Chapter 2: Loading

Chapter 1 * Chapter 2 * Chapter 3 * Chapter 4 * Chapter 5 * Chapter 6 * Chapter 7 * Chapter 8 * Chapter 9 * Chapter 10 * Chapter 11 * Chapter 12 * Chapter 13 * Chapter 14 * Chapter 15 * Chapter 16 * Chapter 17 * Chapter 18 * Chapter 19

2.1 Loading Overview

2.2 What Are Loads?

Structural: displacements, forces, pressures, temperatures (for thermal strain), gravity

Thermal: temperatures, heat flow rates, convections, internal heat generation, infinite surface

Magnetic: magnetic potentials, magnetic flux, magnetic current segments, source current density, infinite surface

Electric: electric potentials (voltage), electric current, electric charges, charge densities, infinite surface

Fluid: velocities, pressures

Figure 2-1 "Loads" include boundary conditions as well as other types of loading

Loads are divided into six categories: DOF constraints, forces (concentrated loads), surface loads, body loads, inertia loads, and coupled-field loads.

• A DOF constraint fixes a degree of freedom (DOF) to a known value. Examples of constraints are specified displacements and symmetry boundary conditions in a structural analysis, prescribed temperatures in a thermal analysis, and flux-parallel boundary conditions.
• A force is a concentrated load applied at a node in the model. Examples are forces and moments in a structural analysis, heat flow rates in a thermal analysis, and current segments in a magnetic field analysis.
• A surface load is a distributed load applied over a surface. Examples are pressures in a structural analysis and convections and heat fluxes in a thermal analysis.
• A body load is a volumetric or field load. Examples are temperatures and fluences in a structural analysis, heat generation rates in a thermal analysis, and current densities in a magnetic field analysis.
• Inertia loads are those attributable to the inertia (mass matrix) of a body, such as gravitational acceleration, angular velocity, and angular acceleration. You use them mainly in a structural analysis.
• Coupled-field loads are simply a special case of one of the above loads, where results from one analysis are used as loads in another analysis. For example, you can apply magnetic forces calculated in a magnetic field analysis as force loads in a structural analysis.

2.3 Load Steps, Substeps, and Equilibrium Iterations

The ANSYS program uses the set of elements which you select for the first load step for all subsequent load steps, no matter which element sets you specify for the later steps. To select an element set, you use either of the following:

Command(s):

ESEL

Utility Menu>Select>Entities

Figure 2-2 shows a load history curve that requires three load steps-the first load step for the ramped load, the second load step for the constant portion of the load, and the third load step for load removal.

Figure 2-2 Using multiple load steps to specify a transient load history curve

Substeps are points within a load step at which solutions are calculated. You use them for different reasons:

• In a nonlinear static or steady-state analysis, use substeps to apply the loads gradually so that an accurate solution can be obtained.
• In a linear or nonlinear transient analysis, use substeps to satisfy transient time integration rules (which usually dictate a minimum integration time step for an accurate solution).
• In a harmonic response analysis, use substeps to obtain solutions at several frequencies within the harmonic frequency range.

Consider, for example, a two-dimensional, nonlinear static magnetic analysis. To obtain an accurate solution, two load steps are commonly used. (Figure 2-3 illustrates this.)

• The first load step applies the loads gradually over five to10 substeps, each with just one equilibrium iteration.
• The second load step obtains a final, converged solution with just one substep that uses 15 to 25 equilibrium iterations.

2.4 The Role of Time in Tracking

Obviously, in a transient analysis or in a rate-dependent static analysis (creep or viscoplasticity), time represents actual, chronological time in seconds, minutes, or hours. You assign the time at the end of each load step (using the TIME command) while specifying the load history curve. To assign time, use one of the following:

Command(s):

TIME

Main Menu>Preprocessor>Loads>Time/Frequenc>Time and Substps Main Menu>Preprocessor>Loads>Time/Frequenc>Time - Time Step
Main Menu>Solution>Time/Frequenc>Time and Substps
Main Menu>Solution>Time/Frequenc>Time - Time Step

In a rate-independent analysis, however, time simply becomes a counter that identifies load steps and substeps. By default, the program automatically assigns time=1.0 at the end of load step 1, time=2.0 at the end of load step 2, and so on. Any substeps within a load step will be assigned the appropriate, linearly interpolated time value. By assigning your own time values in such analyses, you can establish your own tracking parameter. For example, if a load of 100 units is to be applied incrementally over one load step, you can specify time at the end of that load step to be 100, so that the load and time values are synchronous.

In the postprocessor, then, if you obtain a graph of deflection versus time, it means the same as deflection versus load. This technique is useful, for instance, in a large-deflection buckling analysis where the objective may be to track the deflection of the structure as it is incrementally loaded.

Time takes on yet another meaning when you use the arc-length method in your solution. In this case, time equals the value of time at the beginning of a load step, plus the value of the arc-length load factor (the multiplier on the currently applied loads). ALLF does not have to be monotonically increasing (that is, it can increase, decrease, or even become negative), and it is reset to zero at the beginning of each load step. As a result, time is not considered a "counter" in arc-length solutions.

The arc-length method is an advanced solution technique. For more information about using it, see Chapter 8 of the ANSYS Structural Analysis Guide.

A load step is a set of loads applied over a given time span. Substeps are time points within a load step at which intermediate solutions are calculated. The difference in time between two successive substeps can be called a time step or time increment. Equilibrium iterations are iterative solutions calculated at a given time point purely for convergence purposes.

2.5 Stepped Versus Ramped Loads

• If a load is stepped, then its full value is applied at the first substep and stays constant for the rest of the load step, as shown in Figure 2-4(a).
• If a load is ramped, then its value increases gradually at each substep, with the full value occurring at the end of the load step, as shown in Figure 2-4(b).

The KBC command (Main Menu>Solution>Time/Frequenc>Freq & Substeps, Main Menu>Solution>Time/Frequenc>Time and Substps, or Main Menu>Solution>Time/Frequenc>Time & Time Step) is used to indicate whether loads are ramped or stepped. KBC,0 indicates ramped loads, and KBC,1 indicates stepped loads. The default depends on the discipline and type of analysis and if SOLCONTROL is ON or OFF.

