# 34.4.1 APPLYING LOADS: OVERVIEW Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE # References • “General and linear perturbation procedures,” Section 6.1.3 • “Prescribed conditions: overview,” Section 34.1.1 • “Concentrated loads,” Section 34.4.2 • “Distributed loads,” Section 34.4.3 • “Thermal loads,” Section 34.4.4 • “Electromagnetic loads,” Section 34.4.5 • “Acoustic and shock loads,” Section 34.4.6 • “Pore fluid flow,” Section 34.4.7 • “Creating and modifying prescribed conditions,” Section 16.4 of the Abaqus/CAE User’s Guide • “Using the load editors,” Section 16.9 of the Abaqus/CAE User’s Guide, in the HTML version of this guide # Overview External loading can be applied in the following forms: • Concentrated or distributed tractions. • Concentrated or distributed fluxes. • Incident wave loads. Many types of distributed loads are provided; they depend on the element type and are described in Part VI, “Elements.” This section discusses general concepts that apply to all types of loading; see “Prescribed conditions: overview,” Section 34.1.1, for general information that applies to all types of prescribed conditions. Concentrated and distributed tractions are discussed in “Concentrated loads,” Section 34.4.2, and “Distributed loads,” Section 34.4.3, respectively. Thermal loading (heat flux) is discussed in “Thermal loads,” Section 34.4.4. Electromagnetic loads are discussed in “Electromagnetic loads,” Section 34.4.5. Loads due to incident wave fields such as due to sound sources or an underwater explosion are discussed in “Acoustic and shock loads,” Section 34.4.6. Pore fluid flow is discussed in “Pore fluid flow,” Section 34.4.7. All other load types, which are applicable to only a single type of analysis, are discussed in the appropriate sections in Part III, “Analysis Procedures, Solution, and Control.” In some situations, concentrated loads and some commonly used distributed loads (such as pressure applied on a surface) may rotate during a geometrically nonlinear analysis. Such loads are known as follower loads; further details on follower loads can be found in “Follower loads in large-displacement analysis;” “Specifying concentrated follower forces” in “Concentrated loads,” Section 34.4.2; “Follower surface loads” in “Distributed loads,” Section 34.4.3; and “Follower edge and line loads” in “Distributed loads,” Section 34.4.3. Follower loads may also lead to an unsymmetric contribution to the stiffness matrix, which is generally referred to as the load stiffness; some issues related to the load stiffness contribution are discussed in “Improving the rate of convergence in large-displacement implicit analysis” in “Concentrated loads,” Section 34.4.2, and “Improving the rate of convergence in large-displacement implicit analysis” in “Distributed loads,” Section 34.4.3. # Element-based versus surface-based distributed loads There are two ways of specifying distributed loads in Abaqus: element-based distributed loads and surface-based distributed loads. Element-based distributed loads can be prescribed on element bodies, element surfaces, or element edges. Surface-based distributed loads can be prescribed on geometric surfaces or geometric edges. In Abaqus/CAE distributed surface and edge loads can be element-based or surface-based, while distributed body loads are prescribed on geometric bodies or element bodies. # Element-based loads Use element-based loads to define distributed loads on element surfaces, element edges, and element bodies. With element-based loads you must provide the element number (or an element set name) and the distributed load type label. The load type label identifies the type of load and the element face or edge on which the load is prescribed (see Part VI, “Elements,” for definitions of the distributed load types available for particular elements). This method of specifying distributed loads is very general and can be used for all distributed load types and elements. # Surface-based loads Use surface-based loads to prescribe a distributed load on a geometric surface or geometric edge. With surface-based loads you must specify the surface or edge name and the distributed load type. The surface or edge, which contains the element and face information, is defined as described in “Element-based surface definition,” Section 2.3.2. In Abaqus/CAE surfaces can be defined as collections of geometric faces and edges or collections of element faces and edges.This method of prescribing a distributed load facilitates user input for complex models. It can be used with most element types for which a valid surface can be defined. You can specify in the surface definition how the distributed load is applied to the boundary of an adaptive mesh domain in Abaqus/Explicit (see “Defining ALE adaptive mesh domains in Abaqus/Explicit,” Section 12.2.2). # Varying the magnitude of a load The magnitude of a load is usually defined by the input data. The variation of the load magnitude during a step can be defined by the default amplitude variation for the step (see “Prescribed conditions: overview,” Section 34.1.1); by a user-defined amplitude curve (see “Amplitude curves,” Section 34.1.2); or, in some cases, by user subroutine DLOAD, UDECURRENT, UDSECURRENT, UTRACLOAD, or VDLOAD. If the analysis consists of one step only, the loads are defined in that step. If there are several analysis steps, the definition of loading in each analysis step depends on whether that step and the previous steps are general analysis steps or linear perturbation steps. Loading during linear perturbation steps is discussed below. In general analysis steps, load magnitudes must always be given as total values, not as changes in magnitude. Multiple definitions of the same load condition in the same step are applied additively. Element-based and surface-based distributed loads are considered independently. For example, elementbased and surface-based pressures applied to an element face in the same step are added. A