Overview

Test Case

The simulation models a 3D rectangular plate with a central circular hole, a geometric irregularity, subjected to linear static structural analysis to evaluate stress concentration effects. The left end of the plate is fully fixed, while a uniform tensile pressure is applied to the right end. The plate is modeled using 10-node tetrahedral elements with a finer mesh near the hole to capture stress gradients accurately. The schematic of the present test case is shown in Figure 136.

Figure 136: Schematic of the test case: a rectangular plate with circular hole subjected to tensile loading

The table below shows the geometric properties, material properties, as well as loading and boundary conditions. The material is assumed to be linear elastic and isotropic, obeying Hooke's Law. No plasticity, creep, thermal expansion, or failure criteria are included.

The primary output of interest is the maximum normal stress in the x-direction, particularly near the hole where stress concentration is expected. The central circular hole is a stress raiser. Using the theoretical stress concentration factor , the actual maximum normal stress at the geometric discontinuity can be calculated from the nominal stress as

(3)

where depends only on geometry—the ratio of the hole diameter to the width (). The nominal stress can be calculated using either

(4)

(5)

where in Equation 4 is the applied uniform tensile pressure, equal to 100 Pa in the present case, and and represent the plate's dimensions. In Equation 5, denotes the applied force and is the plate thickness. For the present case, . Thus, (unitless) and . Consequently, .

In both implicit and explicit time integration schemes, the spatially uniform tensile pressure was ramped up as shown in Figure 137.

Figure 137: Imposed uniform tensile pressure (Pa) versus time (s)

Analysis Assumptions and Modeling Notes

The entire domain is discretized using ten-node tetrahedral solid elements (ELFORM=16). A refined mesh near the hole is employed to capture stress gradients accurately near this geometric discontinuity which causes stress concentrations. One end of the plate is fully fixed, with all translational and rotational degrees of freedom constrained to prevent rigid body motion. A uniform tensile pressure is applied on the opposite end, normal to the surface, to represent a far-field uniaxial tensile load. No contact interfaces are defined since the model consists of a single continuous solid body. The simulation is conducted in the SI unit system (N, m, kg, s) but could be adapted to other consistent unit systems as needed.

Figure 138: Model setup for 3D rectangular plate with a central circular hole subjected to tensile pressure

Results Comparison

To verify the accuracy of the simulation, the predicted values of the target parameter—that is, the maximum normal stress in the x direction—were compared against the theoretical values calculated with the stress concentration factor. As shown in the results table below, the implicit and explicit solvers predicted the target stress within -0.11% and -0.07%, respectively, of the theoretical values, validating the numerical results. The maximum normal stress is shown in Figure 139, while Figure 140 shows the amplified deformation of the plate at six seconds. Notably, in both time integration schemes, oscillations were observed at the free end prior to the application of global damping.

Figure 139: Maximum normal x-stress (Pa) versus time (s) in the explicit modeling

Figure 140: Contours of maximum normal stress in the x direction (Pa) with deformations amplified for better visualization in the explicit modeling

As the energy plots in Figure 141 indicate, the simulation is stable. The kinetic energy (red curve) peaks early, then drops to near zero, proving that the system reaches a quasi-static state. Internal energy (green curve) increases steadily and plateaus as loading finishes. This is strain energy stored in the plate due to tension. Total energy (blue curve) matches the internal energy closely after time ≈ 2 s, indicating minimal artificial energy input. Thus, the result is dominated by strain energy.

Note that the non-linear explicit plots shown in Figure 139 and Figure 141 would become linear in implicit. To activate the LS-DYNA implicit solver, set IMFLAG to 1 in *CONTROL_IMPLICIT_GENERAL.

Figure 141: Energy plots (J) in the explicit modeling