Load step options is a collective name given to options that control load application, such as time, number of substeps, the time step, and stepping or ramping of loads. Other types of load step options include convergence tolerances (used in nonlinear analyses), damping specifications in a structural analysis, and output controls.

2.6 How to Apply Loads

2.6.1 Solid-Model Loads: Advantages and Disadvantages

• Solid-model loads are independent of the finite element mesh. That is, you can change the element mesh without affecting the applied loads. This allows you to make mesh modifications and conduct mesh sensitivity studies without having to reapply loads each time.
• The solid model usually involves fewer entities than the finite element model. Therefore, selecting solid model entities and applying loads on them is much easier, especially with graphical picking.

• Elements generated by ANSYS meshing commands are in the currently active element coordinate system. Nodes generated by meshing commands use the global Cartesian coordinate system. Therefore, the solid model and the finite element model may have different coordinate systems and loading directions.
• Solid-model loads are not very convenient in reduced analyses, where loads are applied at master degrees of freedom. (You can define master DOF only at nodes, not at keypoints.)
• Applying keypoint constraints can be tricky, especially when the constraint expansion option is used. (The expansion option allows you to expand a constraint specification to all nodes between two keypoints that are connected by a line.)
• You cannot display all solid-model loads.

As mentioned earlier, solid-model loads are automatically transferred to the finite element model at the beginning of solution. The ANSYS program overwrites any loads that already exist on corresponding finite element entities.

Deleting solid-model loads also deletes all corresponding finite-element loads.

2.6.2 Finite-Element Loads: Advantages and Disadvantages

• Reduced analyses present no problems, because you can apply loads directly at master nodes.
• There is no need to worry about constraint expansion. You can simply select all desired nodes and specify the appropriate constraints.

• Any modification of the finite element mesh invalidates the loads, requiring you to delete the previous loads and re-apply them on the new mesh.
• Applying loads by graphical picking is inconvenient, unless only a few nodes or elements are involved.

2.6.3 DOF Constraints

Table 2-2 shows the commands to apply, list, and delete DOF constraints. Notice that you can apply constraints on nodes, keypoints, lines, and areas.

Table 2-1 DOF constraints available in each discipline

Discipline	Degree of Freedom	ANSYS Label
Structural	Translations Rotations	UX, UY, UZ ROTX, ROTY, ROTZ
Thermal	Temperature	TEMP
Magnetic	Vector Potentials Scalar Potential	AX, AY, AZ MAG
Electric	Voltage	VOLT
Fluid	Velocities Pressure Turbulent Kinetic Energy Turbulent Dissipation Rate	VX, VY, VZ PRES ENKE ENDS

Table 2-2 Commands for DOF constraints

Location	Basic Commands	Additional Commands
Nodes	D, DLIST, DDELE	DSYM, DSCALE, DCUM
Keypoints	DK, DKLIST, DKDELE	-
Lines	DL, DLLIST, DLDELE	-
Areas	DA, DALIST, DADELE	-
Transfer	SBCTRAN	DTRAN

Below are examples of some of the GUI paths you can use to apply DOF constraints:

GUI:

Main Menu>Preprocessor>-Loads->Apply>load type>On Nodes
Utility Menu>List>Loads>DOF Constraints>On Keypoints
Main Menu>Solution>Apply>load type>On Lines

See the ANSYS Commands Reference for additional GUI path information and for descriptions of the commands listed in Table 2-2.

2.6.4 Applying Symmetry or Antisymmetry Boundary Conditions

In a structural analysis, for example, a symmetry boundary condition means that out-of-plane translations and in-plane rotations are set to zero, and an antisymmetry condition means that in-plane translations and out-of-plane rotations are set to zero. (See Figure 2-5.) All nodes on the symmetry plane are rotated into the coordinate system specified by the KCN field on the DSYM command. The use of symmetry and antisymmetry boundary conditions is illustrated in Figure 2-6. The DL and DA commands work in a similar fashion when you apply symmetry or antisymmetry conditions on lines and areas.

You can use the DL and DA commands to apply velocities, pressures, temperatures, and turbulence quantities on lines and areas for FLOTRAN analyses. At your discretion, you can apply boundary conditions at the endpoints of the lines and the edges of areas.

Note-If the node rotation angles that are in the database while you are using the general postprocessor (POST1) are different from those used in the solution being postprocessed, POST1 may display incorrect results. This condition usually results if you introduce node rotations in a second or later load step by applying symmetry or antisymmetry boundary conditions. Erroneous cases display the following message in POST1 when you execute the SET command (Utility Menu> List>Results>Load Step Summary):

Warning: Cumulative iteration 1 may have been solved using different model or boundary condition data than is currently stored. POST1 results may be erroneous unless you resume from a .db file matching this solution.

Figure 2-5 Symmetry and antisymmetry boundary conditions in a structural analysis

Figure 2-6 Examples of using symmetry and antisymmetry boundary conditions

2.6.5 Transferring Constraints

Command(s):

DTRAN

Main Menu>Preprocessor>Loads>Operate>-Transfer to FE->Constraints
Main Menu>Solution>Operate>-Transfer to FE->Constraints

To transfer all solid model boundary conditions, use one of the following:

Command(s):

SBCTRAN

Main Menu>Preprocessor>Loads>Operate>-Transfer to FE->
All Solid Lds
Main Menu>Solution>Operate>-Transfer to FE->All Solid Lds

2.6.5.1 Resetting Constraints

NSEL,...          	! Selects a set of nodes
D,ALL,VX,40	! Sets VX = 40 at all selected nodes
D,ALL,VX,50	! Changes VX value to 50 (replacement)
DCUM,ADD          	! Subsequent D's to be added
D,ALL,VX,25	! VX = 50+25 = 75 at all selected nodes
DCUM,IGNORE       	! Subsequent D's to be ignored
D,ALL,VX,1325     	! These VX values are ignored!
DCUM              	! Resets DCUM to default (replacement)

Any DOF constraints you set with DCUM stay set until another DCUM is issued. To reset the default setting (replacement), simply issue DCUM without any arguments.

