^{1}

^{2}

^{*}

In designing a horizontal directional drilling (HDD) pipeline project, designers
face the challenge of determining the regions of maximum and minimum stresses
on pipelines, ensuring the stability of the bore-hole from collapse and minimizing the stresses induced on the pipeline due to the bore-profile. This study analyses the stress induced on an HDD pipeline system using the ANSYS Version 18, mechanical APDL finite element (FE) software. The pipeline used as the case study was a gas transmission pipeline installed in south-west Nigeria. A macro-file for ANSYS Version 18, mechanical APDL used to model the pipeline was developed. The results showed that the maximum and minimum stresses induced on the HDD pipeline were at the top and bottom of the pipe, respectively; while the stresses on the sides were uniform (≈888
kg/cm^{2}) all through the pipeline, irrespective of element number. The maximum stress occurred at the curvature point with the highest entry angle (10
°), resulting in a maximum deflection at this point. The model stress validation performed by comparing results with theoretical solutions, both with respect to radius of curvature and internal pressure, showed percentage difference (errors) less than 10%. The cross sectional area validation showed a percentage difference of 0.059%.

The loads acting on the pipe include its weight, the internal operating pressure and the external pressure due to the overhead soil load [

HDD pipelines are subjected to a combination of tension, bending, and external pressure. Drilled path design and pipe specification may be governed by these installation loads, as they could be more severe than operational loads [

In the analysis and design of underground structures, the finite element method (FEM) has been used extensively as an effective numerical technique. The results more reasonably reflect the actual situation, providing an improved design procedure to avoid pipe wear and breakage [

Its application ranges from the study of aircraft or automobile structural framework, complicated thermal system (nuclear power plant), to the analysis of a fluid flowing through a duct, over a weir, or through the earth [

Spectrum technique with 1D beam units was used by Wu et al. [

Gabar and Bilgin [

Xiao, et al. [

Nirmala and Rajkumar [

The model was created using ANSYS, Version 18, Mechanical APDL following the flow diagram in

At the solution stage, the loads and boundary conditions such as the degree of freedom and model solution setting were clearly specified. The final stage of the model, post-processing stage, was where the deflection plots and the stress contour diagrams of the pipeline system were plotted.

The pipeline used to create the model on ANSYS, Version 18, Mechanical APDL, was a gas pipeline installed by Horizontal Directional Drilling (HDD) in

south-west Nigeria. The gas pipeline design parameters are shown in

These parameters were input into the ANSYS platform to give the section outline in

Four (4) co-ordinates points were identified on the pipeline design profile to

Parameter | Value [units] |
---|---|

Pipe Diameter, OD | 91.44 [cm] |

Wall Thickness, t | 2.06 [cm] |

Pipe Grade | 70 Grade |

Specified Min. Yield Strength, SMYS | 4942.57929[ kg/cm^{2}] |

Entry Angle | 10 [deg] |

Exit Angle | 6 [deg] |

Length of Crossing, L | 175584 [cm] |

Poisson’s Ratio, µ | 0.3 |

Radius of Curvature, R | 100,000 [cm] |

Young Modulus, E | 20,400,000 [kg/cm^{2}] |

Radius from Neutral Axis, y | 45.72 [cm] |

Pressure at Final Hydro-Test, P | 127.5 [kg/cm^{2}] |

serve as the key-points. The pipeline was assumed to move along the x-y direction and therefore no co-ordinate was given for the z-direction. The radius of curvature for the sag-bends was modeled as fillet between lines 1, 2 and lines 2, 3 respectively. For this model, the radius of curvature for both sag-bends was expected to be same, with reference to the design profile. However, the exit and entry angles were different.

The number of pipe section mesh was defined for the model. The “SECNUM” command was used to identify the particular section for meshing. This command reads the section division as the amount of mesh sizes.

The “LMESH” command was used to generate nodes and line elements along lines. For this model, meshing was done on all the lines by selecting “ALL”.

The “ANTYPE” command was used to specify the type of analysis and the restart status. For this model, the static analysis was required. The “DK” command was utilized to state the degree of freedom at the key points. For this model, at all the key points, only one degree of freedom was permitted which was in the x-direction. The y- and z-directions were constrained. The “FK” command was used to define the applied load in the x-direction at the key points. This applied load is the force of the rig which pulls the pipe in the x-direction. The “ALLSEL” command was used to select all entities.

The “NLGEOM” command was used to set out the large displacement static analysis option for the model. The time control for maximum (100), minimum (10) and model’s number (100) of sub-steps for the basic solution control were also set.

