English English
  • English English
CAE-Solutions

cae-solutions

  • Home
    CAE-Solutions
  • Training & Education
    • Ansys
      • ANSYS Training
      • Ansys Projects
    • LS-Dyna
      • LS-Dyna Training
      • LS-Dyna Projects
    • Altair HyperWorks
    • ADAMS
      • ADAMS/Car
      • ADAMS/View
      • ADAMS Projects
  • Projects
    • Automotive
      • Body&Structural
      • Vehicle Dynamic
    • Civil
    • Aerospace
    • Other Projects
    • Ongoing Projects
  • Download
  • About Me
    • Work Experience
    • Quality Policy
  • Contact Me
  • Home
  • Training & Education
    • Ansys
      • ANSYS Training
      • Ansys Projects
    • LS-Dyna
      • LS-Dyna Training
      • LS-Dyna Projects
    • Altair HyperWorks
    • ADAMS
      • ADAMS/Car
      • ADAMS/View
      • ADAMS Projects
  • Projects
    • Automotive
      • Body&Structural
      • Vehicle Dynamic
    • Civil
    • Aerospace
    • Other Projects
    • Ongoing Projects
  • Download
  • About Me
    • Work Experience
    • Quality Policy
  • Contact Me
  • You are here:
  • Home
  • Training & Education
  • Ansys
  • ANSYS Training
  • How To Simulate a Friction Stir Welding with ANSYS

Article content

How To Simulate a Friction Stir Welding with ANSYS

How To Simulate a Friction Stir Welding with ANSYS Featured

Post by: Javad Mehrmashhadi
04/06/2015
Category: ANSYS Training
5618 views
font size
How To Simulation Friction Stir Welding (CAE-Solutions.com) Friction Stir Welding
  • 1
  • 2
  • 3
  • 4
  • 5
(2 votes)

Friction Stir Welding (FSW) is a solid-state welding technique that involves the joining of metals without filler materials. A cylindrical rotating tool plunges into a rigidly clamped workpiece and moves along the joint to be welded. 

In FSW (Friction Stir Welding) process, as the tool translates along the joint, heat is generated by friction between the tool shoulder and the workpiece. Additional heat is generated by plastic deformation of the workpiece material. The generated heat results in thermal softening of the workpiece material. The translation of the tool causes the softened workpiece material to flow from the front to the back of the tool where it consolidates. As cooling occurs, a solid continuous joint between the two plates is formed. No melting occurs during the process, and the resulting temperature remains below the solidus temperature of the metals being joined. FSW offers many advantages over conventional welding techniques, and has been successfully applied in the aerospace, automobile, and shipbuilding industries.

To receive educational and training movie please send me your request.

 Send via request

Friction Stir Wedling simlation in ANSYS

FSW Description

The model used in this tutorial is a simplified version of the thermo-mechanical model and the tool pin is ignored.

The simulation is performed in three load steps, each representing a respective phase (plunge, dwell, and traverse) of the FSW process.

1.      Plunge -- The tool plunges slowly into the workpiece

2.      Dwell -- Friction between the rotating tool and workpiece generates heat at the initial tool position until the workpiece temperature reaches the value required for the welding.

3.      Traverse (or Traveling) -- The rotating tool moves along the weld line.

Material Properties of the Plates

Young’s modulus

193 GPa

Poisson’s ratio

0.3

Coefficient of thermal expansion

18.7 µm/m °C

Bilinear Isotropic Hardening Constants (TB,BISO)

Yield stress

290 MPa

Tangent modulus

2.8 GPa

Temperature Dependent Material Properties

Temperature (°C)

0

200

400

600

800

1000

Thermal Conductivity (W/m °C)

16

19

21

24

29

30

Specific Heat (J/Kg °C)

500

540

560

590

600

610

Density (Kg/m3)

7894

7744

7631

7518

7406

7406

               

 

Material Properties of the PCBN Tool

Young modulus

680 GPa

Poisson’s ratio

0.22

Thermal Conductivity

100 W/m °C

Specific Heat

750 J/Kg °C

Density

4280 Kg/m3

 

 

Modeling

Two rectangular shaped plates 76.2 x 31.75 x 3.18 mm  are used. The tool shoulder diameter is 15.24 mm. Both the workpiece (steel plates) and the tool are modeled using coupled-field element SOLID226 with the structural-thermal option (KEYOPT(1) = 11).

Contact Pair Between the Plates

 A standard surface-to-surface contact pair using TARGE170 and CONTA174, as shown in the following figure. To achieve continuous bonding and simulate a perfect thermal contact between the plates, a high thermal contact conductance (TCC) of 2E06 W/m2 °C is specified. The bonding temperature is considered 1000 °C.

Contact Pair Between Tool and Workpiece

 Two real constants are specified to model friction-induced heat generation. The fraction of frictional dissipated energy converted into heat is modeled first; the FHTG real constant is set to 1 to convert all frictional dissipated energy into heat. The factor for the distribution of heat between contact and target surfaces is defined next; the FWGT real constant is set to 0.95, so that 95 percent of the heat generated from the friction flows into the workpiece and only five percent flows into the tool.

A low TCC value (10 W/m2 °C) is specified for this contact pair because most of the heat generated transfers to the workpiece.