2.6.5.2 Scaling Constraint Values

Command(s):

DSCALE

Main Menu>Preprocessor>Loads>Operate>-Scale FE Loads->Constraints
Main Menu>Solution>Operate>-Scale FE Loads->Constraints

Both the DSCALE and DCUM commands work on all selected nodes and also on all selected DOF labels. By default, DOF labels that are active are those associated with the element types in the model:

Command(s):

DOFSEL

Main Menu>Preprocessor>Loads>Operate>-Scale FE Loads->Constraints (or Forces)
Main Menu>Preprocessor>Loads>Settings>-Replace vs. Add->Constraints (or Forces)
Main Menu>Solution>Operate>-Scale FE Loads->Constraints (or Forces)
Main Menu>Solution>Settings>-Replace vs. Add->Constraints (or Forces)

For example, if you want to scale only VX values and not any other DOF label, you can use the following commands:

DOFSEL,S,VX       	! Selects VX label
DSCALE,0.5	! Scales VX at all selected nodes by 0.5
DOFSEL,ALL        	! Reactivates all DOF labels

Figure 2-7 Scaling temperature constraints with DSCALE

2.6.5.3 Resolution of Conflicting Constraint Specifications

• A DL specification can conflict with a DL specification on an adjacent line (shared keypoint).
• A DL specification can conflict with a DK specification at either keypoint.
• A DA specification can conflict with a DA specification on an adjacent area (shared lines/keypoints).
• A DA specification can conflict with a DL specification on any of its lines.
• A DA specification can conflict with a DK specification on any of its keypoints.

1. In ascending area number order, DOF DA constraints transfer to nodes on areas (and bounding lines and keypoints).

2. In ascending area number order, SYMM and ASYM DA constraints transfer to nodes on areas (and bounding lines and keypoints).

3. In ascending line number order, DOF DL constraints transfer to nodes on lines (and bounding keypoints).

4. In ascending line number order, SYMM and ASYM DL constraints transfer to nodes on lines (and bounding keypoints).

5. DK constraints transfer to nodes on keypoints (and on attached lines, areas, and volumes if expansion conditions are met).

Accordingly, for conflicting constraints, DK commands overwrite DL commands and DL commands overwrite DA commands. For conflicting constraints, constraints specified for a higher line number or area number overwrite the constraints specified for a lower line number or area number, respectively. The constraint specification issue order does not matter.

Note-Any conflict detected during solid model constraint transfer produces a warning similar to the following:

***WARNING***
DOF constraint ROTZ from line 8 (1st value=22) is overwriting a D on node 18 (1st value=0) that was previously transferred from another DA, DL,or set of DK's.

Note-For conflicting constraints on flow degrees of freedom VX, VY, or VZ, zero values (wall conditions) are always given priority over non-zero values (inlet/outlet conditions). "Conflict" in this situation will not produce a warning.

2.6.6 Forces (Concentrated Loads)

Table 2-3 "Forces" available in each discipline

Discipline	Force	ANSYS Label
Structural	Forces Moments	FX, FY, FZ MX, MY, MZ
Thermal	Heat Flow Rate	HEAT
Magnetic	Current Segments Magnetic Flux Electrical Charge	CSGX, CSGY, CSGZ FLUX CHRG
Electric	Current Charge	AMPS CHRG
Fluid	Fluid Flow Rate	FLOW

Table 2-4 Commands for applying force loads

Location	Basic Commands	Additional Commands
Nodes	F, FLIST, FDELE	FSCALE, FCUM
Keypoints	FK, FKLIST, FKDELE	-
Transfer	SBCTRAN	FTRAN

Below are examples of some of the GUI paths to use for applying force loads:

GUI:

Main Menu>Preprocessor>-Loads->Apply>load type>On Nodes
Utility Menu>List>Loads>Forces>On Keypoints
Main Menu>Solution>-Loads->Apply>load type>On Lines

See the ANSYS Commands Reference for descriptions of the commands listed in Table 2-4.

2.6.6.1 Repeating a Force

Command(s):

FCUM

Main Menu>Preprocessor>-Loads->Settings>Forces
Main Menu>Solution>-Loads->Settings>-Replace vs. Add->Forces

For example:

F,447,FY,3000	! Applies FY = 3000 at node 447
F,447,FY,2500     	! Changes FY value to 2500 (replacement)
FCUM,ADD          	! Subsequent F's to be added
F,447,FY,-1000	! FY = 2500-1000 = 1500 at node 447
FCUM,IGNORE       	! Subsequent F's to be ignored
F,25,FZ,350       	! This force is ignored!
FCUM              	! Resets FCUM to default (replacement)

Any force set via FCUM stays set until another FCUM is issued. To reset the default setting (replacement), simply issue FCUM without any arguments.

2.6.6.2 Scaling Force Values

Command(s):

FSCALE

Main Menu>Preprocessor>Loads>Operate>-Scale FE Loads->Forces
Main Menu>Solution>Operate>-Scale FE Loads->Forces

FSCALE and FCUM work on all selected nodes and also on all selected force labels. By default, force labels that are active are those associated with the element types in the model. You can select a subset of these with the DOFSEL command. For example, to scale only FX values and not any other label, you can use the following commands:

DOFSEL,S,FX       	! Selects FX label
FSCALE,0.5	! Scales FX at all selected nodes by 0.5
DOFSEL,ALL        	! Reactivates all DOF labels

2.6.6.3 Transferring Forces

Command(s):

FTRAN

Main Menu>Preprocessor>Loads>Operate>-Transfer to FE->Forces
Main Menu>Solution>Operate>-Transfer to FE->Forces

To transfer all solid model boundary conditions, use the SBCTRAN command:

GUI:

Main Menu>Preprocessor>Loads>Operate>-Transfer to FE->All Solid Lds
Main Menu>Solution>Operate>-Transfer to FE->All Solid Lds

