Analysis of a Spool-Riser System

Analysis of a Spool-Riser System

Renata Hermano Almeida da Silveira

Projeto de Graduacao apresentado ao

Curso de Engenharia Naval e Oceanica da

Escola Politecnica, Universidade Federal do

Rio de Janeiro, como parte dos requisitos

necessarios a obtencao do tıtulo de Engen-

heiro.

Orientadores: Murilo Augusto Vaz

Benjamin Dubois

Rio de Janeiro

Junho de 2021



PROJETO DE GRADUAÇÃO SUBMETIDO AO CORPO DOCENTE DO CURSO DE

ENGENHARIA NAVAL E OCEÂNICA DA ESCOLA POLITÉCNICA DA

UNIVERSIDADE FEDERAL DO RIO DE JANEIRO COMO PARTE DOS REQUISITOS

NECESSÁRIOS PARA A OBTENÇÃO DO GRAU DE ENGENHEIRA NAVAL E

OCEÂNICA

.

Examinada por:

________________________________________________

Prof. Murilo Augusto Vaz, Ph. D.

.

________________________________________________

Marcelo Caire, D.Sc.

________________________________________________

Rafael Familiar Solano, D. Sc.

RIO DE JANEIRO, RJ – BRASIL

Junho de 2021

Silveira, Renata Hermano Almeida da

Analysis of a Spool-Riser System/ Renata Hermano Almeida da Silveira

– Rio de Janeiro: UFRJ/ Escola Politecnica, 2021.

XIV, p.74 : il.; 29,7 cm.

Orientador: Murilo Augusto Vaz, Benjamin Dubois

Projeto de Graduacao – UFRJ / Escola Politecnica / Curso de

Engenharia Naval e Oceanica, 2021.

Referencias Bibliograficas: p.63-64.

1. Pipeline. 2. Riser. 3. Spool. 4. FEA. I. Vaz, Murilo Augusto. II. Uni-

versidade Federal do Rio de Janeiro, UFRJ, Engenharia Naval e Oceanica.

III. Analysis of a Spool-Riser System.

iii

Acknowledgements

Even though this report is signed by one person, several others participated,

helped, guided and supported me to some extent during the activities presented in this

piece of work or even before it ever began. If it were not for the following people, this

report would never find its way to the reader.

I will be acknowledging the orientation and supervision of Benjamin Dubois and

Murilo Vaz during the duration of this project. Thank you for keeping the topic as

interesting as possible and for being patient and helpful whenever I needed.

I would also like to thank UFRJ institution and its employees, specially Professor

Marta Cecilia Tapia Reyes who made possible for me to participate in the ENSTA-

Bretagne double degree exchange program, which has changed me as a professional and

as a person.

It is as important to thank all my new friends made during this exchange, they

became a family across the globe and will always have a special place in my life. My

acknowledgements extend to my friends from Brazil who have always supported me,

being only one phone call away.

Most of all, I want to thank the unconditional encouragement from my parents,

Tania and Renato, who have worked so hard to provide me with the best and that

often gave up their own dreams so that their children could reach theirs. To my sisters,

Marina, Maria Clara and Nathalia, who always stood by my side, believed in me more

than myself and are my forever best friends.

Last but not least, thanks to Daniel who besides of filling my days with laughter,

love and joy, stayed by my side rooting and encouraging for me, no matter what.

iv

Abstract of Undergraduate Project presented to POLI/UFRJ as a partial fulfillment of

the requirements for the degree of Engineer.



Adivisors: Murilo Augusto Vaz and Benjamin Dubois

Course: Naval and Ocean Engineering

A spool is a pipe section which is used to connect a pipeline to another subsea struc-

ture or riser, it ensures the continuity of fluid transport. This element can have various

shapes, and its main function is to absorb efforts coming from the flowline and prevent

them to arise to the riser/subsea equipment. Mechanical analyses of this element be-

haviour under environmental and operation loads are often important subject during a

subsea field project.

This work, through a comparative analysis between AutoPIPE and Abaqus software,

aims to develop a methodology for this structure analyses to be made routinely with

Abaqus. It is focused on model definition approaches to best represent the study case

and the applicability of this methodology in the routine of Pipeline Engineers.

The study was motivated by the lack of accurate information on how to analyse subsea

pipeline systems with AutoPIPE, since this software is primarily intended for topside

analysis. In addition, it was considered that the engineers working with pipelines usually

have greater knowledge in the use of Abaqus instead of AutoPIPE.

Key-words: Pipeline, Riser, Spool, FEA.

v

Resumo do Projeto de Graduacao apresentado a Escola Politecnica/UFRJ como parte

dos requisitos necesserios para obtencao do grau de Engenheiro Naval e Oceanico

Analise de um Sistema Spool-Riser


Orientadores: Murilo Augusto Vaz e Benjamin Dubois

Curso: Engenharia Naval e Oceanica

Um spool e uma secao de tubo que e usada para conectar um duto o a outra es-

trutura submarina ou riser, garantindo a continuidade do transporte de fluido. Esse

elemento pode ter varias formas, mas, seja qual for a sua forma, sua principal funcao

e absorver os esforcos provenientes do duto e impedir que eles cheguem intensamente

ao riser/estruturas subsea. Analises mecanicas do comportamento desse elemento sob

cargas ambientais e operacionais sao frequentemente assuntos importantes durante pro-

jetos novos e de extensao de campo de petroleo.

Este trabalho, atraves de um estudo comparativo entre os softwares AutoPIPE e Abaqus,

visa desenvolver uma metodologia para que essas analises de estrutura sejam feitas

rotineiramente com o Abaqus. Ele se concentra nos parametros de definicao de modelo

para melhor representar o caso de estudo e a aplicabilidade dessa metodologia na rotina

dos engenheiros de dutos.

O estudo foi motivado pela falta de informacoes precisas sobre como analisar sistemas

de dutos submersos com o AutoPIPE, uma vez que esse software e primordialmente des-

tinado a analises topside. Alem disso, foi considerado que os engenheiros que trabalham

com dutos normalmente possuem maior conhecimento na utilizacao do Abaqus que do

AutoPIPE.

Palavras-chave: Pipeline, Riser, Spool, FEA.

vi

Acronyms

BC Boundary Condition(s)

CD Chart Datum

CF Concentrated force

DF Distributed force

DOF Degrees of freedom

FEA Finite Element Analysis

HOC Hang Off Clamp

HY Hydrotest

MSL Mean Sea Level

N/A Not Applicable

NLGeom Geometric non-linearity

OP Operation

PIP Pipe in pipe

RFA Reaction force in A direction

RMA Reaction moment around A direction

SIF Stress intensification factor

UA Displacement in A direction

URA Rotation around the A axis

ULC Unitary load case

VBA Visual Basic for Applications

Y Year(s)

vii

Contents

1 Introduction 1

1.1 Context and Motivation . . . . . . . . . . . . . . . . . . . . . . . . . . 1

1.2 Problem Statement and Objectives . . . . . . . . . . . . . . . . . . . . 2

1.3 Structure of the report . . . . . . . . . . . . . . . . . . . . . . . . . . . 3

2 Theoretical Background 5

2.1 Types of Subsea Piping Structures . . . . . . . . . . . . . . . . . . . . 5

2.1.1 Riser and Pipeline . . . . . . . . . . . . . . . . . . . . . . . . . 5

2.1.2 Spool . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6

2.2 General Coss Section of Rigid Subsea Pipes . . . . . . . . . . . . . . . . 7

2.3 Loads on Subsea Piping Structures . . . . . . . . . . . . . . . . . . . . 8

2.3.1 Loads on Risers . . . . . . . . . . . . . . . . . . . . . . . . . . 8

2.3.2 Loads on Spools and Pipelines . . . . . . . . . . . . . . . . . . . 8

3 Software Overview 13

3.1 AutoPIPE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13

3.2 Abaqus . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14

3.3 FEMAP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15

4 Correlation between Abaqus and AutoPIPE 16

4.1 Straight pipe . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16

4.1.1 Case A: Weight loads . . . . . . . . . . . . . . . . . . . . . . . 17

4.1.2 Case B: Weight, content and buoyancy loads . . . . . . . . . . . 17

4.1.3 Case C: Pressure load . . . . . . . . . . . . . . . . . . . . . . . 18

4.1.4 Case D: Temperature load . . . . . . . . . . . . . . . . . . . . . 21

4.1.5 Case E: Waves and current load . . . . . . . . . . . . . . . . . . 21

viii

4.2 Geometry with a bend . . . . . . . . . . . . . . . . . . . . . . . . . . . 25

4.2.1 Case A: Weight load . . . . . . . . . . . . . . . . . . . . . . . . 26

4.2.2 Case B: Weight, content and buoyancy loads . . . . . . . . . . . 29

4.2.3 Case C: Weight, content, buoyancy, temperature and pressure loads 29

4.2.4 Case D: Weight, content, buoyancy, temperature, pressure, waves

and current loads . . . . . . . . . . . . . . . . . . . . . . . . . 30

4.3 Summary of results and conclusion . . . . . . . . . . . . . . . . . . . . 31

4.3.1 Conclusion . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 31

4.3.2 Findings . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 32

5 Methodology for recreating AutoPIPE simulation into Abaqus 33

5.1 Geometry and Mesh - Femap . . . . . . . . . . . . . . . . . . . . . . . 33

5.2 Pipe design data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 34

5.2.1 Material . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 34

5.2.2 Pipe and coating data . . . . . . . . . . . . . . . . . . . . . . . 35

5.2.3 Pressure and temperature data . . . . . . . . . . . . . . . . . . 36

5.2.4 Fitting data . . . . . . . . . . . . . . . . . . . . . . . . . . . . 36

5.3 Environmental data . . . . . . . . . . . . . . . . . . . . . . . . . . . . 37

5.3.1 Water depth and seawater density . . . . . . . . . . . . . . . . . 37

5.3.2 Waves and currents . . . . . . . . . . . . . . . . . . . . . . . . 37

5.3.3 Hydrodynamic coefficients . . . . . . . . . . . . . . . . . . . . . 38

5.3.4 Marine Growth . . . . . . . . . . . . . . . . . . . . . . . . . . . 38

5.3.5 Soil . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 38

5.4 Interface Data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 39

5.4.1 Pipeline Expansion . . . . . . . . . . . . . . . . . . . . . . . . . 39

5.4.2 Platform Movements . . . . . . . . . . . . . . . . . . . . . . . . 39

5.5 Load cases . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 40

5.6 Modeling choices . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 42

5.6.1 Soil . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 42

5.6.2 Riser guides/supports . . . . . . . . . . . . . . . . . . . . . . . 43

5.6.3 Valve and flanges . . . . . . . . . . . . . . . . . . . . . . . . . 44

5.6.4 Concrete, anti-corrosion and marine growth . . . . . . . . . . . . 44

5.6.5 Load sequence . . . . . . . . . . . . . . . . . . . . . . . . . . . 46

ix

5.7 Results . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 47

5.7.1 Displacement . . . . . . . . . . . . . . . . . . . . . . . . . . . . 47

5.7.2 Reaction force and reaction moment . . . . . . . . . . . . . . . 51

5.7.3 Section force and section moment . . . . . . . . . . . . . . . . . 52

5.7.4 Stress . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 55

5.8 Methodology summary . . . . . . . . . . . . . . . . . . . . . . . . . . . 57

5.9 Software comparison . . . . . . . . . . . . . . . . . . . . . . . . . . . . 60

5.10 Conclusion . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 61

6 Conclusion 62

Bibliografia 63

A Wave theories limits 65

B ASME B31.8 Stress 66

B.1 Hoop Stress . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 66

B.2 Longitudinal Stress . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 66

