**3.1. Modelling approach**

In order to model the behaviour of the hot tie-in field joints, a thermo-mechanical model was required. Although coupled thermo-mechanical modelling is available in commerciallyavailable finite element modelling software such as Abaqus [6], it is computationally expensive. An alternative approach employed in the current work is to separate the analysis into a thermal model to simulate the process of applying the IMPP, followed by a mechanical model simulating the process of bending the pipe that incorporates the temperature field predicted by the thermal model along with temperature-dependent material models.

Thermal modelling was performed using COMSOL Multiphysics [7], with the temperature fields around the field joint exported at a number of defined intervals of cooldown. These fields were then mapped onto an Abaqus mechanical model that simulated bend testing of the pipe. Given that the cooldown times are in the order of hours and that the bending events were performed in a number of minutes, there is a difference in orders of magnitude between the cooldown rates and the strain rate during the bend tests. Thus, it is reasonable to assume that heat flow within the field joints during bending was negligible and so can be accurately modelled by assuming a static temperature field in the mechanical models, thus achieving a considerable degree of efficiency over a fully-coupled thermo-mechanical model.

### **3.2. Thermal modelling**

The bending rig consisted of a reel former with a radius of curvature equal to 8 m, and a straightening former with a radius of curvature equal to 55.84 m (see **Figure 6**); these radii are representative of those of the reel drum and straightener employed onboard DCV *Aegir*. After coating of the field joints was completed in the coating station, the pipe specimen was installed into the bending rig. One end of the pipe was anchored with a pin, while the other end of the pipe was attached to a pull head, which was translated between the two formers by

**Figure 6.** Bend test rig at Heriot Watt University, with a test specimen bent to the reel former.

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

After a pre-defined cooldown period, the test procedure was initiated, whereby the specimen underwent five full bending cycles, with each cycle consisting of a number of steps: (i) the pipe is bent to the reel former and held; (ii) the pipe is released, (iii) the pipe is bent to the straightening former and (iv) the pipe is finally released again. The pipe was held to the reel former overnight in order to simulate the effect of the IMPP cooling down on the reel prior to resumption of reeling operations. The pipe is subjected to five full cycles during qualification testing in order to ensure that pipe integrity is maintained during initial spooling, straightening, bending over the aligner wheel and pipelay, along with contingencies for weather delays or the possibility of requiring to recover the pipe back onto the reel and then to unspool again. Ovality measurements were taken at salient locations after each cycle step, where the ovality

ovality = (*D*max – *D*min)/(*D*nom) (1)

where *D*max is the maximum diameter of the deformed pipe, *D*min is the minimum diameter of the deformed pipe and *D*nom is the original nominal diameter of the pipe. The ovality measurements were taken using optical metrology equipment inserted inside the pipe; thus, the values used in Eq. (1) relate to the inner diameter of the steel pipes with *D*nom = 295.7 mm.

Finite element modelling was used during the planning phase of the campaign in order to select suitable specimens, coating thicknesses and cooldown times for the tests; these models were refined further and validated against the experimental results. In the current section, the

means of a cable attached to a crane.

**3. Numerical modelling**

is defined according to DNV design guidance [5] as:

modelling techniques employed are described.

A time-dependent thermal model was developed in COMSOL Multiphysics, which was chosen due to its relative computational efficiency and modelling flexibility when compared to thermal modelling in comparable finite element modelling software. A section of the pipe around a particular field joint was represented by two-dimensional models assuming axisymmetric conditions about the longitudinal axis, with symmetry also assumed at the weld plane. The models relating to the three different FJC geometries are shown in **Figure 7**. It was found from sensitivity analysis that the change in temperature was negligible at a distance of 2 m from the weld, and thus the extent of the models reflects this. Triangular elements were used

**Figure 7.** Modelling of field joints in COMSOL.

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 conducted by Heerema Innovation were applied in the numerical models.
