1. Boundary Conditions, Loading, And Rigid Bodies
Chapter 5
Boundary Conditions, Loading, And Rigid Bodies

2. Chapter Objectives
Upon completion of this chapter, students will be able to define and utilize loads, rigid bodies, and boundary conditions within the ANSYS/LS-DYNA Program
1. Give an overview of loads and boundary conditions
2. Describe how general loads are applied in ANSYS/LS-DYNA (EDLOAD)
3. Describe constraints (D, EDNROT, EDBOUND)
4. Describe initial velocities (EDVEL)
5. Define and discuss implementation of rigid bodies (EDMP,RIGID)
6. Describe rigid body loads, inertia, and constraints (EDLOAD, EDIPART, and EDCRB)
7. Describe damping controls (EDDAMP)
8. Describe the use of Spotwelds (EDWELD)
9. Given step by step guidance, the students will perform a short exercise on loading in a spotweld failure analysis
March 15, 2001
Inventory #001458
5-2

3. Loading and Boundary Conditions Overview
Unlike most implicit analyses, all loads in an explicit analysis must be applied as a function of time. The load step concept of general ANSYS does not apply.
Therefore, there is a unique procedure for applying loads in an explicit analysis using two array parameters. One array is for time and the other array is for the loading condition.
Because of the time dependence, many standard ANSYS commands (e.g., F, SF, BF) are not valid in an explicit analysis.
FORCE
TIME
Additionally, the D command cannot be used to apply loads because it is not time dependent in nature. It can only be used to apply restraints.
The coupling (CP) and constraint equation (CE) family of commands are only valid for displacement and rotation DOF’s in an explicit dynamic analysis. Exercise caution when specifying CP’s and CE’s in a large deflection analysis.
Initial velocity (EDVEL) and rigid body (EDMP, RIGID) definitions are unique to an explicit dynamic analysis.
March 15, 2001
Inventory #001458
5-3

4. General Loading Procedure
All general transient loads in ANSYS/LS-DYNA are applied using the EDLOAD command with the following three-step procedure:
STEP 1: Define nodal component
STEP 2: Define array parameters
STEP 3: Apply load using the EDLOAD command
STEP 1: Defining Nodal Components
With the exception of pressures & rigid body loads, all loads in an explicit dynamic analysis are applied to nodal components. The first step to applying loads is to select portions of a model that will receive the same loads: Utility Menu: Select->Entities->Nodes
March 15, 2001
Inventory #001458
5-4

5. (continued) General Loading Procedure
Then a nodal component is defined from the selected nodes:
Utility Menu : Select -> Comp/Assembly -> Create Component…
It is always best to give a descriptive name to the component.
Only nodal components are used in an explicit dynamic analysis. (Except for pressures)
STEP 2: Define Array Parameters
In an explicit dynamic analysis all loads are applied over a specific time interval. The time interval and their corresponding load values are grouped together and defined as array parameters.
Utility Menu : Parameters->Array Parameters ->Define/Edit -> Add
After entering the name and number of rows, select OK
March 15, 2001
Inventory #001458
5-5

6. (continued) General Loading Procedure
Then enter the corresponding time array values and select: File->Apply/Quit
Note that any time-load pair must have an identical number of data points
Loads should be applied throughout the entire solution time
An identical procedure should be followed for the corresponding load values:
March 15, 2001
Inventory #001458
5-6

7. (continued) General Loading Procedure
Step 3: Apply the load
Once the nodal component and array parameters have been defined, the load can be directly applied to the model using the EDLOAD command: Solution: Loading Options -> Specify Loads
First select the Load option Add Loads. Options are also available for listing the applied loads and deleting loads.
Then, select the desired type of load. For nodal components, the following loads are valid:
Forces: FX, FY, FZ Disp: UX, UY, UZ
Moment: MX, MY, MZ Velo: VX, VY, VZ
Rot: ROTX,ROTY,ROTZ Accel: AX,AY,AZ
Ang. Vel: OMGX, OMGY, OMGZ
Body Accel: ACLX, ACLY, ACLZ
The surface load key is used when defining pressure loads to elements. Loads can be applied in local CS (CID vector defined with EDLCS). CID not valid for LAB = PRESS, ACLX/Y/Z, OMGX/Y/Z. Local CS for input only (output in global Cartesian CS).
Select the component to which the load is applied and the time and data arrays. These arrays can be left blank if a LCID is used.
March 15, 2001
Inventory #001458
5-7