B.3 Combined Stress . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 67

C Pre-processing sheet 69

D Python script for post-processing 71

x

List of Figures

1.1 Jacket platform and its piping system. . . . . . . . . . . . . . . . . . . 3

2.1 Subsea schematic layout [Ref. [1]]. . . . . . . . . . . . . . . . . . . . . 6

2.2 Most common types of spools: vertical (left) and horizontal (right) [Ref.

[2] and [3]]. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 7

2.3 Pipe Cross Section. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 7

2.4 Force diagram - Spools and Pipelines. . . . . . . . . . . . . . . . . . . . 9

2.5 Pipeline end expansion. . . . . . . . . . . . . . . . . . . . . . . . . . . 9

2.6 Strain distribution along the flowline [Ref. [1]]. . . . . . . . . . . . . . . 10

4.1 Wave phase orientation for Abaqus and AutoPIPE both with 0-degree

phase angle. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 22

4.2 Schematic Case E.1 (left) and E.2 (right). . . . . . . . . . . . . . . . . 23

4.3 Pipe with a 90-degree bend. . . . . . . . . . . . . . . . . . . . . . . . . 25

5.1 FEMAP mesh overview. . . . . . . . . . . . . . . . . . . . . . . . . . . 34

5.2 Abaqus modeled geometry: supports, soil and pipe structure. . . . . . . 42

5.3 Clearance definition for tube-to-tube contact elements. . . . . . . . . . . 43

5.4 Support geometry made for Abaqus model with tube-to-tube contact

elements. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 44

5.5 AutoPIPE loads and BC choices for the main case of study. . . . . . . . 45

5.6 X displacement results - Case GP1T1U20-HY. . . . . . . . . . . . . . . 48

5.7 Y displacement results - Case GP1T1U20-HY. . . . . . . . . . . . . . . 48

5.8 AutoPIPE top view deformed shape, 25 scale factor - Case GP1T1U20-HY. 49

5.9 Abaqus Pipe top view deformed shape, 25 scale factor - Case GP1T1U20-

HY. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 50

xi

5.10 Abaqus Elbow-Pipe top view deformed shape, 25 scale factor - Case

GP1T1U20-HY. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 50

5.11 AutoPIPE local axis definition. . . . . . . . . . . . . . . . . . . . . . . 53

5.12 Effective axial force results in local axis - Case GP1T1U20-HY. . . . . . 53

5.13 Bending moment about the local 1-axis - Case GP1T1U20-HY. . . . . . 54

5.14 Von Mises stress - Case GP1T1U20-HY. . . . . . . . . . . . . . . . . . 55

5.15 Axial stress - Case GP1T1U20-HY. . . . . . . . . . . . . . . . . . . . . 56

5.16 Hoop stress - Case GP1T1U20-HY. . . . . . . . . . . . . . . . . . . . . 56

5.17 Example of .bat file to run Abaqus simulations in a row. . . . . . . . . . 59

A.1 Wave theories limits [Ref. [8]]. . . . . . . . . . . . . . . . . . . . . . . 65

B.1 ASME B31.8 SIF definition [Ref. [4]] . . . . . . . . . . . . . . . . . . . 67

C.1 VBA pre-processing sheet. . . . . . . . . . . . . . . . . . . . . . . . . . 70

D.1 Python preliminary script for post-processing. . . . . . . . . . . . . . . . 74

xii

List of Tables

4.1 Results for a straight pipe - Load case A. . . . . . . . . . . . . . . . . . 17

4.2 Results for a straight pipe - Load case B. . . . . . . . . . . . . . . . . . 18

4.3 Abaqus results for a straight pipe - Load case B where buoyancy was

modeled as CF. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18

4.4 Results for a straight pipe - Load case C without friction. . . . . . . . . 20

4.5 Results for a straight pipe - Load case C with friction. . . . . . . . . . . 20

4.6 Results for a straight pipe - Load case D. . . . . . . . . . . . . . . . . . 21

4.7 Results for a vertical pipe submitted to wave load. . . . . . . . . . . . . 23

4.8 Current data - Load case E.2. . . . . . . . . . . . . . . . . . . . . . . . 24

4.9 Results for a vertical pipe submitted to wave and current load. . . . . . . 24

4.10 AutoPIPE results for the geometry with a bend - Load case A. . . . . . . 26

4.11 Mesh influence on Abaqus results for the geometry with a bend modeled

with Pipe31 - Load case A . . . . . . . . . . . . . . . . . . . . . . . . . 26

4.12 Mesh influence on Abaqus results for the geometry with a bend modeled

with Elbow31 - Load case A. . . . . . . . . . . . . . . . . . . . . . . . 28

4.13 Results for the geometry with a bend modelled with 25 elements - Load

case B. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 29

4.14 Results for the geometry with a bend modeled with 25 elements - Load

case C. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 30

4.15 Current data- Load case D . . . . . . . . . . . . . . . . . . . . . . . . . 30

4.16 Results for the geometry with a bend modeled with 25 elements - Load

case D. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 31

5.1 Material Data - Steel. . . . . . . . . . . . . . . . . . . . . . . . . . . . 35

5.2 Pipe Data - Spool and Pipeline. . . . . . . . . . . . . . . . . . . . . . . 35

5.3 Pipe Data - Riser and Topside. . . . . . . . . . . . . . . . . . . . . . . 35

xiii

5.4 Density of materials . . . . . . . . . . . . . . . . . . . . . . . . . . . . 36

5.5 Pipe Data - Riser and Topside. . . . . . . . . . . . . . . . . . . . . . . 36

5.6 Fitting weight data. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 36

5.7 Current data. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 37

5.8 Wave data. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 37

5.9 Hydrodynamic coefficients. . . . . . . . . . . . . . . . . . . . . . . . . 38

5.10 Marine growth profile. . . . . . . . . . . . . . . . . . . . . . . . . . . . 38

5.11 Soil properties. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 38

5.12 Pipeline expansion. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 39

5.13 Platform displacements. . . . . . . . . . . . . . . . . . . . . . . . . . . 39

5.14 Unitary Load Cases. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 41

5.15 Combined Load Cases. . . . . . . . . . . . . . . . . . . . . . . . . . . . 41

5.16 Abaqus step sequence. . . . . . . . . . . . . . . . . . . . . . . . . . . . 46

5.17 AutoPIPE reaction force on pipe supports - Case GP1T1U20-HY. . . . . 51

5.18 Abaqus reaction force on pipe supports - Case GP1T1U20-HY. . . . . . 52

5.19 Reaction moment on the hang off clamp - Case GP1T1U20-HY. . . . . . 52

5.20 Abaqus step sequence. . . . . . . . . . . . . . . . . . . . . . . . . . . . 59

xiv

Chapter 1

Introduction

Due to energy demands that increase each day, the exploitation of fossil resources

is still necessary and indispensable. In order to meet these needs, many gas and oil

production facilities have been built in the last few years. Consequently the engineering

behind those facilities was, and still is, forced to evolve quickly into finding new solutions

for offshore challenges. It is in this context of oil extraction and offshore structures that

this project is inserted.

When it comes to offshore exploitation fields, the subsea layout is always a com-

plex schema of flowlines, jumpers, spools, manifolds, Christmas Trees etc. which allow

the oil to flow from the well up to the platform. In order to define a layout, a series

of individual analyses of each component and their interaction with each other must be

assessed. This project studies the interaction of Spool, Riser and associated Flowline.

1.1 Context and Motivation

In the offshore production industry, rigid spools are special shaped pipes that

joins a flowline and a production structure. In the studied case, the spool makes the

connection between an underwater pipeline and a riser. On its turn, the riser is guided

along the platform, supported at its higher level and connected to the platform topside.

The main reasons why risers are not directly connected to the flowline are the

thermal expansion and pressure efforts that income from the flowline and would most

certainly affect riser structure. For this reason the spool is used to make their link and to

absorb those incoming efforts from the flowline, not allowing them to arise so intensely

1

on the riser.

In addition to the pressure and the temperature of the transported fluid, those

pipes are submitted to loading specific to the method of installation, to movements of the

platform (settlements, inclinations, etc ...) and they are also subject to hydrodynamic

forces generated by waves and sea currents. Therefore, the system made by riser, spool

and pipeline needs to stand all the efforts in various combinations during its lifetime

without compromising the fluid flow, the environment and the safety of the platform

staff. Therefore, it must not fail under those circumstances.

Since the system is under complex conditions and the structure is requested in

so many ways, usually finite element simulations are made to design and predict the

structure response to such environment. Most often, these studies are carried out with

AutoPIPE or CAESAR II software that are originally dedicated to the analysis of topside

piping. Some companies use AutoPIPE software to analyse the riser and spool system.

Although the creation of the model is fairly easy, the interpretation of results is not

straightforward.

Therefore, this project wants to be able to provide another possibility for riser

and spool structural studies. It aims in a routinely use of FEA software to carry out

these studies, this one having better modelling capacities and making it possible for

simulations to get even closer to the real case of study.

1.2 Problem Statement and Objectives

The development of a finite element methodology to simulate the structural

analysis of Spool-Riser system is the main purpose of this study. In order to do so, an

existing old project will be this study base case. This study was previously carried out

using AutoPIPE software and it refers to the pre-sizing of a Spool-Riser system that is

placed under a jacket platform, Figure 1.1 illustrates this platform type and its piping

system.

The given pipe geometry will have to resist all efforts from waves, currents, im-

posed displacement due to the slight movements of the platform, internal pressure and

thermal expansion. The system is held in place by a hang off clamp and other supports.

Those support elements can be seen in Figure 1.1 as green arrows and will be better

2

detailed later on.

Figure 1.1: Jacket platform and its piping system.

Therefore, the main objective of this project was to recreate the simulation with

Abaqus and to validate its results with the ones given by AutoPIPE. With the purpose

of accomplishing it, a series of simulations with simplified geometry were made to test

and comprehend the series of events that occurs around the Spool-Riser geometry. The

studies of the influence of mesh refinement and element’s types were also made to allow

the choice of the best modeling design.

1.3 Structure of the report

This project is structured in 6 chapters which are described below:

3

• Chapter 2: discusses the theoretical background around the subsea piping system.

The main characteristics of each component will be presented and the principal

loads and responses will be discussed.

• Chapter 3: is destined to a brief presentation of the two software that are concerned

by this study: Abaqus and AutoPIPE.

• Chapter 4: aims to define modelling correlations between Abaqus and AutoPIPE.

This is made through a series of simple load case studies.

• Chapter 5: the real Spool-Riser simulation is modelled in both Abaqus and Au-

toPIPE. All modelling parameters are presented in this section, including geometry,

load sequence, mesh and boundary conditions. Finally, a final comparison between

Abaqus and AutoPIPE outputs is made.

• Chapter 6: conclusion and way forward.

4

Chapter 2

Theoretical Background

This section is dedicated to present basic information which helps elucidate the

comprehension of the following research work. Therefore it is focused on three major

subsea structures: spool, risers and pipelines.

