6.1. Drop Test of a Container (Explicit Dynamics)

6.1.1. Problem Specification

Applicable Products: ANSYS LS-DYNA
Level of Difficulty: Moderate
Interactive Time Required: 60 to 90 minutes
Discipline: Structural
Analysis Type: Transient dynamics (explicit method)
Element Types Used: SHELL163
Features Demonstrated: Direct generation of nodes and elements, array parameters, automatic meshing, animation
Help Resources: The ANSYS LS-DYNA User's Guide, SHELL163.

6.1.2. Problem Description

This is a dynamic analysis problem. It consists of dropping an aluminum container on a steel table top:

  • The container is a five-sided square box, 20 inches on all sides and 0.1 inches thick. It has been rotated 45o about each of the X, Y, and Z axes.

  • The table top is a square steel plate 100 inches on each side and 0.1 inches thick.

  • The only force acting on the box is its own weight.

  • The box is dropped from a distance of 72 inches.

Objective: Demonstrate the explicit dynamics capabilities of ANSYS LS-DYNA, ideal for large-deformation and complex-contact dynamic problems.

6.1.2.1. Given

The dimensions of the container and table top are shown above. The container is made of aluminum alloy with Young's modulus of 10.3E6 psi, density of 2.5E-4 lbf-sec2/in4, Poisson's ratio of 0.334, Yield Stress of 5,000 psi, and a tangent modulus of 20,000 psi. The table top is made of carbon steel with Young's modulus of 30.0E6 psi, density of 7.3E-4 lbf-sec2/in4, and Poisson's ratio of 0.292.

6.1.2.2. Approach and Assumptions

During the free-fall stage, the container is simply accelerating due to gravity. To save CPU time, start the analysis at 20 inches above the table top and apply an initial velocity of 200 inches per second to simulate the first 52 inches of free fall. 200 inches per second is an approximation derived using Vf = SQRT (2*a*s) where Vf is the final velocity, a is the acceleration due to gravity, and s is the displacement. Friction from the air is ignored.

Assume a rigid behavior for the table top and bilinear kinematic hardening with von Mises plasticity for the container.

Solid modeling is used to generate the 3-D model of the container, which is then meshed. Direct generation of nodes and elements is used to model the table top. The table top is modeled as a rigid element; only one element is used to represent it.

6.1.2.3. Summary of Steps

Use the information in the problem description and the steps below as a guideline in solving the problem on your own. Or, use the detailed interactive step-by-step solution by selecting the link for step 1.

Define Analysis Type

1. Set preferences.

Input Geometry

2. Read in geometry of the container.

Define Element Type, Real Constants, Material Model Properties

3. Define element type.

4. Define real constants.

5. Specify material models.

Generate Mesh

6. Mesh the container.

7. Generate table top elements.

8. Create container component.

9. Create table top component.

10. Specify contact parameters.

Apply Loads

11. Apply initial velocity to the container.

12. Apply acceleration to the container.

Obtain Solution

13. Specify Output Controls.

14. Solve.

Review Results

15. Animate stress contours.

16. Animate deformed shape.

17. Exit the program.

6.1.3. Define Analysis Type

6.1.3.1. Step 1: Set Preferences.

Set preferences to filter quantities that pertain to this discipline only.

  1. Main Menu> Preferences

  2. (check) “Individual discipline(s) to show in the GUI” = Structural

  3. (check) “Discipline options” = LS-DYNA Explicit

  4. [OK]

6.1.4. Input Geometry

6.1.4.1. Step 2: Read in geometry of the container.

Read in a file that includes the model of the container.

  1. Utility Menu> File> Read Input from ...

  2. File name: container.inp

    Linux version:

    /ansys_inc/v182/ansys/data/models/container.inp

    PC version:

    \Program Files\ANSYS Inc\V182\ANSYS\data\models\container.inp

  3. [OK]

6.1.5. Define Element Type, Real Constants, Material Model Properties

6.1.5.1. Step 3: Define element type.

Because the model is a container made of thin walls hitting the surface of a table, shell elements are used to simulate the physical model. In this case, use SHELL163, an explicit thin structural shell; this 4-node element supports both in-plane and normal loads.

  1. Main Menu> Preprocessor> Element Type> Add/Edit/Delete

  2. [Add...]

  3. “LS-DYNA Explicit” (left column)

  4. “Thin Shell 163” (right column)

  5. [OK]

    Now, specify the S/R corotational Hughes-Liu element formulation to eliminate certain hourglass modes.

  6. [Options...]

  7. (drop down) “Element Formulation” = S/R corotation

  8. [OK]

  9. [Close]

6.1.5.2. Step 4: Define real constants.

Define the thickness of the shell elements by defining the appropriate real constant.

  1. Main Menu> Preprocessor> Real Constants

  2. [Add...]

  3. [OK] to select element Type 1 for SHELL163.

  4. [OK] to define real constant set No. 1.

  5. “SHRF” = 1

  6. “NIP” = 2 (For demonstration purposes in this tutorial, the default value of 2 is sufficient. However, for most nonlinear analyses, the NIP should be set higher than 2.)

