Welding simulation with Finite Element Analysis

(1)

Department of Technology, Mathematics and Computer Science

DEGREE PROJECT

2004:M028

Johan Elofsson Per Martinsson

Welding Simulation with

Finite Element Analysis

(2)

DEGREE PROJECT

i

Welding Simulation with Finite Element Analysis

Summary

The aim of this work is to develop a manual for simulation of a welding process with the FEA-program ABAQUS. This project has been generated from Aker Kvaerner AB in Gothenburg.

Their manufacturing of power boilers and evaporators requires high quality welding. To simplify the development of new welding routines with new materials, the company would like to create a routine for simulation in ABAQUS. This project is one step in their development of the simulation routine.

To be able to analyze the micro structure of the material during the welding process, the subroutine TRAST will be used with ABAQUS.

This is a simulation of a butt welded plate with filler material. The model is created in the interactive part of ABAQUS/CAE. When the modelling is finished an input data file is created. In this file command strings will be added or changed for calling user defined subroutines. For this purpose several files will be used by ABAQUS and TRAST.

The results of this simulation will be written into two different files, one file is a text file containing the phase transformation data and one file will be used for the plotting of nodal temperature and displacement.

Publisher: University of Trollhättan/Uddevalla, Department of Technology, Mathematics and Computer Science, Box 957, S-461 29 Trollhättan, SWEDEN

Phone: + 46 520 47 50 00 Fax: + 46 520 47 50 99 Web: www.htu.se Examiner: Niklas Järvstråt

Advisor: Per Lindström, Kvaerner Power AB

Subject: Mechanical Engineering Language: English

Level: Advanced Credits: 10 Swedish, 15 ECTS credits Number: 2004:M028 Date: June, 2004

Keywords ABAQUS, Welding, Simulation, TRAST, Phase transformation, Residual stresses

(3)

Welding Simulation with Finite Element Analysis

Preface

We would like to thank our supervisor Niklas Järvstråt at the University of

Trollhättan/Uddevalla for all the support and time during this degree work. We also want to thank Per Lindström at Kvaerner Power AB for the possibility to work on this project.

Johan Elofsson and Per Martinsson

Trollhättan, 2004

(4)

iii

Contents

Summary...i

Preface ... ii

List of symbols ...v

1 Introduction...1

1.1 Background...1

1.2 Aim ...1

1.3 Limitations ...2

2 FEA...2

2.1 General Knowledge ...2

2.2 General modelling in FEA...2

2.2.1 Creating the model... 2

2.2.2 Meshing the model... 3

2.2.3 Loads and boundary conditions... 3

2.2.4 Results ... 3

3 Technical equipment...4

3.1 Used hardware...4

3.2 Used Software ...4

4 Material properties ...4

5 Conclusions...5

5.1 Reflections...5

5.2 Recommendations for further work ...5

6 References...6

7 Overview of the simulation...1

7.1 General work description ...1

7.2 General flowchart for ex1...2

7.3 Detailed flowchart for ex1 ...3

8 Start instructions ...4

8.1 How to read the manual ...4

8.2 Installation of software ...4

8.3 Start the program...5

8.3.1 Start ABAQUS CAE ... 5

8.3.2 Create Model Database... 5

8.3.3 ABAQUS 6.4 work area ... 5

8.3.4 Generate model database ... 6

9 Modelling...6

9.1 Create the model...6

9.1.1 Create part for ex1 ... 6

9.1.2 Split the model in partitions... 8

9.2 Assign the material properties...9

9.2.1 Material properties ...10

9.2.2 Create and assign section...12

9.2.3 Absolute zero temperature ...12

9.2.4 Create the .tdt-file ...12

9.3 Create the assembly ...13

(5)

9.4 Create Boundary Conditions ...14

9.4.1 Displacement/rotation... 14

9.4.2 Symmetry ...15

9.5 Create Mesh...16

9.5.1 Create Sets...18

9.6 Define initial conditions ...18

9.6.1 Temperature ...18

9.6.2 Create the .inp-file ...19

9.6.3 Add subroutine calls and initial conditions on internal variables (SDV’s) in the .inp-file ...19

9.7 Load history definition...21

10 Solve the problem ...23

11 Post processing ...23

11.1 SDV results ...23

11.2 Plot the results ...24

11.2.1Plot the stress result ...24

11.2.2Animate the stress result ...25

11.2.3Plot the temperature result ...26

12 Discussion...27

12.1 Generated files...27

12.2 Results...27

12.3 Approximations...27

13 References...28

Appendices

A Appendix: Manual for ABAQUS 6.4-2 with subroutine TRAST7

(6)

v

List of symbols

FEA = Finite Element Analysis MAG = Metal Active Gas CAD = Computer Aided Design PC = Personal Computer SDV = Solution Dependent Variables

* = Command

** = Comment

NT = Nodal Temperature

U = Displacement

S = Stresses

E = Total strain

(7)

1 Introduction

This project is the final assignment on our education for a Bachelor of Science degree in Mechanical Engineering at the university of Trollhättan/Uddevalla (HTU).

The project took place at HTU during 10 weeks in the spring of 2004.

The main content of this report is a manual for thermal-metallurgical welding simulation in the FEA-program ABAQUS with the subroutine TRAST.