2.1 Types of Subsea Piping Structures

2.1.1 Riser and Pipeline

Risers and pipelines are structures that transport the well fluid to the platform.

When risers are mainly vertical and connect floating units to the seabed, pipelines are

horizontal and lay on the seabed. Both structures can be either rigid (made of steel),

flexible (made using overlapping layers of steel profiles and layers of polymeric materials),

or hybrids, (a system composed by section(s) of rigid riser and section(s) of flexible

riser). There are many types of subsea ducts which could be used for: drilling, export,

production, completion and injection.

Those structures suffer great influence from external means, such as underwater

pressure, waves and currents, as well as from the movements of the platform (for risers

only). This brings an impact on the efforts suffered by the element, consequently the

structures must be capable of standing such efforts.

The following figure shows an arrangement of subsea ducts.

5

Figure 2.1: Subsea schematic layout [Ref. [1]].

2.1.2 Spool

A spool is a special shaped pipe section which connects two subsea structures

and allow the fluid transportation between them. Spools have two main functions [Ref.

[1]]:

• Allow the connection between a flowline and another subsea structure, compen-

sating for possible installation misalignments;

• As flowlines may suffer displacements (axial expansion and/or walking) during its

lifetime, spools are used to avoid the displacement from propagating and high

loads to propagate to adjacent structures.

Spools can have a series of different shapes such as: Z-shaped, M-shaped, L-

shaped etc. The shape choice is highly influenced by the field layout that the structure

is installed in. It is possible to divided spool types into two main categories: vertical and

horizontal. Figure 2.2 illustrates vertical and horizontal Z-shaped spools.

This study is focused on a Z-shaped horizontal spool.

6

Figure 2.2: Most common types of spools: vertical (left) and horizontal (right) [Ref.

[2] and [3]].

2.2 General Coss Section of Rigid Subsea Pipes

Rigid subsea pipe structures are made of high performance steel and, as they

operate under challenging conditions, a number of protection coats are applied inside and

outside of the pipe for protection. Coating mainly protect from corrosive environments,

damage caused by abrasion, falling objects and an insulation coating may be used to

conserve high temperature. Figure 2.3 illustrates a general subsea pipe cross section.

Figure 2.3: Pipe Cross Section.

7

2.3 Loads on Subsea Piping Structures

2.3.1 Loads on Risers

During its lifetime risers are submitted to a number of variant load combinations.

Some loads can be mentioned such as:

• Self weight.

• Waves: the effect depends mostly on the wave period, height and incidental di-

rection.

• Currents: the effect depends mostly on the velocity and incidental direction.

• External and internal pressures.

• Thermal expansion.

• Platform/Vessel displacements.

2.3.2 Loads on Spools and Pipelines

A subsea pipe needs to be stable on the seabed and its stability is directly related

to is weight. However, a structure that is too heavy leads to higher production and

installation costs, on the other hand a structure that is too light will find it hard to be

stable under the effects of waves and currents, being more susceptible to vertical and

horizontal movements.

There are numerous ways to stabilize a flowline on the seabed, varying from

higher wall thickness to concrete coating and anchors, however, the decision making

process usually relies on the global solution cost.

Figure 2.4, originally extracted from Ref. [5] and later adapted for the study

case, illustrates a simplified force diagram acting on a subsea pipe laying on the seabed.

2.3.2.1 Pipeline Expansion

When the pipeline is submitted to pressure and temperature loads it is logically

inclined to expand. However, it may be blocked by the soil interaction with the structure.

8

Figure 2.4: Force diagram - Spools and Pipelines.

The soil frictional behaviour generates a compressive force in the pipeline which works

to restrain the pipe from any movement, expansion included. This friction resistance is

more significant at the middle of the pipe, deceasing toward its end.

As above mentioned, the frictional resistance decreases from the middle towards

the extremities. At a give point along the pipe, the compressive force equals the expan-

sion force and the pipe is restrained from further expansion. This point is considered as

the virtual anchor point (VAP) of the flowline [Ref. [6]].

Figure 2.5 exemplifies the effective axial force acting on a given pipe and the

pipeline end displacement. It is possible to identify the restrained and unrestrained

sections of the pipe.

Figure 2.5: Pipeline end expansion.

9

2.3.2.2 Pipeline Strains

The effects of pressure, temperature and soil-pipe interaction implies to the

pipeline stresses and strains. For length located on the unrestrained section of the struc-

ture, the pipe is free to move and expansion may be noticed. On the other hand, sections

of the restrained zone will face high stresses due to the effects of friction resistance.

In order to get the total pipeline expansion, strains must be integrated along the

flowline from the free end to the anchor point. According to Bai and Bai [Ref. [1]],

a pipeline with zero initial strain and constant cross section, the pressure and thermal

strains are constant along the pipe length and the frictional strain varies linearly. Figure

2.6 shows a graphic representation of the strains along the flowline.

Figure 2.6: Strain distribution along the flowline [Ref. [1]].

The whole expansion is then given by:

∫ Lanchor

o

(εTemperature + εPressure + εfriction) dL (2.1)

10

The following points describe of the possibles strain nature and their mathemat-

ical formulation.

• Temperature Strain

When a high temperature is applied to a pipeline, stresses and strains show up

in the structure. As said before, if the pipeline is found to be unrestrained the thermal

strain will built up on the pipe. This strain is given by:

εTemperature = α∆T (2.2)

where:

α the material thermal expansion coefficient;

∆T thermal variation between initial and final states.

• Pressure Strain - End Cap Effect

Pressure strain can be divided into two natures: End Cap Effect and Poisson

Effect (see next bullet point).

The end cap effect is the contribution of the pressure in the axial direction and

it is related to the pressure effect on closed pipes and bend walls. The end cap strain is

given by:

εPEndCap=

(AiPi − AoPo)

EAs

(2.3)

where:

Ai internal area of the pipe (considering the internal diameter);

Ao external area of the pipe (considering the external diameter);

Pi is the internal pressure;

Po is the external pressure;

As is the steel cross section area.

• Pressure Strain - Poisson Effect

The Poisson effect plays a role in the pipe radial expansion due to the inter-

nal pressure. Once the pipe expands radially it suffers little axial compression. The

longitudinal strain related to the Poisson effect is given by:

11

εPEndCap= (−2ν)

(AiPi − AoPo)

EAs

(2.4)

where:

ν is the Poisson’s ratio.

• Frictional Strain - Soil Interaction

As above discussed, when the pipe starts to expand, frictional resistance builds

up trying to block the imminent movement. To do so, fictional resistance generates

negative strains which oppose the effects of pressure and temperature. For unburied

pipes (which is the study case), the frictional strain is given by:

εfriction =−µwxEAs

(2.5)

where:

µ is the axial friction coefficient;

w is the pipeline line weight;

x is the distance from the free end of the pipe.

12

Chapter 3

Software Overview

3.1 AutoPIPE

Bentley AutoPIPE is a finite element program for calculation of piping stresses,

flange analysis, pipe support design, and equipment nozzle loading analysis under static

and dynamic loading conditions. This software mainly uses the Bernoulli beam theory.

However, in the particular case of a pressure type loading, the theory of thick wall is

considered in order to take into account thickness influence.

The specificity of this software is the integration of different international stan-

dards for the design of pipes. It incorporates ASME, British Standard, API, NEMA,

ANSI, ASCE, AISC, UBC, and WRC guidelines and design limits to provide a compre-

hensive analysis of the entire system. Thus, the stresses as well as bend influence are

calculated according to these codes.

For this software results are given on nodes. For non-nodal data, which is the

case of stresses, two values are provided per node: the value immediately before and the

value immediately after the node. Besides that, stresses are calculated on the external

wall, these are consequently the maximum stresses.

A last subtlety of this software is its way of combining load cases. By default,

each time gap, friction and/or soil elements are used, the analysis is defined as non-

linear. This means that load sequence influences unitary load case results and that this

load sequence is always defined by:

• Gravity case called GR;

13

• Thermal case (T1) applied over the deformed shape of gravitational case.

• Pressure case (P1) applied over the deformed shape of case T1.

• Any user defined case (U) applied over the deformed shape of case P1. This may

comport waves, current, wind, imposed displacement or other load types.

Finally, their combination is made by simple sum of results from each unitary

load case.

3.2 Abaqus

In its turn, Abaqus is a more vast software and is able to analyse any geometry

conceived by the user. It is a multiphysic finite element computation software but

rather adapted to thermomechanical calculations. Abaqus can be assessed by a graphical

interface, called Abaqus CAE, or by input file codes. However, some modelling options

are only available for the last one which is the case of Aqua module used for modelling

all hydro efforts.

Abaqus Aqua module is used to apply steady current, wave, and wind loading

to submerged or partially submerged structures in problems such as the modelling of

offshore piping installations or the analysis of marine risers. This module can calculate

drag, buoyancy, and inertia loading only for beam, pipe, elbow, truss, and certain rigid

elements.

When it comes to element type, Abaqus element library proposes a large variety

capable of analysing models of 2D or 3D beam, linear or quadratic type. As regards

the calculation of pipes, it has two families of recommended elements: Pipe and Elbow.

Unlike others, those two families accept loads of the internal pressure type and are the

ones assessed for this study.

Pipe elements are defined by Bryan [Ref.[7]] as two or three dimensional beams

which mathematical notation includes Timoshenko beam theory, taking into account

shear deformation, axial and bending behaviours. It also includes the response of material

non-linearity and radial expansion of the cross-section caused by internal pressure.

On the other hand, although Elbow elements may also look like beam elements

for the user it has a much more complex formulation. Specially, these elements account

14

for flexibility factors in order to correct results from single beam theory, considering

ovalization and warping of the pipeline cross-section. They are recommended for thin-

walled straight pipes which might suffer collapse or for pipe sections which may already

be curved in its initial configuration (bends).

Just like pipe element, elbow elements use polynomial interpolation along their

length to solve the pipe final condition. However, in order to take into account tube

ovalization, elements from family type elbow use a Fourier-type interpolation on the

circumference. The user has the possibility to choose the desired Fourier number in a

range from 0 to 6, but the higher Fourier number the longer the simulation will take and

more precise results are expected.

Stresses and other outputs in general are calculated per element at its integration

points. The location of those integration points depends on the type of section assigned

to an element, this subject will be later detailed.

Finally, Abaqus load sequence relies on step implementation, being user free to

create any sequence combination according to simulations objectives.

3.3 FEMAP

Just like Abaqus, FEMAP is an engineering analysis program used to model finite

element models to analyse real life engineering problems. Although FEMAP is less used

than Abaqus on engineering problem solving this days, it has an very large scope of

use. Allowing the analysis ranging from basic strength analysis, dynamic simulation,

system-level performance evaluation fluid flow to multi-physics engineering studies.

FEMAP stands out when compared to Abaqus on the subject of modelling and

mesh capacities. it integrates the possibility of CAD import, modelling and meshing

tools that are more user-friendly.

For this study, in chapter 5, FEMAP will be used to define mesh control according

to the study needs.

15

Chapter 4

Correlation between Abaqus and

AutoPIPE

This section describes simple cases that were used to develop a modelling cor-

relation between Abaqus and AutoPIPE. This study was done aiming to understand

how AutoPIPE applies all sorts of loads and, consequently, how to transpose them into

Abaqus. It was also studied with the objective of understanding how both software

interpret pipe geometry, mainly elbows sections.

