Advanced Buckling Analysis of a Reactor Tank Supported by Four Legs
As seen in the July/August 2017 issue of Inspectioneering Journal. Download the PDF version.
INTRODUCTION
The failure of a 15-foot diameter reactor tank supported by
four legs was analyzed using advanced engineering assessment methodology. At
the time of the incident, the cause of the disruption was unknown. However, the
failure was believed to be caused by buckling of the support legs. Shortly
after the reported failure, another tank of identical design was immediately
taken out of service so that an investigation could be performed.
To determine the cause of the failure, a buckling analysis
was executed to determine the buckling capacity of the as-built tank design.
Buckling is a complex phenomenon and requires the application of advanced
finite element analysis (FEA) techniques. Several complexities were involved in
simulating the event of buckling collapse, including precise modeling of
geometric imperfections based on specific fabrication tolerances,
elastic-plastic material behavior simulation, and the use of non-linear and
explicit finite element solving techniques.
An independent design review found that the tanks had been
constructed without a compression ring at the bottom cone floor-to-shell
knuckle weld, which is a violation of API 620 [1]. The results of the buckling
analysis indicated that the failure was likely due to excessive compressive
stress at the floor-to-shell knuckle weld. This article will outline the
engineering and assessment methodologies applied during the analysis of this
tank failure.
BACKGROUND
The number one concern for operators in the oil and gas
industry is avoiding equipment failures. This is true from both a safety
standpoint, as well as an economic standpoint. Common causes of failure
include, but are not limited to, improper operation, inadequate design, and
unexpected loading conditions. No matter the consequence, if a failure occurs,
it is vital for the operator to understand the cause so that lessons can be
learned and future failures can be prevented.
Basic information for this tank is summarized in Table 1.
Table 1. Basic Tank Information
A sister tank of identical design had not yet experienced a
failure, but was taken out of service immediately while an investigation was
carried out. This investigation included an engineering analysis to answer the
following questions:
- What was the cause of failure?
- Is the original design adequate?
- What should be done with the sister tank?
FINITE ELEMENT ANALYSIS
Finite element analysis (FEA) was performed in order to
simulate the failure. The results from the FEA would be used to determine which
components experienced the most severe stresses and strains, and subsequently
which components were expected to fail first.
The finite element model (FEM) was constructed using the
Abaqus [2] CAE finite element modeling program and solved using the Abaqus [2]
2016 explicit FEA solver. The FEM was constructed using linear shell elements
(S4R). Non-linear geometry effects were accounted for and elastic-plastic
material properties were used for the analysis. Figure 1 shows the mesh used
for the FEA.

Figure 1. Mesh used for FEA
Material Properties
In order to perform the elastic-plastic analysis, a
stress-strain needed to be defined. A stress-strain curve for ASTM A36 was obtained from tensile tests performed by University of New Mexico
Civil Engineering Department [3]. This stress-strain curve is shown in Figure
2.

Figure 2. Stress-strain
curve for ASTM A36, obtained from tensile tests performed by University of New
Mexico Civil Engineering Department [3]
Loads and Boundary Conditions
The loads considered for the FEA included gravity loads
(including an additional non-structural mass to account for the weight of
additional internal and external components) and the hydrostatic pressure from
the product. The loads on the tank were increased by adjusting load factor.
Using this approach, the load factor where failure was predicted to occur could
be identified.
The bottom of each support leg was supported by a load cell.
The load cell was designed to fail once its allowable lateral load was
exceeded. In order to simplify this boundary condition, two cases were
analyzed. Case 1 consisted of the bottom of the support columns as fully
restrained against lateral movement. Case 2 consisted of the bottom of the
support columns as un-restrained against lateral movement. Using this approach,
the problem could be bounded since the actual condition was somewhere between
these two cases. These two cases are summarized in Figure 3. Both cases
included a vertical restraint associated with the load cell stiffness.

Figure 3. Support leg boundary condition: Cases 1 and 2
Geometric Imperfections
In order to effectively simulate a buckling failure, small
geometric imperfections need to be considered. This is because small geometric
imperfections will decrease the buckling capacity of a structure. Consider the
classic "soda-can” example: If you take an empty soda can, place it vertically
on a table, and put a weight on the top of it, the can will be able to support
the weight. However, as soon as you touch the center of the can with a pencil
(do not use your finger!), the can collapses. This is because by touching the
can with the pencil, a small imperfection was introduced into the can causing a
decrease in buckling capacity.
Geometric imperfections were included in the support leg
geometry based on fabrication tolerances taken from ASTM A6 "General Requirements
for Rolled Structural Steel Bars, Plates, Shapes, and Sheet Piling” [4]. The
support leg geometry was adjusted based on fabrication tolerances for web
out-of-plumbness and overall camber. This is demonstrated in Figure 4.


