エイシーティ株式会社は、CAE構築・推進のためのベストパートナーです。

A Procedure for Capping Errant Pressure Pipelines

Summary

This study is a preliminary analysis of the possibility of capping a broken pipe with internal pressure such as that shown by the pipe in Deep Horizon.

The study performs the analysis of two models. The first analysis was done to understand the parameters affecting the analysis. The analysis showed that the model would yield unacceptable strains. A second model was designed that would mitigate the large strains found in the first model. Analysis showed that the design would contain the large strains.

Finally a discussion is carried out on the implications of the analysis and the feasibility of constructing a rig to carry out the capping of a pipe with internal pressure.

Introduction

In this note we study a last resort method of capping pressurized oil pipes. The method consists of building a frame around the pipe and using this to clamp two plates to crimp the pipe flat. The details of the frame and the method of applying the force on the plates are left undefined. In many cases the power for such a device might be obtained off the shelf since the loads required are expected to be of the order of the circumferential stresses caused by the internal stresses (per unit length of the loading on the pipe). In this study we only consider the nonlinear behavior of pressurized straight pipes subjected to a flattening load.

The crimping or crushing of pipes is a much-studied problem. It is part of the domain of structural mechanics concerned with the large displacement elastic plastic analysis of doubly curved shells. This is usually performed with a Finite Element Analysis using one of several commercial programs. In this study we use the writer’s general purpose MPACT program.

When one first considers the behavior of doubly curved shells, one is surprised by their complex behavior. The flexibility of the thin shells cause flexing in any direction on the plane of the shell. This behavior is significantly influenced by the ratio of thickness to radius of the shell. [1] The properties of elastic-plastic behavior of steel is such that it can tolerate large strains of the order of 20% for at least 100 cycles, so we can easily withstand a single application of such magnitudes of strains with a lot in hand. Design taking advantage of this property is referred to as limited life design [2]. [See www.lifecyclevnv.com/serve02.htm]

In this study we do not consider the effects of cold temperatures that might cause brittle fracture.

Analysis, Preliminary model

In order to understand the problem, we consider a typical pipe. The dimensions of the pipe are:Radius 12.7” and 50” long with a thickness of 0.6”. The material is assumed to be elastic-perfectly plastic with Young’s modulus 30,000000 psi and a yield stress of 20,000 psi. We assume an internal pressure of 3000 p.s.i. The pipe ends are assumed to be fixed in the longitudinal direction.

The model is made up of 20 X 10 X 2 elements. 27 node hexahedral finite elements were used. Because of the accuracy of these elements and the relatively thick shell, it was thought that the shell only required two elements through the thickness.

Because of symmetry, we consider only a quarter of the pipe. The pipe was loaded in the z direction by a displacement applied to the corner 9 elements, (colored blue) in the first diagram that shows a lightly loaded model. A maximum of 10” z displacement was applied in increments of 0.1” per increment.

　　Fig.1 Lightly loaded model. Contours of equivalent stress
　　Fig.2 Applied displacement of 10 ins.

From it we can already see the complex bending patterns inherent in this shell behavior.

Fig.2 gives the elastic-plastic strains of the model in its maximum applied displacement. The white elements show the model in its original position.
The point of maximum strain is shown in orange at the outer corner of the nine displaced faces. The predicted strain of 50% is probably more than one should subject the pipe to. The bending strains in the axis of symmetry x=0 is of the order of 25% and is more acceptable.

The result shown here is the main conclusion of the analysis. If one were to set up a crimping mechanism, it would have to address this point of maximum strain. In our second model, we try to do so.

Fig.3 Equivalent stress at maximum displacement of 10 ins.

The equivalent stress contour concludes the results of our first model. Several runs were made with an estimated pressure of 3000 psi in the pipe (The pressure was estimated from the depth of the wellhead of 5,000 ft.)

Analysis, Second Model.

In our next model we set up a block that loads our model by contact. The block surface slopes away from the shell so as to mitigate the effect of the sudden transition of load at the edge of the plate.