1.1 Background

Kvaerner Power AB designs and manufactures chemical recovery and power generation system for the global pulp and paper industry e.g. power boilers, evaporators.

The company delivers power boilers worldwide, from small units to giant tailor-made boilers. The technology of manufacturing these boilers is based on more than 100 years of experience. To satisfy their client’s high demands, the company has an intense focus on research and development [1].

The welding department of the company constantly develops new and improved welding routines. To improve this process the welding engineer at the welding department wants to have the possibility to simulate new welding routines with a FEA- program. The results from the FEA-program will reduce the time and simplify the development.

The company will with a number of degree projects develop a routine for this simulation. One project has already been done. That project was a master thesis that concluded that the company should use the FEA-program ABAQUS [2].

1.2 Aim

The aim of this project is to develop a manual for simulation of a welding process. The software that has been used is ABAQUS with the subroutine TRAST. This simulation with TRAST makes it possible to calculate the residual stresses and phase transformations in the material.

(8)

2

1.3 Limitations

The manual should contain a simulation of a “simple” butt-welded plate. The welding process should be a single-pass MAG with filler material that fuses two plates. The energy from the welding process may be given as an initial temperature in the filler material. Proper boundary conditions are not the main purpose of this project. Several simplifications will be used.

2 FEA

2.1 General Knowledge

FEA is the most dominant method for calculation and simulations of computer made models. The name FEA comes from the way a complicated model is divided into a model that is built up by small elements. FEA can be used in some different types of simulations e g structural, thermal, fluid mechanics and electromagnetic analysis [3].

The development of FEA-programs follows the development of computers. The first FEA calculations were made without computer help. There were “simple” analyses of beam structures. The aerospace industries were the first companies to use FEA in their development of new products. Then the car industries and middle size companies have followed. Now when the PC’s are getting higher performance and the usability of the FEA-programs are improved, even small companies can use the technology.

2.2 General modelling in FEA

2.2.1 Creating the model

The first step is to create or import a model. There are possibilities to create the model in the FEA–programs, but most of the FEA-programs are not suitable for modelling.

The most common way is to import the model from a CAD-program. It is important to make the model as simple as possible. Feasible simplifications are to eliminate small details, to use symmetry in the model or make the model in 2D instead of 3D.

(9)

2.2.2 Meshing the model

Next step is to mesh the model. The volume or the shell is divided into small elements.

The number of elements and the type of the elements affects the calculation time.

Therefore it is important not to divide the model into too many elements. Too few elements will affect the calculations negatively and the results will deviate too much from reality.

One way to make a small model that gives good results is to create big elements in areas with lower loads and small elements in areas with higher loads.

When meshing the model it is important to avoid badly shaped elements in order to avoid great miscalculations of the stresses.

2.2.3 Loads and boundary conditions

Next step is to apply loads and boundary conditions. There are many different kinds of loads e g temperature, surface-, point- , line-loads etc. To get results with small deviation from the reality, it is crucial which way the loads and boundary conditions are applied. If the loads or boundary conditions are incorrect or applied inappropriately on the model, it will not move realistically and the results will be misleading. Point loads/boundary conditions or radius equal to zero can give singularities that don’t exist in reality.

2.2.4 Results

The results are visualized with contour plots and can be analyzed. It is important to be aware of that all calculations are approximations and there can be many inaccuracies in the FEA program. The results from FEA are not 100% correct.

(10)

4

3 Technical equipment

The ABAQUS system requirements should be checked at ABAQUS homepage. This may be necessary due to introduction of new ABAQUS versions [4]

3.1 Used hardware

Processor (CPU) speed: 2.8 GHz RAM (Random Access Memory): 512 MB

Monitor: 21”

HDD (Hard Disk Drive): 40 GB

3.2 Used Software

Operating system: Windows XP FEA-program: ABAQUS 6.4-2

Compiler: Compaq Visual Fortran 6.0 and Microsoft Visual C/C++ 6.0 Subroutine: HETVAL subroutine for latent heat and phase transformation,

taken from TRAST7 and adapted for ABAQUS 6.4-2

4 Material properties

The result will be more accurate if the material data is temperature-dependent [5-12]. To be able to get correct results it’s important to use consequent units for all variables. For example decide if (m, N, Pa) will be used.

The material data used in this simulation are:

Young’s modulus Poisson’s ratio Density Specific heat Conductivity Enthalpy

Thermal expansion Data from IT-diagram

(11)

5 Conclusions

5.1 Reflections

The interactive part of ABAQUS has limitations. ABAQUS is developed for users that are familiar in the handling of different files and their contents. These files contain data such as material and different commands that control subroutines etc. The interactive part of ABAQUS is mostly used for the modelling work. For example creating different models and give them their boundaries etc. It is also used for plotting the results.

ABAQUS documentation is very big and confusing. The permanent opportunity of linking to related material makes it very hard to get a good overview of the information.

The documentation has too few examples that really show how to solve a problem.

Often it is only inform that is possible to use different commands, but it’s not giving the step for step information how to use the command in the in-data files.