Those cases were not only studied with Abaqus and AutoPIPE, some times a

third software was used to help guide the comparison. For thermal and pressure cases

a theoretical MathCad sheet gave the expected results for axial expansion and friction

force, on the other hand, cases that included wave and current were also modelled with a

company internal software. More details concerning those software and their application

will be given progressively in the following subsections.

It is known through AutoPIPE documentation that this software is not capable

of computing geometric non linearity and this is to be taken as basis case for all FEA

analysis.

4.1 Straight pipe

For the first tests, a horizontal and a vertical steel pipe, with a 610 mm outside

diameter and 15.9 mm wall thickness have been studied. Those geometries were submit-

ted to several different load cases, results and conclusion can be verified in the following

16

subsections.

4.1.1 Case A: Weight loads

This first case was analysed aiming to allow the author to familiarize with Au-

toPIPE and Abaqus input file method. Besides that, it had also the objective of helping

develop a modelling correlation between software. Thus, a 9km vertical pipe fixed on its

upper end submitted only to weight load was modelled both in AutoPIPE and Abaqus.

In order to make a comparison between software, the following outputs were used for

comparison:

• vertical reaction force on the fixed end;

• vertical displacement on the free end.

Results are shown in table 4.1 for AutoPIPE, Abaqus with Pipe31 elements and

analytical calculations. Since both software were reasonably compatible with the analyt-

ical calculations, no changes were needed to adjust any of the models.

Table 4.1: Results for a straight pipe - Load case A.

Analytical AutoPIPE Abaqus

RFZ [kN ] UZ [m] RFZ [kN ] UZ [m] RFZ [kN ] UZ [m]

-20557 -15.29 -20560 -15.29 -20557 -15.30

4.1.2 Case B: Weight, content and buoyancy loads

This case is essentially the same from section 4.1.1 with an additional content

weight (internal fluid) and buoyancy load that were applied in Abaqus by using the Aqua

module with a distributed load of buoyancy type. This is the first time Aqua module

was implemented in this project, therefore this case aims to understand the way it works

and how to use it properly.

This time result comparison was made once again by the following outputs:

• vertical reaction force on the fixed end;

17

• vertical displacement on the free end.

Results are shown in table 4.2, but in this case they are not a match when it

comes to the vertical displacement on the lower end of the pipe. AutoPIPE calculates

a case where the lower end is in compression, and Abaqus still shows stretching of the

whole pipe. Logically one would expect a result as the one incoming from Abaqus.

It is also noted that a considerable difference between analytical and FEA results

are seen for the axial displacement, this could be realated to the mesh details and will

be further discussed on section 4.2.

Table 4.2: Results for a straight pipe - Load case B.

Analytical AutoPIPE Abaqus

RFZ [kN ] UZ [m] RFZ [kN ] UZ [m] RFZ [kN ] UZ [m]

-17859 -13.26 -17864 6.46 -17839 -12.60

Several tests were made, it was found that for straight vertical pipes AutoPIPE

applies buoyancy as a concentrated force on the lower end of the pipe, this leads to the

different results for axial deformation. Once the same concentrated force was applied on

Abaqus model, it gave almost the same results as AutoPIPE as shown in table 4.3.

Table 4.3: Abaqus results for a straight pipe - Load case B where buoyancy was

modeled as CF.

Abaqus

RFZ [kN ] UZ [m]

-17839 6.49

It is then identified a possible problem when it comes to modelling a Riser on

AutoPIPE: the buoyancy formulation. Other tests were made in section 4.2 to assess the

viability of AutoPIPE modelling for the study case, a Spool-Riser system, as it comprises

a long vertical pipe section.

4.1.3 Case C: Pressure load

This case intends to verify how AutoPIPE calculates section forces related to

pressure load cases and to select an output from Abaqus that corresponds to the same

18

calculation method. To help guide this study, analytical calculations based on section

2.3.2.1 were also carried out using a MathCad sheet which provides the axial displacement

and the effective axial force acting on the pipe. This sheet will be repetitively mentioned

because it was also used for further cases.

The present case consists of a horizontal element that is submitted only to internal

pressure load and is fixed on one of its extremities. The pipe is made of steel, measures

9 km, has an outside diameter of 610 mm and wall thickness of 15.9 mm. A pressure

difference of 100 bar is noticed between external and internal surfaces.

In order to make the correct assumptions on Abaqus, AutoPIPE documentation

was verified and it was discovered that, when it comes to pressure load, this software

takes all pressures as if they were applied in the external diameter of the pipe, having a

conservative approach.

To analyse this situation, three FEA simulations were put in place: AutoPIPE,

Abaqus with Pipe31 elements and Abaqus with Elbow31 elements. This time the fol-

lowing outputs were subject of comparison:

• effective axial section force measured on the fixed end;

• displacement measured on free end .

The effective axial force is a concept commonly used in the offshore industry, it

allows calculation of the global behaviour without having to integrate the internal and

external pressure over the duct wall, according to [Ref. [6]]. The axial section force given

as output by AutoPIPE is the effective axial force, meaning that it does not consider

capped pressure effects.

On the other hand, Abaqus has two different outputs for axial section forces: SF1

and ESF1. The first one is the so-called “true” axial force given by the integral of stresses

over the pipeline cross-section, the other is the effective axial force which simplifies the

influence of the internal and external pressures on the pipeline behaviour. Both outputs

are available for pipe elements, but only SF1 is available for elbow elements. Therefore,

in order to have comparable results between all calculation methods, Abaqus SF1 for

elbow elements was transformed into effective axial force according to the following

equation taken from this software library.

In this equation, pe and pi are respectively external and internal pressures; Ae

19

and Ai are the external and internal pipe section areas as used to define Abaqus pressure

load.

SFaxialAutoPIPE = ESF1Abaqus = SF1Abaqus + peAe − piAi (4.1)

Results from all three FEA simulations are summarized in the table 4.4. This

table provides results obtained with MathCad for analytical calculations, AutoPIPE and

Abaqus for pipe and elbow elements. Results incoming from elbow simulations were

obtained using Fourier ovalization mode varying from 1 to 5 which showed no change in

results for a straight pipe. A perfect compatibility between all methods is noticed. For

this case only, since no friction was applied, the force in the axial direction is zero for all

four calculation methods and therefore is not presented on the results table.

Table 4.4: Results for a straight pipe - Load case C without friction.

MathCad AutoPIPE Abaqus Pipe Abaqus Elbow

Uaxial[m] 1.562 1.562 1.562 1.562

Then, in order to evaluate frictional behaviour of both software, a friction factor

of 0.59 in all directions was imposed in all three calculations methods. Results are

summarized in table 4.5. Displacement results are likely to be considered good enough,

although there is still a slight difference. However, a difference around 4 mm for a 9 km

long pipe is to be considered irrelevant.

Effective axial force this time still has a very good correspondence between meth-

ods, however Abaqus Elbow simulation diverges a little from the others. This is believed

to be related element type modelling approach and the consequent error propagation

when modifying SF1 into ESF1.

Table 4.5: Results for a straight pipe - Load case C with friction.


Faxial[kN ] 1050.2 1050.2 1055.3 1037.1

Uaxial[m] 0.077 0.081 0.074 0.074

20

4.1.4 Case D: Temperature load

For this case, an ambient temperature of 3.7◦C and an internal temperature

of 12.1◦C were taken for a 9 km long pipe, both being constant along the structure

length. The other characteristics of the structure were kept as in case C described above.

Analytical calculations were made using the Mathcad sheet and FEA were carried out

with AutoPIPE and Abaqus. Results are those shown in table 4.6 and were taken in the

same spots as in case C.

Since no friction was applied, the axial force is zero for all four calculation methods

and therefore is not presented on the results table.

Although results may diverge a little, attention is raised to the fact that the

maximum discrepancy is 13mm out of a 9km pipe.

Table 4.6: Results for a straight pipe - Load case D.


Uaxial[m] 0.885 0.884 0.897 0.890

4.1.5 Case E: Waves and current load

In this section waves and current loads will be analysed with Abaqus, AutoPIPE

and a company internal software. This last one allows the analysis of a vertical pipe

that can be submitted to wave and/or currents. It requires as input the wave data, the

pipe geometry, the drag and inertia coefficients and current data. Its outputs are the

force and moment to which the structure is subjected, however, in the internal company

software, no information concerning the application location of this moment is given

and, therefore, only the force output is used for comparison matters.

This case was chosen to be studied to test the use of Abaqus Aqua module for

modelling waves and currents and to define a correspondence between its modelling

methods and AutoPIPE.

One must know that those two FEA software have one major difference when

modelling waves, they have an intrinsic 180◦ phase difference. For AutoPIPE a 0◦ phase

orients the crest of the wave at the origin, whereas 180-degree places its bottom at the

origin. The exact opposite occurs in Abaqus Aqua module as illustrated by figure 4.1.

21

Figure 4.1: Wave phase orientation for Abaqus and AutoPIPE both with 0-degree

phase angle.

This case was modelled as a vertical pipe of 70 m fully submerged, fixed on

its upper end and free on its lowest point. To analyse this situation, two static FEA

simulations were put in place: AutoPIPE and Abaqus with Pipe31 elements. This time

the following outputs were subject of comparison:

• reaction force measured on the fixed end;

• reaction moment measured on the fixed end;

• displacement on free end.

This section first case (case E.1) includes only a wave load. In all three calculation

methods the user must select a wave theory either Airy Wave, Stokes or Stream function.

The region of applicability of each theory can be seen in appendix A.

For the first analysis, a wave height of 15.47 meters and a 12.81 seconds period

was chosen and modelled with Stokes wave theory. This wave has a 90-degree phase

angle for the company internal software and AutoPIPE, therefore a 270◦ for Abaqus.

The considered axis and incoming wave are shown in figure 4.2 below.

Another important point regards the drag, lift and inertia coefficients, they were

set as 1.2 for drag and 3.29 for inertia. This topic is one major difference between soft-

ware, AutoPIPE is able to compute lift efforts, Abaqus Aqua module is not. Therefore,

22

Figure 4.2: Schematic Case E.1 (left) and E.2 (right).

lift was set to zero in AutoPIPE for this section and all that follows, although for this

section it shouldn’t play any role.

Results seem compatible between all three calculations methods as can be seen

in table 4.7.

Table 4.7: Results for a vertical pipe submitted to wave load.

Fy[kN ] Mx[kN.m] Uy[m]

Internal

software

-68.0 -2801.3 (1) -

AutoPIPE -66.6 -1966.0 -8.34

Abaqus -68.1 -1968.5 -8.24

Note:

(1) Result not comparable with the others because its output location is unknown.

The second analysis (case E.2) uses the same wave and coefficients from before

and adds a current defined in table 4.8, see schematic in figure 4.2. Case E.2 results

can be found in table 4.9 and, once again, no major differences were found between all

three software.

23

Table 4.8: Current data - Load case E.2.

Depth [m] Current Velocity, Uc [m/s]

MSL 2.00

-17.5 1.80

-35.0 1.60

-52.5 1.35

-70.0 1.00

Table 4.9: Results for a vertical pipe submitted to wave and current load.

