Abaqus Tutorial: Step-by-Step Guide to Simulate Steel Ball Impact on Aluminum Plate

In this tutorial we are going to set up a finite element analysis (FEA) model in Abaqus to capture the dynamic behavior, material response, and interaction between the steel ball and aluminum sheet . Below is a detailed, step-by-step guide to perform this simulation using Abaqus/CAE, assuming a basic familiarity with the software interface.

Step 1: Define the impact Problem

• Objective: Simulate a steel ball impacting an aluminum sheet to analyze deformation, stress, strain, and potential damage.
• Parameters:
  • Steel Ball: Assume a spherical ball (e.g., 10 mm diameter, density 7800 kg/m³, elastic-plastic behavior).
  • Aluminum Sheet: Assume a thin square sheet (e.g., 100 mm x 100 mm x 2 mm, density 2700 kg/m³, elastic-plastic behavior).
  • Impact Conditions: Initial velocity of the ball (e.g., 10 m/s downward).
  • Material Properties:
    • Steel: Young’s modulus = 210 GPa, Poisson’s ratio = 0.3, yield stress = 300 MPa, plastic hardening data (optional).
    • Aluminum: Young’s modulus = 70 GPa, Poisson’s ratio = 0.33, yield stress = 100 MPa, plastic hardening data (optional).
  • Analysis Type: Dynamic, explicit (suitable for high-speed impact).

Step 2: Create the Geometry in Abaqus

1. Open Abaqus/CAE and create a new model database.
2. Set Units: Abaqus is unitless, but ensure consistency (e.g., mm for length, kg for mass, s for time, N for force, MPa for stress).
3. Create the Steel Ball:
   • Go to the Part module.
   • Create a new part: 3D, Deformable, Solid, Revolution.
   • Sketch a semi-circle (radius = 5 mm) in the XY-plane, with the center at (0,0), and revolve it 360° around the Y-axis to form a sphere.
   • Name the part (e.g., “Steel_Ball”).
4. Create the Aluminum Sheet:
   • Create another part: 3D, Deformable, Solid, Extrusion.
   • Sketch a square (100 mm x 100 mm) in the XY-plane.
   • Extrude it to a thickness of 2 mm along the Z-axis.
   • Name the part (e.g., “Al_Sheet”).
5. Position the Parts:
   • Ensure the ball is positioned above the sheet’s center. For example, place the ball’s center at (0, 0, 7 mm) so its bottom is 5 mm above the sheet’s top surface (Z = 0 to 2 mm).

Step 3: Define Material Properties

1. Go to the Property module.
2. Create Materials:
   • Steel:
     • Name: “Steel”.
     • Mechanical → Elasticity → Elastic: Young’s modulus = 210e3 MPa, Poisson’s ratio = 0.3.
     • Mechanical → Plasticity → Plastic: Enter yield stress (300 MPa) and plastic strain (0). Add hardening data if available (e.g., stress vs. plastic strain curve).
     • General → Density: 7.8e-9 kg/mm³ (7800 kg/m³).
       • Aluminum:
         • Name: “Aluminum”.
         • Mechanical → Elasticity → Elastic: Young’s modulus = 70e3 MPa, Poisson’s ratio = 0.33.
         • Mechanical → Plasticity → Plastic: Yield stress = 100 MPa, plastic strain = 0. Add hardening data if desired.
         • General → Density: 2.7e-9 kg/mm³ (2700 kg/m³).
3. Assign Section Properties:
   • Create a Section for each part (e.g., “Steel_Section” and “Al_Section”).
   • Assign the respective materials (“Steel” to the ball, “Aluminum” to the sheet).
   • Assign sections to the parts: Select the entire geometry of each part in the Assign Section tool.

In the Ductile Damage Suboptions specify a damage evolution with a failure displacement of 0.2

The damage evolution states that once the elements reach the failure criteria, i.e. a displacement of 0.2, then the element is deleted.

