Unlike most implicit analyses, all loads in an explicit analysis must be time-dependent in nature. Hence, when using ANSYS LS-DYNA, many of the standard ANSYS commands are not valid. In particular, the F, SF, and BF family of commands are not applicable in ANSYS LS-DYNA because they can only be used to specify time-independent loads. Additionally, the D command can only be used to define constrained nodes. For this reason, all loads in ANSYS LS-DYNA are applied using a pair of array parameters, one corresponding to the time and the other corresponding to the loading condition.
Note: Although nodal accelerations (AX, AY, AZ) and nodal velocities (VX, VY, VX) appear as degrees of freedom, they are not physical DOFs and cannot be constrained with the D command. To apply these nodal loads, use the EDLOAD command.
In ANSYS LS-DYNA, all loads are applied in one load step. This is much different from an implicit analysis where loads are often applied in multiple steps. In ANSYS LS-DYNA, for certain kinds of loads, you can also specify when a load is imposed on a body (birth time), and when the load is removed (death time) using the EDLOAD command. Please refer to Birth Time, Death Time, and CID Support in the EDLOAD command to check the applicability of the birth/death time.
To apply a load to your model, you will need to follow these steps:
Designate portions of the model that will receive the load as components (or parts, for rigid bodies)
Define array parameters containing time intervals and load data values
Specify load curves
Define the load direction using the EDLCS command if the load is not acting in the global coordinate system
Apply loads to the model
With the exception of loads on rigid bodies, all loads are applied to components in an explicit analysis. Therefore, the first step in applying loads is to gather portions of your model into nodal or element groups called components. Each component should consist of those portions of the model that will receive the same loads and that are related to each other through such things as material properties, position in the model, expected behavior, etc.
For example, if you want to analyze a baseball being hit into a wall, you would probably define the nodes of the ball as one component, the nodes on the bat as another component, and the nodes on the wall as a third component.
You may define as many components as you wish, and then apply loads to each of them. The components must consist of either nodes or elements. (Components consisting of elements are only used when applying pressure loads.) To define a component, you must first select only those entities that you want to be included in the component. Then use the CM command or the following menu path in the GUI to define the component: .
See Selecting and Components in the Basic Analysis Guide for more information on components.
For the case of rigid bodies, loads are applied to a specific part number rather than to components. This is due to the fact that rigid bodies already consist of a specific set of nodes and elements as defined by the command EDMP,RIGID,MAT.
It is important to remember that in an explicit dynamic analysis the loading is applied to the structure over a specified time interval. This is done so that you may observe the model's transient behavior for applied loads over the specific time period. Therefore, you will not only define what type of load you would like to apply to your model (FX, FY, FZ, ROTX, ROTY, ROTZ, etc.), but also the time history of the load for the time interval of interest.
Time intervals and their corresponding load values are grouped together and defined as array parameters. These array parameters should be defined in sets of two, with each entry of the first array specifying a time value, and each entry of the second array specifying a load value. The load entries in the second array correspond to the time values specified in the first array.
In the GUI, use this menu path to define an array parameter: .
See Array Parameters in the ANSYS Parametric Design Language Guide for more information on how to define array parameters.
Note: Load values for intermediate time points are obtained by linear interpolation. However, load values outside of the specified time range are not extrapolated by the program. Therefore, you should ensure that the load time range is at least equal to the solution time. Otherwise, the results near the solution end time may be invalid due to premature load removal.
Once you define a set of array parameters that represent a time dependent load, you can apply the load by inputting the array parameters directly on the EDLOAD command. Or, you may choose to input the array parameters on the EDCURVE command to define a load curve. The corresponding load curve ID (LCID) can then be input on the EDLOAD command.
To illustrate the use of array parameters, consider the baseball example mentioned previously. Suppose that you wish to examine the distortion of the ball from the moment of impact with the bat to one second later. Assume that the displacement of the bat handle is known as a function of time and that the ball is initially traveling at 1600 in/sec (91 MPH) just prior to impact.