5.2 Recommendations for further work

To be able to get good results from the simulation, the appropriate material data for a specific material must be collected. In this project material data from different materials has been used in the simulation. Proper material data for a specific material is hard to get. The high temperature and the need of data for each phase require unusual material data.

If all material data is correct and a more complex model is created, the results between the simulation and an experiment could be compared.

Create a simulation with the subroutine UMAT that calculates the residual stresses [13].

In this simulation the heat source was simplified with an initial temperature in the filler material. An improved heat source model includes even body flux and surface flux. The amount of total power input is approximately divided into filler 38%, body flux 21%

and surface flux 41% [10].

One possible way to get better results from the simulation is to make the moving heat source model as a semi-ovaloid [11].

To be able to get more correct results the initial temperature in the filler material should be homogeneous. In this simulation it is not. This problem occurs when the plate and the filler share a number of nodes. The initial temperature of both the filler material and the plate is given to these shared nodes. One possible way to solve this problem is to model the plate and the filler as different parts with coupled nodes.

Plot the results for SDV (Solution dependent variables) as a contour plot.

(12)

6

6 References

1. Kvaerner Power AB, homepage, http://www.akerkvaerner.com

2. Maneli Faraji, “FE simulation of residual stresses with a software selected for an industrial application”, Master thesis, Chalmers University of Technology 2004.

3. Kjell Niklasson, ”Allmänt om FEM”, University of HTU 2000.

4. Abaqus system requirements,

http://www.abaqus.com/support/v64/v64_sysRqmts.html#win32

5. P. Michaleris and A. DeBiccari, “Prediction of Welding Distortion”, Welding Journal Research Supplement, 1997, pp.172-181

6. P. Michaleris, J. Dantzig and D. Tortrelli, “Minimizing of Welding Residual Stress and Distortion in Large Structures”, Welding Journal Research Supplement, Nov. 1999, pp.361-366

7. B. A. B Andersson, “Thermal Stresses in a Submerged-Arc Welded Joint Considering Phase Transformations”, Transactions of the ASME. Journal of Engineering Materials and Technology, Vol.100 Issue.4, 1978, pp.356-362 8. C. T. Karlsson, “Finite Element Analysis of Temperature and Stresses in a

Single-Pass Butt-Welded Pipe – Influence of Mesh Density and Material Modelling”, Engineering Computations, Swansea, Wales, 1989, Vol.6, pp133- 141

9. B. Taljat, T. Zacharia, X.-L. Wang, J. R. Keiser, R. W. Swindeman, Z. Feng and M. J. Jirinec, ”Numerical Analysis of Residual Stress Distribution in Tubes with Spiral Weld Cladding”, Welding Journal Research Supplement, Aug. 1998, pp.328-335

10. Jan Langkjær Hansen, “Numerical Modelling of Welding Induced Stresses”, Ph.D. thesis, Technical University of Denmark 2003.

11. Dieter Radaj, “Heat effects of welding”, Springer-Verlag, Berlin Heidelberg, 1992.

12. G. F. Vander Voort, “Atlas of Time-Temperature Diagrams for Irons and Steel”, USA 1991.

13. Niklas Järvstråt, ”Two-Dimensional Calculation of Quench Stresses in Steel”, LIU-TEK-LIC-1990:45, Institute of Technology, Linköping 1990, pp I:10.

14. N. Järvstråt, S. Sjösröm, “TRAST7 USER’S MANUAL”, 1995

(13)

A Appendix: Manual for ABAQUS 6.4-2 with subroutine TRAST7

(14)

Department of Technology, Mathematics and Computer Science

DEGREE PROJECT

2004:M028

Manual for ABAQUS 6.4-2 with

HETVAL Subroutine from

TRAST7

(15)

Contents

7 Overview of the simulation...1

7.1 General work description ...1

7.2 General flowchart for ex1...2

7.3 Detailed flowchart for ex1 ...3

8 Start instructions ...4

8.1 How to read the manual ...4

8.2 Installation of software ...4

8.3 Start the program...5

8.3.1 Start ABAQUS CAE ... 5

8.3.2 Create Model Database... 5

8.3.3 ABAQUS 6.4 work area ... 5

8.3.4 Generate model database ... 6

9 Modelling...6

9.1 Create the model...6

9.1.1 Create part for ex1 ... 6

9.1.2 Split the model in partitions... 8

9.2 Assign the material properties...9

9.2.1 Material properties ...10

9.2.2 Create and assign section...12

9.2.3 Absolute zero temperature ...12

9.2.4 Create the .tdt-file ...12

9.3 Create the assembly ...13

9.4 Create Boundary Conditions ...14

9.4.1 Displacement/rotation... 14

9.4.2 Symmetry ...15

9.5 Create Mesh...16

9.5.1 Create Sets...18

9.6 Define initial conditions ...18

9.6.1 Temperature ...18

9.6.2 Create the .inp-file ...19

9.6.3 Add subroutine calls and initial conditions on internal variables (SDV’s) in the .inp-file ...19

9.7 Load history definition...21

10 Solve the problem ...23

11 Post processing ...23

11.1 SDV results ...23

11.2 Plot the results ...24

11.2.1Plot the stress result ...24

11.2.2Animate the stress result ...25

11.2.3Plot the temperature result ...26

12 Discussion...27

12.1 Generated files...27

12.2 Results...27

12.3 Approximations...27

13 References...28

(16)

ii Appendices

B Appendix .inp-file C Appendix .inc-file D Appendix .tdt-file E Appendix .dat-file

