Friction Stir Welding (FSW) Simulation#

This example problem shows how to simulate the friction stir welding (FSW) process. Several characteristics of FSW are presented, including tool-workpiece surface interaction, heat generation due to friction, and plastic deformation. A nonlinear direct coupled-field analysis is performed, as thermal and mechanical behaviors are mutually dependent and coupled together during the FSW process.

Because it is often difficult to find a full set of engineering data to simulate the FSW process, the problem emphasizes the simulation rather than the numerical results. A simplified version of the model created by Zhu and Chao illustrates the FSW simulation method.

The following features and capabilities are highlighted:

• Direct Structural-thermal analysis using coupled-field solid elements

• Plastic heat generation in coupled-field elements

• Frictional heat generation using contact elements

• Surface-projection-based contact method

• Contact elements with bonding capability

The following topics are available:

You can also perform this example analysis entirely in the Ansys Mechanical Application. For more information, see Friction Stir Welding (FSW) Simulation in the Workbench Technology Showcase: Example Problems.

28.1. Introduction#

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. 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.

Thermal and mechanical behaviors are mutually dependent during the FSW process. Because the temperature field affects stress distribution, this example uses a fully thermomechanically coupled model. The model consists of a coupled-field solid element with structural and thermal degrees of freedom. The model has two rectangular steel plates and a cylindrical tool. All necessary mechanical and thermal 28.5. Boundary Conditions and Loading are applied on the model. The simulation occurs over three load steps, representing the 28.5.3. Loading of the process.

The temperature rises at the contact interface due to frictional contact between the tool and workpiece. FSW generally occurs when the temperature at the weld line region reaches 70 to 90 percent of the melting temperature of the workpiece material. The temperature obtained around the weld line region in this example falls within the range reported by Zhu and Chao [Zhu2004] and Prasanna and Rao [Prasanna2010], while the maximum resulting temperature is well below the melting temperature of the workpiece.

The calculated frictional heat generation and plastic heat generation show that the friction between the tool shoulder and workpiece is responsible for generating most of the heat. A bonding temperature is specified at the contact interface of the plates to model the welding behind the tool. When the temperature at the contact surface exceeds this bonding temperature, the contact is changed to bonded.

28.2. Problem Description#

The Zhu and Chao Thermomechanical Model

The model used in this example is a simplified version of the thermomechanical model developed by Zhu and Chao for FSW with 304L stainless steel [Zhu2004]. Zhu and Chao presented nonlinear thermal and thermomechanical simulations using the finite element analysis code WELDSIM. They initially formulated a heat-transfer problem using a moving heat source, and later used the transient temperature outputs from the thermal analysis to determine residual stresses in the welded plates via a 3-D elastoplastic thermomechanical simulation.

A direct coupled-field analysis is performed on a reduced-scale version of the Zhu and Chao model [Zhu2004]. Also, rather than using a moving heat source as in the reference model, a rotating and moving tool is used for a more realistic simulation.

The tool pin is ignored. The heat generated at the pin represents approximately two percent of the total heat and is therefore negligible.

The simulation welds two 304L stainless steel plates (workpiece) with a cylindrical shape tool, as shown in the following figure:

Figure 28.1: 3-D Model of Workpiece and Tool

The FSW process generally requires a tool made of a harder material than the workpiece material being welded. In the past, FSW was used for soft workpiece materials such as aluminium. With the development of tools made from super-abrasive materials such as polycrystalline cubic boron nitride (PCBN), FSW has become possible with high-temperature materials such as stainless steel. A cylindrical PCBN tool is modeled in this case.

The workpiece sides parallel to the weld line are constrained in all the directions to simulate the clamping ends. The bottom side of the workpiece is constrained in the perpendicular (z) direction to simulate support at the bottom. Heat losses are considered on all the surfaces of the model. All 28.5. Boundary Conditions and Loading are symmetric across the weld centerline.

The simulation is performed in three load steps, each representing a respective phase ( 28.5.3. Loading) of the FSW process.

28.3. Modeling#

Modeling is a two-part task, as described in these topics:

28.3.1. Workpiece and Tool Modeling#

Two rectangular shaped plates (similar to those used in the reference model) are used as the workpiece. Dimensions have been reduced to decrease the simulation time.

The plate size is 3 x 1.25 x 0.125 in (76.2 x 31.75 x 3.18 mm). The tool shoulder diameter is 0.6 in (15.24 mm).

