tigue testing. The geometries tested varied with R/d ratio between the diameter and the radius of curvature as described in Fig. 5 for a general setup. The grips were circular without treads. Compression was done with specimens according to Figs. 5 and 6. Table 2 describes the different diameters and ratios used in the tests. The overall length of the specimens was larger than the prescribed values of 20 days + 4 days. This extra length was confined within the grips, so that we also could fit the longitudinal extensometer onto the specimen during testing.
Finite element model
The design of a finite element model is essential in order to predict the experimental behavior. Initially, a model for the whole machine and the specimen was made using a finite element code (Abaqus). This introduced several factors to the model that lead to assumptions and uncertainties. Such a model requires also a substantial amount of run-time of a strong computer. Therefore, a simplified model was developed, which is described in Fig. 7 (part a). It was chosen to use the explicit solver, which is commonly used to solve dynamic problems. However, the explicit method is also used in the literature to solve quasistatic problems similar to the one in this investigation shown by Romanova et al. (2019) and Hu et al. (1994). Full three-dimensional models must be made in order to capture the buckling behavior. Convergence tests of the 3D model were done by refining the element mesh until insignificant difference from the previous mesh size. In addition, an axisymmetric model in tension was modeled with a fine mesh and compared to the 3D model with the mesh used in the modeling of the compression tests. The time of the simulation was set to 1 s. This gave a sufficiently low speed of the deformation to ensure that the kinetic energy was insignificant compared to the total energy. The element chosen was the C3D8R element (8-node linear brick, reduced integration, hourglass control). Example of the geometry and mesh are shown in Fig. 7a and b, respectively. The number of elements were ranging from 646 to 850 elements depending on the geometry of the specimens. The mesh quality was checked with the mesh control in FEM software (Abaqus) using the default settings with respect to corner angles and aspect ratio.
The deformation was applied in the longitudinal direction to the upper part of the model, representing the upper grip. All the other degrees of freedom were fixed for this part. The displacement was given as a linear function up to a chosen maximum limit of deformation. The part within the bottom grip was modeled to be free to move in the plane normal to the longitudinal axis. All the other degrees of freedom were fixed for this part.
The boundary conditions of the presented model over-constrain the rotation of the grips and under-constrain the sideways movement of the bottom grip. Geometrical imperfections and misalignment were not included in the model.
The essential output of this model is the critical buckling force, i.e., this is the force for the onset of sideways movement. The result of the sideways movement (buckling) is shown in Fig. 7c. The simulations of the model were run on a computer equipped with a processor of type Intel® Xeon® W-2123 CPU @ 3.60 GHz and 16-GB RAM. The CPU time for the simulations was ranging from about 1400 to 2300 s. Until the point of sideways movement, the mesh quality remained good.
The finite element model (Abaqus) calculated the sideways movement of the point RP-2 (see Fig. 7a) at the bottom plane of the specimen. The onset of sideways movement was determined by taking the time-derivative of the movement in the X- and Y-direction (U1 and U3 respectively) of the point RP-2 (see Fig. 7a). A typical example is shown in Fig. 8 for R5d8. The derivative of the movements in X-Z plane is stable prior to buckling. They fluctuate around zero, but when the derivative of the movement is drifting away from zero, the sideways movement had started. This represents the onset of buckling. For example, in Fig. 8, the onset of side