The proposed integrated design and process simulation method has the practical aim of predicting the final distortion of a complex structure assembled by welding in the automotive chassis design. The method is based on the local/global approach and is made of three steps, as depicted in Fig. 1 and explained in the following. As input data, the designer provides the CAD model which is processed into the welding environment. Other input data regard the experimental data on material, welding process parameters, Goldak parameters ([34]), boundary and initial conditions for process modelling, as well as the automotive industry quality standards, that are allowable distortions given in reference points locations (i.e. allowable tolerance displacements in reference points). The core part of the weld design method has three steps, namely: the local step, the global step, and the quality check step. In the following section a detailed description of these steps is reported.

## 2.1. Step 1: the local step.

In step 1, the local step, a local model is built for the entire joint to be welded or a part of it, depending on the size of the problem. The local model is used to carry out the TEP analysis. In the TEP analysis, thermal and mechanical simulations are carried out in sequence. First, the transient temperature field is defined by the welding heat transfer model. Hence, the transient and residual deformations due to the cooling phase after welding are found by means of a mechanical model, whose load is the thermal load of the welding process. Temperature dependent material properties are used to simulate the metallurgic phenomena occurring during the changes of phase.

The TEP simulation consists of two sequentially coupled analyses for thermal and mechanical models. The thermal model uses heat transfer elements. The heat flux 𝑄(𝑥’,𝑦’,𝑧’,𝑡) supplied by the moving welding torch is modelled by means of the Goldak model of a double ellipsoidal density distribution ([34]), as usually adopted for the MIG welding simulation ([19], [35]). The Goldak parameters on the welding pool are experimentally found. The welding power input 𝑃=*P*(𝑡) is calculated as in (1):

where 𝜂 is the welding arc efficiency with respect to the input energy (0.8 for MIG technology), ([36]) 𝐼 is the current and 𝑈 the voltage. Taken the heat source in the axis origin, the heat flux distribution has different parameters for the front and rear quadrants:

$$\left\{\begin{array}{c}Q\left({x}^{\text{'}},{y}^{\text{'}},{z}^{\text{'}},t\right)=\frac{6\sqrt{3}fP}{abc\pi \sqrt{\pi }}{e}^{-3\left[\frac{x{\text{'}}^{2}}{{a}^{2}}+\frac{y{\text{'}}^{2}}{{b}^{2}}+\frac{z{\text{'}}^{2}}{{c}^{2}}\right]}\\ f,c=\left\{\begin{array}{c}{f}_{f},{c}_{f}z\text{'}\ge 0\\ {f}_{r},{c}_{r}z\text{'}<0\end{array}\right.\end{array} \right.$$

2

where (𝑥′, 𝑦′, 𝑧′) are the local coordinates in the moving reference system associated with the welding torch, 𝑓𝑓 and 𝑓𝑟 are the fractions of the power applied onto the front and rear quadrants, assuming 𝑓𝑓+𝑓𝑟=2 (as in [34]).

The parameters 𝑎, 𝑏, 𝑐𝑓 and 𝑐𝑟 define shape and dimension of the elliptical distributions. Considering the continuity of the volumetric heat source, 𝑓 factors are linked to 𝑐 parameters by 𝑓𝑓=2𝑐𝑓/(𝑐𝑓+𝑐𝑟) and 𝑓𝑟=2𝑐𝑟/(𝑐𝑓+𝑐𝑟).

The boundary conditions on the local model must be chosen carefully, as they affect the local plastic strain field, as well as the global results.

## 2.2. Step 2: the global step.

In the second step, the global model is built, connecting boundary nodes of the local model to the corresponding ones in the global model. Hence, the local model, now integrated in the whole structure, is loaded with the plastic

deformations **ε****p** computed in the TEP analysis, used as the initial conditions. Hence, an elastic FEA simulation is carried out on the entire structure that is the global model, for evaluating the residual stresses and distortions, according to Eq. 3, in which **E** is the elasticity matrix, and **ε** is the total strain vector

\({\sigma }={E}\left({\epsilon }–{{\epsilon }}_{{p}}\right)\) (3)

## 2.3. Step 3 quality check step

In the third step, the quality check is carried out on the entire structure. Resulting distortions are checked in specific locations, called reference points, to lay within dimensional tolerance specifications required by the automotive industry.

Figure 2 The four-members aluminum chassis as a case study for the welding simulation

A 4-members aluminium chassis of a top-class car has been chosen as a case study. Of the four members, two are shell moulded (1, 3 Figure 2) and two are extruded, (2, 4 Figure 2). The fixture system replicates the real assembly asset, as depicted in Figure 3 and digitally reported on the chassis cad model (Figure 4).

## 2.4. Experimental data

Experiments have been carried out in the OMR (Officine Meccaniche Rezzatesi) Automotive industry in Modena (Italy). More than 50 chassis have been checked for measuring the distortions in specific locations. A robotic system for MIG welding is used for the welding process, using different aluminum alloys for base and filler (EN AW-6082-T6 and S-Al-4043 respectively).

Figure 3 The digital replication of the four-members aluminum chassis with related fixturing system

Welding process parameters have been defined as in Table 1. In Table 2, the Goldak parameters used in the analysis have been derived from experiments ([14]).

