*3.2.1. Boundary conditions*

An air cooling boundary heat flux was imposed on external surfaces, with the convection transfer coefficient set equal to 10 W/m<sup>2</sup> /K. When validating the numerical model against the experimental data, the ambient temperature was set equal to that recorded onsite on the day of testing; for the subsequent parametric study, the ambient temperature was set equal to 20°C.

Initially, it was assumed that internal airflow was negligible and so no boundary heat flux was defined along internal surfaces; this assumption is accurate for considerably long lengths of pipe where air flow is practically non-existent. However, for the shorter test specimens, the effects of internal air cooling on the temperature within the field joint coating are significant since heat is drawn from the polymer coating by the relatively highly-conductive steel pipe, which is being continually cooled by the air. It was found from sensitivity analysis that applying a temperature of 18°C and a heat transfer coefficient of 3 W/m<sup>2</sup> /K along the internal surfaces of the models provided appropriate cooldown rates.

The predictions of the numerical models are shown as dashed lines in **Figure 8**. Good agreement is observed between the experimental observations and the numerical predictions, particularly at the weld and toe locations and also at the internal thermocouples, while some discrepancy is observed to develop at the external overlap locations; this behaviour was also observed in the full FJC and thin hourglass FJC models. This can most likely be attributed to the overestimation of the convection transfer coefficient for the external boundary cooling coefficients. It is noticeable that since this discrepancy is more prevalent on the external boundaries rather than in the rest of the model, the majority of temperature loss in the IMPP is due to conduction through the steel, rather than from air convection. Overall, the accuracy of the numerical predictions is confirmation of the suitability of the modelling techniques and the material models used, and allows for the temperature fields to be applied to the mechani-

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

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

85

**Figure 8.** Experimental and numerical temperature evolutions for the thick hourglass FJC specimen.

Modelling of the bend test procedure was performed using Abaqus 6.12 [6]. For validation of the model, the measured geometry of the test specimens was used, while for the parametric study, nominal dimensions were used. Temperature-dependent material models were used in the simulations as outlined in Section 3.3.2, with the temperature fields predicted by the thermal modelling mapped to the Abaqus models using the procedure outlined in Section 3.3.4. The model was validated successfully against the experimental results for ovality and stress distributions, which then allowed a parametric study to be conducted to identify combina-

The model of the bend test rig is shown in **Figure 9**, with a combination of shell and solid instances used to model the pipe and coating materials, with two FJCs centred at 20 mm girth welds. A pipe with no FJCs was also modelled in order to provide validation against the bare

tions of FJC thickness and cooldown time where buckling is avoided.

cal models in the next stage of the analysis.

*3.3.1. Model geometry and boundary conditions*

**3.3. Mechanical modelling**

pipe tested onsite.

### *3.2.2. Analysis steps*

The analysis was divided into a number of steps representing the IMPP application procedure as conducted onsite. Firstly, induction heating of the steel was modelled using a body heat flux defined appropriately to raise the temperature of the steel pipe to 240°C within the recorded operating time. Next, domains representing the layers of FBE and CMPP were added to the model and the analysis was resumed in order to simulate cooling of the steel substrate to 190°C. Reheating of the chamfers was simulated by applying a surface heat flux to the relevant surfaces in the model, defined appropriately so as to replicate reheating to between 140 and 150°C during the time recorded onsite.

In the final step of the thermal analysis, the IMPP was included at an initial temperature of 200°C. The model was run to simulate 16 h of cooldown to provide comparison with the thermocouple data. Three separate models were created for the full, thick hourglass and thin hourglass FJC geometries, respectively, as shown in **Figure 7**.

### *3.2.3. Validation of thermal model*

The temperature evolution profiles recorded by the thermocouples (located at the positions indicated in **Figure 5**) for the thick hourglass FJC specimen are shown in **Figure 8** as solid lines. It can be seen that, as would be expected, temperatures recorded closer to the outer surface of the FJCs at the overlap reduce quicker than those located internally. Owing to thermal conduction through the steel pipe, the temperatures at the weld and toe locations reduce quicker than at the internal thermocouples where the insulating polymer slows down heat flow considerably. This effect was noticeably more pronounced in the full FJC than in the hourglass FJCs, with the temperature reducing quickest in the thin hourglass FJC.

