*3.3.2. Material modelling*

As part of a campaign of material fingerprinting conducted by Heerema Marine Contractors, moduli of elasticity and full stress-strain curves for the various polymer and steel materials used in the pipes were obtained at a number of ambient temperatures and strain rates. A typical set of stress-strain curves is shown in **Figure 10** for the IMPP material, with testing performed at 5 mm/ min; these curves were converted to true stress and true strain prior to their use in the numerical models. For temperatures outside the tested range, the material curves were based on extrapolation. For the polypropylene materials, an elastic-plastic material model with isotropic hardening was assumed, in keeping with previous studies [8]. Although polypropylene exhibits viscoelastic behaviour in practice, given the strain rates and hold times being modelled in the current study, it was not necessary to model changes in stress owing to viscous flow of the material.

80 N/mm<sup>2</sup>

als was assumed to be 210,000 N/mm<sup>2</sup>

*3.3.3. Elements and meshing*

*3.3.4. Mapping of temperature fields*

linear expansion was set equal to 13 × 10−6.

density increased in the area of interest around the weld.

**Figure 11.** Stress-strain curves for X65 steel at a range of temperatures.

**Figure 10.** Stress-strain curves for the IMPP material obtained from tensile testing.

based on previous project experience. The modulus of elasticity of the steel materi-

In the interests of computational efficiency, the mechanical model employed a combination of quadrilateral shell S4R elements for the steel pipe, and solid C3D8R elements for the thicker coating materials. The steel pipe elements were in fact composite layups in order to include the thin layers of FBE and CMPP. A nominal element size of 15 mm was used, with the mesh

The thermal analysis was performed using two-dimensional axisymmetric models with triangular meshes, while the mechanical analysis used three-dimensional solid brick and quadrilateral shell elements. In order to map the temperature field correctly, an algorithm was developed whereby the COMSOL temperature field was centred on a weld plane and then

with a Poisson's ratio equal to 0.3. The coefficient of

Numerical Analysis of Hot Polymer-Coated Steel Pipeline Joints in Bending

http://dx.doi.org/10.5772/intechopen.72262

87

The moduli of elasticity of the various coating materials were modelled as temperature-dependent, while the Poisson's ratio was set at 0.45. The coefficient of thermal expansion for the three polypropylene materials was temperature-dependent and based on manufacturers' recommendations.

The X65 material was also modelled using an elastic-plastic material model albeit with nonlinear kinematic hardening, and based on test data obtained across a range of temperatures. For temperatures outside the tested range, material curves were extrapolated based on derating the material in accordance with DNV guidelines [5]. The resulting true stress-true strain curves are shown in **Figure 11**. The stress-strain relationship for the welds was assumed to be similar to that of the parent steel, albeit with isotropic hardening and a strength overmatch of

**Figure 10.** Stress-strain curves for the IMPP material obtained from tensile testing.

**Figure 11.** Stress-strain curves for X65 steel at a range of temperatures.

80 N/mm<sup>2</sup> based on previous project experience. The modulus of elasticity of the steel materials was assumed to be 210,000 N/mm<sup>2</sup> with a Poisson's ratio equal to 0.3. The coefficient of linear expansion was set equal to 13 × 10−6.

#### *3.3.3. Elements and meshing*

Analytical rigid instances were used to model the reel former and straightening former, each with a radius of curvature equivalent to those used onsite, respectively. Pin-ended conditions were defined at the anchor end, permitting only rotation in the plane of the rig. Connector elements were used to model the cables from the pullhead to the crane with appropriate displacements imposed on them in order to simulate the pipe being bent to the formers across

Contact interactions were defined between the outer surface of the coating and the former surfaces, with a coefficient of friction of 0.3 to define the tangential behaviour and a pressure

As part of a campaign of material fingerprinting conducted by Heerema Marine Contractors, moduli of elasticity and full stress-strain curves for the various polymer and steel materials used in the pipes were obtained at a number of ambient temperatures and strain rates. A typical set of stress-strain curves is shown in **Figure 10** for the IMPP material, with testing performed at 5 mm/ min; these curves were converted to true stress and true strain prior to their use in the numerical models. For temperatures outside the tested range, the material curves were based on extrapolation. For the polypropylene materials, an elastic-plastic material model with isotropic hardening was assumed, in keeping with previous studies [8]. Although polypropylene exhibits viscoelastic behaviour in practice, given the strain rates and hold times being modelled in the current study, it was not necessary to model changes in stress owing to viscous flow of the material.

The moduli of elasticity of the various coating materials were modelled as temperature-dependent, while the Poisson's ratio was set at 0.45. The coefficient of thermal expansion for the three polypropylene materials was temperature-dependent and based on manufacturers' recommendations. The X65 material was also modelled using an elastic-plastic material model albeit with nonlinear kinematic hardening, and based on test data obtained across a range of temperatures. For temperatures outside the tested range, material curves were extrapolated based on derating the material in accordance with DNV guidelines [5]. The resulting true stress-true strain curves are shown in **Figure 11**. The stress-strain relationship for the welds was assumed to be similar to that of the parent steel, albeit with isotropic hardening and a strength overmatch of

the various analysis steps.