Figure 4. Geometric imperfections for web out-of-plumbness (left) and overall camber (right)
RESULTS
The FEA was run by increasing the load factor until buckling
collapse of the structure was observed. Both boundary conditions cases
experienced similar failure modes. The structural behavior of the tank was
dominated by "catenary action” of the cone bottom which caused the
shell-to-bottom weld area to compress like a "compression ring.” The structural
response (or the load carrying behavior) of the tank is summarized in Figure 5.
This is a plot of vertical reaction force (measured at the floor level) of the
entire tank vs. vertical displacement of the tank. Key failure events are
indicated on the plot.

Figure 5. Geometric imperfections for web out-of-plumbness (left) and overall camber (right)
Catenary action is best explained using an analogy of a
clothes line supported atop two posts. When heavy wet laundry is hung, the
clothes line will pull the two poles toward one another. Similarly, the cone
bottom sagged and pulled the shell inward when hydrostatic pressure was applied.
This can be seen in the contour plot of compressive circumferential stress
shown in Figure 6. As the shell was pulled in, a ring of material at and
adjacent to the shell-to-bottom weld was compressed, forming a "compression
ring” zone. This plot corresponds to when the load factor was at 0.2, or 20% of
the expected design load. Already the maximum allowable compressive stress had
been exceeded at this location.

Figure 6. Compressive circumferential stress in the
compression ring zone at LF = 0.2. Cross
sectional view.
Once the load factor was increased to just above the
expected design conditions (LF ~ 1.1), bulging of the bottom cone to shell
knuckle was observed. At this point, buckling was initiated. As a result of
this, high tensile stresses began to form near the knuckle, leading to a risk
of tensile rupture.
A plot of load factor versus compressive plastic strain is
shown in Figure 7. This plot further supports the observation that the knuckle
was exposed to very severe compressive stress, resulting in the material to
yield in compression. Strain-hardening behavior was observed around LF~1.1 (the
same point when buckling was initiating).

Figure 7. Load factor vs. compressive plastic strain
The tank reached its peak vertical load capacity at LF=2.06,
indicating that buckling of the support legs had initiated. However, by the
time this point was reached, the stresses in the bottom knuckle were to the
point where a failure would have occurred before buckling of the support legs would
initiate.
Results Summary
To summarize the collapse behavior of the tank, catenary
action caused the shell to pull inward, developing compressive stress at the knuckle.
The compressive stress was identified to exceed allowable values at LF=0.2. As
the load factor was increased to about 1.1, excessive compressive stress in the
knuckle caused bulging/buckling. This behavior caused tensile stresses to
develop, and a risk of tensile rupture was observed.
The peak load capacity of support columns was reached at
LF=2.06, indicating that buckling of the support legs had initiated. However, the
analysis suggested that the knuckle failed before the support legs buckled, although
in real time these events likely happened very quickly.
In addition to the analysis described above, an additional
design review found that the vessel was designed without a compression ring. It
was determined that the sister tank was also missing a compression ring,
indicating that a similar failure would likely occur if the sister tank was
returned to service. It was recommended that a properly designed compression
ring be installed on the sister tank before returning it to service.
Additionally, a thorough inspection was carried out to ensure that no other
components were damaged as a result of the tank being operated with an
inadequate design.
CONCLUSION
This engineering analysis served as an important reminder of
what can happen when a piece of equipment is improperly designed. In this case,
the tank had been constructed without a compression ring at the bottom cone
floor-to-shell knuckle weld, which is a violation of API 620 [1]. The results
of the buckling analysis reinforced just how important this component was to
the design, as the FEA results indicated that the failure was likely due to
excessive compressive stress at the floor-to-shell knuckle weld and not due to
buckling of the support legs as originally believed.
REFERENCES
- Design and Construction of Large,
Welded, Low-pressure Storage Tanks,
API 620. February 2008, API 620 Eleventh Edition, American Petroleum Institute,
1220 L Street, NW, Washington, DC 29996-4070, USA.
- ABAQUS/Standard
2016, Dassault Systèmes, 166 Valley St. Providence, RI. www.abaqus.com.
- Tensile Test of Steel. University of New Mexico, Civil
Engineering Department. October 31, 2011. https://civilx.unm.edu/laboratories_ss/mechmat/tensilesteel.html
- Standard Specification for
General Requirements for Rolled Structural Steel Bars, Plates, Shapes, and
Sheet Piling,
ASTM A6 - 13. June 2013, ASTM A6 Thirteenth Edition, ASTM International, 100
Barr Harbor Drive, PO Box C700, West Conshohocken, PA 19428.