PSI - Issue 77

Alireza Shadmani et al. / Procedia Structural Integrity 77 (2026) 221–228

224

4

Shadmani et al. / Structural Integrity Procedia 00 (2026) 000–000

(a)

(b)

Fig. 2: (a) Stress-strain curve of the PU coating [1] and (b) material model calibration results for hyper-viscoelastic PU

where the first term describes the energy stored from distortion. The Marlow model constructs this function by in terpolating the stress-strain data obtained from the uniaxial tensile test. It extracts the relation between the stress and I 1 from the test data and integrates it to build the function W dev . The second term describes the energy stored from the volume change. Moreover, the viscoelastic properties of the studied coating was achieved from the performed dynamic mechanical analysis presented in (Jespersen et al. (2023)). The extracted parameters from the DMA curves were used in as input in the viscoelastic model in ABAQUS. To take viscoelasticity into account, the model mentioned should be combined with a suitable mathematical model so that the time e ff ect is added to the model. The most im portant time e ff ect is the relaxation phenomenon in which the material sti ff ness is reduced during the loading period (Ghoreishy (2012)). This is the well known stress relaxation e ff ect that nearly all polymers show when a certain load or deformation is applied. The most popular mathematical form of this behavior is given by Prony series as:

N i = 1

t τ i )

g i (1 − e −

g R ( t ) = 1 −

(2)

where g i is a material constant and τ i is the relaxation time. For hyperelastic material models, the relaxation in Eq. (3) is normally applied to the constants that describe the energy function. Consequently, for the selected hyperelastic models the relaxation forms are given as:

N i = 1

t τ i ))

g i (1 − e −

0 (1 −

W ( t ) = W

(3)

Accordingly, the finite element model was developed to simulate a PU coating with a dimension of 100 mm × 100 mm × 1.5 mm, as shown in Fig. 3(a). The reason for choosing the planar dimension is to ensure that the boundaries of the model do not a ff ect the stress distribution. The model was discretized using 4-node hexahedral elements with reduced integration (C3D8R). A central fine mesh with an element size of 0.15 mm was used to accurately capture the stress distribution. The mesh gradually coarsens towards the edges of the model to optimize computational e ffi ciency, as shown in Fig. 3(b). The bottom surface of the model was fixed in all directions, assuming it is perfectly bonded to the substrate, while the transient pressure profile obtained from the CFD model was interpolated to the top surface. The interpolation was performed using the cubic spline method in ABAQUS. The simulation was run for a total time of 2.5 µ s , where a high enough sampling frequency must be chosen to accurately extract all the information from the analysis. To this end, 500 output intervals for stresses were chosen as the sampling frequency. The stress components necessary for the damage calculation are explained in the next section.