Create a section for each material and apply them to the geometry
o Ball
▪ Solid, homogenous
▪ Ball component
o Plate
▪ Shell, homogenous
▪ Shell thickness: 1
▪ Plate component

Step 4: Assemble the Parts for impact simulation

1. 1. 1. Go to the Assembly module.
      2. Create Instances:
         • Instance the “Steel_Ball” and “Al_Sheet” parts.
         • Ensure the ball is positioned above the sheet as defined (e.g., ball center at Z = 7 mm, sheet top at Z = 2 mm).
      3. Verify Positioning:
         • Use the Translate or Position tools to confirm the ball is centered above the sheet and offset vertically to avoid initial penetration.

Step 5: Define the Impact Analysis Step

1. 1. 1. Go to the Step module.
      2. Create a Step:
         • Create a new step after the initial step: Dynamic, Explicit.
         • Name: “Impact_Step”.
         • Time Period: Estimate the impact duration (e.g., 0.001 s for a high-speed impact). For a 10 m/s impact over a small distance, 0.001 s is reasonable.
         • Settings:
           • Enable NLgeom (geometric nonlinearity) to account for large deformations.
           • Set Time Incrementation to automatic for stability.
      3. Output Requests:
         • Request field outputs: Stress (S), Strain (PE, LE), Displacement (U), Velocity (V).
         • Request history outputs: Kinetic energy (ALLKE), Internal energy (ALLIE), Reaction forces (RF) at boundaries.
         • Set output frequency to capture sufficient data (e.g., every 50 increments or 0.00001 s).

Step 6: Define Impact Interactions in Abaqus

1. 1. 1. Go to the Interaction module.
      2. Contact Properties:
         • Create a Contact Property: Name (e.g., “Ball_Sheet_Contact”).
         • Mechanical → Tangential Behavior: Friction coefficient (e.g., 0.2 for steel on aluminum).
         • Mechanical → Normal Behavior: Hard contact, allow separation after contact.
      3. General Contact (Explicit):
         • Create an Interaction: Select General Contact (Explicit).
         • Assign the contact property (“Ball_Sheet_Contact”) to all surfaces.
         • Include all part instances (ball and sheet) in the contact domain to account for self-contact if the sheet deforms significantly.
      4. Alternative (Surface-to-Surface Contact):
         • If general contact is too computationally expensive, define a Surface-to-Surface Contact:
           • Master Surface: Steel ball surface (more rigid, smaller contact area).
           • Slave Surface: Top face of the aluminum sheet.
           • Assign the contact property.
         • Note: General contact is preferred for simplicity and robustness in explicit dynamics.

Step 7: Apply Boundary Conditions and Loads for impact

1. 1. 1. Go to the Load module.
      2. Boundary Conditions for the Sheet:
         • Create a Boundary Condition in the Initial Step.
         • Name: “Fix_Edges”.
         • Select the outer edges or perimeter of the sheet (e.g., all four sides).
         • Apply: U1 = U2 = U3 = 0 (fix translation in X, Y, Z) to simulate clamped edges. Alternatively, fix only the bottom face or corners depending on the physical setup.
      3. Initial Velocity for the Ball:
         • Create a Predefined Field in the Initial Step.
         • Select Velocity.
         • Select the entire steel ball.
         • Set: V3 = -10,000 mm/s (downward, assuming Z is up). V1 = V2 = 0.
         • Note: Do not apply velocity in the “Impact_Step” to avoid overriding the initial condition.

Step 8: Mesh the Model

1. 1. 1. Go to the Mesh module.
      2. Seed the Parts:
         • Steel Ball:
           • Global seed size: ~0.5 mm (fine mesh for accuracy in contact and deformation).
           • Local seed near the contact region (bottom of the ball): ~0.2 mm for higher resolution.
         • Aluminum Sheet:
           • Global seed size: ~2 mm.
           • Local seed in the central impact zone (e.g., 20 mm x 20 mm area): ~0.5 mm to capture deformation gradients.
      3. Element Type:
         • Steel Ball: C3D8R (3D, 8-node linear brick, reduced integration, hourglass control) for solid elements.
         • Aluminum Sheet: C3D8R for solid elements. If the sheet is very thin, consider S4R (4-node shell elements) with 5 integration points through thickness, but solid elements are better for impact.
      4. Mesh the Parts:
         • Mesh both parts using Structured or Free meshing techniques.
         • Ensure a refined mesh in the contact zone to improve accuracy.
         • Verify mesh quality (no distorted elements) using the Query tool.

