Overview

Test Case

The finite element simulation presented in this test case models the two-dimensional (2D) impact between two long cylinders (a moving striker and a stationary incident bar). The test case is a 2D axisymmetric adaptation of VM-LSDYNA-IMPACT-004, Compressive Elastic Wave Analysis in a 3D Split-Hopkinson Pressure Bar.

The simulation results show the magnitude and duration of the first compressive elastic stress wave transmitted to the bar after impact. These values are validated against calculated values for an identical impact scenario to verify the accuracy of the LS-DYNA explicit solver.

Figure 373 provides a schematic of the test case, showing the incident bar and striker modeled as rectangular shells to represent two two-dimensional cylinders with identical diameters, D, of 20 mm. The striker rests 0.1 mm from the impact surface surface of the incident bar and has an initial velocity, V_s, of 15 mm/ms.

The table that follows shows the corresponding material and geometric properties as well as the loading conditions. The material of both parts is linear elastic and isotropic with typical steel properties.

Figure 373: Test Case Schematic

This test case uses length in mm, time in ms, mass in kg, force in kN, and stress in GPa.

Analysis Assumptions

In the compressive configuration of a Split-Hopkinson Pressure Bar, a compressive stress wave is generated and propagates through the incident bar. This wave is transmitted to the rest of the testing apparatus, which includes the specimen and the transmission bar attached to the incident bar’s end. However, in the current test case, only the stress wave within the incident bar is considered. The specimen and transmission bar are excluded from the analysis.

The striker impacts the incident bar, generating two compressive stress waves: one through the striker (moving right to left) and another through the incident bar (moving left to right).

Figure 374 illustrates the propagation of the compressive stress wave moments after impact.

Figure 374: Stress Wave Propagation through the Striker and Incident Bar

When waves reach the end of a given structure, they reflect back in the opposite direction. After the striker impacts the bar, the total length of the resulting compressive wave traveling through the striker and reflecting back is then twice the length of the striker ().

The duration period of the first stress wave at a fixed particle in the incident bar () can be calculated using the striker’s length () and the speed of sound in the material ():

(135)

The speed of sound in the material () can be calculated using its Young’s modulus () and density (). Material properties for the current test case are included in the test case description.

(136)

The resulting speed of sound for the steel-like material used in this test case is 5,189 mm/ms. Therefore, using Equation 135, the duration period () of the first stress wave in the incident bar is 0.1156 ms.

To calculate the magnitude of the first bar wave (), Equation 137 is used to obtain the force equilibrium at the impact plane.

(137)

Where:

represents the axial stress of the striker () and incident bar ().

represents the cross-sectional area of the striker () and incident bar ().

Using momentum conservation, the axial stress of each component (, ) caused by an impact can be calculated using Equation 138:

(138)

Where:

is the change of velocity in the structure's particles.

Immediately after the impact, the particle velocity at the impact plane, , is the same for the two structures. Since the rest of the striker is moving with a velocity of , its velocity change is . Substituting Equation 138 in Equation 137:

(139)

The acoustic impedance of a structure ( ) is calculated as the product of its cross-sectional area ( ), its density ( ), and the speed of sound in the material ( ). Therefore, the particle velocity can be obtained:

(140)

(141)

The magnitude of the compressive stress in the incident bar can then be calculated by substituting equation Equation 141 in Equation 137:

(142)

Therefore, the magnitude of the first stress wave transmitted to the incident bar is 0.3035 GPa.

Modeling Notes

Figure 375: Model Setup

Figure 376: Mesh Details for the Incident Bar (Red) and Striker (Blue)

In the simulation two parts are defined: one to represent the incident bar (PID 1) and another to represent the striker (PID 2). The parts are meshed with 2D quadrilateral shell elements with a length of 3 mm in the axial direction and 1.25 mm in the radial direction.

The parts use a the axisymmetric shell element formulation (*SECTION_SOLID with ELFORM=15), which considers the y-axis the axis of symmetry (see Figure 373).

The parts use an elastic material card (*MAT_ELASTIC) with density of 7.8⋅10^-6 kg/mm³, Young’s modulus of 210 GPa, and Poisson’s ratio of 0.3.

The contact definition between the striker and the flange is defined with the keyword *CONTACT_2D_AUTOMATIC_SURFACE_TO_SURFACE using the sets of nodes that represent the contact surfaces.

The initial velocity of the striker is defined using the keyword *INITIAL_VELOCITY_GENERATION with a translational velocity in global y-direction of 15 mm/ms.

The keyword *CONTROL_TERMINATION is used to define the termination time of 0.6 ms.

Results Comparison for ANSYS Product

Figure 377 below shows the y-stress contour plot for the incident bar and striker at different timesteps. The plot illustrates that the compressive stress wave moves through the striker and reflects back during the initial 0.12 ms. Meanwhile, a compressive stress wave of the same magnitude propagates through the incident bar.

Figure 377: Axial Stress (GPa) at Different Timesteps

To validate the model and verify the accuracy of the LS-DYNA explicit solver, the magnitude and duration of the first compressive stress wave transmitted through the incident bar resulting from the simulation were compared to the analytical solution. For this purpose, an element located at 1,000 mm from the impact surface (y-coordinate) in the incident bar is used to track the variation of y-stress and calculate the wave magnitude and period. Figure 378 shows the y-stress (GPa) for the bar element versus time (ms).

Figure 378: Axial Stress (GPa) of Incident Bar Element Versus Time

To quantify the error between the analytical and LS-DYNA solutions, the magnitude and period of the first compressive stress wave and their relative errors are calculated in the following results table. For the LS-DYNA model, the stress magnitude is calculated by averaging the stress values between the first and last local peaks of the stress wave. The time period is calculated between two points located in the middle of the pulse rise and fall. As shown in the results table below, the average stress magnitude is calculated as 0.3045 ± 0.0217 GPa, and the wave is experienced during 0.1175 ms. The results show excellent agreement with the analytical solution.