(17)

7 Overview of the simulation

7.1 General work description

Create input data Assign material

data

Create mesh

Solve the problem

Plot the results Assign boundary

conditions

• Define initial conditions

• Call the subroutine HETVAL

• Create .inc-file

Create the model

• Create .tdt-file

(18)

2

7.2 General flowchart for ex1

ABAQUS/CAE (modelling)

ex1.inp ex1.inc vtt.tdt

ABAQUS (solver) Trast7_tv

ex1.odb ex1.dat

ABAQUS/CAE (post processing)

(19)

7.3 Detailed flowchart for ex1

ex1.inp

• Edit inp-file 4.1

• Make ABAQUS call the subroutine HETVAL from TRAST.

• Give the initial conditions to the different phases in HETVAL

ex1.inc

• Create inc-file 4.2

• Give the step data for the simulation ex1.

• Request the result of SDV from HETVAL in TRAST

vtt.tdt

• Create tdt-file 4.3

• Give the material data that HETVAL requires for calculation of the phase transformations.

ABAQUS (solver)

• Solve the problem in ABAQUS command window 4.5

• Compile and link the subroutines in Trast7_tv.

Trast7_tv

• Contains the subroutine HETVAL, that calculate the phase transformation.

ex1.odb

• Contain the results readable for

ABAQUS/CAE 5.2

ex1.dat

• Contain the results from the different phase transformations 5.1

ABAQUS/CAE (post processing)

• Plotting the results for temperature, stresses and displacement 5.2

ABAQUS/CAE (modelling)

• Create model 3.1

• Assign the material properties 3.2

• Create assembly 3.3

• Create boundary conditions 3.4

• Create Mesh 3.5

• Create Sets and Fields 3.7-3.8

• Create .inp-file 3.9

(20)

4

8 Start instructions

8.1 How to read the manual

This description shows generally how to follow the manual.

When the text is written in Bold text after > or between | | , it means that the user should “click” on this icon.

When the text is Italic, it is a describing sentence for the particular step.

Plain text describes were to look for next command or gives the instructions what to do.

It can also give the instruction what to write after : (for example a number or a string).

8.2 Installation of software

Install ABAQUS 6.4-2 and Compaq Visual Fortran compiler.

Before the simulation can start, the TRAST subroutines must be compiled and linked with ABAQUS.

Copy the subroutine trast7_tv.f to C:\Temp and change the name to trast7_tv.for, so that it is recognised as a Fortran source code file.

START > My Computer > C: > Temp Open trast7_tv.for

Check that the user subroutine interface is the same as the call for subroutine HETVAL in ABAQUS. [3]

For this simulation in ABAQUS 6.4-2 the interface of the only used subroutine HETVAL is:

SUBROUTINE HETVAL

(CMNAME,TEMP,TIME,DTIME,SVAR,FLUX,PREDEF,DPRED) Check that the dimensions are correct:

DIMENSION TEMP(2), SVAR(9), PREDEF(*),TIME(2), FLUX(2), DPRED(*)

This simulation is compiled and linked every time a new job is created. (4.5)

(21)

8.3 Start the program

8.3.1 Start ABAQUS CAE

START > Program > ABAQUS 6.4-2 > ABAQUS CAE

8.3.2 Create Model Database

When ABAQUS/CAE program has started the first question is if a new model should be created or an old model should be opened.

The “Start Session” window pops up. | Create Model Database |

8.3.3 ABAQUS 6.4 work area

These are the names and titles of areas that will be used in this manual.

(Figure 1)

Figure 1

(22)

6 8.3.4 Generate model database

To make it possible to reopen and modify the model it is important to save the model in a model database.

Give the model database a “name” where the model information can be saved.

Menu bar > File > Save As > “ex1” | OK |

9 Modelling

9.1 Create the model

9.1.1 Create part for ex1

The first step in this simulation is to create and give the model the right geometrical dimensions. It is also possible to import an already existing model from a CAD program.

Context bar > Module > Part (Figure 2)

Figure 2

Toolbox area > Create Part

The “Create Part” window pops up: Pick name: Part-1

(23)

Modeling Space: 3D

Type: Deformable

Base Feature: Solid, Extrusion

Approximate size: 0.2

| continue |

Toolbox area > Create Lines: Rectangle > Prompt area > Give the coordinates for the first corner: 0, 0 | Enter |

Prompt area > Give the coordinates for the second corner: 0.1, 0.01 | Enter |

Deactivate: Create Lines: Rectangle > Prompt area > | Done | The “Edit Base Extrusion” window pops up. Give the depth of the model: 0.05 | OK | (Figure 3)

Figure 3

(24)

8 9.1.2 Split the model in partitions

The welding simulation requires the possibility to remove and add elements. To simplify the simulation groups of elements are removed and added to the model. These groups of elements (sets) must be named. To be able to create these sets the model is divided into partitions.

This is one way to simulate a welding process with a filler material.

First step is to divide the model into two parts, filler material and the plate.