single redefinition of that same load condition in a subsequent step, however, replaces all the like definitions (same load option, same load type) given in previous steps according to the rules described in “Removing loads” below. Any combination of loads can be applied together during a step. For a linear step it is possible to analyze several load cases based on the same stiffness. # Modifying loads At each new step the loading can be either modified or completely redefined. To redefine a load, the node, element, node set, element set, or surface name must be specified in exactly the same way and the load type must be identical. For example, if a node is part of a loaded node set in one step and is loaded as an individual node (by listing its node number) in another step, the loads will be added. All loads defined in previous steps remain unchanged unless they are redefined. When a load is left unchanged, the following rules apply: • If the associated amplitude was specified in terms of total time, the load continues to follow the amplitude definition. • If no amplitude was associated with the load or if the amplitude was given in terms of step time, the load remains constant at the magnitude associated with the end of the previous step. If you apply multiple loads of the same type at the same node, element, node set, element set, or surface, you cannot modify these loads in the following steps; you need to remove the loads and respecify them. Input File Usage: Use either of the following options to modify an existing load or to specify an additional load (\*LOADING OPTION represents any load type): $$ \begin{array}{l} ^ {*} L O A D I N G O P T I O N \\ ^ {*} L O A D I N G O P T I O N, O P = M O D \\ \end{array} $$ Abaqus/CAE Usage: Load module: Create Load or Load Manager: Edit # Removing loads If you choose to remove any load of a particular type (concentrated load, element-based distributed load, surface-based distributed load, etc.) in a step, no loads of that type will be propagated from the previous general step. All loads of that type that are in effect during this step must be respecified. To redefine a load, the node, element, node set, element set, or surface name must be specified in exactly the same way and the load type must be identical. Refer to “Prescribed conditions: overview,” Section 34.1.1, for a discussion of amplitude variations when removing loads. # Input File Usage: Use the following option to release all previously applied loads of a given type and to specify new loads (\*LOADING OPTION represents any load type): \*LOADING OPTION, OP=NEW For example, \*CLOAD, OP=NEW with no data lines will remove all concentrated forces and moments from the model. If the OP=NEW parameter is used on any loading option in a step, it must be used on all loading options of the same type within the step. # Abaqus/CAE Usage: Use the following option to remove a load within a step: Load module: Load Manager: Deactivate Abaqus/CAE automatically respecifies any loads that should remain in effect during this step. # Example In the history definition input file section shown below, the distributed load (type BX) applied to element set A2 has a magnitude of 20.0 in the first step, which is changed to 50.0 in the second step. Both the set identifier (or element or node number) and the load type must be identical in both steps for Abaqus to identify a load for redefinition. In Step 1 a concentrated load of magnitude 10.0 is applied to degree of freedom 3 of all nodes in node set NLEFT. In Step 2 a concentrated load of magnitude 5.0 is applied to degree of freedom 3 of node 1. If node 1 is in node set NLEFT, the total load applied in Step 2 at this node is 15.0: the loads add. The two distributed loads of type P1 acting on element set E1 in Step 1 will be added to give a total distributed load of 43.0. The pressure loads on element sets B3 and E1 are active during both steps. ```txt *STEP Step 1 *STATIC *CLOAD NLEFT, 3, 10. *DLOAD A2, BX, 20. B3, P1, 5. E1, P1, 21. *DLOAD E1, P1, 22. *END STEP ** *STEP Step 2 ``` ```csv *STATIC *CLOAD 1, 3, 5. *DLOAD, OP=MOD A2, BX, 50. *END STEP ``` # Follower loads in large-displacement analysis In large-displacement analysis distributed loads will be treated as follower forces when appropriate. For beam and shell elements point (concentrated) loads may be fixed in direction or they may rotate with the structure depending on whether you specify follower forces for the load (see “Concentrated loads,” Section 34.4.2). Follower loads defined at a rigid body tie node rotate with the rigid body in Abaqus/Explicit. # Loading during linear perturbation steps In a linear perturbation step (available only in Abaqus/Standard) the state at the end of the previous general analysis step is considered as the “base state.” If the linear perturbation step is the first step of the analysis, the initial conditions of the model form the base state. Loading during a linear perturbation step must be defined as the change in load from the base state (the perturbation of load), not the total of the base state load plus the perturbation load. In consecutive linear perturbation steps, the perturbation of load that applies to each step must be defined completely within that step—the analysis within each such step always starts from the base state (except when you specify that a modal dynamic step should use the initial conditions from the immediately preceding step—see “Transient modal dynamic analysis,” Section 6.3.7). In nonlinear steps that follow linear perturbation analysis steps, the analysis is continued from the base state as if the intermediate linear perturbation steps did not exist. # Loading during linear (mode-based) dynamics procedures If a user subroutine is used to define loading in a mode-based linear dynamics analysis, the subroutine will be called only at the beginning of the step to obtain the magnitude of the load. The load magnitude then remains constant in the step