Rigid Surface Constraint

 The workpiece remains fixed in all stages of the simulation. The tool rotates and moves along the weld line. A pilot node is created at the center of the top surface of the tool in order to apply the rotation and translation on the tool. The motion of the pilot node controls the motion of the entire tool. A rigid surface constraint is defined between the pilot node (TARGE170) and the nodes of the top surface of the tool (CONTA174). A multipoint constraint (MPC) algorithm with contact surface behavior defined as bonded always is used to constrain the contact nodes to the rigid body motion defined by the pilot node.

The following contact settings are used for the CONTA174 elements:

·         To include MPC contact algorithm: KEYOPT(2) = 2

·         For a rigid surface constraint: KEYOPT(4) = 2

·         To set the behavior of contact surface as bonded (always): KEYOPT(12) = 5

Boundary Conditions

For thermal Boundary Conditions, all external surfaces except the bottom surface, the value of the convection coefficient is 30 W/m2°C for workpiece and tool. A high overall heat-transfer coefficient (about 10 times the convective coefficient) of 300 W/m2 °C is assumed for the conductive heat loss through the bottom surface of the workpiece. An initial temperature of 25 °C is applied on the model.

For mechanical Boundary Conditions, the workpiece is fixed by clamping each plate.

Loading

As indicated previously, there are 3 steps in loading condition.

Load Step

Time Period (sec)

Loadings on Pilot Node

Boundary Condition

1  

plunge

1

Displacement boundary condition

UZ = -7.95E-07 m

 

2

Dwell

5.5

Rotational boundary condition

ROTZ = 60 RPM

 

3

Travelling

22.5

Displacement and rotational boundary conditions together on the pilot node

ROTZ = 60 RPM

UY = 60.96E-03 m

 

 

The tool plunges into the workpiece at a very shallow depth, then rotates to generate heat. The depth and rotating speeds are the critical parameters for the weld temperatures. The tool travels from one end of the welding line to the other at a speed of 2.7 mm/s.

Analysis

A transient analysis is done with large deformation effect and ramped boundary condition. According to the time period and the problem nonlinearity, the maximum time step is restricted to 0.2.

Results

Figure 1-Deflection at Workpiece After Load Step 1

 

Figure 2-von Mises Stress After Load Step

 

Figure 3-Frictional Stress After Load Step 1

Figure 4-Frictional Stress After Load Step 2

Figure 5-Temperature After Load Step 2

Figure 6-Temperature After Load Step 3

Figure 7- Contact status After Load Step 3

 

I have provided a tutorial to create a pilot node in ANSYS which enables rotation DOF in the solid pin. The tutorial starts with modeling a cubic rectangular and ends with animating the results using small displacement solution type. The cubic rotates while it expands confirming that the analysis is incorrect.

In the second part of the film, I employed large displacement solution type that resulted in correct deformation.

Part1:

http://youtu.be/dqFygtKZxXo

Part2: http://youtu.be/a4NoK_d3uVg

 

I hereby inform that I am well able to work as a senior consultant in order to assist you to perform a very good simulation whether the pin is included in the tool or not. The simulation can be done via implicit and explicit code using ANSYS and LS-Dyna respectively.

I actively encourage you to send me a request for further process.

 

Last modified on 10/09/2015

Share this article

Tagged under
  • FSW,
  • FRICTION STIR WELDING,
  • ANSYS Projects,
  • ANSYS Training,
  • Ansys,
  • Tutorial,
More in this category: « A Guideline to Submodeling in ANSYS

Latest from Javad Mehrmashhadi

  • Front Crash Analysis of Toyota Camry
  • Waterjet cutting simulation using ALE simulation
  • Investigation of Tsunami Force on Superstructure Using Explicit Code
  • Standard Guardrail Impact Simulation of Pickup and Sedan Vehicle
  • Drawing Analysis of a Wheel Rim with Fatigue Evaluation with Various Holes

Related items

  • Drawing Analysis of a Wheel Rim with Fatigue Evaluation with Various Holes
  • Design and analyze a wind damper for space shuttle
  • Optimization and weight lightening of typical shear wall with different shapes of openings
  • Welding Simulation of a Train Wheel
  • Friction Stir Welding With Pin

About Author

Javad Mehrmashhadi

Javad Mehrmashhadi

Javad Mehrmashhadi is the owner of CAE-Solutions.

Login to post comments
  • Home
  • Training & Education
  • Projects
  • Download
  • About Me
  • Contact Me

About Me


I have been doing simulation support on variety of projects within automotive and aerospace industries as well as on civil projects since 2004. Regarding my CAE skills using LS-Dyna, ANSYS, Altair Hyperworks and ADAMS I am well able to perform simulations on the following areas:
  • Crashworhiness, Pedestrian
  • Static & Dynamic and Coupled-Field
  • Friction Stir Welding (FSW)
  • Multi-body Dynamic

Please contact me if you need technical support in your projects by sending your request to mehrmashhadi@gmail.com

Javad Mehrmashhadi

Custom Link

  • Iranian Society of Automotive Engineering
Copyright © {2020} Javad Mehrmashhadi. All Rights Reserved
Designed by SmartAddons.Com
Template Settings
Reset

Styling

For each color, the params below will give default values
Blue Red Green Oranges Violet Cyan

Layout

Patterns for Layour Style: Boxed
pattern1 pattern2 pattern3 pattern4 pattern5 pattern6 pattern7 pattern8