PSI - Issue 57

Cristian Bagni et al. / Procedia Structural Integrity 57 (2024) 598–610 Author name / Structural Integrity Procedia 00 (2019) 000 – 000

602

5

Fig. 2. Example of theproposedmodelling strategy applied to a lap shear specimen, with the adherends in grey and the adhesive in cyan.

Two typical specimen geometries, namely lap shear (LS) and coach peel (CP), were modelled in ANSYS using the FE modelling strategy described above. For this exercise, a unit load was applied and the adherends were modelled as a generic structural steel, while the adhesive as a generic epoxy resin using the material properties available in ANSYS material library. The LS specimen was modelled as 370 mm long, 50 mm wide and with a 30 mm overlap, 2 mm thick adherends and 0.5 mm thick adhesive. The CP specimen was modelled as 130.5 mm long, 60 mm wide and with a 25 mm overlap, 2 mm thick adherends and 0.5 mm thick adhesive. A convergence study was also carried out, for both geometries. In the initial meshes, the adhesive was modelled as one single layer of solid elements (element size = 2.5 mm) and the membrane shell elements had the same size as the solid elements. The mesh of the solid elements was then refined four times, by halving the element size at each refinement, while the size of the membrane shell elements wrapping the solid elements was kept constant. For comparison purposes the peel stresses from the centroid of both membrane shell elements and solid elements were extracted. The results of the analyses are graphically shown in Fig. 3 and Fig. 4. It is possible to observe that for both geometries the predicted highest peel stresses were in the adhesive, as expected, and that the maximum peel stress estimated at the centroid of the solid elements and of the membrane shell elements was approximately in the same location, regardless of the mesh refinement. Furthermore, from Fig. 5 it can be observed that while the maximum peel stress calculated at the centroid of the solid elements increased at each mesh refinement, the maximum peel stress calculated at the centroid of the membrane shell elements remained reasonably constant. This showed that the addition of the membrane shell elements on the exposed faces of the solid elements, used to model the adhesive, effectively transfers the peel stresses from the solid elements, with the advantage of making the stresses of interest reasonably mesh insensitive. Modifications to the proposed modelling strategy can be used such as modelling the adherends with solid elements or modelling the adherends with mid-surface shell elements or modelling the adhesive with solid elements and the actual adhesive thickness, and joining the adherends with the adhesive using bar/beam elements. However, these modifications would make the model more onerous from a modelling and/or computational point of view. Therefore, these modifications should be applied only if necessary. Finally, life/damage predictions can be performed using the DesignLife standard SN Analysis Engine, where the inputs are the peel stresses at the centroid of the membrane elements from the FE model, the load history and materials’ properties as well as fatigue parameters obtained through testing. An example of a fatigue analysis workflow using nCode DesignLife is illustrated in Fig. 6. The next section describes a possible process to derive bespoke fatigue parameters of the adhesive joints through physical testing.