You will first need to define some nodal components that will be used to define the loading and contact surfaces. Create a component named ball that contains all of the nodes of the ball, for which an initial velocity (EDVEL) of 1600 in/sec will be applied (discussed later in this chapter). Then create a second component named ballsurf which contains only the nodes on the surface of the ball. This component will be used later in the contact specification. You also need to define a third component named batsurf, which contains the nodes on the surface of the bat. Contact algorithms are discussed in Contact Surfaces.
nsel,s,node,... ! select all nodes comprising the ball cm,ball,node ! define the component ball nsel,s,node,... ! select the nodes on the ball surface cm,ballsurf,node ! define the component ballsurf nsel,s,node,... ! select the nodes on the bat surface cm,batsurf,node ! define the component batsurf nsel,all
Now select the nodes at the base of the bat handle (bathand) for which a displacement versus time loading curve will be applied.
Define an array named time to store the time values. Remember to use time values that are consistent with all loads, dimensions, and material properties in your model. Next, define an array named xdisp to contain the corresponding X displacements of the component bathand. Likewise, define arrays ydisp and zdisp to contain the corresponding Y and Z displacements of bathand.
nsel,s,node,... ! select the nodes at the bat handle base cm,bathand,node ! define the component bathand nsel,all *dim,time,,4 ! dimension the array parameter time *dim,xdisp,,4 ! dimension the array parameter xdisp *dim,ydisp,,4 ! dimension the array parameter ydisp *dim,zdisp,,4 ! dimension the array parameter zdisp time(1)=0,0.25,0.5,0.75,1 ! times at specified displacements xdisp(1)=0,-1,-2,-1,3 ! X displacement of the bat handle ydisp(1)=0,1,2,3,4 ! Y displacement of the bat handle zdisp(1)=0,3,6,8,9 ! Z displacement of the bat handle
The example given is actually a simple version of a more complex phenomenon. In a more accurate simulation, additional displacement locations (and corresponding load curves) should be defined to better simulate the true motion of the bat handle. Further, the initial velocities of the nodes comprising the bat are all different. Finally, the ball is a composite of several different materials and material models.
Once you have defined the components and array parameters, you are ready to apply loads to your model [EDLOAD command]. In the GUI choose the following menu path: .
You may now choose to add loads (via the ADD label on EDLOAD) such as forces, moments, nodal accelerations, surface pressures, etc. Loads applied with the EDLOAD command are in the global Cartesian direction by default.
The dialog box in the GUI will give you a listing of all valid loads, as well as the components and parameters that have been previously defined. You simply choose the desired load label along with the combination of components (part numbers for rigid bodies) and array parameters (or previously defined load curve ID) you wish to use for that load. It is important to note, as listed below, that all load labels are not valid for all components or part numbers.
The following load labels are valid only for nodal components:
| Forces: FX, FY, FZ |
| Moments: MX, MY, MZ |
| Displacements: UX, UY, UZ |
| Rotations: ROTX, ROTY, ROTZ |
| Velocities: VX, VY, VZ |
| Nodal Accelerations: AX, AY, AZ |
| Body Accelerations: ACLX, ACLY, ACLZ |
| Angular Velocities: OMGX, OMGY, OMGZ |
| Temperature: TEMP |
Note: Although V (X, Y, Z) and A (X, Y, Z) appear as DOFs, they are not actually physical DOFs. However, these quantities are computed as DOF solutions and stored for postprocessing.
The following labels are valid only for rigid bodies (part numbers):
| Forces: RBFX, RBFY, RBFZ |
| Moments: RBMX, RBMY, RBMZ |
| Displacements: RBUX, RBUY, RBUZ |
| Rotations: RBRX, RBRY, RBRZ |
| Velocities: RBVX, RBVY, RBVZ |
| Angular Velocities: RBOX, RBOY, RBOZ |
The following label is valid only for element components:
| Pressure: PRESS |
Returning to our baseball example, the necessary displacement versus time load curves are automatically created with the EDLOAD command from the time and x/y/zdisp array parameters.
edload,add,ux,,bathand,time,xdisp ! X displacement of bathand edload,add,uy,,bathand,time,ydisp ! Y displacement of bathand edload,add,uz,,bathand,time,zdisp ! Z displacement of bathand
Alternatively, the very stiff bat could have been modeled as a rigid body to simplify the required input and to reduce the CPU time. For this case, the appropriate rigid body loads would be applied to valid part numbers (and not to nodal components).
edload,add,rbux,,2,time,xdisp ! X displ. (if bat = part #2) edload,add,rbuy,,2,time,ydisp ! Y displ. (if bat = part #2) edload,add,rbuz,,2,time,zdisp ! Z displ. (if bat = part #2)
If the pressure that the bat imparts on the baseball was known as a function of time, the loading could be accomplished without defining any contact surfaces. Instead, the element component containing the elements on the surface of the ball would be loaded with the “PRESS” label of the EDLOAD command.
edload,add,press,1,cover,battime,batload
In this last scenario, the elements contained in the element component cover are loaded on face number one (face number is
input in the KEY field) with the load curve produced by
the battime and batload
array parameters.