8. (continued) General Loading Procedure
STEP 3 (continued)
If the data and time arrays are left blank, a previously defined load curve LCID (via EDCURVE) can be referenced to define the load.
A SCALE factor can be used to scale the ordinate values (not the time) of the referenced LCID.
Using the LCID option eliminates the need to create duplicate load curves when the same load is applied to multiple components
Load birth and death times can be specified. Valid for UX, ROTX, VX, AX, PRESS, RBUX, RBRX, RBVX, RBOX labels (and corresponding Y & Z labels)
March 15, 2001
Inventory #001458
5-8

9. Plotting Load Curves
After a load curve has been defined, it can be plotted to ensure its accuracy using the EDPL command and a load reference number.
Load reference numbers can be obtained using the load listing box which is automatically generated when the Plot Load Curve option is selected. Solution>Loading Options...
March 15, 2001
Inventory #001458
5-9

10. Plotting Load Curves
March 15, 2001
Inventory #001458
5-10

11. Load Symbol Display
In addition to plotting load curves, loads symbols can also be displayed using the EDFPLOT command:
Solution: Loading Options -> Show Forces
March 15, 2001
Inventory #001458
5-11

12. Constraints
Unlike ANSYS Implicit, ANSYS/LS-DYNA distinguishes between zero and nonzero constraints. All nonzero constraints are handled as loads (EDLOAD).
Only zero constraints can be applied with the D command, because it is used to restrain (fix) certain portions of a model:
Solution: - Constraints - Apply
After selecting the desired nodes, the ANSYS/LS-DYNA program will automatically apply a zero constraint.
If lines or areas are selected, constraints will be directly applied to the nodes belonging to the lines or areas.
March 15, 2001
Inventory #001458
5-12

13. Constraints - Nodal Rotations
In addition to standard nodal constraints, rotated nodal coordinate constraints can be applied using the EDNROT command:
Solution: Constraints - Apply ->Rotated Nodal
Select the option Add Constraint. Options are also available for listing and deleting the defined rotated nodal coordinate constraints
Select the local coordinate system ID to which the constraint will be added (Defined with EDLCS)
Select the desired nodal component to which the load will be applied.
Select the degrees of freedom for which the rotated coordinate constraint will be applied. Up to six degrees of freedom are valid: UX, UY, UZ, ROTX, ROTY, ROTZ.
NOTE: Solution results are not given in terms of the local coordinate system defined by the EDNROT command.
March 15, 2001
Inventory #001458
5-13

14. Constraints - Boundary Planes
The features of sliding and cyclic symmetry are also available in the ANSYS/LS-DYNA program using the EDBOUND command.
Sliding and cyclic symmetry can greatly reduce model size by allowing the analysis of small symmetric sections of a complete model.
Solution: - Constraints - Apply ->-Symmetry B.C.-Bndry Plane
Select the option Add plane. Options are also available for listing and deleting the defined boundary planes
Choose sliding or cyclic symmetry
Select the desired nodal component to which the load will be applied.
Input normal coordinate vectors (sliding) or axes of rotation (cyclic)
For cyclic symmetry, a second boundary plane can be applied to a nodal component
For sliding symmetry, a constraint option is available to define whether nodes will only move normal to the plane or in a specific vector direction.
March 15, 2001
Inventory #001458
5-14

15. Constraints - Nonreflecting Boundaries
When modeling geomechanical systems, an infinite domain is often required to represent the ground.
To limit model size, nonreflecting boundaries can be used to such domains (SOLID 164 elements only).
Nonreflecting boundaries prevent artificial stress wave reflections from the boundary of a model.
To define a non-reflective boundary, first create a nodal component of the external surface of a body. Then use the EDNB command to eliminate the reflection of dilatational and shear waves along the specified component.
Solution > Constraints > Apply > Non-Refl Bndry…..
March 15, 2001
Inventory #001458
5-15

