Before initiating the solution, you will need to apply constraints to your model. Additionally, you may wish to set initial velocities for moving objects.
Unlike the ANSYS implicit program, ANSYS LS-DYNA does distinguish between zero and nonzero constraints. Nonzero constraints are handled as loads (together with a load curve; see earlier discussion in this chapter). Only zero constraints can be applied with the D command, i.e., the value specified must always be 0 (zero). No other values are valid, as the D constraints are only used to fix certain portions of the model. You may use symmetry/antisymmetry boundary conditions to apply these “zero” constraints.
You can use the EDNROT command to apply zero constraints in terms of a rotated nodal coordinate system. You must first define the local coordinate system with the EDLCS command.
When modeling small symmetric sections of a geometry, you may need to define sliding or cyclic symmetry. You can use the EDBOUND command to define symmetry boundary planes for sliding or cyclic symmetry. You use nodal components to identify the boundaries and a direction vector to define a normal (sliding symmetry) or axis of rotation (cyclic symmetry).
Various other types of constraints can be modeled in ANSYS LS-DYNA using the EDCNSTR command. The available constraint types are extra node set (ENS), nodal rigid body (NRB), shell edge to solid (STS), and rivet (RIVET). In the GUI, you access these constraints by picking:
The extra node set constraint type (EDCNSTR,ADD,ENS) allows the addition of nodes (via a nodal component) to an existing rigid body that was defined with the EDMP command. The nodal component that is added must not be attached to any other rigid body. The extra nodes that are added to a rigid body may be located anywhere in the model, and may have coordinates outside those of the original rigid body. The ENS option has many potential applications, including placing nodes where joints will be attached between rigid bodies, defining nodes where point loads will be applied, and defining a lumped mass at a specific location.
Unlike typical rigid bodies that are defined with the EDMP command, nodal rigid bodies defined with the EDCNSTR,ADD,NRB command are not associated with a part number, but are based on a node component. The NRB option can be advantageous when modeling rigid (welded) joints in a model. For a rigid joint, portions of different flexible components (having different MAT IDs) act together as a rigid body. It is difficult to define this type of rigid body with a unique MAT ID (and corresponding part number). However, the rigid joint can be easily defined using a nodal rigid body. Because nodal rigid bodies are not associated with a part number, other options that use rigid bodies (such as loads applied with the EDLOAD command ) cannot be used with a nodal rigid body.
The shell to solid edge option (EDCNSTR,ADD,STS) ties regions of solid elements to regions of shell elements. As shown in Figure 4.1: Constrained Shell to Solid, a single shell node may be tied to up to nine solid nodes that define a 'fiber' vector. The solid element nodes that define the fiber remain linear (straight) throughout the analysis but can move relative to each other in the fiber direction. The shell node must be coincident with one of the solid element nodes along the fiber.
Similar to spotwelds defined with the EDWELD command, the RIVET option (EDCNSTR,ADD,RIVET) defines a massless rigid constraint between two nodes that are noncoincident. Unlike a spotweld, however, failure cannot be specified for a rivet. When a rivet is defined, the distance between the nodes is kept constant throughout any motion that occurs during a simulation. Nodes connected by a rivet cannot be part of any other constraints specified in the model.
In an explicit dynamic analysis, it is common to model components that are physically welded together. This is especially true in automotive applications where parts are often assembled using welds. In such cases, welded constraints can be modeled in ANSYS LS-DYNA using the EDWELD command. Two different types of welds can be modeled: massless spotwelds and generalized welds. Nodes connected by the EDWELD command cannot be constrained in any other way.
For a massless spotweld, you must specify two noncoincident nodes. You can define failure within the spotweld by inputting failure parameters on the EDWELD command. This failure is based on the following relationship:
In the GUI, use the following menu path to define a massless spotweld:
A generalized weld is typically used to model a long-welded section of two parts. For a generalized weld, you must specify a valid nodal component. Coincident nodes are permitted. However, if you use coincident nodes, you must specify a local coordinate system (EDLCS) which will be used for output data. Failure within the generalized weld is also defined with the failure parameters on the EDWELD command using the same relationship as shown in the equation above.
In the GUI, use the following menu path to define a generalized weld:
In transient dynamic simulations, it is often necessary to specify initial conditions. In the ANSYS LS-DYNA program, initial velocities are defined using the EDVEL and EDPVEL commands. You can use these commands to apply both translational and rotational velocities to various entities. Use EDVEL to apply velocities to a nodal component or to a single node; use EDPVEL to apply velocities to a part or part assembly.
The EDVEL and EDPVEL commands provide two
methods for specifying rotational velocities, Option =
VGEN and Option = VELO. The VGEN method applies a rigid
body rotation to an entity (node component, part, etc.) around a specified axis. The
VELO method applies the rotational velocities directly to each node's rotation
degree of freedom. Since only shell and beam elements have rotation degrees of
freedom, the rotations input with the VELO method are only applicable to
SHELL163 and BEAM161 elements.
For both the VGEN and VELO methods, the translational velocities are always defined
relative to the global Cartesian coordinate system.
Note: To model a rotating body, with or without translations, you should use
Option = VGEN since this method applies a rigid
body rotation.
Due to the LS-DYNA architecture, the two methods for defining initial velocities,
Option = VELO and Option = VGEN, cannot be used in the
same analysis.
To define an initial velocity, use the following procedure:
Define the entity to which you want to apply the initial velocity. This may be a single node, a nodal component [CM], a part [EDPART], or a part assembly [EDASMP].
Decide whether the VELO or VGEN option is appropriate for your application.
Specify the initial velocity [EDVEL or EDPVEL] by using one of the following menu paths in the GUI:
For either the VELO or the VGEN option, input the translational velocities
relative to the global Cartesian coordinate system (VX,
VY, and VZ fields on the
EDVEL or EDPVEL command). For the VELO
option, input the nodal rotations in terms of the global Cartesian coordinate system
(OMEGAX, OMEGAY, and
OMEGAZ fields). For the VGEN option, input the
magnitude of the angular velocity (OMEGAX), the
coordinate axis for rotation (XC,
YC, and ZC fields) and
directional angles (ANGX,
ANGY, and ANGZ fields)
relative to the global X, Y, and Z axes.
If you do not specify initial velocities using EDVEL or
EDPVEL, all initial velocities in the model will be zero.
Likewise, if you only specify the Cname field on the
EDVEL command (e.g.,
EDVEL,VGEN,Cname) or the
PID field on the EDPVEL command,
(e.g., EDPVEL,VGEN,PID), zero initial
velocities will be applied since the remaining fields on these two commands default
to zero.
If you wish to change an initial velocity previously specified using EDVEL, just respecify a new velocity with the same component name or node number. This new value will overwrite the old data for the component or node. To list or delete initial velocities previously applied to node components or nodes, use the EDVEL,LIST and EDVEL,DELE commands (in the GUI, use and ).
Similarly, if you wish to change an initial velocity previously specified using EDPVEL, just respecify a new velocity with the same part or part assembly ID number. This new value will overwrite the old data for the part or part assembly. To list or delete initial velocities previously applied to parts or part assemblies, use the EDPVEL,LIST and EDPVEL,DELE commands (in the GUI, use and ).
For our baseball example, the initial velocity of the baseball would be specified as follows:
edvel,velo,ball,,,-1600.0 ! Component ball initially moving
! in -Z direction at 1600 in/secOr, assuming the component ball was part number 1 in the model, you could specify the velocity of the baseball as:
edpvel,velo,1,,,-1600.0 ! Part number 1 initially moving ! in -Z direction at 1600 in/sec