1.
Nonlinear Post­Buckling Analysis of a 12,000 Gallon Transport Tank
Ronald Boutilier
CEE 506: Nonlinear Analysis of Structural Systems
University of Washington
June 9, 2016

2.
TABLE OF CONTENTS
1 Objectives of the Study…………….………………………...………………………………3
2 Development of the Analytical Model………………………………………...……………….3
2.1 Vessel Geometry………………………………………………………....…………….3
2.2 Materials………………………………………………………………...……………..4
2.3 Load and Boundary Conditions……………………………………….………………..4
3 Method of Analysis…………………………………………………………...………………4
3.1 Analysis Parameters………………………………………………..……………………4
3.2 Expected Elastic Behavior of Vessel Under Compressive Loading…………………….….5
3.3 Eigenvalue Analysis Procedure to Determine Critical Buckling…………………….……...6
3.4 Post­buckling Analysis Procedure………………………………………....……………..6
4 Results of the Finite Element Simulations……………………………………….……………...6
4.1 Results from the Eigenvalue Analysis………………………………....…………………..6
4.2 Results from the Post­buckling Analysis…………………………....…………………….7
4.2.1 Post­buckling of the Empty Vessel……………………………....…………………7
4.2.1.1 Simulation of the Model With 15993 Elements……………………….……..7
4.2.1.2 Simulation of the Model With 8853 Elements……………………….………8
4.2.1.3 Simulation of the Model With 4993 Elements………………………..……...9
4.2.1.4 Mesh Refinement Comparison of Empty Vessel Models…………………...10
4.2.2 Post­buckling of the Vessel Under Normal Operating Conditions………………....10
4.2.2.1 Simulation of the Model With 15993 Elements………………………….....11
4.2.2.2 Simulation of the Model With 8853 Elements…………………………..….11
4.2.2.3 Simulation of the Model with 4993 Elments…………………………….….12
4.2.2.4 Mesh Refinement Comparison of Empty Vessel Models…………………...13
5. Conclusions………………………………………………………………………….13
6. References…………………………………………………………………………...14
2

3.
I n the cargo tank manufacturing industry it has long been argued that the U.S. Department of
Transportation (DOT) rules for the design of cargo tanks (49 CFR 178.337­3), which requires a safety
factor of 4.0 for the allowable stress in the tank wall during an extreme event, are too conservative for
practical application. In addition, the U.S. DOT rules require the use of the 1998 edition of Section VIII
of the ASME Boiler and Pressure Vessel Code, which is now over 10 years out of date, and there has
been much improvement on the code since then, and it has been shown that leaks in the cargo tank wall
due to an accident are indeed an extremely rare occurence (see example:
http://www.fireengineering.com/articles/print/volume­156/issue­7/features/lpg­tanker­rollover­lessons­le
arned­in­suffolk­virginia.html ) .
1. Objectives of the Study
The goal of this analysis is to examine the post­buckling behavior of a cargo tank shell as a result of an
extreme longitudinal compressive force applied at the rear end. Interpretation of the results may be
useful to further support the implementation of Section XII (Rules for Construction and Continued
Service of Transport Tanks) of the ASME Boiler and Pressure Vessel Code in current US DOT
regulations.
2. Development of the Analytical Model
2.1 Vessel Geometry
The overall geometry of the transport tank is shown in Figure 1 below. The component that was
analyzed was the tank bullet, which is herein referred to as the vessel. The vessel consists of a cylindrical
shell with a hemispherical head at each end. For simplicity, the vessel is modeled with a uniform
thickness of 0.375”. In addition, the vessel is assumed to be seamless, so that the potential effects of
weld geometry are not considered.
Figure 1: Dimensions of the 12,000 gallon transport tank
3

4.
2.2 Materials
The material used for construction of the vessel wall is ASME specification SA­517 grade E. Data for
the plastic behavior cannot be obtained, so for simplicity, data from typical ASTM A36 steel was
extrapolated. The extrapolated plastic behavior is summarized below, and used to take into
consideration the projected material nonlinearity of the system. Lastly, irregularities due to welding
heat­affected zone, quenching, tempering, and post­weld heat treatment are not considered.
Yield Stress (psi) Inelastic Strain (in/in)
100,000 0
100,000 0.016
120,000 0.098
Table 1: Projected plastic behavior data for SA­517E high strength QT steel
2.3 Loads and Boundary Conditions
Shown in Figure 2 below is the general FBD for the vessel model. The buckling load (discussed in later
sections) will be imposed on the rear end of the tank, while the front end is pinned.
Figure 2: Free­body diagram of the vessel
3. Method of Analysis
Finite element modeling was used to simulate the critical buckling and post­buckling behavior of the
system. The software used to perform the finite element simulation was ABAQUS. The type of elements
used consisted entirely of thin plate 3D shell elements, using a full integration scheme.
3.1 Analysis Parameters
The effects of mesh refinement of the finite element model were considered for the entire model
consisting of 15,993 elements, 8,853 elements, and 4,993 elements, respectively. Then, for each mesh
refinement considered, the vessel was analyzed as (a) an empty vessel under ambient conditions, and
4