2.6.7 Surface Loads

Table 2-5 Surface loads available in each discipline

Discipline	Surface Load	ANSYS Label
Structural	Pressure	PRES 1.
Thermal	Convection Heat Flux Infinite Surface	CONV HFLUX INF
Magnetic	Maxwell Surface Infinite Surface	MXWF INF
Electric	Maxwell Surface Surface Charge Density Infinite Surface	MXWF CHRGS INF
Fluid	Fluid-Structure Interface Impedance	FSI IMPD
All	Superelement Load Vector	SELV

1. Do not confuse this with the PRES degree of freedom

Table 2-6 Commands for applying surface loads

Location	Basic Commands	Additional Commands
Nodes	SF, SFLIST, SFDELE	SFSCALE,SFCUM,SFFUN, SFGRAD
Elements	SFE, SFELIST, SFEDELE	SFBEAM,SFFUN,SFGRAD
Lines	SFL, SFLLIST, SFLDELE	SFGRAD
Areas	SFA, SFALIST, SFADELE	SFGRAD
Transfer	SFTRAN	-

Below are examples of some of the GUI paths to use for applying surface loads.

GUI:

Main Menu>Preprocessor>-Loads->Apply>load type>On Nodes
Utility Menu>List>Loads>Surface Loads>On Elements
Main Menu>Solution>-Loads->Apply>load type>On Lines

See the descriptions of the commands listed in Table 2-6 in the ANSYS Commands Reference for more information.

Note-The ANSYS program stores surface loads specified on nodes internally in terms of elements and element faces. Therefore, if you use both nodal and element surface load commands for the same surface, only the last specification will be used.

ANSYS applies pressures on axisymmetric shell elements or beam elements on their inner or outer surfaces, as appropriate. In-plane pressure load vectors for layered shells (SHELL91 and SHELL99) are applied on the nodal plane. KEYOPT(11) determines the location of the nodal plane within the shell. When you use flat elements to represent doubly curved surfaces, values which should be a function of the active radius of the meridian will be inaccurate.

2.6.7.1 Applying Pressure Loads on Beams

Command(s):

SFBEAM

Main Menu>Preprocessor>Loads>Apply>-Structural->Pressure>On Beams
Main Menu>Solution>Apply>-Structural->Pressure>On Beams

You can apply lateral pressures, which have units of force per unit length, both in the normal and tangential directions. The pressures may vary linearly along the element length, and can be specified on a portion of the element, as shown in the following figure. You can also reduce the pressure down to a force (point load) at any location on a beam element by setting the JOFFST field to -1. End pressures have units of force.

Figure 2-8 Example of beam surface loads

2.6.7.2 Specifying Node Number Versus Surface Load

Assuming that these are heat flux values, you would apply them as follows:

*DIM,ABC,ARRAY,4              ! Declares dimensions of array parameter ABC
ABC(1)=400,587.2,965.6,740    ! Defines values for ABC
SFFUN,HFLUX,ABC(1)            ! ABC to be used as heat flux function
SF,ALL,HFLUX,100              ! Heat flux of 100 on all selected nodes,
                              !  100 + ABC(i) at node i.

The SF command in the example above specifies a heat flux of 100 on all selected nodes. If nodes 1 through 4 are part of the selected set, those nodes are assigned heat fluxes of 100+ABC(i): 100+400=500 at node 1, 100+587.2=687.2 at node 2, and so on.

Note-What you specify with the SFFUN command stays active for all subsequent SF and SFE commands. To remove the specification, simply use SFFUN without any arguments.

2.6.7.3 Specifying a Gradient Slope

Command(s):

SFGRAD

Main Menu>Preprocessor>Loads>Settings>-For Surface Ld->Gradient
Main Menu>Solution>Settings>-For Surface Ld->Gradient

You can also use this command to apply a linearly varying surface load, such as hydrostatic pressure on a structure immersed in water.

To create the gradient specification, you specify the type of load to be controlled (the Lab argument), the coordinate system and coordinate direction the slope is defined in (SLKCN and Sldir, respectively), the coordinate location where the value of the load (as specified on a subsequent surface load command) will be in effect (SLZER), and the slope (SLOPE).

For example, the hydrostatic pressure (Lab=PRES) shown in Figure 2-9 is to be applied. Its slope can be specified in the global Cartesian system (SLKCN=0) in the Y direction (Sldir=Y). The pressure (to be specified as 500 on a subsequent SF command) is to have its as-specified value (500) at Y=0 (SLZER=0), and will decrease by 25 units per length in the positive Y direction (SLOPE=-25).

Figure 2-9 Example of surface load gradient [SFGRAD]

The commands would be as follows:

SFGRAD,PRES,0,Y,0,-25 	! Y slope of -25 in global Cartesian
NSEL,...               	! Select nodes for pressure application
SF,ALL,PRES,500         	! Pressure at all selected nodes:
                        	!  500 at Y=0, 250 at Y=10, 0 at Y=20

Guideline 1: Set CSCIR (for controlling the coordinate system singularity location) such that the surface to be loaded does not cross the coordinate system singularity.

Guideline 2: Choose SLZER to be consistent with the CSCIR setting. That is, SLZER should be between ±180° if the singularity is at 180° [CSCIR,KCN,0], and SLZER should be between 0° and 360° if the singularity is at 0° [CSCIR,KCN,1].

The following example illustrates why these guidelines are suggested. Consider a semi-circular shell as shown in Figure 2-10, located in a local cylindrical system 11. The shell is to be loaded with an external tapered pressure, tapering from 400 at -90° to 580 at +90°. By default, the singularity in the cylindrical system is located at 180°, therefore the coordinates of the shell range from -90° to +90°. The following commands will apply the desired pressure load:

SFGRAD,PRES,11,Y,-90,1 	! Slope the pressure in the theta direction
                          	!   of C.S. 11.  Specified pressure in effect
                           	!   at -90 degrees, tapering at 1 unit per degree
SF,ALL,PRES,400         	! Pressure at all selected nodes:
                        	!  400 at -90 deg., 490 at 0 deg., 580 at +90 deg.