Plate thickness remains the same as that of the reference model, but the plate length and width are reduced. The plate width is reduced because the regions away from the weld line are not significantly affected by the welding process, and this example focuses primarily on the heat generation and temperature rise in the region nearest the weld line.

The height of the tool is equal to the shoulder diameter. Both the workpiece (steel plates) and the tool are modeled using coupled-field element SOLID226 with the structural-thermal option (KEYOPT(1)= 11).

import numpy as np
import pyvista

from ansys.mapdl.core import launch_mapdl
mapdl = launch_mapdl()
mapdl.prep7()

# ***** Problem parameters ********
l = 76.2e-03     # Length of each plate,m
w = 31.75e-03    # Width of each plate,m
t = 3.18e-03     # Tickness of each plate,m
r1 = 7.62e-03    # Shoulder radius of tool,m
h = 15.24e-03    # Height of tool, m
l1 = r1          # Starting location of tool on weldline
l2 = l-l1
tcc1 = 2e06      # Thermal contact conductance b/w plates,W/m^2'C
tcc2 = 10        # Thermal contact conductance b/w tool &
# workpiece,W/m^2'C
fwgt = 0.95      # weight factor for distribution of heat b/w tool
# & workpiece
fplw = 0.8       # Fraction of plastic work converted to heat
uz1 = t/4000     # Depth of penetration,m
nr1 = 3.141593*11  # No. of rotations in second load step
nr2 = 3.141593*45  # No. of rotations in third load step
uy1 = 60.96e-03  # Travelling distance along weld line
tsz = 0.01       # Time step size

# ==========================================================
# * Geometry
# ==========================================================
# * Node for pilot node
mapdl.n(1, 0, 0, h)
# * Workpiece geometry (two rectangular plates)
mapdl.block(0, w, -l1, l2, 0, -t)
mapdl.block(0, -w, -l1, l2, 0, -t)
# * Tool geometry
mapdl.cyl4(0, 0, r1, 0, r1, 90, h)
mapdl.cyl4(0, 0, r1, 90, r1, 180, h)
mapdl.cyl4(0, 0, r1, 180, r1, 270, h)
mapdl.cyl4(0, 0, r1, 270, r1, 360, h)
mapdl.vglue(3, 4, 5, 6)


A hexahedral mesh with dropped midside nodes is used because the presence of midside nodes (or quadratic interpolation functions) can lead to oscillations in the thermal solution, leading to nonphysical temperature distribution. A hexahedral mesh is used instead of a tetrahedral mesh to avoid mesh-orientation dependency. For more accurate results, a finer mesh is used in the weld-line region. The following figure shows the 3-D meshed model:

# ==========================================================
# * Meshing
# ==========================================================
mapdl.et(1, "SOLID226", 11)  # Coupled-field solid element,KEYOPT(1) is
# set to 11 for a structural-thermal analysis
mapdl.allsel()
mapdl.lsel("s", "", "", 4, 5)
mapdl.lsel("a", "", "", 14, 19, 5)
mapdl.lesize("all", "", "", 22, 5)
mapdl.lsel("s", "", "", 16, 17)
mapdl.lsel("a", "", "", 2, 7, 5)
mapdl.lesize("all", "", "", 22, "1/5")
mapdl.lsel("s", "", "", 1)
mapdl.lsel("a", "", "", 3)
mapdl.lsel("a", "", "", 6)
mapdl.lsel("a", "", "", 8)
mapdl.lsel("a", "", "", 13)
mapdl.lsel("a", "", "", 15)
mapdl.lsel("a", "", "", 18)
mapdl.lsel("a", "", "", 20)
mapdl.lesize("all", "", "", 44)
mapdl.lsel("s", "", "", 9, "")
mapdl.lsel("a", "", "", 22)
mapdl.lesize("all", "", "", 2)
mapdl.allsel("all")
mapdl.mshmid(2)  # midside nodes dropped
mapdl.vsweep(1)
mapdl.vsweep(2)
mapdl.vsel("u", "volume", "", 1, 2)
mapdl.mat(2)
mapdl.esize(0.0015)
mapdl.vsweep("all")
mapdl.allsel("all")

mapdl.eplot(vtk=True, background='white')


Figure 28.2: 3-D Meshed Model of Workpiece and Tool

28.3.2. Contact Modeling#

Contact is modeled as follows for the FSW simulation:

• Contact Pair Between the Plates

• Contact Pair Between Tool and Workpiece

• Rigid Surface Constraint

28.3.2.1. Contact Pair Between the Plates#

During the simulation, the surfaces to be joined come into contact. A standard surface-to-surface contact pair using TARGE170 and CONTA174, as shown in the following figure:

The surface-projection-based contact method (KEYOPT(4) = 3 for contact elements) is defined at the contact interface. The surface-projection-based contact method is well suited to highly nonlinear problems that include geometrical, material, and contact nonlinearities.