In order to check the accuracy of the results of the simulations, the tolerance zones for the displacements of some reference points located on the chassis (Fig. 5) have been reported in Table 3. The values of these tolerance zones are defined from the automotive industry standards and will be compared to resulting simulated distortions on the same points.

Table 1

Welding process parameters used for the experiments

Welding speed v | Current (I) | Voltage (U) | Efficiency (η) | Wire feed (vwire) | Wire diameter (dwire) |

0.01 m/s | 88A | 18.8 V | 0.8 | 0.067 m/s | 0.0012 m |

Table 2

Goldak parameters used for the TEP simulation

Goldak parameters | *a* | *b* | *c**f* | *c**r* | *f**f* | *f**r* |

**Value (mm)** | 2.33 | 2.85 | 2.55 | 4.02 | 0.78 | 1.22 |

Table 3

tolerance zones of the displacements in reference points located on the chassis

Reference points | | 1000 | 1001 | 1010 | 1013 | 1014 | 1015 | 1017 | 2001 | 2010 | 2013 | 2014 | 2015 |

**Requested Tolerance zones** | **Tol****X** | ± 0,8 | ± 0,3 | | | ± 0,8 | | ± 0,8 | ± 0,3 | | | ± 0,8 | |

**Tol****Y** | ± 0,3 | ± 0,3 | | | | | ± 0,3 | ± 0,3 | | | | |

**Tol****Z** | ± 0,5 | ± 0,3 | ± 0,5 | ± 1 | | ± 0,5 | ± 0,5 | ± 0,3 | ± 0,5 | ± 1 | | ± 0,5 |

## 2.5. TEP analysis of the local models

A procedure for building the FEA model has been followed. First, a CAD model has been simplified in order to clean up geometries, for better mesh handling. Fillets or holes that have not been loaded and far from the welding beads have been closed or simplified. The local models are a sub-assembly of 4 contiguous joints, in order to increase accuracy on the boundary conditions between the joints. The plastic deformations have been applied on the global model at the same time, without considering the welding sequence.

Two local models have been built, as to carry out a TEP analysis for each local model. The local model is made of 4 overlap joints, modelled together to increase the accuracy of the boundary conditions on the nodes of the joints (Fig. 6). Tetrahedral elements have been used for the FEA models built in the Altair Hypermesh® software. Boundary conditions are applied on each local model, to replicate the actual fixture system.

Hence, the TEP analysis has been carried out on the two local models separately, by using the SimufactWelding® software. The transient heat transfer analysis (welding + cooling phases) is carried out to determine the temperature distribution, used as the initial load condition of a mechanical analysis, yielding distortions. The Goldak model has been used for describing the heat flux distribution, using parameters defined in Table 2. Analyses have been carried out on an Intel(R) Xeon(R) CPU E5-1620 0 @ 3.60GHz, with 8.00 GB RAM.

On the Simufact Welding® software, a selected refinement of the mesh has been performed on the bead elements, as to increase the accuracy. The elements of the weld bead are created during the welding process according to the birth-death method. Given the temperature range as the initial thermal load condition (Fig. 7), the corresponding stress values on the local models are evaluated (Fig. 8).

## 2.6. Elastic analysis on the global model

For the global model, a tetrahedral mesh is built on Altair Hypermesh® software and imported in ABAQUS 6.13® environment for setting up the elastic analysis. In the joint zones, “tie” constraints are applied as to stitch nodes of the extruded and the moulded parts (Fig. 9). This is aimed to ensure that the corresponding nodes behave in a conforming manner and penetration is avoided. Fixturing system is replicated as to restrain the global model during welding, as depicted in Fig. 10. Residual stress on the welded joints are used as initial conditions for the evaluation of the distortions in the global model (Fig. 11)

Results related to the stresses and displacements on the chassis, after the elastic analysis carried out in the global model, have been depicted in Fig. 12 and Fig. 13.

Results are compared to the experimental ones. In Table 4, simulated values of displacements (UXsim, UYsim, UZsim) are compared to tolerance zone requested by the automotive industry standards (TolX, TolY, TolZ). Results show that the values of the simulated displacements lay within the tolerance zones.

Table 4

Displacements resulting from the FEA analysis, evaluated in given reference points, are compared to requested tolerance zones

Reference points | 1000 | 1001 | 1010 | 1013 | 1014 | 1015 | 1017 | 2001 | 2010 | 2013 | 2014 | 2015 |

**U****Xsim** | **0,093** | **-0,025** | **0,037** | **-0,033** | **0,113** | **-0,183** | **0,054** | **-0,073** | **0,018** | **-0,074** | **-0,104** | **0,18** |

**U****Ysim** | **-0,012** | **-0,004** | **0,025** | **-0,009** | **-0,031** | **-0,036** | **0,013** | **0,063** | **0,006** | **0,012** | **0,033** | **0,016** |

**U****Zsim** | **0,017** | **0,001** | **-0,017** | **0,021** | **0,256** | **0,069** | **-0,018** | **-0,063** | **-0,002** | **0,018** | **-0,226** | **-0,064** |