16. Initial Velocities
In transient dynamic problems, it is often necessary to define initial conditions. In ANSYS/LS-DYNA, rotational and translational initial velocities are applied to nodal components using the EDVEL command.
There are two options for defining initial velocities with the EDVLE command: 1) VGEN and 2) VELO
EDVEL,Option, …
VGEN - Option that allows rotations to be defined about a specified axis. Can not be used in a small restart.
VELO - Option where rotational velocities are applied directly to nodes within the model. This option can also be used in small restart analyses (i.e., not limited to only new analyses)
VGEN and VELO cannot both be used in same analysis
Initial Velocities can also be listed and deleted
March 15, 2001
Inventory #001458
5-16

17. Initial Velocities VGEN Option - w/Axial Rotate
Specify the node or nodal component to which the initial velocity will be applied. Options are also available for listing and deleting
Enter the translational velocity in the global x, y, z directions
Specify the angular velocity (W), the x, y , and z coordinates of the rotational axes, and the angles relative to the global X, Y, and Z axes.
Reissuing the EDVEL command on the same nodal component will overwrite previous initial velocities on that component.
If the EDDRELAX command (Chapter 11) is issued prior to the EDVEL command the velocities will be applied after stress initialization or dynamic relaxation.
March 15, 2001
Inventory #001458
5-17

18. Initial Velocities VELO Option - w/Nodal Rotate
Specify the node or nodal component to which the initial velocity will be applied. Options are also available for listing and deleting
Enter the translational velocity in the global x, y, z directions
Specify the angular velocity (W) in the global X, Y, and Z axes.
March 15, 2001
Inventory #001458
5-18

19. Rigid Bodies - Overview
Using rigid bodies to define stiff parts in a model can greatly reduce the computation time required to perform an explicit analysis.
In ANSYS/LS-DYNA, all rigid bodies have their degrees of freedom coupled to the bodies center of mass. Hence, rigid bodies have only six degrees of freedom, regardless of the number of nodes that define it.
The mass, center of mass, and inertia properties are automatically calculated by the program from the rigid bodies’ volume and density of elements. These properties can be overwritten with EDIPART.
Forces and moments acting on a rigid body are summed from nodal quantities at each time step. Motion of the body is then calculated for the center of mass and the displacements are transferred to the nodes.
Rigid bodies do not have to be linked by mesh connectivity.
Accurate values of the rigid bodies’ material properties (EX, NUXY, and DENS) are required for contact stiffness calculations.
March 15, 2001
Inventory #001458
5-19

20. Defining Rigid Bodies OK
Rigid bodies are defined in ANSYS/LS-DYNA using the EDMP command: Preprocessor: Material Properties -> Define Mat Model...->Add
Specify the Material Number that will make up the rigid body. Elements with the same MATID are in this one rigid body.
Select: Other-Rigid OK
Enter accurate values for the material properties of the rigid body
Specify the translational and rotational constraint parameters for the rigid body
March 15, 2001
Inventory #001458
5-20

21. (continued) Defining Rigid Bodies
Because constraints should be applied to the center of mass of a rigid body, it is important to input proper values for the rotational and translational constraints.
Translational Constraint Values (parallel to global Cartesian coordinates) :
0 - no global translational constraint
1 - constrain UX only
2 - constrain UY only
3 - constrain UZ only
4 - constrain UX and UY
5 - constrain UY and UZ
6 - constrain UX and UZ
7 - constrain UX, UY, and UZ
Rotational Constraint Values (parallel to global Cartesian coordinates):
0 - no global rotational constraint
1 - constrain ROTX only
2 - constrain ROTY only
3 - constrain ROTZ only
4 - constrain ROTX and ROTY
5 - constrain ROTY and ROTZ
6 - constrain ROTX and ROTZ
7 - constrain ROTX, ROTY, and ROTZ
March 15, 2001
Inventory #001458
5-21

22. Loading Rigid Bodies
Similar to nodal components, displacements and velocities are applied to rigid bodies using the EDLOAD command. All rigid body loads, however, are applied to a PART number rather than to a component name. Solution: Loading Options -> Specify Loads
Select desired type of load. For rigid bodies, the following loads are valid:
Forces: RBFX, RBFY, RBFZ
Displacement: RBUX, RBUY, RBUZ
Moment: RBMX, RBMY, RBMZ
Velocity: RBVX, RBVY, RBVZ
Rotations: RBRX, RBRY, RBRZ
Ang. Velocity: RBOX, RBOY, RBOZ
The surface load key is not used for rigid bodies
Specify the PART # for which the load is to be applied
Finally, select the corresponding time and data values. LCID and SCALE factors can also be used.
March 15, 2001
Inventory #001458
5-22