Under the solution options, the “program chosen solver” and number (N) of subsets—1000 were selected for the equation solvers. Under the non-linear solution options of the solution controls, the highest number of iterations (1000), line search and DOF solution predictor was logged in and selected. The solution was generated using the macro file. A screen shot of the non-linear solution while converging can be viewed on

The equivalent resultant stress or Von Mises stress, expressed as a combination of all the stresses acting on the walls of the pipe includes: bending, longitudinal, hoop and radial stresses. However, the radial stress for thin wall material can be taken as negligible. Hence, the equivalent resultant stress can be expressed as Equation (1).

S t h e o r y = ( σ l 2 − ( σ l * σ h ) + σ h 2 2 (1)

where bending stress, hoop stress and longitudinal stress are defined by equations (2), (3) and (4), respectively.

1) Bending stress,

σ b = E * y R (2)

2) Hoop stress,

σ h = P * O D 2 * t (3)

3) Longitudinal stress,

σ l = ( μ * σ h ) + σ b (4)

After running the ANSYS model using the relevant input parameters, the maximum equivalent stress obtained was S_{ANSYS}. The percentage error when comparing the resultant equivalent stress values from both theoretical calculation and ANSYS model was evaluated using Equation (5).

Percentage Difference = ( S ANSYS − S theory S ANSYS + S theory ) * 100 % (5)

For the ANSYS model validation and investigate the effect of the HDD radius of curvature on the pipeline stresses, the internal pressure was kept constant at P = 127.5 kg/cm^{2} and different R-values (90,000 cm ≤ R ≤ 120,000 cm) were applied to obtain different S_{theory}, S_{ANSYS} and percentage (%) difference which results were shown in ^{2} ≤ P ≤ 127.5 kg/cm^{2} to obtain different S_{theory}, S_{ANSYS} and percentage (%) difference and the results shown in

^{2} and a minimum difference of 1.44% at an internal pressure of 127.5 kg/cm^{2}.

A comparison was also done between the theoretically calculated cross-section area of steel pipe and the ANSYS model cross-sectional area. The theoretically calculated cross-sectional area of the pipe is given as Equation (6).

A s = A e − A i (6)

where A e and A i are the external and internal cross-sectional area of the pipe, respectively; and A_{s} was calculated as A_{s} = 579.12 cm^{2}.

From ^{2}. Therefore, the percentage difference in the cross-sectional area was obtained as:

Percentage Difference = ( 579.12 − 578.439 579 .12 + 578.439 ) * 100 % = 0.059 %

The pipeline was discretized into 24 elements with 3 node points each by the ANSYS program for FEA to be done on each element. However, the element numbering was not arranged sequentially by APDL, but as shown in

The stress contour diagram for the equivalent stress or Von Mises stress was plotted to investigate the stress distribution on the pipe.

It can be observed from ^{2} was induced at the top-side on element number 21. This element was on the curved section close to the entry point where the angle of 10˚ was

used and which was much higher than the 6˚ used on the exit point. Although the radius of curvature was the same on both sides (entry and exit side), the maximum stress was experienced by the side with the highest angle. The bottom-side maximum stress 2399.9 kg/cm^{2} was obtained at element number 2. Also, it can be observed from the stress contour diagram,

However, the stress at the left-side and right-side of the pipeline was relatively uniform at approximately 888 kg/cm^{2} all through the pipeline regardless of the section where it was located. It would have been easily concluded that the stress at the curved sections would be higher than all other sections all-round the pipe, it can be seen that this was not the case.

The topside minimum stress was 17.237 kg/cm^{2} at element number 21, while the bottom-side minimum stress was 96.784 kg/cm^{2} obtained at element number 2. The left-side and right-side minimum stress remained uniform at approximately 888 kg/cm^{2} irrespective of the element number.

A nodal solution of the pipe deflection was plotted to show the deflection at each section of the pipe. From

The plot of the pipeline deflection was shown on

indicates that the maximum deflection on the pipeline was experienced at the point of maximum stress level. While,

Hence, ANSYS can be used as veritable tool for the analyses and design of a pipeline system to be installed by horizontal directional drilling (HDD). The results obtained from this study using the ANSYS model were corroborated those of theoretical methods. The point of curvature with the higher angle (that is, if both points of curvature are the same and the entry and exit angles are different) experiences the maximum induced stress. Maximum deflection of the pipeline should be expected at the point with maximum stress as this was due to the high bending moment experienced at this point. On a particular pipeline system, the maximum and minimum stresses were induced at the pipe top-side and bottom-side, respectively; while the stresses at the sides of the pipeline remained relatively uniform with slight variation.

The authors declare no conflicts of interest regarding the publication of this paper.

Olumoko, F.T. and Ossia, C.V. (2019) Stress Analysis of Buried Pipeline Installed by Horizontal Directional Drilling Using ANSYS Finite Element Software. World Journal of Engineering and Technology, 7, 365-378. https://doi.org/10.4236/wjet.2019.73027