Fy[kN ] Mx[kN.m] Uy[m]

Internal

software

-137.3 -5708.7 (1) -

AutoPIPE -126.1 -3753.4 -15.81

Abaqus -128.9 -3763.4 -15.62

Note:

(1) Result not comparable with the others because its output location is unknown.

24

4.2 Geometry with a bend

The second geometry can be seen in Figure 4.3, it is composed by a horizontal

45 meters long pipe followed by a 90◦ bend with radius of 3.05 meters. The bend is

connected to a vertical section that goes from the seabed to sea free surface and mea-

sures 90 meters. The model rests on a rigid soil with no friction and is tied on its lower

edge (Dx, Dy, Dz, Rx, Ry and Rz = 0) as illustrated by the gray element.

Since the main case of study has several bends along its length this new geometry

was studied to understand how to model bend zones in Abaqus as it is in AutoPIPE.

Therefore two elements families were used in Abaqus: Pipe and Elbow. Their perfor-

mance will be discussed in the following sections. Besides that, this section also means to

define a correct way to combine load cases so Abaqus can represent the same conditions

as AutoPIPE.

Figure 4.3: Pipe with a 90-degree bend.

25

4.2.1 Case A: Weight load

In this case the geometry is only submitted to weight load. The reaction force

on the soil and displacement on the highest point of the pipe were measured, this point

is identified by a green cross in figure 4.3.

AutoPIPE results are shown in the table 4.10. Results from Abaqus shown in

table 4.11, these were obtained using 4 elements type Pipe31 along the bend area. Since

results were not compatible when it comes to the displacement on the upper end, the

number of elements along the bend was increased in order to study its influence and

choose a mesh that has already converged. Results emerging from this approach can

also be seen in table 4.11.

Table 4.10: AutoPIPE results for the geometry with a bend - Load case A.

RFZ [kN ] UX [m] UY [m] UZ [m]

-312.3 0.0 2.261 -0.064

Table 4.11: Mesh influence on Abaqus results for the geometry with a bend modeled

with Pipe31 - Load case A

Elements along the bend RFZ [kN ] UX [m] UY [m] UZ [m]

4 -312.2 0.0 1.546 -0.050

12 -312.2 0.0 1.543 -0.051

25 -312.3 0.0 1.543 -0.051

50 -312.3 0.0 1.529 -0.052

100 -312.3 0.0 1.529 -0.052

It was noticed that, although the quantity of elements increased, results don’t

seem to be converging to the same values as AutoPIPE simulation. This was taken as an

indication that maybe element type used in Abaqus was not the right one in comparison

to AutoPIPE. The present led to the use of elbow elements for the bend section and some

attempts were made to find the correct Fourier mode, results for different combinations

between mesh and Fourier modes are shown in table 4.12.

Elbow elements were developed to better model bend zone in which ovalization

may occur. Those elements are modelled as beams but their mathematical theory is

26

actually shell type with quite complex deformation patterns allowed. Because elbow

elements use shell formulation, the number of degrees of freedom per element is high.

Those elements also use Fourier modes to model ovalization, all of which leads to more

expensive computational simulations than beam common elements.

From all these results, it is concluded that at least a mode 3 is required in order

to achieve quality results in comparison with AutoPIPE. When it comes to the number

of elements along the bend, although results don’t change enormously from one mesh

to another, a longer analysis of convergence must be done if the required precision is

not yet achieved.

27

Table 4.12: Mesh influence on Abaqus results for the geometry with a bend modeled

with Elbow31 - Load case A.

Elements along the bend Fourier mode RFZ [kN ] UX [m] UY [m] UZ [m]

1 0.0 1.550 -0.051

2 0.0 2.223 -0.065

4 3 -312.3 0.0 2.277 -0.066

4 0.0 2.283 -0.066

5 0.0 2.284 -0.066

1 0.0 1.541 -0.051

2 0.0 2.189 -0.064

12 3 -312.3 0.0 2.229 -0.065

4 0.0 2.236 -0.065

5 0.0 2.236 -0.065

1 0.0 1.539 -0.051

2 0.0 2.186 -0.064

25 3 -312.3 0.0 2.226 -0.065

4 0.0 2.233 -0.066

5 0.0 2.233 -0.066

1 0.0 1.506 -0.050

2 0.0 2.182 -0.064

50 3 -312.3 0.0 2.222 -0.065

4 0.0 2.233 -0.065

5 0.0 2.233 -0.065

28

4.2.2 Case B: Weight, content and buoyancy loads

Since case B in section 4.1.2, page 17, was contradictory when it comes to the

way AutoPIPE applies buoyancy load, this load case aimed to verify that when pipes

with different orientations are put together, the buoyancy is applied as a line load on

AutoPIPE and that results are in line with Abaqus.

The same approach from case A above was used, starting by AutoPIPE followed

by Abaqus with Pipe31 only and then with Elbow31 on the bend area. Results from all

three methods are shown in table 4.13. Based on the analysis made in case A, Abaqus

results were obtained with 25 elements along the bend zone and Fourier mode 3 for

elbow simulations.

Table 4.13: Results for the geometry with a bend modelled with 25 elements - Load

case B.


AutoPIPE -271.4 0.0 1.963 -0.056

Abaqus Pipe31 -271.3 0.0 1.252 -0.045

Abaqus Elbow31 -271.4 0.0 1.934 -0.057

Once again, as happened in the previous section, results from Abaqus with el-

ements Pipe31 are not as close to those from AutoPIPE and the implementation of

elbow elements gave better results. It is concluded that elbow elements have a better

correspondence with AutoPIPE and, therefore, should be rather preferred.

4.2.3 Case C: Weight, content, buoyancy, temperature and

pressure loads

This case in based on the previous one and applies temperature and pressure

loads on top of it. The initial state was defined by a temperature of 3.7◦C and the final

by a temperature of 12.1◦C, besides a internal pressure of 100 bar was applied.

Since previous cases suggested that element quantity, for this cases, did not make

a difference in output quality, Abaqus simulations were carried out with 25 elements

around the bend area and Fourier mode 3 for elbows. Results may be seen in table 4.14

for all three simulation methods.

29

Once again they are more consistent between AutoPIPE and Abaqus Elbow el-

ements which restates the need of this type of elements to model bend areas when

resuming AutoPIPE modeling in Abaqus.

Table 4.14: Results for the geometry with a bend modeled with 25 elements - Load

case C.


AutoPIPE -271.4 0.0 1.975 -0.062

Abaqus Pipe31 -271.3 0.0 1.337 -0.051

Abaqus Elbow31 -271.4 0.0 1.994 -0.064

4.2.4 Case D: Weight, content, buoyancy, temperature, pres-

sure, waves and current loads

This case applies waves and current loads on the condition of load case C from

above section. A wave height of 15.47 meters and a 12.81 seconds period was chosen

and modelled with Stokes wave theory. This wave has a 90-degree phase angle for

AutoPIPE, therefore a 270◦ for Abaqus as explained in section 4.1.5, page 21.

Besides, a current defined in table 4.15 was applied. Results seem compatible

between all three calculations methods as can be seen in table 4.16, however Abaqus

with pipe elements have a disadvantage because they can’t calculate precisely the dis-

placement. Abaqus simulations were carried out with 25 elements around the bend and

Fourier mode 3 for Elbow elements.

Table 4.15: Current data- Load case D

Depth [m] Current Velocity, Uc [m/s]

MSL 1.81

-22.5 1.66

-45.1 1.63

-67.7 1.45

Seabed 1.37

30

Table 4.16: Results for the geometry with a bend modeled with 25 elements - Load

case D.


AutoPIPE 426.1 0.0 2.640 -0.0025

Abaqus Pipe31 426.0 0.0 2.324 -0.0017

Abaqus Elbow31 426.0 0.0 2.639 -0.0019

4.3 Summary of results and conclusion

This section of this report intended to gather useful information concerning

AutoPIPE-Abaqus modelling correlation. It had three main objectives:

• test Abaqus Aqua module;

• verify the coherence between both software;

• define recommended modelling choices to analyse pipes with Abaqus.

4.3.1 Conclusion

Firstly it is concluded that Abaqus Aqua module is able to model correctly almost

all hydrodynamic efforts, applying buoyancy, drag and inertia efforts and applying waves

and currents. However it is not yet capable of modelling lift effort which is a real

drawback. In order to consider lift efforts it should be modelled using a subroutine.

During this phase, a comparison between two types of elements used by the

Abaqus software, pipe and elbow elements, were also matter of analysis. The calculation

being faster with the pipe elements, there was a strong urge to validate the use of such

elements. However, it was proven that those elements do not quite represent the same

as AutoPIPE simulations and, consequently, Elbow elements with Fourier mode of at

least 3 were found to be a better option.

Thanks to this first modelling phase, it was possible to acquire all the necessary

knowledge to model the Spool-Riser system with Abaqus.

31

4.3.2 Findings

The main findings gathered by all tests are listed hereafter and are recommended

for further analysis:

• Weight: should be modelled as line load or gravity load in Abaqus.

• Buoyancy and content loads: well modelled by Abaqus Aqua module with line load

type.

• Waves: waves with 180◦ phase difference from AutoPIPE referential and modelled

via Abaqus Aqua module.

• Current: well modelled by Abaqus Aqua module.

• Hydrodynamics efforts: Drag and inertia well modelled by Abaqus Aqua module,

although Abaqus is not yet capable of analysing lift forces. Lift forces are important

to analyse the spool and the pipeline that rest on the soil.

• Mesh: at bend area it doesn’t seem to influence results.

• Bends geometry: better represented by elbow elements with high Fourier mode.

• Step type: static general without geometric non-linearity shall be used for compar-

ison with AutoPIPE.

32

Chapter 5

Methodology for recreating

AutoPIPE simulation into Abaqus

In this section the export line geometry, composed by topside, riser, spool and

pipeline, was analysed using Abaqus software in both operating and hydrotest condi-

tions. At first, the geometry and mesh were modelled using FEMAP software. Later an

initial Abaqus model case was put in place to adjust simulation parameters, to assure

convergence and to allow initial comparison between AutoPIPE and Abaqus results.

Once the global model was working properly, VBA macros were developed to

generate all Abaqus input files, each of them representing one of AutoPIPE load cases.

AutoPIPE simulations analyses 53 load combinations for hydrotest conditions and 53 for

operations, those cases combine waves and displacements in different direction besides

cases GR, T1 and P1 previously mentioned.

The next step was the comparison of results in terms of displacement, reaction

force and moment, section forces and moments and stresses.

5.1 Geometry and Mesh - Femap

As mentioned before, geometry and mesh parameters were defined with FEMAP.

This choice was made because this software is more user-friendly than Abaqus CAE when

it comes to geometry definition and mesh control. Moreover, FEMAP exports geometry

directly into Abaqus input file format and allows direct manipulation of nodes, elements

and sections.

33

A view of FEMAP geometry and mesh model is shown in figure 5.1, it is composed

of 756 nodes and, consequently, 755 elements. The element size along elbow areas

is around 0.1 meters. For straight sections, elements length has been progressively

increased towards the next bend and reduced close to the bend (bias on both ends). This

strategy was used to reduce the global number of elements and to make de simulation

faster.

Figure 5.1: FEMAP mesh overview.

5.2 Pipe design data

This section presents all pipe parameters that were used in AutoPIPE original

simulations and in Abaqus.