It is important to note that in the examples listed above, the pressure load uses
the KEY field of the EDLOAD command to
specify a load key. Load keys (1,2,3, etc.) are associated with surface loads and
are listed under "surface loads" in the input data tables for each element type in
the Element Reference. For most load types other than pressure loads, you can use the
KEY field to specify a coordinate system
identification number, CID, from the
EDLCS command. The load will act in a direction you define on
EDLCS, or in the global coordinate system direction if
CID is not specified. See Defining Loads in a Local Coordinate System for more information.
Note: To avoid timing problems on some platforms, it is a good practice to always add a very small time value (such as 1.0 × 10-6) to the value in the final item in the time array. For example, instead of the value 3.0, such an array might contain the following value for the last item:
timeint(1)=0,1,2,3.00001
The addition of this very small “padding” factor does not affect the accuracy of the results.
In addition to adding loads, you can also list and delete loads with the commands EDLOAD,LIST and EDLOAD,DELE. You can display load symbols on the element plot with the EDFPLOT command, and you can plot load curves with the EDPL command.
Data curves, which are defined with the EDCURVE command, have various uses in ANSYS LS-DYNA. They can be used to define material data curves (for example, stress-strain) and load data curves (force-deflection) associated with explicit dynamics material models. Data curves can also be used to define load curves that represent time dependent loads (force, displacement, velocity, etc.). These load curves can then be input on the EDLOAD command.
Certain material models (for example, TB,PLAW or TB,HONEY) require specification of material property data which may be a function of effective strain rate, plastic strain, or volumetric strain. For such data, property curves need to be defined using the EDCURVE command prior to specifying the material behavior with the data table [TBDATA] command. Data curves are also used for defining force deflection behavior in rigid-body and drawbead contact.
Similar to placing loads on components, data curves are grouped into array parameters and then associated with a particular curve reference number (LCID) which can be used by a specified material model (PLAW, HONEY, etc.) or contact type (RNTR, ROTR) and drawbead. Use the following steps to specify data curves:
Define an array parameter that contains the abscissa values for the material or friction force behavior (e.g., effective plastic strain, effective strain rate, displacement, etc.).
Define a second array parameter that contains the ordinate values for the material behavior or friction force (e.g., initial yield stress, elastic modulus, force, etc.).
Specify the data curve that will be used to identify this data [EDCURVE]. During this step you will choose a data curve ID number that will be used to associate this data with a particular material behavior when setting up the data table [TBDATA].
After the parameters have been specified, use one of the following menu paths in the GUI to define a data curve:
Defined data curves can be listed using EDCURVE,LIST. They can be plotted using EDCURVE,PLOT and can be deleted using EDCURVE,DELETE.