5.
(b) a fully loaded vessel under normal operating conditions. The definition of “normal operating
conditions” is as follows:
1. Cargo tank internal pressure = 250 psi
2. Cargo tank loaded with liquefied petroleum gas (LPG) to 85% of nominal capacity
Calculations performed in MATLAB, for the gravity loading imposed by the weight of LPG are shown
below:
3.2 Expected Elastic Behavior of Vessel Under Compressive Loading
The calculations are shown below for the expected first­order elastic behavior of the vessel under
compression. The calculation is idealized for a cylinder under uniform compressive loading. These
calculations are taken from Timoshenko Book on Elastic Stability.
5

6.
3.3 Eigenvalue Analysis Procedure to Determine Critical Buckling
In addition to the calculations above, ABAQUS was used to determine the eigenvalues for buckling.
This was done by choosing the linear­perturbation procedure for the time step used in the solution
algorithm. The parameters for this time step are as follows:
1. Number of Eigenvalues requested: 5
2. Vectors used per iteration: 10
3. Maximum number of iterations: 300
A file was then created with the buckling information from this solution, and was imported into the
post­buckling analysis, described in the next section.
3.4 Post­buckling Analysis Procedure
The post­buckling analysis was performed using an incremental force­based approach. In ABAQUS,
the Rik’s Algorithm was the chosen solution algorithm. The parameters for this time step are as follows:
1. Maximum number of increments: 1000
2. Initial arc length increment: 0.01
3. Minimum arc length increment: 1e­5
4. Maximum arc length increment: 1
5. Estimated total arc length: 1
To add an initial imperfection to the system, the results from the eigenvalue analysis were loaded for the
first step. Then the imperfection was introduced by taking the displacements from the eigenvalues of the
first 3 modes and applying a scaling factor. The scaling factors were taken to be 0.0375, 0.01875, and
0.009375, respectively.
Finally geometric nonlinearity was analyzed due to the effect of large displacements as the tank buckles,
by choosing the NLGeom feature in ABAQUS.
4. Results of the Finite Element Simulations
The results shown below are for the eigenvalue and post­buckling simulations ran by ABAQUS,
including the results for the empty vessel, and the vessel under normal operating conditions, with respect
to mesh refinement.
4.1 Results from the Eigenvalue Analysis
In the figure shown below details the results from the Eigenvalue analysis. The 5 eigenvalues are shown
below.
6

7.
Figure 3: Illustration and summary of the results from the eigenvalue analysis using ABAQUS
4.2 Results from the Post­buckling Analysis
After determining the eigenvalues from the previous analysis, a total load of 5e6 lbs was applied to the
rear end of the vessel to impose buckling. The results for each case are detailed in the next sections.
4.2.1 Post­buckling of the Empty Vessel
The results for the buckling of the empty vessel with respect to mesh refinement are detailed in the next
sections. Each mesh consisted of a combination of triangular and quadrilateral shaped shell elements.
Initially, there were some distorted elements identified. These distortions were eliminated by refining the
edge seed distances around the problematic areas. Each simulation ran for approximately 10­40
minutes, until at least 100 load increments were applied.
4.2.1.1 Simulation of the Model With 15993 Elements
The simulation of the empty vessel model with a mesh size of 15993 elements is illustrated below.
7

8.
Figure 4: Illustration of the evolution of deformation and Von Mises stress for the empty
vessel model with a mesh size of 15993 elements
4.2.1.2 Simulation of the Model WIth 8853 Elements
The simulation of the empty vessel model with a mesh size of 8853 elements is illustrated below.
Figure 4: Illustration of the evolution of deformation and Von Mises stress for the empty
vessel model with a mesh size of 8853 elements
8

9.
4.2.1.3 Simulation of the Model With 4993 Elements
The simulation of the empty tank model with a mesh size of 4993 elements is illustrated below.
Figure 5: Illustration of the evolution of deformation and Von Mises stress for the empty
vessel model with a mesh size of 4993 elements
9