5.2.1 Material

Material properties for all pipes are provided in table 5.1.

34

Table 5.1: Material Data - Steel.

Steel Parameters Value

Density [kg/m3] 7850

Thermal expansion coefficient [C−1] 1.17 x 10−5

Young's modulus [MPa] 207 000

Poisson's ratio 0.30

5.2.2 Pipe and coating data

Pipeline and coating data are presented in tables 5.2, 5.3 and 5.4 .

Table 5.2: Pipe Data - Spool and Pipeline.

Steel Grade Value [mm]

Nominal outer diameter 610.0

Corrosion allowance 3.0

Nominal wall thickness 15.9 / 19.05 (1)

Anticorrosive coating thickness 2.2 / 3.5 (2)

Concrete coating thickness 70.0

Notes:

(1) Thickness of 19.05 mm has been considered only for spool bends.

(2) 3.5 mm of coating is considered for line pipes without concrete.

Table 5.3: Pipe Data - Riser and Topside.

Steel Grade Value [mm]

Nominal outer diameter 610.0

Nominal wall thickness 19.05

Anticorrosive coating thickness 3.5

Concrete coating thickness N/A

35

Table 5.4: Density of materials

Material density Value [kg/m3]

Hydrotest fluid 1030

Operation fluid 92

Steel 7850

Anticorrosive coating 940

Concrete Weight coating 3050 (High Density)

5.2.3 Pressure and temperature data

Data in table 5.5 was used for AutoPIPE analysis and consequently for this

project.

Table 5.5: Pipe Data - Riser and Topside.

Parameter Value

Design pressure [barg] 96.5

Maximum design temperature [◦C] 71.0

Hydrotest pressure [barg] 101.3

Hydrotest fluid temperature [◦C] 12.2

5.2.4 Fitting data

The geometry of study is composed of a valve and two flanges that represents an

additional weight to the structure, their weight can be found in table 5.6. Their location

will be shown later on.

Table 5.6: Fitting weight data.

Fittings Weight [kg]

Flange 870

Valve 7000

36

5.3 Environmental data

5.3.1 Water depth and seawater density

For the spool and riser stress analysis, a water depth of 70 m/CD is used and a

seawater density is defined as 1026 kg/m3 .

5.3.2 Waves and currents

Extreme omni-directional wave and current data are presented in table 5.7 and

table 5.8, they are both used for stress analyses. This wave is considered to be applied

at MSL = CD + 4.8 m.

Table 5.7: Current data.

Current Velocity, Uc [m/s]

Depth [m] Return Period

1 year 10 years 100 years

MSL 1.44 1.61 1.78

-10.0 1.35 1.50 1.66

-20.0 1.32 1.47 1.63

-30.0 1.30 1.45 1.60

-40.0 1.27 1.42 1.56

-50.0 1.27 1.38 1.52

-60.0 1.18 1.32 1.45

-73.4 0.96 1.07 1.18

Table 5.8: Wave data.

Extreme Hmax [m] Extreme Thmax [s]

Return Period Return Period

1 year 10 years 100 years 1 year 10 years 100 years

11.9 15.47 19.06 11.21 12.81 14.25

Note that CD stands for Chart Datum which is level to which both tidal levels and water depths are

reduced. Generally it matches the lowest astronomical tide.

37

5.3.3 Hydrodynamic coefficients

Hydrodynamic coefficients that have been used in the original AutoPIPE calcula-

tions are shown in table 5.9. However, Abaqus is not yet capable of applying lift efforts

and for comparison objectives this factor was suppressed from AutoPIPE simulations.

Table 5.9: Hydrodynamic coefficients.

Hydrodynamic coefficients Drag Lift Inertia

Riser 1.2 0.0 3.29

Single pipe with concrete 0.9 0.9 3.29

5.3.4 Marine Growth

Marine growth profile used in AutoPIPE modeling approach is shown in table

5.10. Its density is considered as 1435 kg/m3.

Table 5.10: Marine growth profile.

Depth [m/CD] Radial Thickness

-20.0 to +4.8 100 mm

-30.0 to -20.0 Linear variation form 30 mm to 100 mm

-seabed to -30.0 Linear variation form 10 mm to 30 mm

5.3.5 Soil

Table 5.11 summarizes soil properties.

Table 5.11: Soil properties.

Parameters

Type of soil Sand/Gravel

Soil stiffness 1250 N/mm/m

Axial friction coefficient 0.49

Lateral friction coefficient Hydrotest / Operation 1.16 / 1.06

38

5.4 Interface Data

5.4.1 Pipeline Expansion

Table 5.12 presents pipeline expansion considered for AutoPIPE and Abaqus

analysis.

Table 5.12: Pipeline expansion.

Load Case Pipeline Expansion [m]

Hydrotest 0.11

Operation 1.38

5.4.2 Platform Movements

Table 5.13 resumes the imposed displacement at platform levels considered for

this study, considering 100 years return-period meteocean data. Those displacements

were applied on support levels since those structures are the connection between the

pipe and the platform.

Table 5.13: Platform displacements.

Element Elevation Extreme 100-year Displacements [mm]

Topsides + 21.50 m/CD 130.6

HOC + 14.00 m/CD 124.8

Support 1 + 7.30 m/CD 121.9

Support 2 - 5.50 m/CD 107.9

Support 3 - 19.50 m/CD 88.4

Support 4 - 27.60 m/CD 73.6

Support 5 - 35.50 m/CD 43.9

Support 6 - 43.50 m/CD 25.0

Support 7 - 53.50 m/CD 9.9

39

5.5 Load cases

Since AutoPIPE analyses very quickly lots of load case combinations, it was

needed to put in place a code to generate all Abaqus input files and to turn all simulations

one at a time. Therefore, four main input files were written and used to compare results

from AutoPIPE and Abaqus and to evaluate element type influence on result quality.

Those four files were:

• Hydrotest case with pipe elements only

• Hydrotest case with elbow and pipe elements

• Operation case with pipe elements only

• Operation case with elbow and pipe elements

Those files had general information concerning the model, for instance: the ge-

ometry, material, element and section definition, wall thickness, sea level, soil properties

among others.

Later, a VBA code was used to manipulate strings and write all steps and load

definition in accordance with what was presented by AutoPIPE model for both Hy-

drotest and Operation conditions. Input information for each case was transposed from

AutoPIPE into Excel which later fed the VBA code. This code created the input file

for all unitary load cases shown in table 5.14 and for their combination, shown in table

5.15. To allow all cases to turn one at a time, a file .bat was used to fed Abaqus.

40

Table 5.14: Unitary Load Cases.

Load Case Corresponding load

G Weight with marine growth and buoyancy

T1 Pipeline expansion and thermal expansion of the riser and spool

P1 Pressure (Depending on studied case hydrotest pressure or design pressure)

U1 Support displacement following +X (operating displacement) (1)

U2 Support displacement following -X (operating displacement) (1)

U3 Support displacement following +Y (operating displacement) (1)

U4 Support displacement following -Y (operating displacement) (1)

U6 Wave and current following +Y (100 Y in Operating, 10 Y in Hydrotest) (1)

U7 Wave and current following +X (100 Y in Operating, 10 Y in Hydrotest) (1)

U8 Wave and current following -X (100 Y in Operating, 10 Y in Hydrotest) (1)

U9 Wave and current following -Y (100 Y in Operating, 10 Y in Hydrotest) (1)

Notes:

(1) Sign convention as per Figure 5.5.

Table 5.15: Combined Load Cases.

Combination Name Corresponding ULC Combination Name Corresponding ULC

GT1 G+T1 GT1P1U13 G+T1+P1+U4+U9

GT1P1 G+T1+P1 GT1P1U14 G+T1+P1+U1+U9

GT1P1U1 G+T1+P1+U1 GT1P1U15 G+T1+P1+U2+U6








GT1P1U10 G+T1+P1+U1+U6 GT1P1U23 G+T1+P1+U2+U8



41

5.6 Modeling choices

5.6.1 Soil

Soil was chosen to be modeled as a rigid surface. An interaction between this

surface and all pipes nodes was set so the pipe would not be able to pierce the soil.

Friction was defined in Abaqus according to table 5.3.5, page 38, meaning that axial

friction coefficient was determined as 0.49 and lateral as 1.16 for hydrotest and 1.06 for

operation.

However, this represents a difference between software modeling approaches.

AutoPIPE only accepts one friction coefficient per soil element. This means that the

user needs to predict in which direction (axial or lateral) each pipe element is more likely

to move and define consequently its friction coefficient. In this case, Abaqus seems to

have a more realistic approach.

Figure 5.2 bellow illustrates the soil in green and the pipe structure in red, its

possible to verify that the pipe is not capable of passing thought the soil.

Figure 5.2: Abaqus modeled geometry: supports, soil and pipe structure.

42

5.6.2 Riser guides/supports

Riser guides and supports were modeled using tube-to-tube contact elements (

named ITT elements). This type of element is used model the interaction between two

tubes where one tube lies inside the other or between two tubes that lie next to each

other [Ref. [9]]. As stated before in previous sections, along riser length seven supports

were modeled according to AutoPIPE model.

For the study case, those supports where modeled as pipe-in-pipe structure and

one of the parameters to model such interaction between tubes is contact clearance.

Clearance is defined as the distance between the outer pipe inner diameter and the inner

pipe outer diameter, as shown in Figure 5.3 taken from [Ref. [10]].

Figure 5.3: Clearance definition for tube-to-tube contact elements.

On the original model made in AutoPIPE, supports have no clearance however,

to make convergence easier on Abaqus it was set as 2 mm in this software. Figure 5.4

shows a section of Abaqus model and illustrates tube-to-tube contact modeling.

A modeling difference relies on the fact that, for AutoPIPE, those supports are

defined as points that are blocked in their local horizontal plane. On the other hand,

Abaqus modeling has a pipe-in-pipe approach which is more realistic from interaction

point of view, but blocks movement on global horizontal plane.

A last parameter regarding support modeling is its rigidity. On AutoPIPE model

supports are defined as rigid and according to its documentation that means that the

Young’s modulus of this element is a thousand times the Young’s modulus of the defined

material. Therefore, the same modeling choice was made for Abaqus model, although

this software could provide a more realistic analysis of support behavior if it was desired.

Figure 5.2 in the above section shows the pipe geometry in red, its supports in

blue and the soil in green. This image is provided in order to give the reader a visual

reference on the model geometry.

43

Figure 5.4: Support geometry made for Abaqus model with tube-to-tube contact

elements.

5.6.3 Valve and flanges

The original geometry is composed by a valve and two flanges that should be

correctly modeled on Abaqus. Both components are modeled as an additional weight

on AutoPIPE, however valves are considered as line loads and flanges as concentrated

forces. Both structures can be seen and located on the geometry sketch in figure 5.5.

Another detail concerns those elements rigidity. According to [Ref. [11]], al-

though flanges are more rigid than a regular pipe, its real rigidity does not affect analysis

results to any significant extent. Thus, AutoPIPE uses regular pipe rigidity for flange

elements and the same approach is used on Abaqus.

On the other hand, according to [Ref. [11]] , valves rigidity influences results and

are consequently considered on AutoPIPE and, in this software, its Young’s modulus is

a thousand times the Young’s modulus of the regular pipe. Logically the same approach

was used for Abaqus modeling. It has to be noted that this valve is located on the

topside area where loads are limited (no waves).