The following example shows how data curves can be used to define a piecewise linear plasticity curve (TB,PLAW,,,,8) for steel:
! "3" was arbitrarily chosen as the material reference (MAT) number. mp, ex,3,30.0e6 ! elastic (Young’s) modulus (psi) mp,dens,3,7.33e-4 ! mass density (lbf-sec^2/in^4) mp,nuxy,3,0.30 ! Poisson’s ratio (unitless) !Note: First convert engineering stress versus engineering strain data ! into true stress versus true (hencky) strain data. Then subtract ! off the elastic true strain from the total true strain to find ! the plastic true strain, which is used with the total true stress ! in LS-DYNA *MAT_PIECEWISE_LINEAR_PLASTICITY material model #24. !------------------------------------------------------------------------ ! Stress-Strain Data used with Piecewise Linear Plasticity (Power Law 8): !------------------------------------------------------------------------ ! Total Total Total Total Elastic Plastic ! Stress/ Eng. Eng. True True True True ! Strain Stress Strain Stress Strain Strain Strain ! Point (psi) (in/in) (psi) (in/in) (in/in) (in/in) !------------------------------------------------------------------------ ! 1 0 0.0000 0 0.0000 0.0000 0.0000 ! 2 60,000 0.0020 60,120 0.0020 0.0020 0.0000 ! 3 77,500 0.0325 80,020 0.0320 0.0027 0.0293 ! 4 83,300 0.0835 90,260 0.0802 0.0030 0.0772 ! 5 98,000 0.1735 115,000 0.1600 0.0038 0.1562 ! 6 98,300 0.2710 124,940 0.2398 0.0042 0.2356 ! 7 76,400 1.2255 170,030 0.8000 0.0057 0.7943 !------------------------------------------------------------------------ !Note: The first point on the stress/strain curve is NOT entered. ! Start with the second point (where ordinate = yield stress). ! Also, please follow the limits imposed by the *SET command. *dim,strn,,6 ! define array for effective plastic true strain data *dim,strs,,6 ! define array for effective total true stress data strn(1)= 0.0, 0.0293, 0.0772, 0.1562, 0.2356, 0.7943 ! strain (in/in) strs(1)= 60120., 80020., 90260., 115000., 124940., 170030. ! stress (psi) edcurve,add,1,strn,strs ! curve #1: abscissa=strain & ordinate=stress tb,plaw,3,,,8 ! specify power law #8 for material (MAT) #3 tbdata,6,1 ! use load curve #1 for stress/strain data !Note: If desired, a plastic failure strain can be defined. Further, ! strain rate effects can be included by specifying the necessary ! strain rate parameters or the load curve defining the strain rate ! scaling effect on the yield stress. Please refer to Chapter 7 of ! this guide for a complete description of this material model.
In addition to their use with certain material models, data curves (also known as load curves) can be used in the definition of time dependent loads. The procedure to define a load curve is the same as described above for material data curves, except that the first array parameter must contain the time values and the second array parameter must contain the corresponding load values. After you define a load curve with the EDCURVE command, the corresponding load curve reference number (LCID) can be input on the EDLOAD command.
The following 3-step example shows how load curves are used with the EDLOAD command.
! Step 1: Define Array Parameters *dim,time,,5 time(1)=0,.025,.05,.075,.1 *dim,yforce,,5yforce(1)=0,100,200,300,400 ! ! Step 2: Define Load Curve and Corresponding LCID (#11) edcurve,add,11,time,yforce ! ! Step 3: Refer to LCID on the EDLOAD Command edload,add,fy,,comp,,,,11,1.0
As shown above, the LCID is referenced in the ninth
field of the EDLOAD command. It is important to note that if
you use an LCID with the EDLOAD
command, array parameters should not also be specified to define the load. Using
an LCID instead of array parameters on the
EDLOAD command is particularly useful when a specific
load curve is to be applied to multiple components or load labels.
ANSYS LS-DYNA allows you to apply a load to a component or part in any coordinate
direction for which a local coordinate system has been defined. This is accomplished
using the KEY field of the EDLOAD
command in conjunction with the local coordinate system (EDLCS
command). Once a local coordinate system has been defined with the
EDLCS command
(EDLCS,ADD,CID,X1,Y1,Z1,X2,Y2,Z2,
X3,Y3,Z3),
the local coordinate system ID (CID) is used in the
KEY field of the EDLOAD command to
define the direction in which the load acts. For force and moment loads
(Lab = FX, MX, etc. on EDLOAD), the load will be applied in the direction of the local
coordinate system defined by EDLCS. For prescribed motion degrees
of freedom (Lab = UX, ROTX, VX, AX, etc. on EDLOAD), the motion will act in the direction of a
vector from point (X1,
Y1, Z1) to point
(Z2, Y2,
Z2) as input on EDLCS. If
CID is not specified, the load will act in the global
Cartesian coordinate direction. Some load types do not support the use of local
coordinate systems; see Birth Time, Death Time, and CID Support in the Notes section of the
EDLOAD command for more information.
For each load definition, you can specify a birth time and a death time by using
the BTIME and DTIME fields of the EDLOAD command
(EDLOAD,ADD,Lab,KEY,Cname,Par1,Par2,PHASE,LCID,SCALE,BTIME,DTIME).
These options allow you to activate a load at any time during an analysis and then
deactivate it at a later time. Such an option can be very useful in applications
such as a multistage forming process where more than one load is applied in
succession. Some load types do not support birth and death time; see Birth Time, Death Time, and
CID Support in the Notes section of the EDLOAD
command for more information.