Figure 2-10 Tapered load on a cylindrical shell

You might be tempted to use 270°, instead of -90°, for SLZER:

SFGRAD,PRES,11,Y,270,1 	! Slope the pressure in the theta direction
                          	!   of C.S. 11.  Specified pressure in effect
                           	!   at 270 degrees, tapering at 1 unit per degree
SF,ALL,PRES,400         	! Pressure at all selected nodes:
                        	!  400 at -90 deg., 490 at 0 deg., 580 at +90 deg.

Figure 2-11 Violation of guideline 2 (left) and guideline 1 (right)

Suppose that you change the singularity location to 0°, thereby satisfying the second guideline (270° is then between 0° and 360°). But then the coordinates of the nodes range from 0° to +90° for the upper half of the shell, and 270° to 360° for the lower half. The surface to be loaded crosses the singularity, a violation of Guideline 1:

CSCIR,11,1              	! Change singularity to 0 degrees
SFGRAD,PRES,11,Y,270,1 	! Slope the pressure in the theta direction
                          	!   of C.S. 11.  Specified pressure in effect
                           	!   at 270 degrees, tapering at 1 unit per degree
SF,ALL,PRES,400         	! Pressure at all selected nodes:
                        	!  400 at 270 deg., 490 at 360 deg., 220 at +90 deg.
                            	!  and 130 at 0 deg.

Note-The SFGRAD specification stays active for all subsequent load application commands. To remove the specification, simply issue SFGRAD without any arguments. Also, if an SFGRAD specification is active when a load step file is read, the program erases the specification before reading the file.

Large deflection effects can change the node locations significantly. The SFGRAD slope and load value calculations, which are based on node locations, are not updated to account for these changes. If you need this capability, use SURF19 or SURF153 with face 3 loading or SURF22 or SURF154 with face 4 loading.

2.6.7.4 Repeating a Surface Load

Command(s):

SFCUM

Main Menu>Preprocessor>Loads>Settings>-Replace vs. Add->Surface Loads
Main Menu>Solution>Settings>-Replace vs. Add->Surface Loads

Any surface load you set stays set until you issue another SFCUM command. To reset the default setting (replacement), simply issue SFCUM without any arguments. The SFSCALE command allows you to scale existing surface load values. Both SFCUM and SFSCALE act only on the selected set of elements. The Lab field allows you to choose the surface load label.

2.6.7.5 Transferring Surface Loads

Command(s):

SFTRAN

Main Menu>Preprocessor>Loads>Operate>-Transfer to FE->Surface Loads
Main Menu>Solution>Operate>-Transfer to FE->Surface Loads

To transfer all solid model boundary conditions, use the SBCTRAN command. (See Section 2.6.3 for a description of DOF constraints.)

2.6.7.6 Using Surface Effect Elements to Apply Loads

2.6.8 Body Loads

Table 2-7 Body loads available in each discipline

Discipline	Body Load	ANSYS Label
Structural	Temperature Fluence	TEMP 1. FLUE
Thermal	Heat Generation Rate	HGEN
Magnetic	Temperature Current Density Virtual Displacement Voltage Drop	TEMP 1. JS MVDI VLTG
Electric	Temperature Volume Charge Density	TEMP 1. CHRGD
Fluid	Heat Generation Rate Force Density	HGEN FORC

1. Do not confuse this with the TEMP degree of freedom.

Table 2-8 Commands for applying body loads

Location	Basic Commands	Additional Commands
Nodes	BF, BFLIST, BFDELE	BFSCALE, BFCUM, BFUNIF
Elements	BFE, BFELIST, BFEDELE	BFESCAL, BFECUM
Keypoints	BFK, BFKLIST, BFKDELE	-
Lines	BFL, BFLLIST, BFLDELE	-
Areas	BFA, BFALIST, BFADELE	-
Volumes	BFV, BFVLIST, BFVDELE	-
Transfer	BFTRAN	-

For the particular body loads that you can apply, list or delete with any of the commands listed in Table 2-8, see the ANSYS Commands Reference.

Below are examples of some of the GUI paths to use for applying body loads:

GUI:

Main Menu>Preprocessor>Loads>-Loads-Apply>load type>On Nodes
Utility Menu>List>Loads>Body Loads>On Picked Elems
Main Menu>Solution>-Loads-Apply>load type>On Keypoints
Utility Menu>List>Loads>Body Loads>On Picked Lines
Main Menu>Solution>-Loads-Apply>load type>On Volumes

See the ANSYS Commands Reference for descriptions of the commands listed in Table 2-8.

Note-Body loads you specify on nodes are independent of those specified on elements. For a given element, ANSYS determines which loads to use as follows:

• It checks to see if you specified elements for body loads.
• If not, it uses body loads specified for nodes.
• If no body loads exist for elements or nodes, the body loads specified via the BFUNIF command take effect.

2.6.8.1 Specifying Body Loads for Elements

• For 2-D and 3-D solid elements (PLANEn and SOLIDn), the locations for body loads are usually the corner nodes.

• For shell elements (SHELLn), the locations for body loads are usually the "pseudo-nodes" at the top and bottom planes, as shown below.

• Line elements (BEAMn, LINKn, PIPEn, etc.) are similar to shell elements; the locations for body loads are usually the pseudo-nodes at each end of the element.

• In all cases, if degenerate (collapsed) elements are involved, you must specify element loads at all of its locations, including duplicate values at the duplicate (collapsed) nodes. A simple alternative is to specify body loads directly at the nodes, using the BF command.

2.6.8.2 Specifying Body Loads for Keypoints

Figure 2-15 Transfers of BFK loads to nodes

2.6.8.3 Specifying Body Loads on Lines, Areas and Volumes

2.6.8.4 Specifying a Uniform Body Load

Another way to specify a uniform temperature is as follows:

Command(s):

BFUNIF

Main Menu>Preprocessor>Loads>Apply>Temperature>Uniform Temp
Main Menu>Preprocessor>Loads>Settings>Uniform Temp
Main Menu>Solution>Apply>Temperature>Uniform Temp
Main Menu>Solution>Settings>Uniform Temp

2.6.8.5 Repeating a Body Load Specification

Command(s):

BFCUM, BFECUM

Main Menu>Preprocessor>Loads>Settings>Nodal Body Ld
Main Menu>Preprocessor>Loads>Settings>Elem Body Lds
Main Menu>Solution>Settings>Nodal Body Ld
Main Menu>Solution>Settings>Elem Body Lds

The settings you specify with either command or its equivalent GUI paths stay set until they are reuse the command or path. To reset the default setting (replacement), simply issue the commands or choose the paths without any arguments.