The problem simulates welding using the bonding capability of contact elements. To achieve continuous bonding and simulate a perfect thermal contact between the plates, a high thermal contact conductance (TCC) of 2 ⋅ 10E6 W/m2 °C is specified. (A small TCC value yields an imperfect contact and a temperature discontinuity across the interface.) The conductance is specified as a real constant for CONTA174 elements.

The maximum temperature ranges from 70 to 90 percent of the melting temperature of the workpiece material. Welding occurs after the temperature of the material around the contacting surfaces exceeds the bonding temperature (approximately 70 percent of the workpiece melting temperature). In this case, 1000 °C is considered to be the bonding temperature based on the reference results. The bonding temperature is specified using the real constant TBND for CONTA174. When the temperature at the contact surface for closed contact exceeds the bonding temperature, the contact type changes to bonded. The contact status remains bonded for the remainder of the simulation, even though the temperature subsequently decreases below the bonding value.

# * Define contact pair between two plates
mapdl.et(6, "TARGE170")
mapdl.et(7, "CONTA174")
mapdl.keyopt(7, 1, 1)  # Displacement & Temp dof
mapdl.keyopt(7, 4, 3)  # To include Surface projection based method
mapdl.mat(1)
mapdl.asel("s", "", "", 5)
mapdl.nsla("", 1)
#mapdl.nplot()
mapdl.cm("tn.cnt", "node")  # Creating component on weld side of plate1

mapdl.asel("s", "", "", 12)
mapdl.nsla("", 1)
#mapdl.nplot()
mapdl.cm("tn.tgt", "node")  # Creating component on weld side of plate2

mapdl.allsel("all")
mapdl.type(6)
mapdl.r(6)
mapdl.rmodif(6, 14, tcc1)  # A real constant TCC,Thermal contact
# conductance coeffi. b/w the plates, W/m^2'C
mapdl.rmodif(6, 35, 1000)  # A real constant TBND,Bonding temperature
# for welding, 'C
mapdl.real(6)
mapdl.cmsel("s", "tn.cnt")
mapdl.nplot(title='Example of Contact Nodes', background='white')
mapdl.esurf()
mapdl.type(7)
mapdl.real(6)
mapdl.cmsel("s", "tn.tgt")
mapdl.esurf()
mapdl.allsel("all")


28.3.2.2. Contact Pair Between Tool and Workpiece#

The tool plunges into the work piece, rotates, and moves along the weld line. Because the frictional contact between the tool and workpiece is primarily responsible for heat generation, a standard surface-to-surface contact pair is defined between the tool and workpiece. The CONTA174 element is used to model the contact surface on the top surface of the workpiece, and the TARGE170 element is used for the tool, as shown in this figure:

Figure 28.4: Contact Pair Between Tool and Workpiece. CONTA174 in blue, and TARGE170 in red.

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. Some additional heat is also generated by plastic deformation of the workpiece material. Because the workpiece material softens and the value of friction coefficient drops as the temperature increases, a variable coefficient of friction (0.4 to 0.2) is defined (Mapdl.tb("FRIC") with mapdl.tbtemp() and Mapdl.tbdata()).

