| 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. |
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.
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.
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.
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.
2. Read in geometry of the container.
7. Generate table top elements.
8. Create container component.
9. Create table top component.
10. Specify contact parameters.
11. Apply initial velocity to the container.
12. Apply acceleration to the container.
14. Solve.
Set preferences to filter quantities that pertain to this discipline only.
(check) “Individual discipline(s) to show in the GUI” = Structural
(check) “Discipline options” = LS-DYNA Explicit
[OK]
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.
[Add...]
“LS-DYNA Explicit” (left column)
“Thin Shell 163” (right column)
[OK]
Now, specify the S/R corotational Hughes-Liu element formulation to eliminate certain hourglass modes.
[Options...]
(drop down) “Element Formulation” = S/R corotation
[OK]
[Close]
Define the thickness of the shell elements by defining the appropriate real constant.
[Add...]
[OK] to select element Type 1 for SHELL163.
[OK] to define real constant set No. 1.
“SHRF” = 1
“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.)
“T1” = 0.1
“T2” = 0.1
“T3” = 0.1
“T4” = 0.1
“NLOC” = Mid surface
[OK]
[Close]
Specify material models for the contact and target surfaces.
(double-click) “LS-DYNA”, then “Rigid Material” to specify the table top, which is “Material Model Number 1”.
“DENS” = 7.3e-4
“EX” = 30e6
“NUXY” = 0.292
(drop down) “Translational Constraint Parameter” = All disps.
(drop down) “Rotational Constraint Parameter” = All rotations
[OK]
to specify the material for the container, which is “Material Model Number 2”.
“Define Material ID” = 2
[OK]
(double-click) “Nonlinear”, then “Inelastic”, then “Kinematic Hardening”, then “Bilinear Kinematic”
“DENS” = 2.5e-4
“EX” = 10.3e6
“NUXY” = 0.334
“Yield Stress” = 5000
“Tangent Modulus” = 20000
[OK]
Toolbar: SAVE_DB
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.
(drop down) “Element Attributes” = Global; then [Set]
(drop down) “Material number” = 2
[OK]
(drop down) “Mesh” = Areas
(check) “Mapped”
[Mesh]
[Pick All]

Toolbar: SAVE_DB
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.
[Obliq]
[Close]
(check) “Node numbers” = On
[OK]

(drop down in MeshTool) “Element Attributes” = Global; then [Set]
(drop down) “Material number” = 1
[OK]
[Close] MeshTool
“Node number” = Leave blank so it defaults to the next available node number.
“X Y Z Location in active CS” = -50, -20, -50
[Apply] to generate the node in the far left corner.
“X Y Z Location in active CS” = -50, -20, 50
[Apply] to generate the node in the near left corner.
“X Y Z Location in active CS” = 50, -20, 50
[Apply] to generate the node in the near right corner.
“X Y Z Location in active CS” = 50, -20, -50
[OK] to generate the node in the far right corner.
Now create the element.
In a counterclockwise direction, pick the four nodes just created.

[OK]

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.
(first drop down) “Elements”
(second drop down) “By Attributes”
(check) “Material num”
“Min,Max,Inc.” = 2
[Apply]
(first drop down) “Nodes”
(second drop down) “Attached to”
(check) “Elements”
[OK]
“Component name” = BOX
(drop down) “Component is made of” = Nodes
[OK]

Create a component made of nodes from the table top.
(first drop down) “Elements”
(second drop down) “By Attributes”
(check) “Material num”
“Min,Max,Inc” = 1
[Apply]
(first drop down) “Nodes”
(second drop down) “Attached to”
(check) “Elements”
[OK]
“Component name” = TABLE
(drop down) “Component is made of” = Nodes
[OK]

Toolbar: SAVE_DB
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.
“Contact Type” = “Surface to Surf” (left column); “Automatic (ASTS)” (right column)
[OK]
(drop down) “Contact Component or Part no.” = BOX
(drop down) “Target Component or Part no.” = TABLE
[OK]
Toolbar: SAVE_DB
(drop down) “Input velocity on component” = BOX
“Global (Translational) Y-component” = -200
[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.
[Add...]
“Parameter name” = TIME
[OK]
[Edit...]
“1” = 0
“2” = 1
[Add...]
“Parameter name” = ACCG
[OK]
(highlight) “ACCG”
[Edit...]
“1” = 386.4
“2” = 386.4
[Close]
“Terminate at Time:” = 1.0
[OK]
“Specify Results File Output Interval” = 50
“Specify Time History Output Interval” = 50
[OK]
[OK] to turn on all energy options
Toolbar: SAVE_DB
Review the information in the status window, then select:
(Windows) or
(Linux), to close the window.

[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.
[Yes]
[Close]
[Front]
[Close]
(check) “Node numbers” = Off
[OK]

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.
(check) “Auto contour scaling” = On (Make sure that the box is checked.)
“Contour data for animation” = Stress (left column); von Mises SEQV (right column)
[OK]

Make selections in the Animation Controller (not shown), if necessary, then [Close].
(check) “Auto contour scaling” = On
“Contour data for animation” = DOF Solution (left column); Deformed Shape (right column)
[OK]

Make selections in the Animation Controller (not shown), if necessary, then [Close].
Toolbar: Quit
(check) “Quit - No Save!”
[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.