2.6.8.6 Transferring Body Loads

Command(s):

BFTRAN

Main Menu>Preprocessor>Loads>Operate>Body Loads
Main Menu>Solution>Operate>Body Loads

To transfer all solid model boundary conditions, use the SBCTRAN command. (See Section 2.6.3 for a description of DOF constraints.)

2.6.8.7 Scaling Body Load Values

Command(s):

BFSCALE

Main Menu>Preprocessor>Loads>Operate>Nodal Body Ld
Main Menu>Solution>Operate>Nodal Body Ld

Command(s):

BFESCAL

Main Menu>Preprocessor>Loads>Operate>Elem Body Lds
Main Menu>Solution>Operate>Elem Body Lds

BFCUM and BFSCALE act on the selected set of nodes, whereas BFECUM and BFESCAL act on the selected set of elements.

2.6.8.8 Resolution of Conflicting Body Load Specifications

BFV, BFA, and BFL specifications transfer to associated volume, area, and line elements, respectively, where they exist. Where elements do not exist, they transfer to the nodes on the volumes, areas, and lines, including nodes on the region boundaries. The possibility of conflicting specifications depends upon how BFV, BFA, BFL and BFK are used as described by the following cases.

CASE A: There are elements for every BFV, BFA, or BFL, and every element belongs to a volume, area or line having a BFV, BFA, or BFL, respectively.

Every element will have its body loads determined by the corresponding solid body load. Any BFK's present will have no effect. No conflict is possible.

Elements not getting a direct BFE transfer from a BFV, BFA, or BFL are unaffected by them, but will have their body loads determined by the following: (1 - highest priority) directly defined BFE loads, (2) BFK loads, (3) directly defined BF loads, or (4) BFUNIF loads. No conflict among solid model body loads is possible.

Elements not getting a direct BFE transfer from a BFV, BFA, or BFL will have their body loads determined by the following: (1 - highest priority) directly defined BFE loads, (2) BFK loads, (3) BFL loads on an attached line that did NOT transfer to line elements, (4) BFA loads on an attached area that did not NOT transfer to area elements, (5) BFV loads on an attached volume that did not NOT transfer to volume elements, (6) directly defined BF loads, or (7) BFUNIF loads.

• A BFL specification can conflict with a BFL specification on an adjacent line (shared keypoint).
• A BFL specification can conflict with a BFK specification at either keypoint.
• A BFA specification can conflict with a BFA specification on an adjacent area (shared lines/keypoints).
• A BFA specification can conflict with a BFL specification on any of its lines.
• A BFA specification can conflict with a BFK specification on any of its keypoints.
• A BFV specification can conflict with a BFV specification on an adjacent volume (shared areas/lines/keypoints).
• A BFV specification can conflict with a BFA specification on any of its areas.
• A BFV specification can conflict with a BFL specification on any of its lines.
• A BFV specification can conflict with a BFK specification on any of its keypoints.

1. In ascending volume number order, BFV loads transfer to BFE loads on volume elements, or, if there are none, to BF loads on nodes on volumes (and bounding areas, lines, and keypoints).

2. In ascending area number order, BFA loads transfer to BFE loads on area elements, or, if there are none, to BF loads on nodes on areas (and bounding lines and keypoints).

3. In ascending line number order, BFL loads transfer to BFE loads on line elements, or, if there are none, to BF loads on nodes on lines (and bounding keypoints).

4. BFK loads transfer to BF loads on nodes on keypoints (and on attached lines, areas, and volumes if expansion conditions are met).

Accordingly, for conflicting solid model body loads in "Case C" situations, BFK commands overwrite BFL commands, BFL commands overwrite BFA commands, and BFA commands overwrite BFV commands. For conflicting body loads, a body load specified for a higher line number, area number, or volume number overwrites the body load specified for a lower line number, area number, or volume number, respectively. The body load specification issue order does not matter.

Note-Any conflict detected during solid model body load transfer produces a warning similar to the following:

***WARNING***
Body load TEMP from line 12 (1st value=77) is overwriting a BF on node 43 (1st value=99) that was previously transferred from another BFV, BFA, BFL or set of BFK's.

2.6.9 Inertia Loads

Table 2-9 Inertia loads commands

Command	GUI Menu Paths
ACEL	Main Menu>Preprocessor>FLOTRAN Set Up>Flow Environment>Gravity Main Menu>Preprocessor>Loads>Apply>Gravity Main Menu>Preprocessor>Loads>Delete>Gravity Main Menu>Solution>FLOTRAN Set Up>Flow Environment>Gravity Main Menu>Solution>Apply>Gravity Main Menu>Solution>Delete>Gravity
CGLOC	Main Menu>Preprocessor>FLOTRAN Set Up>Flow Environment>Rotating Coords Main Menu>Preprocessor>Loads>Apply>Other>Coriolis Effects Main Menu>Preprocessor>Loads>Delete>Other>Coriolis Effects Main Menu>Solution>FLOTRAN Set Up>Flow Environment>Rotating Coords Main Menu>Solution>Apply>Other>Coriolis Effects Main Menu>Solution>Delete>Other>Coriolis Effects
CGOMGA	Main Menu>Preprocessor>FLOTRAN Set Up>Flow Environment>Rotating Coords Main Menu>Preprocessor>Loads>Apply>Other>Coriolis Effects Main Menu>Preprocessor>Loads>Delete>Other>Coriolis Effects Main Menu>Solution>FLOTRAN Set Up>Flow Environment>Rotating Coords Main Menu>Solution>Apply>Other>Coriolis Effects Main Menu>Solution>Delete>Other>Coriolis Effects
DCGOMG	Main Menu>Preprocessor>Loads>Apply>Other>Coriolis Effects Main Menu>Preprocessor>Loads>Delete>Other>Coriolis Effects Main Menu>Solution>Apply>Other>Coriolis Effects Main Menu>Solution>Delete>Other>Coriolis Effects
DOMEGA	Main Menu>Preprocessor>Loads>Apply>Other>Angular Accel Main Menu>Preprocessor>Loads>Delete>Other>Angular Accel Main Menu>Solution>Apply>Other>Angular Accel Main Menu>Solution>Delete>Other>Angular Accel
IRLF	Main Menu>Preprocessor>Loads>Other>Inertia Relief Main Menu>Preprocessor>Loads>Output Ctrls>Incl Mass Summry Main Menu>Solution>Other >Inertia Relief Main Menu>Solution>Output Ctrls>Incl Mass Summry
OMEGA	Main Menu>Preprocessor>Loads>Apply>Other>Angular Velocity Main Menu>Preprocessor>Loads>Delete>Other>Angular Velocity Main Menu>Solution>Apply>Other>Angular Velocity Main Menu>Solution>Delete>Other>Angular Velocity