# * Define contact pair between tool & workpiece
mapdl.et(4, "TARGE170")
mapdl.et(5, "CONTA174")
mapdl.keyopt(5, 1, 1)  # Displacement & Temp dof
mapdl.keyopt(5, 5, 3)  # Close gap/reduce penetration with auto cnof
mapdl.keyopt(5, 9, 1)  # Exclude both initial penetration or gap
mapdl.keyopt(5, 10, 0)  # Contact stiffness update each iteration
# based

# Bottom & lateral(all except top) surfaces of tool for target
mapdl.vsel("u", "volume", "", 1, 2)
mapdl.allsel("below", "volume")
mapdl.nsel("r", "loc", "z", 0, h)
mapdl.nsel("u", "loc", "z", h)
mapdl.type(4)
mapdl.r(5)
mapdl.tb("fric", 5, 6)  # Definition of friction co efficient at
# different temp
mapdl.tbtemp(25)
mapdl.tbdata(1, 0.4)  # friction co-efficient at temp 25
mapdl.tbtemp(200)
mapdl.tbdata(1, 0.4)  # friction co-efficient at temp 200
mapdl.tbtemp(400)
mapdl.tbdata(1, 0.4)  # friction co-efficient at temp 400
mapdl.tbtemp(600)
mapdl.tbdata(1, 0.3)  # friction co-efficient at temp 600
mapdl.tbtemp(800)
mapdl.tbdata(1, 0.3)  # friction co-efficient at temp 800
mapdl.tbtemp(1000)
mapdl.tbdata(1, 0.2)  # friction co-efficient at temp 1000
mapdl.rmodif(5, 9, 500e6)  # Max.friction stress
mapdl.rmodif(5, 14, tcc2)  # Thermal contact conductance b/w tool and
# workpiece, 10 W/m^2'C
mapdl.rmodif(5, 15, 1)  # A real constant FHTG,the fraction of
# frictional dissipated energy converted
# into heat
mapdl.rmodif(5, 18, fwgt)  # A real constant  FWGT, weight factor for
# the distribution of heat between the
# contact and target surfaces, 0.95
mapdl.real(5)
mapdl.mat(5)
mapdl.esln()
mapdl.esurf()
mapdl.allsel("all")


28.3.2.3. 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

Figure 28.5: Rigid Surface Constrained. Pilot node or master with applied boundary conditions and the constrained top surface of the tool (blue).**

# * Define Rigid Surface Constraint on tool top surface
mapdl.et(2, "TARGE170")
mapdl.keyopt(2, 2, 1)  # User defined boundary condition on rigid
# target nodes

mapdl.et(3, "CONTA174")
mapdl.keyopt(3, 1, 1)  # To include Temp DOF
mapdl.keyopt(3, 2, 2)  # To include MPC contact algorithm
mapdl.keyopt(3, 4, 2)  # For a rigid surface constraint
mapdl.keyopt(3, 12, 5)  # To set the behavior of contact surface as a
# bonded (always)

mapdl.vsel("u", "volume", "", 1, 2)  # Selecting Tool volume
mapdl.allsel("below", "volume")
mapdl.nsel("r", "loc", "z", h)  # Selecting nodes on the tool top surface
mapdl.type(3)
mapdl.r(3)
mapdl.real(3)
mapdl.esln()
mapdl.esurf()  # Create contact elements
mapdl.allsel("all")

# * Define pilot node at the top of the tool
mapdl.nsel("s", "node", "", 1)
mapdl.tshap("pilo")
mapdl.type(2)
mapdl.real(3)
mapdl.e(1)  # Create target element on pilot node
mapdl.allsel()

# Top surfaces of plates nodes for contact
mapdl.vsel("s", "volume", "", 1, 2)
mapdl.allsel("below", "volume")
mapdl.nsel("r", "loc", "z", 0)
mapdl.type(5)
mapdl.real(5)
mapdl.esln()
mapdl.esurf()
mapdl.allsel("all")


28.4. Material Properties#

Accurate temperature calculation is critical to the FSW process because the stresses and strains developed in the weld are temperature-dependent. Thermal properties of the 304L steel plates such as thermal conductivity, specific heat, and density are temperature-dependent. Mechanical properties of the plates such as Young’s modulus and the coefficient of thermal expansion are considered to be constant due to the limitations of data available in the literature.

It is assumed that the plastic deformation of the material uses the von Misses yield criterion, as well as the associated flow rule and the work-hardening rule. Therefore, a bilinear isotropic hardening model (TB,PLASTIC,,,,BISO) is selected.

The following table shows the material properties of the workpiece:

Table 28.1: Workpiece Material Properties

Property

Value

Linear Properties

Young’s modulus

193 GPa

Poisson’s ratio

0.3

Coefficient of thermal expansion

18.7 µm/m °C

Bilinear Isotropic Hardening Constants (TB,PLASTIC,,,,BISO)

Yield stress

290 MPa

Tangent modulus

2.8 GPa

Temperature-Dependent Material Properties

Temperature (°C)

0

Thermal Conductivity (W/m °C)

16

Specific Heat (J/Kg °C)

500

Density (Kg/m3)

7894

Mapdl.tbdata() defines the yield stress and tangent modulus.