10.
4.2.1.4 Mesh Refinement Comparison of Empty Vessel Models
The figure below illustrates the load­displacement of the rear­end of the empty tank, for each mesh size,
and the theoretical elastic behavior of the vessel as calculated earlier. It is observed that initially the mesh
size has no effect on the relative elastic behavior, but immediately after buckling it appears that the
higher mesh refinement results in a lower load, then converges after 1.5 inches.
Figure 6: Plot of the load vs. displacement for each empty vessel model with respect to mesh
size, in comparison with the theoretical elastic behavior
4.2.2 Post­buckling of the Vessel Under Normal Operating Conditions
The results for the buckling of the vessel under normal operating conditions, with respect to mesh
refinement are detailed in the next sections. Each mesh consisted of a combination of triangular and
quadrilateral shaped shell elements. Initially, there were some distorted elements identified. These
distortions were eliminated by refining the edge seed distances around the problematic areas. Each
simulation ran for approximately 10­40 minutes, until at least 100 load increments were applied.
10

11.
4.2.2.1 Simulation of the Model With 15993 Elements
The simulation of the vessel under normal operating conditions model with a mesh size of 15993
elements is illustrated below.
Figure 7: Illustration of the evolution of deformation and Von Mises stress for the vessel
model under normal operating conditions with a mesh size of 15993 elements
4.2.2.2 Simulation of the Model With 8853 Elements
The simulation of the vessel under normal operating conditions model with a mesh size of 8853 elements
is illustrated below.
11

12.
Figure 8: Illustration of the evolution of deformation and Von Mises stress for the vessel
model under normal operating conditions with a mesh size of 8853 elements
4.2.2.3 Simulation of the Model With 4993 Elements
The simulation of the vessel under normal operating conditions model with a mesh size of 15993
elements is illustrated below.
Figure 9: Illustration of the evolution of deformation and Von Mises stress for the vessel
model under normal operating conditions with a mesh size of 4993 elements
12

13.
4.2.2.4 Mesh Refinement Comparison of Vessel Under Normal Operating Conditions
The figure below illustrates the load­displacement of the rear­end of the vessel under normal operating
conditions, for each mesh size, and the theoretical elastic behavior of the vessel as calculated earlier.
The results for the buckling loads are higher than in Figure 6. This is because the internal pressure
provides additional stability by resisting bending forces normal to the vessel wall. The relative effect of
mesh refinement is the same as shown in Figure 6.
Figure 10: Plot of the load vs. displacement for each vessel model under normal operating
conditions with respect to mesh size, in comparison with the theoretical elastic behavior
5. Conclusions
The purpose of this study was to use ABAQUS to examine the post­buckling behavior of a transport
tank. Geometric nonlinearity, material nonlinearity, and mesh refinement were all considered in the
analysis.
The results conclude that the ABAQUS finite element method provides a reasonable analysis
simulation of the post­buckling behavior of a cargo tank vessel. It can be observed that the behavior in
the elastic region for both vessel models closely match the theoretical elastic behavior under
compressive loading. However, in each case, the elastic strength of the vessel is higher for the finite
element simulations. One reason for this is that the hemispherical heads provide stability to the cylinder,
whereas the theoretical calculation assumes an open end.
The critical buckling loads, which are close to 3000 kips in each case are very high, and there
would likely never be a case in which an impact due to an accident would impose such a force to cause
the vessel to buckle. Therefore, at least in terms of buckling, the safety factor of 3.5 for allowable stress,
used in ASME Section VIII Division 1, or Section XII is a conservative enough value for application.
For the extensive time it took (approximately 2 hours total) to simulate the
13

14.
buckling/post­buckling behavior of the vessel, it is probably not feasible to use the results for persuasion
of the U.S. government to update its regulations, especially when they already continue to implement
codes that are over 10 years out of date. Furthermore, buckling is only one aspect of vessel failure to be
investigated. Finally, only the longitudinal direction of loading was examined. Loadings in the lateral and
vertical directions should also be examined to compare with the load requirements in current regulations.
References:
Goodman, Kent. "Buckling Stress Check for a Vertical Vessel." Www.maximumreach.com . Maximum
Reach Enterprises, 2 Nov. 2012. Web. 9 June 2016.
<http://www.maximumreach.com/Buckling%20Stress%20Check.pdf>.
Haring, Raymond. "LPG Tanker Truck Rollover: Lessons Learned in Suffolk Virginia."
Fireengineering.com . Fire Engineering, July 2003. Web. 9 June 2016.
< http://www.fireengineering.com/articles/print/volume­156/issue­7/features/lpg­tanker­rollover­l
essons­learned­in­suffolk­virginia.html >.
ASME Bolier and Pressure Vessel Code Section VIII
US Code of Federal Regulations: Transportation, 49 CFR 178.337­3, Design and Construction of MC
331 Cargo Tanks
14