Toolbox area > Create Datum Points > Prompt area > Give the coordinates for the first point: 0, 0, 0.045 | Enter |

Repeat previous step for datum point 2: (0, 0.01, 0.045) | Enter | Repeat previous step for datum point 3: (0.1, 0, 0.045) | Enter | Toolbox area > Partition Cell > Prompt area > 3 Points

Second step is to divide the filler material into eight partitions.

Toolbox area > Create Cell > Pick the part of the model that should be partitioned Prompt area > | Done |

Prompt area > | 3 Points |

> Pick the 3 points in the middle of the filler material

> Prompt area > | Create Partition |

> Repeat the last step until all partitions are created

> | Done | (Figure 4)

(25)

Figure 4

9.2 Assign the material properties

In this step the material properties is given to the model. The name of the material is also given. If the HETVAL subroutine from TRAST is used, as it is in this simulation, the material name must be identical with the name of the .tdt-file. The creation of the .tdt- file is described in 4.3.

The material data in this simulation is taken from a number of sources. This data is not from a specific material. The data for density, specific heat, conductivity and the enthalpy are taken from the TRAST manual [4]. The thermal expansion is taken from a welding journal [5]. Young’s modulus and Poisson’s ratio are taken from an ordinary table for structure material [6].

The material data in the .tdt-file are taken from the TRAST manual [4]. This material data is collected from an IT-diagram. Pick a number of points for each phase and read the result from the diagram. For points when the time variable is short, it is very important that the reading is accurate.

In this simulation the material data are:

Young’s modulus Poisson’s Ratio

(26)

10 Conductivity

Specific Heat Thermal expansion Enthalpy

IT-diagram

9.2.1 Material properties Context bar > Module > Property

Toolbox area > Create Material > The ”Edit Material” window pops up.

Type the material name: VTT General > Density > 7.81E3

Mechanical > Elasticity > Elastic > Young’s Modulus: 210E9

Poisson’s Ratio: 0.3

9 variables are assigned by HETVAL. [4]

General > Depvar > Number of solution dependent state variables: 9

To be able to use temperature-dependent data select “Use temperature-dependent data”.

To make more rows, place the “cursor” in the window and right click.

Select “Insert Row After”. (Figure 5)

Mechanical > Expansion > Expansion Coefficient alpha: Exp. Temp.

0.0 0

12E-6 125

13E-6 250

14E-6 500

15E-6 750

16E-6 900

18E-6 1200

(27)

Thermal > Conductivity > Conductivity: Cond. Temp.

43.5 0

42.5 200

37.7 400

33.1 600

29.0 800

30.0 1000

Thermal > Specific Heat > Specific Heat: Spec. Temp.

473.8 0

502.0 100

551.9 300

650.5 500

851.5 700

563.4 900

| OK | (Figure 5)

Figure 5

(28)

12 9.2.2 Create and assign section

In this step the material property is assigned to the specific area of the model.

Toolbox area > Create Section > The “Create Section” window pops up.

Name: Section 1 Category: Solid

Type: Homogeneous | continue | The “Edit Section” window pops up Pick material: VTT | OK |

Toolbox area > Assign Section > Select the whole model with a “window”

Prompt area > | Done |

The ”Assign Section” window pops up | OK | Done |

9.2.3 Absolute zero temperature

The model is given the absolute zero temperature for the Celsius scale.

Menu bar > Model > Edit Attributes > Model-1 The “Edit Model Attributes” window pops up Write: -273.15 (for Celsius) | OK |

9.2.4 Create the .tdt-file

The .tdt-file is a user defined input file. It contains the IT-diagram for the material. The data from the IT-diagram is required in HETVAL for the calculation of phase transformations.

START > Program > accessories > wordpad

Open an old .tdt-file or create a new. In this simulation an old .tdt-file has been used (see Appendix C).

The .tdt-file contains (see [4] for a detailed format description):

IPH = The material phase condition.

CEUT = Eutectic carbon content.

(29)

The start (VL) and finish (VR) of the curves in IT-diagram gives the volume fraction of phase constituent for each phase (IPH). These values (VL and VR) indicate how much of the austenite that has been transformed into another phase. These results are shown as curves in the IT-diagram. It is usually 1% and 99%.

CC = Carbon content in the material.

TEF = Finish temperature for each phase transformation (Celsius degrees). This variable is read from the IT-diagram

TES = Start temperature for each phase transformation (Celsius degrees). This variable is read from the IT-diagram

VEQ = Equilibrium volume fraction for each phase.

LOG(TIL) = This variable is the start time as a function of temperature TEL for each phase. This variable is picked from the IT-diagram. The vertical axis is the temperature (Celsius degrees). Select one temperature and follow that line out to the curve. Then read the time in seconds on the horizontal axis. In this simulation eleven points are used to show the different values on the curve. It is also important that the points are picked so they give a good reflection of the curve.

LOG(TIR) = This variable is the finish time as a function of temperature TER for each phase. As above the finish time is read at the horizontal axis. When a temperature is selected, read first the start time and then the finish time for the same temperature. The use of a logarithmic time scale gives benefits when both a very short time and a extremely long time intervals are considered.

HS = The enthalpy released by transformation for each phase.