5.6.4 Concrete, anti-corrosion and marine growth

To take into account those three terms on Abaqus model, their weight was incor-

porated as equivalent density applied to the simple pipe itself. Besides, this parameter

also influenced hydrodynamic efforts, the total outer diameter related to the additional

external coating was used on the Aqua module for buoyancy, drag and inertia forces.

44

Figure 5.5: AutoPIPE loads and BC choices for the main case of study.

45

5.6.5 Load sequence

AutoPIPE has a specific load sequence that was previously mentioned. It is

recalled that the software starts by applying gravity case, composed by weight, buoyancy

and content loads. Then from this case deformed shape of case it applies thermal

case and, on top of that, pressure case. Finally, it applies imposed displacement and

hydrodynamic forces together. Creating combined cases as defined on section 5.5.

On the other hand, Abaqus load sequence is defined by steps. Consequently,

for this model steps were set in the same order as AutoPIPE, but due to convergence

difficulty imposed displacement and waves were separated in two different steps. Step

sequence, loads and time can be seen in table 5.16 below. This is not truly the same

modeling approach from AutoPIPE, but the following sections will prove it to be a good

one.

To model a complete wave in Abaqus Aqua module the total simulation time

should be equal to or a multiple of the wave period, because in Abaqus waves starts to

propagate from the beginning of the simulation. Therefore, in this study, the step time

of all steps that come before wave loading was defined as very small in comparison with

the last one. This last step is used for wave propagation, adding drag and inertia efforts

into the simulation.

Table 5.16: Abaqus step sequence.

Case

condition

Step

number

Total

timeLoads

HY/OP 1 0.01 Self weight, content weight and buoyancy

HY/OP 2 0.01Loads Step 1 + thermal expansion and

internal pressure

OP 3 0.01 Loads Step 2 + change of temperature

HY/OP 3/4 0.01 Loads Step 2/3 + platform displacement

HY/OP 4/512.78/

14.21Loads Step 3/4 + wave and current loading

46

5.7 Results

To allow the post processing of all load cases for both Hydrotest and Operation

conditions the best approach would be the implementation of python codes that interact

with Abaqus .odb/.dat files and extracts the desired information. However, due to this

report deadline the mentioned code has not yet been implemented and this section results

were extracted using only recorded macros on Abaqus.

Due to the enormous amount of results, only case GP1T1U20-HY will be pre-

sented but all others should have given results with around the same quality and will

likely be correctly validated by comparison with AutoPIPE. This case was randomly cho-

sen among those that combine all types efforts and as described in section 5.5, table

5.15, case GP1T1U20 is the junction of cases G, T1, P1, U3 and U6.

5.7.1 Displacement

Displacement results for case GP1T1U20 in hydrotest conditions can be seen in

figures 5.6 and 5.7 that show the displacement along the pipe length in X and Y direction

respectively. In those figures the blue area corresponds to the topside part, the green

area stands for the riser length, yellow part for the spool section and the amber for the

pipeline. Besides, the dotted lines show the location of the hang off clamp and the other

seven guides. Continuous lines correspond to results from AutoPIPE, Abaqus with pipe

elements and with both elbow and pipe elements.

The most significant difference seen in figure 5.6 between Abaqus and AutoPIPE

is located at the end of the spool and along the pipeline. This difference is believed

to be related to the friction assessment on AutoPIPE. This software can only take one

friction factor per element, this means that a pipeline would have either its true axial

friction or its lateral friction, on the other hand Abaqus can set two different frictions,

one in each direction. AutoPIPE friction was chosen in accordance with the expected

movement of the element, therefore it was defined an axial friction coefficient of 0.49

for the pipeline.

47

Figure 5.6: X displacement results - Case GP1T1U20-HY.

Figure 5.7: Y displacement results - Case GP1T1U20-HY.

48

In figure 5.7 there is also a divergence along the pipeline. It is believed that

Abaqus represents a closer situation to the reality since in this area this graphic stands

for the lateral movement of the pipeline and the friction coefficient should be 1.16 and

not 0.49 as it was defined in AutoPIPE. It is believed that, if pipeline lateral movement

was restricted in AutoPIPE, axial displacement would increase and be compatible with

Abaqus.

On the other hand, the start of the topside also shows incompatible results

between Abaqus and AutoPIPE. This time, although the difference is minor, results

coming from Abaqus seem more reliable. This because for this specific load case the

start end of the topside has an imposed displacement on +Y as described in section

5.5, page 40. Therefore, the displacement on this node should be equal to the imposed

one, this result is as expected for both Abaqus simulations, but AutoPIPE presents a

displacement that is inferior to the one applied.

Spool deformed shapes from all three simulation methods may be seen in figures

5.8, 5.9 and 5.10. In figure 5.8, AutoPIPE deformed shape is represented in red and

the unformed geometry in black. For the other two images, extracted from Abaqus,

deformed shape is rainbow colored and unformed is, once again, represented in black.

Figure 5.8: AutoPIPE top view deformed shape, 25 scale factor - Case GP1T1U20-

HY.

49

Figure 5.9: Abaqus Pipe top view deformed shape, 25 scale factor - Case GP1T1U20-

HY.

Figure 5.10: Abaqus Elbow-Pipe top view deformed shape, 25 scale factor - Case

GP1T1U20-HY.

Those images show deformed shapes that are very close to each other in shape

and magnitude as also indicated by figures 5.6 and 5.7. Although little divergences

show that Abaqus simulations using elbow-pipe elements may give closer results to the

50

ones from AutoPIPE, this divergence is so tiny, as endorsed by figures 5.8 to 5.10, that

simulations using only pipe elements may be a better choice from displacement point of

view, since it takes around 1/10 of the total time of an elbow-pipe simulation.

5.7.2 Reaction force and reaction moment

The following tables, table 5.17 and 5.18, provide the reaction force on the

supports in the global axis for all three models. Results seem a little more compatible

for AutoPIPE and Abaqus Elbow-Pipe simulation. This was expected since simple cases

from section 4.1, page 16, had already given good results for reaction forces when

Abaqus Aqua is used.

Table 5.19 provides the reaction moment on the hang off clamp in the global

axis for all three models. In section 4.1 indicated that reaction moment wouldn’t have

a great divergence between FEA methods, however it is not the reality. Results provide

around the same magnitude, but components seem a little off and further investigations

are recommended.

Table 5.17: AutoPIPE reaction force on pipe supports - Case GP1T1U20-HY.

RFX [kN ] RFY [kN ] RFZ [kN ]

HOC 8.9 31.8 262.4

+7.3m/CD 8.0 132.4 0.8

-5.5m/CD 5.1 122.1 0.5

-19.5m/CD 2.8 54.7 0.2

-27.6m/CD 3.1 50.1 0.3

-43.5m/CD 5.9 52.1 0.5

-53.5m/CD 3.1 0.9 0.3

-63.5m/CD 11.5 33.6 34.0

51

Table 5.18: Abaqus reaction force on pipe supports - Case GP1T1U20-HY.

Abaqus Elbow/Pipe Abaqus Pipe

RFX [kN ] RFY [kN ] RFZ [kN ] RFX [kN ] RFY [kN ] RFZ [kN ]

HOC 8.8 31.3 260.4 8.8 31.8 262.4

+7.3m/CD 7.1 129.0 0.7 7.1 128.9 0.7

-5.5m/CD 4.5 123.3 0.4 4.5 123.4 0.4

-19.5m/CD 2.6 54.7 0.2 2.6 54.6 0.2

-27.6m/CD 3.3 50.5 0.3 3.3 50.6 0.3

-43.5m/CD 5.2 52.2 0.5 4.5 51.4 0.4

-53.5m/CD 3.7 3.3 0.3 2.1 5.8 0.2

-63.5m/CD 17.1 32.0 33.4 19.9 29.0 30.7

Table 5.19: Reaction moment on the hang off clamp - Case GP1T1U20-HY.

MX [kN.m] MY [kN.m] MZ [kN.m] MR[kN.m]

AutoPIPE 3.877 8.027 22.955 24.625

Abaqus Pipe31 0.443 18.110 26.480 32.658

Abaqus Elbow31 10.605 7.002 31.962 34.406

5.7.3 Section force and section moment

Section forces and moments were also subject of comparison between software.

In order to compare those variables, their value in local axis was rather used. Therefore

it was important to define a beam direction on Abaqus that corresponds to the one from

the base software. For AutoPIPE, pipe main axis is defined by the points order. As an

example, if there is a point called A00 that is linked to one A01, the element main axis

is defined from A00 to A01, as illustrated by figure 5.11.

AutoPIPE gives 6 outputs for section forces, three in global axis: x, y, z; and other

three in local axis: axial, shear in local direction 1 and 2. But one may be aware that,

for axial section force this software does not consider capped pressure loads, meaning

that it actually presents the effective axial section force.

52

Figure 5.11: AutoPIPE local axis definition.

As stated in section 4.1.3, page 18, Abaqus has an output called SF (section

force) and another called SM (section moment), both being measured in local axis.

By default, Abaqus axial section force, SF1, takes pressure load into consideration, but

fortunately the software has also an output called ESF1 (effective axial section force) that

simply recalculates axial force without capped pressure effect. Therefore, comparison

between section force in axial direction should be made between AutoPIPE axial force

and Abaqus EFS1 output, as per section 4.1.3.

Other section forces and section moments are calculated in the same way in both

software and, consequently, Abaqus output SF and SM can be used. Magnitude results

from both, outputs, may be seen in images 5.12 and 5.13 bellow.

Figure 5.12: Effective axial force results in local axis - Case GP1T1U20-HY.

53

Figure 5.13: Bending moment about the local 1-axis - Case GP1T1U20-HY.

From those graphics it is possible to conclude:

• Topside and riser:

– results are in very good agreement.

• Spool and pipeline:

– Effective axial force shows some disagreement specially on the pipeline area

which could be related to friction assessment. This was not the case in the

simple cases from section 4.1, page 16.

– Section moment is overestimated with Pipe31 which can be explained by the

stiffness of those elements. However, for elbow model a better result was

expected since it takes it account bend flexibility.

54

5.7.4 Stress

As for the section force, both software have different methods for calculating

stress and consequently some adjustments must be done in order to compare the correct

outputs.

As previously mentioned, AutoPIPE integrates different international standards

for pipe design and, thus, the stresses and bend influence are calculated according to

the user chosen code. For the study case ASME B31-8-2003 [Ref.[4]] code was used.

This standard provides stress intensification and flexibility factors to analyse elbows and

its methods are described in appendix B.

When it comes to Abaqus, correct outputs choices must be taken in order to

have comparable results with AutoPIPE. Abaqus has integrated outputs for the von

Mises Stress which is calculated according to analytical formula given below:

σvm =

√1

2[(σ11 − σ22)2 + (σ22 − σ33)2 + (σ33 − σ11)2 + 6(σ2

12 + σ223 + σ2

31) (5.1)

However, results from AutoPIPE are based on standards and in order to compare

them, Abaqus results were reassessed based on ASME standard.

The following three graphics present the von Mises stress, axial stress and hoop

stress for all three simulations.

Figure 5.14: Von Mises stress - Case GP1T1U20-HY.

55

Figure 5.15: Axial stress - Case GP1T1U20-HY.

