Case 2 (temperature) 1.231E+07
Case 3 (case 1 + case 2) 5.551E+08
Case 1: Internal pressure
This case represented a thick-walled pressure vessel under the 34 MPa internal pressure. The plot
of maximum stress and corresponding strain outputs for this case are shown below in Figures 4 and 5.
The maximum Von-mises stress reached was 504.8 MPa, as specified with a dashed rectangle at the
inside filleted corner and top edge (two loctions).
Figure 4- Von-mises stress distribution for case 1

9
The strain distribution for the case 1 in shown in Figure 5, below and it could be noticed that the
maximum strain was just 0.00247 mm/mm.
Figure 5- Strain distribution for case 1

10
Case 2: Internal temperature only
The second case represented the thick-walled cylinder with an internal temperature. The
temperature distribution on the internal surface of the cylinder, which is constant, is shown in Figure 6
(373.15 K). The outside temperature on the outer surface of the pressure vessel is also shown in Figure 6
(right). The outside temperature is 365.5 K at the top curved portion of the vessel, while it is around 367.4
K at the flat middle edge of the cylinder. The consistent deviation of the temperature throughout the
vessel thickness is noticed from Figure 6. It is noted that not significant portion of the temperature is
deviated from the inside to the outside surface of the vessel.
Figure 6- Temperature distribution on the inner (left) and outer (right) surface for case 2

11
The stress distribution for case 2 is included below in Figure 7. It is clear that only one spot on the top
filleted portion in the inner surface of the vessel exhibited the maximum
Figure 7- Von-mises stress distribution for case 2

12
The strain distribution for the case 2 is also plotted in the Figure 8. It could be noticed that the strain
values, and corresponding stress values similarly, are significantly smaller for case 2 compared with case
1, when the temperature deviation exists only. The maximum strain for case 2 was 4.507E-03 mm/mm.

13
Case 3: Internal pressure and temperature
This case represented the 34 MPa internal pressure and the temperature gradient. The temperature
on the inner and outer surface of the vessel is presented in the Figure 9. It is seen from the results that the
inner temperature is 373.1 K, while the outside temperature is in the range of 359.5~361.5 K on the
outside surface of the vessel. It is seen that no deviation on the temperature gradient exists between the
cases 2 and 3, which is expected. The thermal and physical mechanical properties are identical between
these two cases, leading to same temperature gradient throughout the thickness.
Figure 9- Temperature distribution for case 3

14
The Von-mises stress distribution for the case 3 is also presented in Figure 10. The maximum
Von-mises stress is 555.1 MPa for this case. It is seen that at two locations (top center and filleted corner),
the maximum stress values occur. However, the maximum stress for this case is larger than the case 1,
which is expected due to the combined stresses from internal pressure and thermal interaction.
Figure 10- Stress distribution for case 3

15
The maximum strain and strain distribution for the case 3 is also plotted in Figure 11. It is seen
that the maximum strain is 7.148E-03 mm/mm in this case. As expected, the maximum strain value
reached in this case is also greater than both last cases 1 and 2 due to applied actions.

FEA Project-Pressure Vessel & Heat Loss Analysis

Recommended

Recommended

More Related Content

What's hot

What's hot (18)

Viewers also liked

Viewers also liked (9)

Similar to FEA Project-Pressure Vessel & Heat Loss Analysis

Similar to FEA Project-Pressure Vessel & Heat Loss Analysis (20)

FEA Project-Pressure Vessel & Heat Loss Analysis