Fill out the form to download

Required field
Required field
Not a valid email address
Required field
Required field

  • Set up your own cloud-native simulation in minutes.

    Start Simulating Now

    • Documentation

    SimScale DocumentationValidation CasesValidation Case: Impact of an Elastoplastic Bar

    Validation Case: Impact of an Elastoplastic Bar

    This validation case belongs to an elastoplastic impact in solid mechanics. The aim of this test case is to validate the following parameters:

    • Dynamic analysis
    • Frictional contact
    • Elastoplasticity
    • Large deformations

    The simulation results of SimScale were compared to the numerical results presented in [SDNV103]\(^1\).

    View Project

    Geometry

    The geometry used for the case is as follows:

    geometrical model for dynamic elastoplastic impact validation case
    Figure 1: Geometrical model of the impact bar and plate

    It represents an elastoplastic bar in the z-direction and a rectangular plate in the x-y plane with the following coordinates for each point:

    PointX [m]Y [m]Z [m]
    A000
    B0.01600
    C0.0160.0160
    D00.0160
    E000.001
    F0.01600.001
    G0.0160.0160.001
    H00.0160.001
    I000.00327
    J0.003200.00327
    K00.00320.00327
    L000.03567
    M0.003200.03567
    N00.00320.03567
    Table 1: Coordinates of the geometry vertices

    Analysis Type and Mesh

    Tool Type: Code Aster

    Analysis Type: Dynamic

    Mesh and Element Types: The meshes used in this project were created in SimScale with the standard algorithm. Manual refinements are used to control the cell sizes.

    CaseElement TypeNumber of
    Nodes    		Element Technology
    A1st Order Tetrahedral10435Standard
    B2nd Order Tetrahedral70001Reduced Integration
    Table 2: Mesh details for each case.

    Find below the mesh used for case B. It’s a standard mesh with second-order tetrahedral cells.

    hexahedral mesh for dynamic elastoplastic impact validation case
    Figure 2: Finite elements mesh as used on case B

    Simulation Setup

    Material:

    • Bi-linear Plasticity Isotropic:
      • \( E = \) 117 \( GPa \)
      • \( \nu = \) 0.35
      • \( \sigma_y = \) 400 \( MPa \)
      • \( E_T = \) 500 \( MPa \)
    material elastoplastic model for dynamic elastoplastic impact validation case
    Figure 3: Material elasto-plastic stress-strain curve

    Boundary Conditions:

    • Initial Conditions:
      • Velocity of 227 \(m/s \) to volume IJKLM (bar)
    • Constraints:
      • Volume ABCDEFGH (plate) fixed
      • Face IKLN zero x-displacement
      • Face IJLM zero y-displacement

    Reference Solution

    The reference solution is from a numerical computation as presented section 2 of [SDNV103]\(^1\), which are taken as the mean results of [Stainer]\(^2\):

    \( DX_J = 3.87 mm \)

    \( DZ_L = 13.46 mm \)

    Result Comparison

    Comparison of displacements at points J (DX) and L (DZ) at time \( t = 9×10^{-5}\ s \):

    CASEPOINTCOMPCOMPUTEDREFERROR
    AJDX0.002890.00387-25.4%
    ALDZ-0.01250-0.01346-7.1%
    BJDX0.003650.00387-5.8%
    BLDZ-0.01265-0.01346-6.0%
    Table 3: Results comparison and computed error.

    An illustration of the final shape (case B) can be found in Figure 4. The elastoplastic deformation due to the impact can be appreciated:

    results plot for dynamic elastoplastic impact validation case
    Figure 4: Deformed shape with stress plot at t = 9e-5 \(s\) from case B

    References

    Note

    If you still encounter problems validating you simulation, then please post the issue on our forum or contact us.

    Last updated: September 30th, 2021

    Contents