The first step in an explicit dynamic analysis is to create the model that will represent the physical system to be analyzed. Use the PREP7 Preprocessor to build the model.
If you perform your analysis through the ANSYS graphical user interface (GUI), it is important to first set the Preferences options () to “LS-DYNA Explicit” so that menus are properly filtered to show explicit dynamics input options. (Note that setting the preference to LS-DYNA explicit does not activate an LS-DYNA solution. To do so, you must specify an explicit element type such as SHELL163.)
Once you have set the analysis preference, you can build the model as you normally would for any analysis type. First, enter the preprocessor by issuing the /PREP7 command or by picking in the GUI. In the preprocessor, perform the following tasks:
Define the element types and real constants
Specify material models
Define the model geometry
Mesh the model
Define contact surfaces
If you have never used an ANSYS product before, you should review the Basic Analysis Guide and the Modeling and Meshing Guide to learn the general procedures used to build a model in ANSYS.
Element types available for an explicit dynamic analysis are described briefly in Elements. More detailed descriptions of each explicit element can be found in the Element Reference. It is recommended that you read these descriptions carefully before deciding which element types to use in your model.
Once you have chosen appropriate elements to represent your physical system, you specify element types using the ET command (or in the GUI pick ).
Each element description in the Element Reference lists all real constants that are associated with the element. You must determine which real constants (if any) are required for each element type you include in the model. Then specify the real constants using the R command (or in the GUI pick ).
There are numerous material models available for use in an explicit dynamic analysis. You should refer to the element descriptions in the Element Reference to find out which material models are valid for a particular element. Also, review Material Models of this document, which contains detailed descriptions for all of the available material models.
Once you have decided which material model (or models) to use in your analysis, you must define all of the properties associated with the model (as described in Material Models). To do so in batch or command mode, you typically use the MP, TB, and TBDATA commands (and in some cases, the EDMP command). Temperature dependent models may also require the MPTEMP, MPDATA, and TBTEMP commands. In the GUI, material models are defined via the following menu path:
After you select the appropriate material model, you will be prompted to define the necessary properties for that model. See Defining Explicit Dynamics Material Models for more information on defining material models through the GUI.
In order to specify an orthotropic model that is not aligned with the global Cartesian coordinate system, you must first define the local coordinate system with the EDLCS command (menu path: .)
For some material models, you may also need to use the EDCURVE command to define data curves associated with the material (e.g., a stress-strain curve). (To access EDCURVE in the GUI, pick: .)
The easiest way to create the model geometry is with the solid modeling capabilities of the ANSYS program. Refer to Solid Modeling in the Modeling and Meshing Guide for detailed information on all solid modeling functions.
For simple models (e.g., line elements only), you may choose to use the direct generation modeling method. By this method, you define the nodes and elements of the model directly. See Direct Generation in the Modeling and Meshing Guide for details.
After building the solid model, you are ready to mesh the model with nodes and elements. The procedure for generating the mesh is outlined in Generating the Mesh in the Modeling and Meshing Guide. If you are not familiar with ANSYS meshing, you should review that chapter before meshing an explicit dynamics model. Since all of the details are contained in that chapter, we will discuss only a few key points in this section.
Meshing involves three main steps:
Set the element attributes
Set mesh controls
Generate the mesh
To set the element attributes, you specify which previously defined element type, real constant set, and material property set to use for subsequent meshing. Use the TYPE, MAT, and REAL commands, or menu paths:
Mesh controls allow you to indicate the general size and shape of elements to use during meshing. There are numerous mesh controls available in the ANSYS program (see the Modeling and Meshing Guide for details). In the GUI, these controls are accessed by picking .
Keep the following points in mind when choosing mesh controls:
Avoid degenerate shell and solid element shapes (such as a triangular shell or a tetrahedral solid). They are generally too stiff and less accurate than quadrilateral and hexahedral shapes.
Try to achieve a mesh with uniform element sizes (i.e., avoid areas with relatively small elements). A large difference in element sizes can cause a small minimum time step size and, therefore, a long run time. If a relatively few number of small elements are required to mesh a particular geometry, mass scaling (see Mass Scaling) can be used to increase the minimum time step.
Do not use the SmartSizing method of element size control (SMRTSIZE command), which can create a large variation in element sizes within the mesh. Instead, use the ESIZE and related commands to control element sizes.
Avoid poorly shaped elements which can cause hourglassing.
Do not make the mesh too coarse when reduced element formulations are used, or elements may experience hourglassing.
If hourglassing is a problem, try to use fully integrated elements in a part of the model or in the entire model.
After specifying the desired mesh controls, mesh the model using typical meshing commands (AMESH, VMESH, etc.). In the GUI, meshing functions are accessed by picking or via the Mesh Tool ().
An explicit dynamic analysis often includes contact between surfaces. Contact Surfaces of this document describes the types of contact available and the procedure to define contact. A brief overview of that procedure is given here.
Defining contact involves four basic steps:
Determine the type of contact which best defines the physical model (EDCGEN command)
Identify contact surfaces (CM, or EDPART, or EDASMP commands, with the EDCGEN command)
Specify friction coefficient parameters (EDCGEN command)
Specify additional input required for the chosen contact type (EDCGEN and EDCONTACT commands)
If automatic contact is not being used, you must define contact surfaces by grouping the nodes on each surface into a component with the CM command. Once these components are created, use the EDCGEN command to specify contact between the desired surfaces (i.e., node components). You must also identify the type of contact with the EDCGEN command. For the single surface contact algorithms, the outer surfaces of the contacting bodies are determined by ANSYS LS-DYNA.
Note: Contact surfaces can alternatively be identified by a PART number (using EDPART), or by an assembly of parts (using EDASMP) rather than by a node component. Part and assembly definitions are discussed in The Definition of Part.
The EDCGEN command is also used to specify friction coefficient parameters and other input specific to different contact types. Another command, EDCONTACT is used to specify miscellaneous contact controls such as contact penetration checking and sliding interface penalties. (Contact options are found in the GUI under .)
The following are guidelines that you should consider when planning your explicit dynamics model:
Use rigid bodies whenever possible to represent relatively stiff, unyielding objects in the model. Using rigid bodies simplifies the solution and results in shorter run times. (See Rigid Bodies for information on defining rigid bodies.)
Use realistic values for material properties. For example, do not use an unrealistically high elastic modulus to represent a rigid body, and do not use unrealistic thickness values for shell elements.
Consider using damping (EDDAMP command) to prevent unrealistic oscillations in your model’s structural response. Refer to the EDDAMP command description in the Command Reference for detailed information.
If you have performed 2-D dynamic analyses with the regular ANSYS program, consider extruding these models to 3-D and analyzing them with ANSYS LS-DYNA. You may achieve more accurate results in a shorter run time.
Note that the submodeling and substructuring features of the ANSYS program cannot be used in ANSYS LS-DYNA.