Some Other Parameters in Abaqus Impact Tutorial

Modeling the Part

For an Abaqus Impact Simulation, start by modeling the object that will be impacted or that will do the impacting. We’re simulating a cylindrical rod hitting a rigid wall. The cylinder has a length of 2.54 cm and a radius of 0.381 cm.

In Abaqus:

Go to Part → Create → 3D, Deformable, Solid, Extrusion, and continue by drawing the rod's cross-section.

After completing the sketch, specify the cylinder's height as 2.54 cm.

This step gives you a 3D model of the rod, which is the first requirement for running an analysis.

What Do We Need to Know for Abaqus Impact Analysis?

For an accurate impact simulation, you need a thorough understanding of the mechanical properties of the materials involved and the analysis type best suited for the event.

Material Properties

In high-speed impacts, materials exhibit behaviors that differ from static conditions. For example, the strain rate plays a significant role. In our simulation, the Johnson-Cook model is used. This material model is designed for high strain-rate scenarios and accounts for plasticity, strain rate sensitivity, and temperature effects. In the picture below, you can see the all parameters you need to know for this example in one glance:

Figure 1: Material parameters for the cylindrical rod hitting a rigid wall example

and in figure 2, you can see that where to insert the Johnson-Cook parameters:

Figure 2: Inserting Johnson-Cook parameters

These parameters are entered into Abaqus through the Material Module:

Property → Material → Create, and define the mechanical properties as mentioned above.

Are There Any Specific Parameters We Need to Know About?

Yes, impact analysis in Abaqus involves several key parameters. Some of the most critical ones include mesh density, boundary conditions, and the analysis step type.

1. Mesh Density

The mesh in an impact simulation must be fine enough to capture detailed deformations but coarse enough to keep computation time reasonable. In our case, we use a structured mesh with Hex elements, which are suitable for solid structures like the cylinder. Follow these steps in Abaqus:

Mesh Module → Seed Edges and choose by number:

• Set 10 elements along the radial edges.
• Set 40 elements along the length.
• Set 14 elements along the curved edges.

Then, select the Hex element shape and assign Explicit elements for high-speed impact calculations.

2. Boundary Conditions

Boundary conditions are essential for defining how the model interacts with its surroundings. For this simulation:

Apply Gravity: Go to Load Module → Gravity, and define the gravitational forces acting on the model.

Initial Velocity: Define the initial speed of the rod as 19000 cm/sec by selecting Load Module → Predefined Field → Velocity.

Fixing the Bottom Surface: The bottom of the rod, which impacts the rigid wall, needs to be constrained:

Use Load Module → Boundary Condition → Displacement/Rotation and set U3 = 0.

Also, symmetry boundary conditions should be applied along the X and Y planes to reduce computation time while maintaining accuracy.

3. Choosing the Right Analysis Step

The Dynamic, Explicit step is the best choice for high-speed impacts. It’s designed to handle large deformations, contact interactions, and rapid changes in momentum. Here’s how to set it up:

Go to Step → Create Step, select Dynamic, Explicit, and set the Time Period to 7e-5 seconds.

Enable Nlgeom for non-linear geometric effects, and turn on adiabatic heating to account for temperature rise during the plastic deformation of the rod.

These parameters ensure that Abaqus accurately simulates the behavior of the rod during the impact with the rigid wall.

The full Abaqus Impact Tutorial of this example is available in this PDF file.

How to Determine if It’s a High-Speed or Low-Speed Impact?

Impact Velocity:

• High-Speed Impact: Typically above 10 m/s.
• Low-Speed Impact: Typically below 10 m/s.

Strain Rate:

• High-Speed Impact: Strain rates between 10^3 to 10^6 s⁻¹.
• Low-Speed Impact: Strain rates below 10^3 s⁻¹.

Material Response:

• High-Speed Impact: Strain rate sensitivity and thermal effects are critical.
• Low-Speed Impact: Material behaves more predictably, with elastic or slow plastic deformation.

Analysis Type:

• High-Speed Impact: Requires a Dynamic, Explicit analysis in Abaqus to handle rapid changes and large deformations.
• Low-Speed Impact: Can often be handled with quasi-static analysis or Dynamic, Implicit for more gradual load application.