See more: How to Mesh a 3D Model in Abaqus: A Step-by-Step Guide

Step 9: Create and Submit the Job

1. 1. 1. Go to the Job module.
      2. Create a Job:
         • Name: “Ball_Impact_Simulation”.
         • Select the model.
      3. Job Settings:
         • Set Precision: Single or Double, depending on your system (Single is usually sufficient for explicit).
         • Allocate sufficient memory and CPUs if available (e.g., 4 CPUs for faster computation).
      4. Submit the Job:
         • Click Submit to run the analysis.
         • Monitor the job in the Job Monitor for errors (e.g., excessive element distortion, contact issues).
      5. Debugging Tips:
         • If the job aborts due to element distortion, refine the mesh or add Adaptive Meshing (ALE) in the Step module.
         • If contact issues arise, check surface definitions or reduce the friction coefficient.

Step 10: Post-Processing and Analysis

1. 1. 1. Go to the Visualization module.
      2. Open the Output Database (.odb file).
      3. Visualize Results:
         • Displacement (U): Plot the deformation of the sheet (e.g., U3 for Z-displacement) to see the dent depth.
         • Stress (S): Plot von Mises stress (S, Mises) to identify high-stress regions.
         • Strain (PE): Plot plastic strain (PE, PEQM) to assess permanent deformation.
         • Velocity (V): Check the ball’s velocity to confirm it slows upon impact.
         • Energy Outputs:
           • Plot ALLKE (kinetic energy) to verify energy transfer to the sheet.
           • Plot ALLIE (internal energy) to check energy absorption.
           • Ensure energy balance: Total energy (ALLKE + ALLIE) should remain nearly constant.
      4. Create Contour Plots:
         • Use Contour plots to visualize stress/strain distribution on the sheet.
         • Section the sheet to view internal stresses if needed.
      5. Extract Quantitative Data:
         • Use Probe to measure maximum displacement, stress, or strain at the impact point.
         • Create XY Data plots for energy histories (e.g., kinetic vs. time).
      6. Validate Results:
         • Compare maximum deformation or stress with analytical estimates (e.g., Hertzian contact theory for elastic impact).
         • Check for unrealistic results (e.g., excessive penetration, negative energies).

Step 11: Optional Enhancements for impact simulation in Abaqus

1. 1. 1. Damage Modeling in Abaqus:
         • Add Ductile Damage for aluminum in the Material definition to simulate fracture:
           • Define damage initiation (e.g., equivalent plastic strain at onset).
           • Define damage evolution (e.g., softening behavior).
           • Enable Element Deletion to remove failed elements.
         • This allows modeling of perforation if the impact energy is high.
      2. Rigid Body Approximation:
         • If the steel ball deforms minimally, model it as a Rigid Body:
           • In the Part module, set the ball as Rigid instead of Deformable.
           • Assign a Reference Point at the ball’s center and apply mass (e.g., 0.032 kg for a 10 mm diameter steel ball) and velocity to the reference point.
           • This reduces computation time but ignores ball deformation.
      3. Adaptive Meshing:
         • Enable Adaptive Meshing in the Step module for the sheet to handle large deformations without element distortion.
         • Use ALE Adaptive Mesh Domain and set remeshing sweeps (e.g., 10 per increment).
      4. Refine Contact:
         • Add Contact Stabilization in the Interaction properties to prevent initial oscillations.
         • Use a small damping factor (e.g., 0.0001) to stabilize without affecting results.

Step 12: Save and Document

1. 1. • Save the Model: Save the .cae and .odb files for future reference.
      • Document Results:
        • Export plots (e.g., stress contours, energy curves) as images or data files.
        • Note key findings: Maximum deformation, peak stress, energy transfer.
      • Report Assumptions:
        • Document simplifications (e.g., no strain-rate effects, no damage unless modeled).
        • Mention mesh size, contact settings, and boundary conditions for reproducibility.