PSI - Issue 68

Tuncay Yalçinkaya et al. / Procedia Structural Integrity 68 (2025) 325–331 Yalc¸inkaya et al. / Structural Integrity Procedia 00 (2024) 000–000

328

4

2.3. Plasticity and Damage Parameters Calibration

Due to the uncoupled nature of the models, the hardening parameters are calibrated using experimental data inde pendent from the damage parameters. The force-displacement data obtained from the experiments are used to derive the true stress-strain curves from the smooth tension (ST) specimen up to the necking point. Subsequently, the pa rameters of the hardening law are fitted using MATLAB’s curve-fitting tool. The yield stress and material constants of the hardening laws are presented in Table 2. The density, Young’s modulus, and Poisson’s ratio of the IN718 alloy are assumed to be 8.22 g / cm 3 , 200 GPa, and 0.294, respectively. The damage parameters are also calibrated using

Table 2: Plasticity model parameters.

σ 0 [MPa]

q 1 [MPa]

c 1

b 1

q 2 [MPa]

c 2

b 2

789

499.6

0.1731

106.7

499.6

1.761

4.351

C

˙ ε 0

θ trans (K)

θ melt (K)

m

C p (J / kgK)

χ

0.01

1

293

1593

1.65

0.6

435

the ST specimen Several explicit FE analyses using the ST specimen for each damage model is prescribed. The dam age accumulation rule is implemented in all models using the user-defined subroutine (VUSDFLD). Subsequently, the critical value is subtracted from the experimentally observed failure point derived from the FE analysis results. For the identification of the critical damage parameters ( C i ), the force-displacement curve of the ST specimen is employed, ensuring that the same failure point is selected for all models. The critical damage values determined for the each criteria are presented in Table 3.

Table 3: Damage parameters of criteria for IN718.

Ayada ( C 1 )

Ayada-m( C 2 )

Brozzo ( C 3 )

KH( C 4 ) 3.1.421 CL ( C 9 ) 978.061

LR( C 5 ) 615.327

0.240

0.449

0.657

MC( C 6 )

OH( C 7 )

RT ( C 9 )

Freudenthal ( C 10 )

1.483

0.656

1.118

924.863

2.4. Finite Element Modelling

Displacement-controlled explicit FE tensile simulations are conducted to calibrate the plasticity and damage mod els and to evaluate the capabilities of these models under various stress triaxial conditions. All failure models are implemented using a user-defined field subroutine (VUSDFLD). The ST specimen is used for plasticity and damage calibration. The geometries and meshes of the all specimens are illustrated in Fig. 1. For the ST, NT, and PST speci mens, the element size in the gauge length is 0.2 mm, the element size of the edge of the tensile direction is 0.1 mm to ensure controlled extension of elements, and a quarter model is utilized to reduce computational cost due to symmetry. For the ISS specimen, the element size in the thickness direction is 0.2 mm, and it is 0.1 mm in the gauge region. As there is no plane of symmetry of ISS like the other specimens, a full model is employed. Eight-node linear brick elements (C3D8R) with reduced integration are used, and element deletion is utilized to represent material failure. In the finite element analysis, the upper and lower parts clamped in the testing machine are modeled as rigid sections. FE simulations are performed using calibrated and validated damage models in the backward flow generating FE model. The FE model shown in Fig. 1 consists of three rigid rollers, a mandrel and a preform. The preform is modeled as deformable, whereas the mandrel and rollers are modeled as rigid bodies. To simplify the modeling process, the preform, which actually moves, is kept stationary, and the movement is applied to the rollers in both axial and radial directions. Hexahedral elements with reduced integration (C3D8R) are selected for the preform tube, with enhanced hourglass and distortion control implemented to prevent mesh distortion. A mesh study reveals that a non-uniform element edge ratio of 0.7 provides optimal results, based on damage distribution and equivalent plastic strain evaluations. The element size in the radial direction is 0.589 mm, while the element size in the axial direction is 0.421 mm. Six elements are along the thickness. Tangential and normal contact are added to the model by including