The fraction of the plastic work dissipated as heat during FSW is about 80 percent. Therefore, the fraction of plastic work converted to heat (Taylor-Quinney coefficient) is set to 0.8 (Mapdl.mp("QRATE")) for the calculation of plastic heat generation in the workpiece material.

To weld a high-temperature material such as 304L stainless steel, a tool composed of hard material is required. Tools made from super-abrasive materials such as PCBN are suitable for such processes, and so a cylindrical PCBN tool is used here. The material properties of the PCBN tool are obtained from the references: [Ozel2008] and [Mishra2007].

The following table shows the material properties of the PCBN tool:

Table 28.2: Material Properties of the PCBN Tool

Property

Value

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

The following code setup the material properties:

# ==========================================================
# * Material properties
# ==========================================================
# * Material properties for 304l stainless steel Plates
mapdl.mp("ex", 1, 193e9)  # Elastic modulus (N/m^2)
mapdl.mp("nuxy", 1, 0.3)  # Poisson's ratio
mapdl.mp("alpx", 1, 1.875e-5)  # Coefficient of thermal expansion, µm/m'c
# Fraction of plastic work converted to heat, 80%
mapdl.mp("qrate", 1, fplw)

# *BISO material model
EX = 193e9
ET = 2.8e9
EP = EX*ET/(EX-ET)
mapdl.tb("plas", 1, 1, "", "biso")  # Bilinear isotropic material
mapdl.tbdata(1, 290e6, EP)  # Yield stress & plastic tangent modulus
mapdl.mptemp(1, 0, 200, 400, 600, 800, 1000)
mapdl.mpdata("kxx", 1, 1, 16, 19, 21, 24, 29, 30)  # therm cond.(W/m'C)
mapdl.mpdata("c", 1, 1, 500, 540, 560, 590, 600, 610)  # spec heat(J/kg'C)
mapdl.mpdata("dens", 1, 1, 7894, 7744, 7631, 7518, 7406, 7406)  # kg/m^3

# * Material properties for PCBN tool
mapdl.mp("ex", 2, 680e9)  # Elastic modulus (N/m^2)
mapdl.mp("nuxy", 2, 0.22)  # Poisson's ratio
mapdl.mp("kxx", 2, 100)  # Thermal conductivity(W/m'C)
mapdl.mp("c", 2, 750)  # Specific heat(J/kg'C)
mapdl.mp("dens", 2, 4280)  # Density,kg/m^3


28.5. Boundary Conditions and Loading#

This section describes the thermal and mechanical boundary conditions imposed on the FSW model:

28.5.1. Thermal Boundary Conditions#

The frictional and plastic heat generated during the FSW process propagates rapidly into remote regions of the plates. On the top and side surfaces of the workpiece, convection and radiation account for heat loss to the ambient. Conduction losses also occur from the bottom surface of the workpiece to the backing plate.

Figure 28.6: Thermal Boundary Conditions. Convection loads (red) and conduction loads (yellow)

Available data suggest that the value of the convection coefficient lies between 10 and 30 W/m2 °C for the workpiece surfaces, except for the bottom surface. The value of the convection coefficient is 30 W/m2°C for workpiece and tool. This coefficient affects the output temperature. A lower coefficient increases the output temperature of the model. 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. As a result, the bottom surface of the workpiece is also treated as a convection surface for modeling conduction losses. Because the percentage of heat lost due to radiation is low, radiation heat losses are ignored. An initial temperature of 25 °C is applied on the model. Temperature boundary conditions are not imposed anywhere on the model.