The pipe part of the model remained the same. The block is modeled with 1 element through the thickness and the dimensions were selected to result in low stresses in the block, viz. a very stiff block.

　Fig. 4 shows the pipe being loaded by contact from a stiff block. Slope starts after 10” in x dir.

This shows the block, which applies the displacement to our model by contact.

　Fig. 5 shows the stress at initial contact.

The analysis progressed smoothly. In the next two diagrams we show the results for the model loaded to 1.8 ins.

　Fig. 6 shows the contact region. Max elastic-plastic strain of 7.08% was observed.

This figure shows the loading has progressed to the start of the slope of the block. As expected the maximum observed plastic strain was limited from then on by contact with the sloping part of the block.

　Fig. 7 Equivalent strain, sideview, 3.6 ins. Displacement.

We note that the maximum elastic-plastic strain has been contained by our design of the sloping contact face.

　Fig. 8 Deformed and original geometry shown at x=0. 3.6 ins. Disp.
　Fig. 9 Side view of displaced and original geometry.

The above diagram gives a good idea of the controlled deformation imposed on the pipe. It is intended to show the closing of the pipe. Note from the equivalent strain contours that the maximum elastic-plastic strains have been contained.

The Figure shows the calculation of the compressive load obtained at the top of the block by integration of the zz stresses. The stress contours gives an idea of the load concentration in the corner of the block. We recall that this was the area in which we applied our displacements in our original model.

This shows the vertical applied load for each time/step. Each time/step is equivalent to the application of 0.1 ins of vertical displacement.

This diagram shows the variation of maximum plastic strain calculated with time, i.e. with applied displacement. Note that the maximum strains are contained at 8.5%.

Discussion and Conclusions.

The analysis has demonstrated the limiting of the maximum plastic strains at 8.5%. Even with a linear extrapolation of the applied displacement we would obtain a maximum strain of 27%. This is well within our fatigue limit. It is unfortunate that the instability occurred at a low displacement of 3.6. The instability point will vary with the parameters of the shell. The analysis shows the large loads associated with the vertical loading. This is in fact the force required to overcome the internal pressure.

If one were to pursue this avenue of capping of the pressurized pipe, it would be necessary to construct a frame where two plates could be bolted together in a vertical position to the ocean floor. However one would expect that if the capping were performed near the wellhead, the horizontal pipe would have a tendency to rise towards the vertical position. This is because of the effect of the internal pressure in the longitudinal direction.

The quarter loads of 133,000 pounds are large and would require bolting together with steel bolts of 10 sq. ins. The loads associated with the frame designed to implement this are small compared to the forces associated with the construction of an oil platform. So it is well within the oil industry’s capability to design and construct this and probably within a time scale measured in days. However it is noted that in the longer term only one of these capping frames would need to be constructed and this would free the industry from the environmental consequences of a burst pipe such as that happening for the Deep Horizon pipe.

Future work would consist of trying a dynamic approach known as slow dynamics in FEA to get past the instability point of the analysis. Clearly this and some experimental work would be undertaken if the construction of such a capping device would be made.

References.

1. Zienkiewicz, O.C. and Taylor, R. L. ´The Finite Element Method, Solid Mechanics”, Vol 2, Butterworth and Heinemann, 2000
2. Marcal, P. V. and Turner, C.E. “Limited Life of Shells of Revolution Subjected to Severe Local Bending”, J. Mech. Eng. Sci., 1965, 7, 4.
   
   

コメント欄 (Comment)

• コメントの入力方法　
  • 下記記入欄で、[お名前]を入力してください。
  • [認証コード(****)]で、数字****をそのまま入力してください。
  • コメント記載欄に、あなたのコメントを書いてください。
  • [コメントの挿入]をクリックしてください。
    操作は以上です。コメント欄のすぐ上にあなたのコメントが表示されます。

• どうぞ、ご自由に皆様のご意見、ご質問等をお送りください。
  
  
  
  お名前: 認証コード(9635)