2.1 FEA method
A key issue involved in the development of the FEM for furniture engineering is the transformation of a geometric model into a reasonable FEM. Figure 1 shows the general steps(Tankut et al. 2014).
(1) Creation of the solid model
In this paper, L-shaped and T-shaped members of solid wood furniture were used as the basic structural units, the solid FEM was established in accordance with the actual size of the members and round tenons in the test and the modelling function in the ABAQUS software was used. Figure 2 shows the geometry and FEM assembly of the members.
(2) Assignment of the material properties and orientations
In the experiments, larch and birch materials were used. In the materials module of ABAQUS software, larch and birch were defined as orthogonal anisotropic materials. Table 1 summarizes the nine elastic constants(Liu et al. 2019; Liyu et al. 2003). The numbers 1, 2 and 3 in the table corresponded to the axial (L), radial (R) and chord (T) directions of the wood in ABAQUS, respectively, and a local coordinate system was established to assign the direction of anisotropic materials(Cuan-Urquizo et al. 2019; Hassani et al. 2015).
Table 1
Nine elastic constants of the base material
Elastic
constants
|
Elastic modulus /MPa
|
Shear modulus/MPa
|
Poisson’s ratio
|
E1
|
E2
|
E3
|
G12
|
G13
|
G23
|
µ12
|
µ13
|
µ23
|
Larch
|
16272
|
1103
|
573
|
1172
|
676
|
66
|
0.42
|
0.51
|
0.68
|
Birch
|
3176
|
334.3
|
171.7
|
334.3
|
248.8
|
77.8
|
0.46
|
0.55
|
0.83
|
(3) Creation of interaction properties
In this study, the FEM of a mortise and tenon joint node in the glued state was developed using the cohesive model as the theoretical basis. Figure 3 shows the cohesive model, which describes the mechanical behaviour of node damage via an intrinsic relationship between the traction stress and separation distance. At the start of loading, the traction stress was linearly related to the separation distance, and when the traction stress reached the maximum value of σmax, the separation displacement was δ0; this turning point corresponds to the starting point for the damage of the glue layer until the node is completely damaged at a separation displacement of δ𝑓(Goyal et al. 2016). Therefore, the cohesive model can be divided into two stages: the initial damage stage and the damage evolution stage.
The cohesive model in ABAQUS can be set up by two methods: one is to create cohesive elements and the other is to create cohesive contact(Su et al. 2010). In this paper, the latter approach was adopted, where contact was established between the surface of the tenon hole and tenon; that is, the cohesive behaviour was selected as the contact characteristic to simulate the glue state of the tenon joint. This method was advantageous as it considerably reduced the difficulty of FEM modelling as well as the analysis time while simultaneously ensuring accurate results. When establishing the cohesive contact model, the maximum stress criterion was adopted in the initial damage phase, and the energy law was adopted in the damage evolution stage, which was concretely defined as shown in Fig. 4.
(4) Application of loads and boundary conditions
The boundary conditions shown in Fig. 5 were set to the degrees of freedom of the corresponding nodes and surfaces of the model, all of the degrees of freedom of the two lateral surfaces of the horizontal members were constrained and a displacement load of 20 mm in the vertical direction (Y axis) to the coupling point RP was applied on the upper end face of the vertical member.
(5) Division of mesh
After considering the accuracy of the results and the uniformity of the mesh, the approximate global mesh size was set to 5 mm, the mesh type was hexahedral and a combined structured and sweep division technique was used. The default algorithm was used, the part of the distorted mesh at the tenon and tenon hole was optimized, the overall model was checked and calculations were conducted after confirming its accuracy.
2.2 Experimental materials and equipment
Larch was used as the test substrate, with an average moisture content of 10.7%. The size of the L-shaped member was 150 mm × 60 mm × 20 mm, and the size of the T-shaped member was 100 mm × 60 mm × 20 mm. Straight-grained birch was used as the round tenon material, with a moisture content of 7%. Its specifications were Φ6 * 40 mm, Φ8 * 40 mm, Φ10 * 40 mm, Φ12*40 mm. Polyvinyl acetate (PVAc) emulsion adhesive was used(Su et al. 2010), with a pH value of 4.9, a solid content of 49.6% and a viscosity of 17.8 Pa⋅s. The following equipment and instruments were used for the experiments: a microcomputer-controlled electronic universal wood mechanics tester(model LD26.305), a bench-top multi-purpose drilling machine (model LT-16) and an electronic scale with an accuracy of 0.001 g.
2.3 Experimental methods
Experiments were conducted using a round tenon with four diameters: 6 mm, 8 mm, 10 mm and 12 mm; the length of all these tenons was 40 mm. Figure 2 shows the machining dimensions. The holes were drilled at the specified locations on the specimens; hence, the centre distance of two holes is 32 mm. The diameter of the round tenon and the tenon hole exhibited a fit of 0, and the length of the round tenon and the depth of the tenon hole exhibited a clearance fit of 2 mm; hence, after assembly, a 1-mm gap between the round tenon and the bottom of the tenon hole is left to permit the escape or release of excess glue and air(Karaman 2021). The machined specimens were glued and assembled using the round tenon. After 150–200 g/m2 glue was evenly applied on both sides of the outer surface of the tenon and the inner surface of the tenon hole, two L-shaped and T-shaped members were obtained, which were aged in the laboratory for 7 days before being fixed on a universal mechanical testing machine in accordance with the clamping method shown in Fig. 6 for pull-out strength testing(Elek et al. 2020).
The loading speed of the mechanical testing machine was set to 5 mm/min at an experimental displacement loading value of greater than 30 mm. When the experiment was completed, the load–displacement curve was obtained, and the final damage load was estimated. To reduce the experimental error, each group of experiments was repeated 5 times, and the average value of the ultimate damage load estimated from the five experiments was taken as the test result.