# Initial boundary conditions.
mapdl.tref(25)  # Reference temperature 25'C
mapdl.allsel()
mapdl.nsel("all")
mapdl.ic("all", "temp", 25)  # Initial condition at nodes,temp 25'C

# Thermal Boundary Conditions
# Convection heat loss from the workpiece surfaces
mapdl.vsel("s", "volume", "", 1, 2)  # Selecting the workpiece
mapdl.allsel("below", "volume")
mapdl.nsel("r", "loc", "z", 0)
mapdl.nsel("a", "loc", "x", -w)
mapdl.nsel("a", "loc", "x", w)
mapdl.nsel("a", "loc", "y", -l1)
mapdl.nsel("a", "loc", "y", l2)
mapdl.sf("all", "conv", 30, 25)

# Convection (high)heat loss from the workpiece bottom
mapdl.nsel("s", "loc", "z", -t)
mapdl.sf("all", "conv", 300, 25)
mapdl.allsel("all")

# Convection heat loss from the tool surfaces
mapdl.vsel("u", "volume", "", 1, 2)  # Selecting the tool
mapdl.allsel("below", "volume")
mapdl.csys(1)
mapdl.nsel("r", "loc", "x", r1)
mapdl.nsel("a", "loc", "z", h)
mapdl.sf("all", "conv", 30, 25)
mapdl.allsel("all")

# Constraining all DOFs at pilot node except the Temp DOF
mapdl.d(1, "all")
mapdl.ddele(1, "temp")
mapdl.allsel("all")


28.5.2. Mechanical Boundary Conditions#

The workpiece is fixed by clamping each plate. The clamped portions of the plates are constrained in all directions. To simulate support at the bottom of the plates, all bottom nodes of the workpiece are constrained in the perpendicular direction (z direction).

Figure 28.7: Mechanical Boundary Conditions: X-direction (UX) in red, Y-direction (UY) in green, and Z-direction (UZ) in blue.

# Mechanical Boundary Conditions
# 20% ends of the each plate is constraint
mapdl.nsel("s", "loc", "x", -0.8*w, -w)
mapdl.nsel("a", "loc", "x", 0.8*w, w)
mapdl.d("all", "uz", 0)  # Displacement constraint in x-direction
mapdl.d("all", "uy", 0)  # Displacement constraint in y-direction
mapdl.d("all", "ux", 0)  # Displacement constraint in z-direction
mapdl.allsel("all")

# Bottom of workpiece is constraint in z-direction
mapdl.nsel("s", "loc", "z", -t)
mapdl.d("all", "uz")  # Displacement constraint in z-direction
mapdl.allsel("all")


28.5.3. Loading#

The FSW process consists of three primary phases:

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.

During the traverse phase, the temperature at the weld line region rises, but the maximum temperature values do not surpass the melting temperature of the workpiece material. As the temperature drops, a solid continuous joint appears between the two plates.

For illustrative purposes, each phase of the FSW process is considered a separate load step. A rigid surface constraint is already defined for applying loading on the tool.

The following table shows the details for each load step.

Table 28.3: Load Steps

Load Step

Time Period (sec)

Loadings on Pilot Node

Boundary Condition

1

1

Displacement boundary condition

UZ = -7.95E-07 m

2

5.5

Rotational boundary condition

ROTZ = 60 RPM

3

22.5

Displacement and rotational boundary conditions together on the pilot node

ROTZ = 60 RPM UY = 60.96E-3 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 parameters are determined based on the experimental data of Zhu and Chao [Zhu2004]. The tool travels from one end of the welding line to the other at a speed of 2.7 mm/s.

28.6. Analysis and Solution Controls#

A nonlinear transient analysis is performed in three load steps using structural-thermal options of SOLID226 and CONTA174.

FSW simulation includes factors such as nonlinearity, contact, friction, large plastic deformation, structural-thermal coupling, and different loadings at each load step. The solution settings applied consider all of these factors.

The first load step in the solution process converges within a few substeps, but the second and third load steps converge only after applying the proper solution settings shown in the following table:

Table 28.4: Solution Settings

Solution Setting

Description of Setting and Comments

Mapdl.antype(4)

Transient analysis.

Mapdl.lnsrch("ON")

For contact problems,this option is useful for enhancing convergence.

Mapdl.cutcontrol("PLSLIMIT", 0.15)

Controls the time-step cutback during a nonlinear solution and specifies the maximum equivalent plastic strain allowed within a time-step. If the calculated value exceeds the specified value, the program performs a cutback (bisection). PLSLIMIT is set at 15 percent (from the default five percent) because solution-control support is not available.

Mapdl.nlgeom("ON")

Includes large-deflection effects or large strain effects, according to the element type.

Mapdl.nropt("UNSYM")

Recommended for contact elements with high friction coefficients.

Mapdl.timint("OFF", "STRUC")

To speed up convergence in a coupled-field transient analysis, the structural dynamic effects are turned off. These structural effects are not important in the modeling of heat generation due to friction; however,the thermal dynamic effects are considered here.