Appendix C

9.3 Create the assembly

If the model contains several parts, it is possible to create one model assembly of these parts. For this model there is only one part so that is the part to be added to the assembly.

Context bar > Module > Assembly

Toolbox area > Instance part > The “Create Instance” window pops up.

Pick: Part 1-1 | OK |

(30)

14

9.4 Create Boundary Conditions

To get accurate results from the simulation, it is important that the model have correct boundary conditions. This simulation of two plates welded together is simplified by using symmetry. The model has a symmetry boundary in the symmetry plane. To prevent the model to translate along the X- and Y-axis boundary conditions are given to selected areas.

9.4.1 Displacement/rotation

Create the boundaries for the backside that will prevent the model to translate out of the XY-plane

Context bar > Module > Load

Toolbox area > Create Boundary Condition > The “Create Boundary Condition”

window pops up.

Pick: Mechanical, Displacement/Rotation | continue |

Prompt area > Show/Hide Selection Option > The “Options” window pops up.

(Figure 6)

Activate: Select the Entity closest to the Screen

Place the marker over the hidden back > The top area is selected To be able to select the back > Prompt area > | Next | OK | Done | The “Edit Boundary Condition” window pops up.

Select: U3 and UR3 | OK |

Create the boundary conditions that will prevent the model to translate along X-axis Select a point in the XY-plane. Repeat the previous instructions

Select: U1 | OK |

(31)

Create the boundary conditions that will prevent the model to translate along Y-axis and rotate around Z-axis. Pick the upper line on the back of the model. Repeat the previous instructions

Select: U2 | OK |

9.4.2 Symmetry

Create the boundary conditions for the symmetry-plane

Toolbox area > Create Boundary Condition > The “Create Boundary Condition”

window pops up.

Pick: Mechanical, Symmetry/Antisymmetry/Encastre | continue |

Prompt area > Show/Hide Selection Option > The “Options” window pops up.

Activate: Select the Entity closest to the Screen Pick one symmetry-area | Done |

The “Edit Boundary Condition” window pops up.

Select: ZSYMM | OK |

Repeat for all symmetry-areas (Figure 7)

(32)

16 Figure 7

9.5 Create Mesh

In this simulation the size of the elements are chosen for fast calculations and not for accuracy. The mesh in this model has equal size through the whole model.

Context bar > Module > Mesh

Toolbox area > Seed Part Instance > Assign the element size Prompt area > 0.005 | Enter | Enter |

Toolbox area > Assign mesh controls > The “Options” window pops up.

Select the whole model with a “window”.

Prompt area > | Done | The ”Mesh Controls” window pops up.

Pick: Hex, Structured | OK | Prompt area > | Done |

(33)

Toolbox area > Assign element type > The “Options” window pops up.

Select the whole model with a “window”.

Prompt area > | Done | The ”element type” window pops up.

Select: Element Library: Standard

Geometric Order: Linear

Family: Completed Temperature-Displacement

| OK | Prompt area > | Done |

Toolbox area > Mesh part instance > Prompt area > | Yes | (Figure 8)

Figure 8

(34)

18 9.5.1 Create Sets

In this simulation groups of elements that simulate the filler material are given names.

These groups are called “sets”.

Menu bar > Tools > Set > Manager > The “Set Manager” window pops up

| Create | The “Create Set” window pops up

Write name: element1 | Continue | The “Options” window pops up Activate “Select the Entity Closest to the Screen”

Pick a surface on the first partition > Prompt area > | Next | (to select the whole volume of the partition)

Prompt area | OK | Done |

Repeat seven times to create the eight sets with names:

ELEMENT1, …., ELEMENT8.

| Dismiss |

9.6 Define initial conditions

9.6.1 Temperature

To give the Plate and the Filler a correct initial temperature, they must be assigned to a field.

Context bar > Module > Load

Menu bar > Field > Manager > The “Field Manager” window pops up

| Create | The “Create Field” window pops up Category: Other, Temperature | Continue |

Select the whole volume of the plate with a “window” | Done | Magnitude: 20 | OK |

| Create | The “Create Field” window pops up Category: Other, Temperature | Continue |

Select the whole volume of the filler material with a “window” | Done |

(35)

Magnitude: 2000 | OK |

| Dismiss | (Some initial conditions are also defined in 3.6.3)

9.6.2 Create the .inp-file

This step will create the .inp-file containing the data input from all previous steps (3.1- 3.6).

Context bar > Module > Job

Toolbox area > Create Job > The “Create Job” window pops up Pick name: exempel1 | Continue |

The “Edit Job” window pops up | OK |

Toolbox area > Job Manager > The ”Job Manager” window pops up (Figure 9)

| Write Input | Dismiss |

Figure 9

9.6.3 Add subroutine calls and initial conditions on internal variables (SDV’s) in the .inp-file

START > My Computer > C: > Temp Open the file: ex1.inp (with e.g. notepad) Add the string: *HEAT GENERATION

This command string will make ABAQUS call the subroutine HETVAL [2]. (The subroutine must be linked with ABAQUS, see 2.2)

(36)

20

**

** MATERIALS

**

*Material, name=VTT

*HEAT GENERATION

**

To assign initial conditions, a set that contain the whole model must be used. The set that has been “picked” is called “_PickedSet13”. This set is created by the program when the material data is assigned to the model. The name of this set is found in the .inp-file. This is an example from the .inp-file (Appendix B)

** Section: Section-1

*Solid Section, elset=_PickedSet13, material=VTT 1.,

*End Instance

The initial condition for each variable must be assigned if the subroutine HETVAL is used. Add these strings to the .inp-fil, and use the set “_PickedSet13” to give the material its initial condition for the solution dependent variables in HETVAL. These variables are the different phases and the temperature in the simulation. Variable 1-6 are the phase fractions and variable 7 is the temperature [4]. The sum of variables 1-6 must be equal to 1.

