Low Stress Welding Simulations

Welding is a fundamental manufacturing technique used to join metal components. While a variety of welding processes exist,  most involve the application of heat to induce coalescence of the metal in the adjoining parts.
The gas welding technique uses the heat from a gas flame to melt together the contacting edges of the parts being joined. A filler material may or may not be used.

The introduction of very high temperatures in the region of the welded joint causes steep temperature gradients in the structure. As a weld cools, residual stresses may be produced in the weld zone; such stresses may cause the structure to distort. The ability to predict the residual stress state allows for the prediction of final part shapes and a more complete understanding of how residual stresses can affect the load capacity of a structure.

The finite element models described in this article represent structural beams. These structures are formed by welding plate sections together rather than producing the section directly in a mill. The cross-sectional size of these components can make direct manufacture impractical.

The techniques discussed here are based on a generic model but are transferable to a range of applications.

The simulation uses a sequentially coupled approach in which a thermal analysis is followed by a stress analysis. The temperature results from the thermal analysis are read into the stress analysis as loading to calculate the thermal stress effects. The thermal analysis makes use of ABAQUS user subroutines DFLUX, GAPCON, and FILM. The objective of the simulation is to predict post-weld deformation and residual stress distribution.

Figure 1: Mesh of the structure being welded.

The thermal analysis is performed to calculate the heat transfer resulting from the thermal load of the moving torch. Three user subroutines are activated for the thermal analysis:

DFLUX: Used to define the welding torch heat input as a concentrated flux. The heat source travels along the weld line to simulate the torch movement.

GAPCON: Used to activate the conduction of heat between the deposited weld material and the parent materials once the torch has passed a given location.

FILM: Similar to GAPCON in functionality, but used to activate film coefficients to simulate convective ambient cooling once the torch passes a given location.

The simulation is run as a fully transient heat transfer analysis.

The structural analysis uses the thermal analysis (temperature) results as the loading. The objective of the structural analysis is to determine the stresses and strains induced in the weld region during the cooling transient. Boundary conditions are applied to restrain the system against rigid body motion.

Figure 2: Nodal temperatures in a typical region of the weld as the torch traverses the weld line.

Typical thermal results are shown in Figure 2 (left), which displays a contour of nodal temperature as the torch travels along the weld line.

The weld is initialized at 1800° C, but no heat is allowed to transfer from the weld until the torch passes. As the torch passes a given point on the weld line, the flux input is initiated, resulting in a localized increase in temperature to more than 2000° C.

Figure 3: Transient temperature profile at three points in the torch path.

Figure 4: Von Mises stress in the weld region at t=35 s.

Figure 5: Effective plastic strain in the weld region at t=35 s.