Notice that there are no specific commands to list or delete inertia loads. To list them, issue STAT, INRTIA (Utility Menu>List>Status>Solution>Inertia Loads) To remove an inertia load, simply set the load value to zero. You can set an inertia load to zero, but you cannot delete it. For ramped load steps, inertia loads are ramped to zero. (This is also true when you apply inertia loads.)

The ACEL, OMEGA, and DOMEGA commands specify acceleration, angular velocity, and angular acceleration, respectively, in global Cartesian directions.

Note-The ACEL command applies an acceleration field (not gravity) to a body. Therefore, to apply gravity to act in the negative Y direction, you should specify a positive Y acceleration.

Use the CGOMGA and DCGOMG commands to specify angular velocity and angular acceleration of a spinning body which is itself revolving about another reference coordinate system. The CGLOC command specifies the location of the reference system with respect to the global Cartesian origin. You can use these commands, for example, to include Coriolis effects in a static analysis.

Inertia loads are effective only if your model has some mass, which is usually supplied by a density specification. (You can also supply mass to the model by using mass elements, such as MASS21, but density is more commonly used and is more convenient.) As with all other data, the ANSYS program requires you to use consistent units for mass. If you are accustomed to the British system of units, you might sometimes wish to use weight density (lb/in³) instead of mass density (lb-sec²/in/in³), for convenience.

Use weight density in place of mass density only under these conditions:

• The model will only be used in a static analysis.
• No angular velocity or angular acceleration is applied.
• Gravitational acceleration is unity (g=1.0).

Table 2-10 Ways of specifying density

Convenient Form	Consistent Form	Description
g=1.0	g=386.0	Parameter definition
MP,DENS,1,0.283/g	MP,DENS,1,0.283/g	Density of steel
ACEL,,g	ACEL,,g	Gravity load

2.6.10 Coupled-Field Loads

Command(s):

LDREAD

Main Menu>Preprocessor>-Loads->Apply>load type>From source
Main Menu>Solution>Apply>load type>From source

See the ANSYS Coupled-Field Analysis Guide for details about how to use this command in different types of coupled-field analyses.

2.6.11 Axisymmetric Loads and Reactions

F,N,FY,47124

Axisymmetric harmonic elements require that their loads be supplied in a form that the program can interpret as a Fourier series. The MODE command (Main Menu>Preprocessor>Loads>Other>For Harmonic Ele or Main Menu> Solution>Other>For Harmonic Ele), together with other load commands (D, F, SF, etc.), is required for these elements. See the ANSYS Elements Reference for details.

Figure 2-16 Concentrated axisymmetric loads are defined on a "360° basis"

2.6.11.1 Further Hints and Restrictions

Figure 2-17 Central constraint for solid axisymmetric structure

2.6.12 Loads to Which the DOF Offers No Resistance

2.7 How to Specify Load Step Options

• General Options
• Dynamics Options
• Nonlinear Options
• Output Controls
• Biot-Savart Options
• Spectrum Options

2.7.1 General Options

2.7.1.1 The Time Option

2.7.1.2 Number of Substeps and Time Step Size

Command(s):

DELTIM

Main Menu>Preprocessor>Loads>Time/Frequenc>Time & Time Step
Main Menu>Solution>Time/Frequenc>Time & Time Step

Command(s):

NSUBST

Main Menu>Preprocessor>Loads>Time/Frequenc>Freq & Substeps
Main Menu>Preprocessor>Loads>Time/Frequenc>Time and Substps
Main Menu>Solution>Time/Frequenc>Freq & Substeps
Main Menu>Solution>Time/Frequenc>Time and Substps

NSUBST specifies the number of substeps, and DELTIM specifies the time step size. By default, the ANSYS program uses one substep per load step.

2.7.1.3 Automatic Time Stepping

GUI:

Main Menu>Preprocessor>Loads>Time/Frequenc>Time & Time Step
Main Menu>Solution>Time/Frequenc>Time & Time Step
Main Menu>Preprocessor>Loads>Time/Frequenc>Time and Substps
Main Menu>Solution>Time/Frequenc>Time and Substps

In automatic time stepping, the program calculates an optimum time step at the end of each substep, based on the response of the structure or component to the applied loads. When used in a nonlinear static (or steady-state) analysis, AUTOTS determine the size of load increments between substeps.

2.7.1.4 Stepping or Ramping Loads

Some notes about stepped and ramped loads are:

• If you specify stepped loads, the program handles all loads (constraints, forces, surface loads, body loads, and inertia loads) in the same manner. They are step-applied, step-changed, or step-removed, as the case may be.
• If you specify ramped loads, then:
  • All loads applied in the first load step, except film coefficients, are ramped (either from zero or from the value specified via BFUNIF or its GUI equivalent, depending on the type of load; see Table 2-11). Film coefficients are step-applied. Note-The concept of stepped versus ramped loading does not apply to temperature-dependent film coefficients (input as -N on a convection command). These are always applied at the value dictated by their temperature function.