These strings should be reordered after the material data.

**

*RESTART, WRITE, FREQUENCY=20

*INITIAL CONDITIONS, TYPE=FIELD, VARIABLE=1 _PickedSet13, 1.0

**

(37)

Add this string last of all to include the separate .inc-file that contains the step data:

*include,input=ex1.inc

File > Save Appendix A

9.7 Load history definition

The .inc-file contains all the step data. This file is written in “Notepad”. It is also possibly to reuse old .inc-files. In this simulation some parts of the .inc-file has been copied from an old simulation. It is also possible to copy the step information from the .inp file generated in a fully interactive execution.

START > Program > Accessories > Notepad

In the inc-file the information for each step is created, these steps will be included in the calculation of the results.

An alternative to write a new inc-file is to open an old one, edit and save it with a new name.

File > Save as

Save in directory C:\Temp File name: ex1.inc | Save |

This is a part of the ex1.inc-file. In step1 the elements 2-8 are removed, In step 2-8 the elements are added one by one.

In this simulation only the ELEMENT2’s phase results will be viewed. One way to view these results is to write them into the .dat-file.

The command block *EL PRINT write the SDV (Solution Dependent Variables) results for ELEMENT2 to the .dat-file [3].

** STEP: Step-1

**

*Step, name=Step-1

*Coupled Temperature-Displacement, creep=none 1., 10.,

(38)

22

**

*MODEL CHANGE, REMOVE

ELEMENT2, ELEMENT3, ELEMENT4, ELEMENT5, ELEMENT6, ELEMENT7, ELEMENT8

**

*NODE FILE,FREQUENCY=1,GLOBAL=YES U,NT

**

*EL FILE,FREQUENCY=1,POSITION=NODES,DIRECTIONS=YES S,E

*EL PRINT, ELSET=ELEMENT2, FREQUENCY=1 SDV

**

*End Step

** ---

**

** STEP: Step-2

**

*Step, name=Step-2

*Coupled Temperature-Displacement, creep=none 1., 10.,

**

*MODEL CHANGE, ADD ELEMENT2,

**

*NODE FILE,FREQUENCY=1,GLOBAL=YES U,NT

**

*EL FILE,FREQUENCY=1,POSITION=NODES,DIRECTIONS=YES S,E

**

*EL PRINT, ELSET=ELEMENT2, FREQUENCY=1 SDV

*End Step

** --- Appendix B

(39)

10 Solve the problem

The execution solves the problem with subroutines from trast7_tv.for and creates a number of files ( 7.1). One is the .odb-file. This file makes it possible to plot the results in ABAQUS/CAE.

START > Program > ABAQUS 6.4 > ABAQUS Command

Write the command in the ABAQUS Command window: C:\Temp>

Write: abaqus user=trast7_tv job=ex1.inp | Enter | (Figure 10) The .odb-file will be created in the directory C:\Temp

Figure 10

11 Post processing

11.1 SDV results

The SDV results are written to the .dat-flie. In this simulation the results of ELEMENT2 are written for every increment in each step.

Open ex1.dat with notepad. The SDV results “1-9” for ELEMENT2 are listed for each step in the file.

Appendix D

(40)

24

11.2 Plot the results

The data from the post-processing that have been written in the .odb-file will be opened in ABAQUS/CAE and plotted as a contour plot.

11.2.1 Plot the stress result Open ABAQUS/CAE

Menu bar > File > Open > The ”Open Database” window pops up Change File Filter: Output Database(*.odb)

Select: ex1.odb | OK | (Figure 11)

(41)

11.2.2 Animate the stress result

Toolbox area > Plot Contours > Toolbox area > Animate: Time History

Figure 11

(42)

26 11.2.3 Plot the temperature result

Menu bar > Result > Field Output > The “Field Output” window pops up Select: NT11 (to plot temperature) | OK | (Figure 12)

Figure 12

(43)

12 Discussion

12.1 Generated files

.inp-file: In data file. This file contains the models geometrical data, sets, material data, boundaries, commandos for subroutine calls and a “link” to the step data file.

.inc-file: This file contains the step data for the calculation. The file also contains the commands for the output results.

.log-file: In this file it is possible to check the status of the calculation that is in progress.

.sta-file: This file shows what has been done during the calculation.

.dat-file: In this file it is possible to check for errors and warnings when the simulation stops due to fails. The file also contains results when the command *EL PRINT is used.

.msg-file: If there are serious errors and warnings, the .dat-file will direct to the .msg- file. The .msg-file will tell the reason for the errors in the simulation.