Mapdl.kbc(0)

The loads applied to intermediate substeps within the load step are ramped because the structural dynamic effects are set to off.

To allow for a faster solution, automatic time-stepping is activated (Mapdl.autots("on")). The initial time step size (Mapdl.deltim()) is set to 0.1, and the minimum time step is set to 0.001. The maximum time step is set as 0.2 in load steps 2 and 3. A higher maximum time-step size may result in an unconverged solution.

The time step values are determined based on mesh or element size. For stability, no time-step limitation exists for the implicit integration algorithm. Because this problem is inherently nonlinear and an accurate solution is necessary, a disturbance must not propagate to more than one element in a time step; therefore, an upper limit on the time step size is required. It is important to choose a time step size that does not violate the subsequent criterion (minimum element size, maximum thermal conductivity over the whole model, minimum density, and minimum specific heat).

mapdl.solu()
mapdl.antype(4)  # Transient analysis
mapdl.lnsrch('on')
mapdl.cutcontrol('plslimit', 0.15)
mapdl.kbc(0)  # Ramped loading within a load step
mapdl.nlgeom("on")  # Turn on large deformation effects
mapdl.timint("off", "struc")  # Structural dynamic effects are turned off.
mapdl.nropt('unsym')

## Solving
# Load Step1
mapdl.time(1)
mapdl.nsubst(10, 1000, 10)
mapdl.d(1, "uz", -uz1)  # Tool plunges into the workpiece
mapdl.outres("all", "all")
mapdl.allsel()
mapdl.solve()
mapdl.save()

# Load Step2
mapdl.time(6.5)
mapdl.d(1, "rotz", nr1)  # Rotation of tool, 60rpm
mapdl.deltim(tsz, 0.001, 0.2)
mapdl.outres("all", 10)
mapdl.allsel()
mapdl.solve()
mapdl.save()

# Load Step3
mapdl.time(29)
mapdl.d(1, "rotz", nr2)  # Rotation of tool,60rpm
mapdl.d(1, "uy", uy1)  # Displacement of tool along weldline
mapdl.deltim(tsz, 0.001, 0.2)
mapdl.outres("all", 10)
mapdl.solve()
mapdl.finish()
mapdl.save()


28.7. Results and Discussion#

The following results topics for the FSW simulation are available:

28.7.1. Deformation and Stresses#

It is important to observe the change in various quantities around the weld line during the FSW process. The following figure shows the deflection of the workpiece due to plunging of the tool in the first load step:

Figure 28.9: Deflection at Workpiece After Load Step 1

The deflection causes high stresses to develop on the workpiece beneath the tool, as shown in this figure:

Figure 28.10: von Mises Stress After Load Step 1

Following load step 1, the temperature remains unchanged (25 °C), as shown in this figure:

Figure 28.11: Temperature After Load Step 1

As the tool begins to rotate at this location, the frictional stresses develop and increase rapidly. The following two figures show the increment in contact frictional stresses from load step 1 to load step 2:

Figure 28.12: Frictional Stress After Load Step 1

Figure 28.13: Frictional Stress After Load Step 2

All frictional dissipated energy is converted into heat during load step 2. The heat is generated at the tool-workpiece interface. Most of the heat is transferred to the workpiece (FWGT is specified to 0.95). As a result, the temperature of the workpiece increases rapidly compared to that of the tool.

28.7.2. Temperature Results#

The following two figures shows the temperature rise due to heat generation in the second and third load steps:

Figure 28.14: Temperature After Load Step 2

Figure 28.15: Temperature After Load Step 3

The maximum temperature on the workpiece occurs beneath the tool during the last two load steps. Heat generation is due to the mechanical loads. No external heat sources are used. As the temperature increases, the material softens and the coefficient of friction decreases. A temperature-dependent coefficient of friction (0.4 to 0.2) helps to prevent the maximum temperature from exceeding the material melting point.

The observed temperature rise in the model shows that heat generation during the second and third load steps is due to friction between the tool shoulder and workpiece, as well as plastic deformation of the workpiece material.

The melting temperature of 304L stainless steel is 1450 °C. As shown in the following figure, the maximum temperature range at the weld line region on the workpiece beneath the tool is well below the melting temperature of the workpiece material during the second and third load steps, but above 70 percent of the melting temperature: