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

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.

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.

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.

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.