.odb-file: This file is the result-file. In ABAQUS/CAE it is possible to open this file and plot the results with contour plot.

12.2 Results

The manual contain a detailed step by step instruction for a welding simulation in ABAQUS 6.4. with the HETVAL subroutine from TRAST. It is addressed to first time users in ABAQUS. For the manual to be useful, the user should have some FEA experience. Further work on this project also requires some programming knowledge.

12.3 Approximations

When the filler material is simulated, sets with elements are created. These sets are named. In the first step the elements are removed. Then they are added one by one in each step. This makes it possible to create a moving heat source with filler material.

To reduce time in the simulations, it is a good idea to have a separate step file. The .inc- file can be saved and reused. This will reduce the need of making step data for every simulation.

(44)

28

13 References

15. ABAQUS support, http://www.abaqus.com

16. Niklas Järvstråt, ”Two-Dimensional Calculation of Quench Stresses in Steel”, LIU-TEK-LIC-1990:45, Institute of Technology, Linköping 1990, pp I:4.

17. ABAQUS documentation

18. N. Järvstråt, S. Sjösröm, “TRAST7 USER’S MANUAL”, 1995

19. B. Taljat, T. Zacharia, X.-L. Wang, J. R. Keiser, R. W. Swindeman, Z. Feng and M. J. Jirinec, ”Numerical Analysis of Residual Stress Distribution in Tubes with Spiral Weld Cladding”, Welding Journal Research Supplement, Aug. 1998, pp.328-335

20. B. Bodelind, A. Persson, ”Hållfasthets- och materialtabeller”, Akademiförlaget i Göteborg AB, 1999

(45)

B Appendix .inp-file

*Heading

** Job name: ex1 Model name: Model-1

*Preprint, echo=NO, model=NO, history=NO, contact=NO

**

** PARTS

**

*Part, name=Part-1

*End Part

**

** ASSEMBLY

**

*Assembly, name=Assembly

**

*Instance, name=Part-1-1, part=Part-1

*Node

1, 0.0875, 0.01, 0.045 2, 0.0875, 0.01, 0.05 3, 0.1, 0.01, 0.05 4, 0.1, 0.01, 0.045 5, 0.0875, 0., 0.05 6, 0.1, 0., 0.05 7, 0.1, 0., 0.045

. .

455, 0.00625, 0.005, 0.03214286 456, 0.00625, 0.005, 0.02571429 457, 0.00625, 0.005, 0.01928571 458, 0.00625, 0.005, 0.01285714 459, 0.00625, 0.005, 0.006428571

*Element, type=C3D8T

1, 46, 48, 148, 147, 1, 2, 41, 42 2, 147, 148, 47, 45, 42, 41, 3, 4 3, 8, 5, 43, 44, 46, 48, 148, 147 4, 44, 43, 6, 7, 147, 148, 47, 45 5, 54, 56, 150, 149, 9, 10, 49, 50 6, 149, 150, 55, 53, 50, 49, 11, 12 7, 16, 13, 51, 52, 54, 56, 150, 149

. .

251, 112, 172, 106, 40, 262, 459, 368, 127 252, 172, 100, 39, 106, 459, 352, 129, 368 253, 13, 56, 54, 16, 128, 353, 369, 145 254, 56, 10, 9, 54, 353, 144, 146, 369 255, 128, 353, 369, 145, 35, 82, 81, 36 256, 353, 144, 146, 369, 82, 33, 34, 81

** Region: (Section-1:Picked)

*Elset, elset=_PickedSet13, internal, generate 1, 256, 1

** Section: Section-1

*Solid Section, elset=_PickedSet13, material=VTT 1.,

(46)

*Nset, nset=_PickedSet4, internal, instance=Part-1-1

37, 38, 39, 40, 93, 106, 113, 114, 115, 116, 117, 118, 119, 120, 121, 122

123, 124, 125, 126, 127, 129, 130, 131, 132, 133, 134, 135, 136, 137, 138, 139

140, 141, 142, 143, 354, 355, 356, 357, 358, 359, 360, 361, 362, 363, 364, 365

366, 367, 368

*Elset, elset=_PickedSet4, internal, instance=Part-1-1

41, 42, 55, 56, 69, 70, 83, 84, 97, 98, 111, 112, 125, 126, 139, 140

153, 154, 167, 168, 181, 182, 195, 196, 209, 210, 223, 224, 237, 238, 251, 252

*Nset, nset=_PickedSet5, internal, instance=Part-1-1 40,

*Nset, nset=_PickedSet6, internal, instance=Part-1-1 26, 27, 29, 30, 69, 71, 75, 76, 156

*Elset, elset=_PickedSet6, internal, instance=Part-1-1, generate 17, 20, 1

*Nset, nset=ELEMENT1, instance=Part-1-1

25, 26, 27, 28, 29, 30, 31, 32, 69, 70, 71, 72, 73, 74, 75, 76

155, 156

*Elset, elset=ELEMENT1, instance=Part-1-1, generate 17, 20, 1

19, 20, 22, 23, 25, 26, 29, 32, 65, 67, 74, 76, 83, 84, 85, 86

159, 160

17, 18, 19, 20, 21, 22, 23, 24, 61, 62, 63, 64, 65, 66, 67, 68

153, 154