*3.3.2. Material modelling*

overclosure to define the normal behaviour.

**Figure 9.** Model of the bend test rig and pipe specimen in Abaqus.

86 Finite Element Method - Simulation, Numerical Analysis and Solution Techniques

In the interests of computational efficiency, the mechanical model employed a combination of quadrilateral shell S4R elements for the steel pipe, and solid C3D8R elements for the thicker coating materials. The steel pipe elements were in fact composite layups in order to include the thin layers of FBE and CMPP. A nominal element size of 15 mm was used, with the mesh density increased in the area of interest around the weld.

#### *3.3.4. Mapping of temperature fields*

The thermal analysis was performed using two-dimensional axisymmetric models with triangular meshes, while the mechanical analysis used three-dimensional solid brick and quadrilateral shell elements. In order to map the temperature field correctly, an algorithm was developed whereby the COMSOL temperature field was centred on a weld plane and then

*3.3.5. Analysis procedure*

**4. Results and comparisons**

predictions of the numerical model.

observable in the compression zone.

**4.1. Pipe deformation, buckling and ovality**

A geometrically-nonlinear static analysis was employed, divided into a number of steps, as shown in **Figure 13**: (i) firstly, the temperature field was applied to the model; (ii) next the pipe was bent to the reel former and held; (iii) the temperature field was then set equal to the appropriate ambient temperature (either that recorded onsite for the validation study, or 20°C for the parametric study) in order to simulate the pipe and FJCs cooling down; (iv) next, the pipe was released, then (v) bent to the straightening former, and finally (vi) released again, thus completing the first bend cycle. The model simulated five full bending cycles in total (the latter four all with the temperature field set equal to the appropriate ambient temperature). As can be seen in **Figure 13**, after a full bend cycle there is a noticeable amount of plastic deformation present in the pipe after straightening; limiting this plastic deformation and avoiding buckling of the pipe and tearing of the coating are two of the main challenges posed by the reel-lay procedure.

Numerical Analysis of Hot Polymer-Coated Steel Pipeline Joints in Bending

http://dx.doi.org/10.5772/intechopen.72262

89

In this section, the results of the bend tests are discussed, and comparison is made with the

A bare pipe with no FJCs was tested first in the bend rig as a control specimen, whereupon it buckled at the first bend to the reel former, as shown in **Figure 14a**; this early onset buckle can be attributed to the stiffness mismatch between the full linepipe coating and the bare steel pipe causing strains to concentrate within the bare steel. It can also be seen that the point of initiation of the buckle is located to the left of the weld. The strain field predicted by the numerical model is shown in **Figure 14b**, where the strain concentration can indeed be observed in the uncoated region of the pipe. It can be seen that the pipe was also predicted to buckle after the first bend to the reel, albeit with the point of initiation of the buckle located closer to the weld. Given the high imperfection sensitivity of cylindrical shells in compression, this discrepancy in buckle location is likely down to a localised thinning of the pipe wall in the area around the buckle due to corrosion. It can be seen that, in areas in the steel pipe away from the buckle, the

Despite the presence of the polymer coating, one of the field joints on the pipe with the thin hourglass FJC also buckled on the first bend to the reel. During initial simulations prior to the test campaign, ovalities in excess of 10% were expected; based on previous experience [9] this level of ovality is a strong predictor of the occurrence of buckling. The buckled field joint is shown in **Figure 15a**; as can be seen, there is noticeable lift-off from the reel former. In **Figure 15b**, the equivalent numerical prediction of the stress field is shown, with rippling

The pipes with the thick hourglass and full FJCs did not buckle throughout the five bending cycles; the numerical models also predicted that no buckling would occur. In **Figure 16**, the ovalities recorded along the length of the pipe with the thick hourglass FJC after the first bend

tensile strain is approximately 2.5%, in keeping with analytical predictions.

**Figure 12.** Example of transferral of COMSOL temperature output to a discrete field in Abaqus.

translated and rotated to cylindrical coordinates. A least-squares node-matching routine then identified the nodes in the COMSOL mesh closest to each node in the Abaqus mesh within longitudinal neighbourhoods of 100 mm. The resulting field was then inputted as a discrete field into the Abaqus model. An example of the result of running the algorithm is shown in **Figure 12**, with the COMSOL temperature output on the left hand side and the resulting temperature field in Abaqus shown on the right. For the validation of the numerical models against the experiments, temperature fields were outputted at the appropriate cooldown times related to the time after IMPP application recorded during the bend tests. Since there was a half hour to an hour difference in application time between the two FJCs for a particular test pipe, and thus a noticeable difference in temperature, separate temperature fields were mapped around the two joints.

**Figure 13.** Bend cycle steps modelled in Abaqus.