  7. “T1” = 0.1

  8. “T2” = 0.1

  9. “T3” = 0.1

  10. “T4” = 0.1

  11. “NLOC” = Mid surface

  12. [OK]

  13. [Close]

6.1.5.3. Step 5: Specify material models.

Specify material models for the contact and target surfaces.

  1. Main Menu> Preprocessor> Material Props> Material Models

  2. (double-click) “LS-DYNA”, then “Rigid Material” to specify the table top, which is “Material Model Number 1”.

  3. “DENS” = 7.3e-4

  4. “EX” = 30e6

  5. “NUXY” = 0.292

  6. (drop down) “Translational Constraint Parameter” = All disps.

  7. (drop down) “Rotational Constraint Parameter” = All rotations

  8. [OK]

  9. Material> New Model to specify the material for the container, which is “Material Model Number 2”.

  10. “Define Material ID” = 2

  11. [OK]

  12. (double-click) “Nonlinear”, then “Inelastic”, then “Kinematic Hardening”, then “Bilinear Kinematic”

  13. “DENS” = 2.5e-4

  14. “EX” = 10.3e6

  15. “NUXY” = 0.334

  16. “Yield Stress” = 5000

  17. “Tangent Modulus” = 20000

  18. [OK]

  19. Material> Exit

  20. Toolbar: SAVE_DB

6.1.6. Generate Mesh

6.1.6.1. Step 6: Mesh the container.

In an explicit solver, such as ANSYS LS-DYNA, analysis time is highly dependent on the smallest element in the model. To obtain results efficiently, therefore, use a uniform element size.

In this case, select the default element size, which should give a 3x3 mesh on each face of the container.

  1. Main Menu> Preprocessor> Meshing> MeshTool

  2. (drop down) “Element Attributes” = Global; then [Set]

  3. (drop down) “Material number” = 2

  4. [OK]

  5. (drop down) “Mesh” = Areas

  6. (check) “Mapped”

  7. [Mesh]

  8. [Pick All]

  9. Toolbar: SAVE_DB

6.1.6.2. Step 7: Generate table top elements.

Mesh the table top by direct element generation. The table top is defined as a rigid surface, so only one element is needed to model the surface. Create the model by defining its four corner nodes, then building the elements from those nodes.

  1. Utility Menu> PlotCtrls> Pan, Zoom, Rotate

  2. [Obliq]

  3. [Close]

  4. Utility Menu> PlotCtrls> Numbering

  5. (check) “Node numbers” = On

  6. [OK]

  7. (drop down in MeshTool) “Element Attributes” = Global; then [Set]

  8. (drop down) “Material number” = 1

  9. [OK]

  10. [Close] MeshTool

  11. Main Menu> Preprocessor> Modeling> Create> Nodes> In Active CS

  12. “Node number” = Leave blank so it defaults to the next available node number.

  13. “X Y Z Location in active CS” = -50, -20, -50

  14. [Apply] to generate the node in the far left corner.

  15. “X Y Z Location in active CS” = -50, -20, 50

  16. [Apply] to generate the node in the near left corner.

  17. “X Y Z Location in active CS” = 50, -20, 50

  18. [Apply] to generate the node in the near right corner.

  19. “X Y Z Location in active CS” = 50, -20, -50

  20. [OK] to generate the node in the far right corner.

    Now create the element.

  21. Main Menu> Preprocessor> Modeling> Create> Elements> Auto Numbered> Thru Nodes

  22. In a counterclockwise direction, pick the four nodes just created.

  23. [OK]

  24. Utility Menu> Plot> Elements

6.1.6.3. Step 8: Create container component.

Most contact algorithms require contact parameters, which can be components, part IDs, or part assembly IDs. In this case, create a component made of nodes from the container.

  1. Utility Menu> Select> Entities

  2. (first drop down) “Elements”

  3. (second drop down) “By Attributes”

  4. (check) “Material num”

  5. “Min,Max,Inc.” = 2

  6. [Apply]

  7. (first drop down) “Nodes”

  8. (second drop down) “Attached to”

  9. (check) “Elements”

  10. [OK]

  11. Utility Menu> Select> Comp/Assembly> Create Component

  12. “Component name” = BOX

  13. (drop down) “Component is made of” = Nodes

  14. [OK]

  15. Utility Menu> Plot> Nodes

  16. Utility Menu> Select> Everything

6.1.6.4. Step 9: Create table top component.

Create a component made of nodes from the table top.

  1. Utility Menu> Select> Entities

  2. (first drop down) “Elements”

  3. (second drop down) “By Attributes”

  4. (check) “Material num”

  5. “Min,Max,Inc” = 1

  6. [Apply]

  7. (first drop down) “Nodes”

  8. (second drop down) “Attached to”

  9. (check) “Elements”

  10. [OK]

  11. Utility Menu> Select> Comp/Assembly> Create Component

  12. “Component name” = TABLE

  13. (drop down) “Component is made of” = Nodes

  14. [OK]

  15. Utility Menu> Plot> Nodes

  16. Utility Menu> Select> Everything

  17. Toolbar: SAVE_DB

6.1.6.5. Step 10: Specify contact parameters.

In an analysis where the contact behavior is known, an appropriate contact algorithm can be selected for the best results. Due to the nature of this problem, however, contact conditions are unpredictable. By selecting automatic surface-to-surface contact, the program automatically adjusts for changing contact behavior during the simulation.