Figure 5.16: Hoop stress - Case GP1T1U20-HY.

It can be seen that:

• Von Mises:

– AutoPIPE stress profile generally matches the one from Abaqus Pipe sim-

ulation. However, at bend locations Abaqus Pipe elements tend to super

56

estimate stresses, which could be seen as conservative behaviour.

– Abaqus Elbow-Pipe simulation show stresses that have less significant differ-

ence when compared to AutoPIPE. However, considerable discrepancies are

found at the end of the spool which could be better understood with further

spool studies.

• Axial Stress:

– All three curves have similar profiles although offset off 40 MPa can be seen

in some specific zones.

– Those peaks follow the tendency of section moment results in section 5.7.3,

page 52 and were expected to be seen at axial stresses.

• Hoop Stress:

– The two valleys seen in the spool zone (yellow) correspond to the spool bend

which are modelled with a higher thickness than the rest of this element.

Therefore a lower hoop stress was expected.

– All three similations show a hoop stress profile that generally matches each

other.

In conclusion, stress profiles are pretty much compatible between all three simu-

lations, however, Elbow elements seem to be more suitable to bend modelling based on

the better superposition of von Mises stress it has shown.

5.8 Methodology summary

Based on the previous sections a preliminary methodology for the analysis of

spool-riser system using Abaqus is drafted below.

• Geometry:

– Created using FEMAP based on isometric drawings.

– Mesh generated in FEMAP.

57

– Careful element and node numbering shall be done in FEMAP to avoid

Abaqus post-processing difficulties.

– Geometry is then exported from FEMAP as .inp file to be used in Abaqus.

• Abaqus model:

– Sections should be defined either as Thick pipe, Pipe or eventually Elbow.

– Material shall be defined and assigned to sections.

– Riser guides shall be modelled with ITT elements in accordance with its

isometric drawings dimensions and emplacement.

– Soil is defined as rigid surface with axial and lateral frictions.

– Valve is ideally modelled as line loads with increased rigidity.

– Flanges are to be defined as concentrated load with no extra rigidity.

– Buoyancy is modelled as distributed load by the use of Abaqus Aqua module.

– Waves and currents are modelled with Aqua module. Note that waves with

0◦ phase have its bottom at the origin.

– Drag and Inertia are modelled as distributed loads by the use of Aqua module.

• Abaqus step sequence:

– All steps together must lead to a total simulation time equal to a wave period

and initial steps must be shorter that the one destined to waves, because in

Abaqus waves start to propagate from the beginning of the simulation. The

following table provides the recommended step sequence based on the waves

analysed during this study.

• Load case definition - VBA:

– Complete the input sheet for each load case for HY an OP conditions (see

appendix C );

– Click on the blue button and all the .inp files will be automatically generated.

– This pre-processing toll also generates a .bat to run all .inp files one at a

time.

58

Table 5.20: Abaqus step sequence.

Case

condition

Step

number

Total

timeLoads

HY/OP 1 0.01 Self weight, content weight and buoyancy

HY/OP 2 0.01Loads Step 1 + thermal expansion and

internal pressure

OP 3 0.01 Loads Step 2 + change of temperature

HY/OP 3/4 0.01 Loads Step 2/3 + platform displacement

HY/OP 4/512.78/

14.21Loads Step 3/4 + wave and current loading

• Run Abaqus .inp files:

– Use of the .bat generated by VBA macro.

– This file can be schedule to run in specific time and looks like the one bellow.

Figure 5.17: Example of .bat file to run Abaqus simulations in a row.

• Post-processing VBA and Python:

– This code is being developed. Ideally the user will fill a form made in Ex-

cel/VBA or python thinker and would get a file with all the worse cases results

of all required outputs.

59

– An example of Abaqus python scripting that was used in this report can be

seen in appendix D. Post-processing automatic scripts shall be inspired in

this one.

5.9 Software comparison

Based on the different studies performed, the advantages and disadvantages of

Abaqus compared to AutoPIPE are provided.

• Advantages:

– Better mesh and element control;

– Possible to use NLGeom if desired;

– Possible to consider plastic behaviour if desired;

– Possible to model internal pressure/temperature on the internal wall;

– Better control of load cases and load sequence;

– More realistic friction assessment;

– Better assessment of imposed displacement;

– Support modelled via PIP which it more realistic.

• Disadvantages:

– Not possible to directly model lift efforts. To do so a subroutine should be

implemented/programmed;

– Takes more time to run;

– Input file requires careful manipulation because once node quantity is elevated

it can get complex;

– Takes more time for model creation;

– Knowledge of integration point location and quantity is required for right and

quick post-processing;

– When post-processing several different load cases, it is recommended and

automatized tool to make this task easier.

60

5.10 Conclusion

The goal of this second phase was to compare results incoming from Abaqus

and AutoPIPE when considering a Spool-Riser geometry. To do so, although a first

comparison between elements type had already taken place and indicated that elbow

elements were a better choice, this factor was once again studied when modelling the

spool-riser system and two models were compared:

• with only pipe elements

• with pipe elements on the straight parts and the elbow elements on the bent parts

After result post-processing for displacement, reaction force and moments, they

were all validated as sufficiently good matches between both software approaches. How-

ever, section force, section moment and stress results were less compatible between

software. It is believed that is has mostly to do with the soil modelling that is not the

exact same in Abaqus and AutoPIPE. To better evaluate it, new simpler cases like the

ones from chapter 4 should be done focusing on soil behaviour.

Although Pipe simulations had shown a good stress profile, it had sometimes an

offset around 40MPa that was not irrelevant for the study case. On the other hand,

elbow-pipe simulations better compatibility to AutoPIPE simulations. For now it seems

reasonable to affirm that Spools could be modelled using pipe elements for the straight

parts and Elbow elements with high Fourier number for bend zones.

To continue such analysis it should be first verified that other load cases men-

tioned in section 5.5 also lead to the same conclusions as case GP1T1U20-HY.

However, it is recommended a longer comparison between Abaqus and AutoPIPE

with simple cases focusing on soil behaviour, lift analysis, and bend stresses.

61

Chapter 6

Conclusion

The objective of this project was to define the methods to model and analyse a

spool-riser system with Abaqus software and to prove its feasibility. A first step was the

discovery of each of the studied offshore structures, followed up by a phase of simple

cases study under AutoPIPE and Abaqus to calibrate all modelling choices. This first step

led to the assumption that both Pipe and Elbow element families would be sufficiently

good to re-model AutoPIPE simulation.

Once the main modelling choices had been made based on the simple cases,

the geometry was defined with FEMAP software, exported into .inp format and, finally,

manipulated with a VBA macro to generate all load cases. Abaqus cases were ran to

allow a comparison with AutoPIPE and pyhton scripts were written for result extraction.

It was confirmed that both Pipe and Elbow had quite good correspondence with

AutoPIPE simulation. Finally, although the model behaviour is globally the same, the

comparison highlighted significant discrepancies that shall be later investigated, partic-

ularly for the parts in contact with the soil. This can be done by performing additional

tests on simple cases (e.g. Z-shape spool in contact with the soil).

Therefore, it is necessary to perform additional tests on the models prior to use

Abaqus on a complete project. Furthermore, given the relative complexity of the model

definition and elevated computational time it is recommended to use Abaqus only for

spool optimization, unless pre- and post-processing tools are developed and validated in

the future.

62

Bibliography

[1] BAI, Q. B. E. Y., Subsea Pipeline Design, Analysis, and Installation. Gulf Profes-

sional Publishing, 2014.

[2] LYSSAND, T., “Design of Subsea Spools: Investigating the Effect of Spool Shape”,

University of Stavanger/Subsea7 Norway, , 2015.

[3] NOGUEIRA, G., “Avaliacao da fadiga em jumpers rıgidos devido a vibracoes in line

produzidas pelo fenomeno do VIV”, Escola Politecnica, UFRJ, , 2015.

[4] ASME, Gas Transmission and Distribution piping systems, Report ASME B31.8-

2003, The American Society of Mechanical Engineers, 2003.

[5] QUEIROZ, J. O., “Analise de estabilidade de dutos rıgidos submarinos sujeitos a

acao de ondas e correntes marinhas”, Escola Politecnica, UFRJ, , 2011.

[6] SPARKS, C., “Comportement mecanique des tuyaux: influence de la traction, de la

pression et du poids lineique”, Oil & Gas Science and Technology, v. 38, pp. 475–

490, 1983.

[7] BRYAN, B. J., “STATIC ANALYSIS OF A PIPING SYSTEM WITH ELBOWS”,

ASME PVP Conference, pp. 02–03, 1994.

[8] MEHAUTE, B. L., An Introduction to Hydrodynamics & Water Waves. Springer,

1976.

[9] SIMULIA, “Abaqus 6.14 Analysis User’s Guide”, http://ivt-

abaqusdoc.ivt.ntnu.no:2080/v6.14/books/usb/default.htm, 2014, (Acesso em

23 Maio 2020).

[10] UNKNOWN, “Abaqus Tube-to-Tube modeling”, http://www.lhe.no/.

63

[11] BENTLEY, “Bentley Technical Support Group”,

https://communities.bentley.com/products, 2020, (Acesso em 23 Maio 2020).

64

Appendix A

Wave theories limits

Figure A.1: Wave theories limits [Ref. [8]].

65

Appendix B

ASME B31.8 Stress

B.1 Hoop Stress

Hoop stress is calculated as shown in equation below:

Sh =(Pi − Pe).D

2t≤ Sy.F1.T (B.1)

In which:

Pi = Internal design pressure

Pe = External pressure

D = Nominal outside diameter of pipe

F1 = Hoop stress design factor (=0.5 in operation, 0.9 in hydrotest as per ASME B31.8,

[Ref. [4]]

Sy = Specified minimum yield strength (SMYS)

T = Temperature derating factor

t = Pipe wall thickness

B.2 Longitudinal Stress

The Longitudinal stress (SL) is calculated as below:

| SL |≤ Sy.F2.T (B.2)

In which:

66

SL = max(σa + σb;σa − σb)

σb = Resultant bending stress =

√(iiMi)2+ioMo)2

Z

Mi = In-plane bending moment

Mo = Out-of-plane bending moment

ii = In-plane stress intensification factor for bends, see bellow image B.1, shall not be

less than unity

io = Out-of-plane stress intensification factor for bends, see bellow image B.1, shall not

be less than unity

Z = Pipe Section Modulus

σa = Axial stress(positive tensile or negative compressive) = Faxl

A

Faxl = Axial force

A = Pipe section area

F2 = Longitudinal stress design factor (=0.8)

Figure B.1: ASME B31.8 SIF definition [Ref. [4]]

B.3 Combined Stress

To comply with B31.8 requirement, the combined stress formula shall be checked

as follows:

√S2h − SLSh + S2

L − 3S2t ≤ Sy.F3 (B.3)

Sh = Maximum hoop stress

St = Torsion stress

F3 = Combined stress design factor (=0.9)

67

Sy = SMYS (including temperature de-rating as per DNV OS F101)

68

Appendix C

Pre-processing sheet

69

Figure C.1: VBA pre-processing sheet.

70

Appendix D

Python script for post-processing

71

72

73

Figure D.1: Python preliminary script for post-processing.

74

Documents

Analysis of a Spool-Riser System