Numerical Analysis of Hot Polymer-Coated Steel Pipeline Joints in Bending http://dx.doi.org/10.5772/intechopen.72262 85

**Figure 8.** Experimental and numerical temperature evolutions for the thick hourglass FJC specimen.

The predictions of the numerical models are shown as dashed lines in **Figure 8**. Good agreement is observed between the experimental observations and the numerical predictions, particularly at the weld and toe locations and also at the internal thermocouples, while some discrepancy is observed to develop at the external overlap locations; this behaviour was also observed in the full FJC and thin hourglass FJC models. This can most likely be attributed to the overestimation of the convection transfer coefficient for the external boundary cooling coefficients. It is noticeable that since this discrepancy is more prevalent on the external boundaries rather than in the rest of the model, the majority of temperature loss in the IMPP is due to conduction through the steel, rather than from air convection. Overall, the accuracy of the numerical predictions is confirmation of the suitability of the modelling techniques and the material models used, and allows for the temperature fields to be applied to the mechanical models in the next stage of the analysis.

#### **3.3. Mechanical modelling**

to mesh the model. Temperature-dependent thermal conductivities and heat capacities from an extensive campaign of material fingerprinting of coating materials and steel pipe materials

An air cooling boundary heat flux was imposed on external surfaces, with the convection

experimental data, the ambient temperature was set equal to that recorded onsite on the day of testing; for the subsequent parametric study, the ambient temperature was set equal to 20°C. Initially, it was assumed that internal airflow was negligible and so no boundary heat flux was defined along internal surfaces; this assumption is accurate for considerably long lengths of pipe where air flow is practically non-existent. However, for the shorter test specimens, the effects of internal air cooling on the temperature within the field joint coating are significant since heat is drawn from the polymer coating by the relatively highly-conductive steel pipe, which is being continually cooled by the air. It was found from sensitivity analysis that

The analysis was divided into a number of steps representing the IMPP application procedure as conducted onsite. Firstly, induction heating of the steel was modelled using a body heat flux defined appropriately to raise the temperature of the steel pipe to 240°C within the recorded operating time. Next, domains representing the layers of FBE and CMPP were added to the model and the analysis was resumed in order to simulate cooling of the steel substrate to 190°C. Reheating of the chamfers was simulated by applying a surface heat flux to the relevant surfaces in the model, defined appropriately so as to replicate reheating to between

In the final step of the thermal analysis, the IMPP was included at an initial temperature of 200°C. The model was run to simulate 16 h of cooldown to provide comparison with the thermocouple data. Three separate models were created for the full, thick hourglass and thin

The temperature evolution profiles recorded by the thermocouples (located at the positions indicated in **Figure 5**) for the thick hourglass FJC specimen are shown in **Figure 8** as solid lines. It can be seen that, as would be expected, temperatures recorded closer to the outer surface of the FJCs at the overlap reduce quicker than those located internally. Owing to thermal conduction through the steel pipe, the temperatures at the weld and toe locations reduce quicker than at the internal thermocouples where the insulating polymer slows down heat flow considerably. This effect was noticeably more pronounced in the full FJC than in the

hourglass FJCs, with the temperature reducing quickest in the thin hourglass FJC.

/K. When validating the numerical model against the

/K along the internal

conducted by Heerema Innovation were applied in the numerical models.

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

applying a temperature of 18°C and a heat transfer coefficient of 3 W/m<sup>2</sup>

surfaces of the models provided appropriate cooldown rates.

hourglass FJC geometries, respectively, as shown in **Figure 7**.

140 and 150°C during the time recorded onsite.

*3.2.3. Validation of thermal model*

*3.2.1. Boundary conditions*

*3.2.2. Analysis steps*

transfer coefficient set equal to 10 W/m<sup>2</sup>

Modelling of the bend test procedure was performed using Abaqus 6.12 [6]. For validation of the model, the measured geometry of the test specimens was used, while for the parametric study, nominal dimensions were used. Temperature-dependent material models were used in the simulations as outlined in Section 3.3.2, with the temperature fields predicted by the thermal modelling mapped to the Abaqus models using the procedure outlined in Section 3.3.4. The model was validated successfully against the experimental results for ovality and stress distributions, which then allowed a parametric study to be conducted to identify combinations of FJC thickness and cooldown time where buckling is avoided.

### *3.3.1. Model geometry and boundary conditions*

The model of the bend test rig is shown in **Figure 9**, with a combination of shell and solid instances used to model the pipe and coating materials, with two FJCs centred at 20 mm girth welds. A pipe with no FJCs was also modelled in order to provide validation against the bare pipe tested onsite.

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

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 the various analysis steps.

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 overclosure to define the normal behaviour.