unless it is modified by an amplitude curve. # 34.4.2 CONCENTRATED LOADS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE # References • “Applying loads: overview,” Section 34.4.1 • \*CLOAD • “Defining a concentrated force,” Section 16.9.1 of the Abaqus/CAE User’s Guide, in the HTML version of this guide • “Defining a moment,” Section 16.9.2 of the Abaqus/CAE User’s Guide, in the HTML version of this guide • “Defining a generalized plane strain load,” Section 16.9.10 of the Abaqus/CAE User’s Guide, in the HTML version of this guide • “Defining a fluid reference pressure,” Section 16.9.23 of the Abaqus/CAE User’s Guide, in the HTML version of this guide # Overview Concentrated loads: • apply concentrated forces and moments to nodal degrees of freedom; and • can be fixed in direction; or • can rotate as the node rotates (referred to as follower forces), resulting in an additional, and possibly unsymmetric, contribution to the load stiffness In steady-state dynamic analysis both real and imaginary concentrated loads can be applied (see “Directsolution steady-state dynamic analysis,” Section 6.3.4, and “Mode-based steady-state dynamic analysis,” Section 6.3.8, for details). Multiple concentrated load cases can be defined in random response analysis (see “Random response analysis,” Section 6.3.11, for details). Concentrated loads are also used to apply the pressure-conjugate at nodes with pressure degree of freedom in acoustic analysis (see “Acoustic and shock loads,” Section 34.4.6) and to specify a fluid reference pressure for incompressible flow (see “Incompressible fluid dynamic analysis,” Section 6.6.2). Actuation loads in connector elements can be defined as connector loads, applied similarly to concentrated loads. See “Connector actuation,” Section 31.1.3, for more detailed information. The procedures in which these loads can be used are outlined in “Prescribed conditions: overview,” Section 34.1.1. See “Applying loads: overview,” Section 34.4.1, for general information that applies to all types of loading. # Concentrated loads In Abaqus/Standard and Abaqus/Explicit analyses concentrated forces or moments can be applied at any nodal degree of freedom. You should not apply a moment load at the origin of a cylindrical coordinate system; doing so would make the radial and tangential loads indeterminate. Input File Usage: \*CLOAD node number or node set, degree of freedom, magnitude Abaqus/CAE Usage: Load module: Create Load: choose Mechanical for the Category and Concentrated force, Moment, or Generalized plane strain for the Types for Selected Step # Specifying concentrated follower forces You can specify that the direction of a concentrated force should rotate with the node to which it is applied. This specification should be used only in large-displacement analysis and can be used only at nodes with active rotational degrees of freedom (such as the nodes of beam and shell elements or, in Abaqus/Explicit, tie nodes on a rigid body), excluding the reference node of generalized plane strain elements. If you specify follower forces, the components of the concentrated force must be specified with respect to the reference configuration. Follower loads lead to an unsymmetric contribution to the stiffness matrix that is generally referred to as the load stiffness. Some issues associated with the load stiffness contribution are discussed in “Improving the rate of convergence in large-displacement implicit analysis.” Input File Usage: \*CLOAD, FOLLOWER Abaqus/CAE Usage: Load module: Create Load: choose Mechanical for the Category and Concentrated force or Moment for the Types for Selected Step: Follow nodal rotation # Defining the values of concentrated nodal force from a user-specified file You can define nodal force using nodal force output from a particular step and increment in the output database (.odb) file of a previous Abaqus analysis. The part (.prt) file from the original analysis is also required when reading data from the output database file. In this case both the previous model and the current model must be defined consistently, including node numbering, which must be the same in both models. If the models are defined in terms of an assembly of part instances, part instance naming must be the same. Input File Usage: \*CLOAD, FILE=file, STEP=step, INC=inc Abaqus/CAE Usage: Defining the values of concentrated nodal force from a user-specified file is not supported in Abaqus/CAE. # Specifying a fluid reference pressure For incompressible fluid dynamic analyses in Abaqus/CFD, when no other pressure condition is prescribed, you must specify a fluid reference pressure at one node to set the hydrostatic pressure level. Multiple reference pressures can be specified, but only the last specified hydrostatic pressure load is applied. For more information, see “Incompressible fluid dynamic analysis,” Section 6.6.2, and “Boundary conditions in Abaqus/CFD,” Section 34.3.2. Input File Usage: \*CLOAD node number or node set, HP, magnitude Abaqus/CAE Usage: Load module: Create Load: choose Fluid for the Category and Fluid reference pressure for the Types for Selected Step # Defining time-dependent concentrated loads The prescribed magnitude of a concentrated load can vary with time during a step according to an amplitude definition, as described in “Prescribed conditions: overview,” Section 34.1.1. If different variations are needed for different loads, each load can refer to its own amplitude. # Modifying concentrated loads Concentrated loads can be added, modified, or removed as described in “Applying loads: overview,” Section 34.4.1. # Improving the rate of convergence in large-displacement implicit analysis When concentrated follower forces are specified in a geometrically nonlinear static and dynamic analysis, the unsymmetric matrix storage and solution scheme should normally be used. See “Defining an analysis,” Section 6.1.2, for more information on the unsymmetric matrix storage and solution scheme.