  1. Main Menu> Preprocessor> LS-DYNA Options> Contact> Define Contact

  2. “Contact Type” = “Surface to Surf” (left column); “Automatic (ASTS)” (right column)

  3. [OK]

  4. (drop down) “Contact Component or Part no.” = BOX

  5. (drop down) “Target Component or Part no.” = TABLE

  6. [OK]

  7. Toolbar: SAVE_DB

6.1.7. Apply Loads

6.1.7.1. Step 11: Apply initial velocity to the container.

  1. Main Menu> Solution> Initial Velocity> On Nodes> w/Nodal Rotate

  2. (drop down) “Input velocity on component” = BOX

  3. “Global (Translational) Y-component” = -200

  4. [OK]

    In a transient dynamic analysis, loads must be defined for the duration of the analysis. To do so, create an array containing this data.

  5. Utility Menu> Parameters> Array Parameters> Define/Edit

  6. [Add...]

  7. “Parameter name” = TIME

  8. [OK]

  9. [Edit...]

  10. “1” = 0

  11. “2” = 1

  12. File> Apply/Quit

  13. [Add...]

  14. “Parameter name” = ACCG

  15. [OK]

  16. (highlight) “ACCG”

  17. [Edit...]

  18. “1” = 386.4

  19. “2” = 386.4

  20. File> Apply/Quit

  21. [Close]

6.1.7.2. Step 12: Apply acceleration to the container.

  1. Main Menu> Solution> Loading Options> Specify Loads

  2. “Load Labels” = ACLY

  3. (drop down) “Component name or PART number:” = BOX

  4. (drop down) “Parameter name for time values:” = TIME

  5. (drop down) “Parameter name for data values:” = ACCG

  6. [OK]

6.1.8. Obtain Solution

6.1.8.1. Step 13: Specify output controls.

  1. Main Menu> Solution> Time Controls> Solution Time

  2. “Terminate at Time:” = 1.0

  3. [OK]

  4. Main Menu> Solution> Output Controls> File Output Freq> Number of Steps

  5. “Specify Results File Output Interval” = 50

  6. “Specify Time History Output Interval” = 50

  7. [OK]

  8. Main Menu> Solution> Analysis Options> Energy Options

  9. [OK] to turn on all energy options

  10. Toolbar: SAVE_DB

6.1.8.2. Step 14: Solve.

  1. Main Menu> Solution> Solve

  2. Review the information in the status window, then select:

    File> Close (Windows) or

    Close (Linux), to close the window.

  3. [OK] to initiate solution.

    A verification window appears notifying you of a warning message. The warning is generated because you constrained the table top by defining it as a rigid element rather than by using degree-of-freedom constraints. You can therefore ignore the warning.

  4. [Yes]

  5. [Close]

6.1.9. Review Results

6.1.9.1. Step 15: Animate stress contours.

  1. Utility Menu> Plot> Elements

  2. Utility Menu> PlotCtrls> Pan, Zoom, Rotate

  3. [Front]

  4. [Close]

  5. Utility Menu> PlotCtrls> Numbering

  6. (check) “Node numbers” = Off

  7. [OK]

  8. Main Menu> General Postproc> Read Results> First set

    Linux users: To capture the animation sequence in terminal segment memory, reduce the size of the Graphics Window or you will run out of terminal memory. For this analysis, use a ratio of 3:1 for the original window size to the reduced window size.

  9. Utility Menu> PlotCtrls> Animate> Over Results

  10. (check) “Auto contour scaling” = On (Make sure that the box is checked.)

  11. “Contour data for animation” = Stress (left column); von Mises SEQV (right column)

  12. [OK]

  13. Make selections in the Animation Controller (not shown), if necessary, then [Close].

6.1.9.2. Step 16: Animate deformed shape.

  1. Utility Menu> PlotCtrls> Animate> Over Results

  2. (check) “Auto contour scaling” = On

  3. “Contour data for animation” = DOF Solution (left column); Deformed Shape (right column)

  4. [OK]

  5. Make selections in the Animation Controller (not shown), if necessary, then [Close].

6.1.9.3. Step 17: Exit the program.

  1. Toolbar: Quit

  2. (check) “Quit - No Save!”

  3. [OK]

Although you have exited the Mechanical APDL program, you can still view animations via the ANIMATE program. The program runs only on Windows computers and is useful for:

  • Viewing Mechanical APDL animations on a Windows computer regardless of whether the files were created in Windows (AVI files) or Linux (ANIM files).

  • Converting ANIM files to AVI files.

  • Sending animations via email or sharing via the Web.


Release 18.2 - © ANSYS, Inc. All rights reserved.