23. Merging Rigid Bodies
Two rigid bodies can be merged together so that they act as a single rigid body using the EDCRB command:
Specify the equation reference number
The PART # for the master rigid body
The Part # for the slave rigid body
Care should be taken not to issue more than one EDCRB command with the same reference number.
When merging two rigid bodies, the slave rigid body becomes absorbed into the master. Any subsequent references to the slave body are meaningless.
March 15, 2001
Inventory #001458
5-23

24. Rigid Body Part Inertia
EDIPART Manually defines inertia for existing rigid bodies
Default is to have LS-DYNA calculate rigid body inertia properties from the finite element mesh
Manually specifying properties is more accurate than the default when the object is complicated and the mesh is coarse
Allows meshing only a portion of the total structure
Parts must already be defined (EDPART,CREATE)
Preprocessor: LS-DYNA Options ->Inertia Options->Define Inertia
March 15, 2001
Inventory #001458
5-24

25. Rigid Body Part Inertia
Specify inertia properties and initial conditions
Location of center of mass (X, Y, Z)
Translational mass
Inertia tensor (IXX, IXY, IXZ, IYY, IYZ, IZZ)
Initial velocity (RBVX, RBVY, RBVZ, RBOX, RBOY, RBOZ)
March 15, 2001
Inventory #001458
5-25

26. Guidelines for Rigid Bodies
Unlike in ANSYS implicit, do not use high values of EX to stiffen a part to make it rigid. Accurate material properties are required for contact stiffness calculations.
Constraints (D command) on the nodes of a rigid body are not allowed. All constraints must be applied to the center of mass of the rigid body.
Two rigid bodies can not share a common node. Use the EDCRB command to link rigid bodies together.
Always use rigid bodies for parts of a model where the deformation results are not important. Rigid bodies save significant amounts of CPU time.
March 15, 2001
Inventory #001458
5-26

27. Damping Control
Damping is an excellent method for preventing unrealistic oscillations in the structural response in an explicit analysis.
Both mass weighted (alpha) and stiffness weighted (beta) damping can be applied to a model in ANSYS/LS-DYNA using the EDDAMP command.
Preprocessor: Material Props -> Damping ...
Specify the Part # for which the damping is to be applied. If Part=ALL, damping will be applied to the entire model
A load curve ID can be used to specify the damping vs time (EDCURVE)
A constant damping coefficient can also be applied instead of a damping vs time curve for beta damping
When Part=ALL or a Curve ID is specified, alpha damping is automatically applied to the model. Mass proportional damping is effective for low frequencies and will damp out rigid body motion.
When Curve ID = 0 and a damping constant is specified, beta damping is used for the specified Part. Stiffness damping is effective for high frequency oscillations.
March 15, 2001
Inventory #001458
5-27

28. Spotwelds Specify a weld reference ID
Spotwelds are similar to constraint equations between two nodes having rotary inertia. The connection between the nodes is mass-less and rigid. The nodes must not be coincident and cannot have any other constraints applied to them.
A failure force can be defined to model failure along a Spotweld connection. Preprocessor: LS-DYNA Optns ->Spotweld->Create
Specify a weld reference ID
Select the nodes to which the Spotweld will be applied
Specify the normal and shear failure forces, along with the exponents EXPn and EXPs that define failure:
March 15, 2001
Inventory #001458
5-28

29. Plotting Spotwelds Symbol shows rigid beam
Spot weld (EDWELD command) symbols verify that constraints have been applied correctly.
The WELD field has been added to the /PBC command to show rigid beam constraints between two nodes that are not coincident.
Symbol shows rigid beam
March 15, 2001
Inventory #001458
5-29

30. Spotweld Failure Exercise
The exercise for this chapter begins on page E5-1 of Volume II.
A spotweld failure mechanism is demonstrated.
March 15, 2001
Inventory #001458
5-30