• All loads changed in later load steps are ramped from their previous values. Note that in a full harmonic analysis (ANTYPE,HARM with HROPT,FULL), surface and body loads ramp as they do in the first load step and not from their previous values, except for PLANE2, SOLID45, SOLID92, and SOLID95, which do ramp from their previous values.
• All loads newly introduced in later load steps are ramped (either from zero or from BFUNIF, depending on the type of load; see Table 2-11).
• All loads deleted in later load steps are step-removed, except body loads and inertia loads. Body loads are ramped to BFUNIF. Inertia loads, which you can delete only by setting them to zero, are ramped to zero.
• Loads should not be deleted and respecified in the same load step. Ramping may not work the way the user intended in this case.

Load Type1	Applied in Load Step 1	Introduced in Later Load Steps
DOF Constraints · Temperatures · Others	Ramped from TUNIF2 Ramped from zero	Ramped from TUNIF3 Ramped from zero
"Forces"	Ramped from zero	Ramped from zero
Surface Loads · TBULK · HCOEF · Others	Ramped from TUNIF2 Stepped Ramped from zero	Ramped from TUNIF Ramped from zero4 Ramped from zero
Body Loads · Temperatures · Others	Ramped from TUNIF2 Ramped from BFUNIF3	Ramped from previous TUNIF3 Ramped from previous BFUNIF3
Inertia Loads1	Ramped from zero	Ramped from zero

1. For OMEGA loads, note that the OMEGA itself is linearly ramped; therefore, the resulting force will vary quadratically over the load step.

2. The TUNIF command specifies a uniform temperature at all nodes.

3. In this case, the TUNIF or BFUNIF value from the previous load step is used, not the current value.

4. Temperature-dependent film coefficients are always applied at the value dictated by their temperature function, regardless of the KBC setting.

5. The BFUNIF command is just a generic form of TUNIF, meant to specify a uniform body load at all nodes.

2.7.1.5 Other General Options

• The reference temperature for thermal strain calculations, which defaults to zero degrees. Specify this temperature as follows:

TREF

Main Menu>Preprocessor>Loads>Other>Reference Temp
Main Menu>Preprocessor>Loads>Settings>Reference Temp
Main Menu>Solution>Other>Reference Temp
Main Menu>Solution>Settings>Reference Temp

• Whether a new triangularized matrix is required for each solution (that is, each equilibrium iteration). You can do this only in a static (steady-state) or transient analysis, using one of these methods:

KUSE

Main Menu>Preprocessor>Loads>Other>Reuse Tri Matrix
Main Menu>Solution>Other>Reuse Tri Matrix

By default, the program decides whether a new matrix is required, based on such things as changes in DOF constraints, temperature-dependent material properties, and the Newton-Raphson option. If KUSE is set to 1, the program reuses the previous triangularized matrix. This setting is useful during a restart: if you are restarting an analysis for additional load steps and you know that the existing triangularized matrix (on the file Jobname.TRI) can be reused, you can save a significant amount of computer time by setting KUSE to 1. The command KUSE,-1 forces the triangularized matrix to be reformulated at every equilibrium iteration. Analyses rarely require this; you will use it mainly for debugging purposes.

• A mode number (the number of harmonic waves around the circumference) and whether the harmonic component is symmetric or antisymmetric about the global X axis. When you use axisymmetric harmonic elements (axisymmetric elements with non-axisymmetric loading), the loads are specified as a series of harmonic components (a Fourier series). To specify the mode number, use one of the following:

MODE

Main Menu>Preprocessor>Loads>Other>For Harmonic Ele
Main Menu>Solution>Other>For Harmonic Ele

See your ANSYS Elements Reference for a description of harmonic elements.

• The type of scalar magnetic potential formulation to be used in a 3-D magnetic field analysis, specified via one of the following:

MAGOPT

Main Menu>Preprocessor>Loads>Magnetics>potential formulation method
Main Menu>Solution>Magnetics>potential formulation method

• The type of solution to be expanded in the expansion pass of a reduced analysis, specified via one of the following:

NUMEXP, EXPSOL

Main Menu>Preprocessor>Loads>ExpansionPass>Range of Solu's
Main Menu>Solution>ExpansionPass>Range of Solu's
Main Menu>Preprocessor>Loads>ExpansionPass>By Load Step
Main Menu>Preprocessor>Loads>ExpansionPass>By Time/Freq
Main Menu>Solution>ExpansionPass>By Load Step
Main Menu>Solution>ExpansionPass>By Time/Freq

2.7.2 Dynamics Options

Table 2-12 Dynamic and other transient analyses commands

Command	GUI Menu Paths	Purpose
TIMINT	Main Menu>Preprocessor>Loads> Time/Frequenc>Time Integration Main Menu>Solution>Time/Frequenc> Time Integration	Activates or deactivates time integration effects
HARFRQ	Main Menu>Preprocessor>Loads> Time/Frequenc>Freq & Substeps Main Menu>Solution>Time/Frequenc> Freq & Substeps	Specifies the frequency range of the loads in a harmonic response analysis
ALPHAD	Main Menu>Preprocessor>Loads> Time/Frequenc>Damping Main Menu>Solution>Time/Frequenc>Damping	Specifies damping for a structural dynamic analysis
BETAD	Main Menu>Preprocessor>Loads> Time/Frequenc>Damping Main Menu>Solution>Time/Frequenc>Damping	Specifies damping for a structural dynamic analysis
DMPRAT	Main Menu>Preprocessor>Loads> Time/Frequenc>Damping Main Menu>Solution>Time/Frequenc>Damping	Specifies damping for a structural dynamic analysis
MDAMP	Main Menu>Preprocessor>Loads> Time/Frequenc>Damping Main Menu>Solution>Time/Frequenc>Damping	Specifies damping for a structural dynamic analysis

2.7.3 Nonlinear Options

Table 2-13 Nonlinear analyses commands

Command	GUI Menu Paths	Purpose
NEQIT	Main Menu>Preprocessor>Loads>Nonlinear> Equilibrium Iter Main Menu>Solution>Nonlinear>Equilibrium Iter	Specifies the maximum number of equilibrium iterations per substep (default=25)
CNVTOL	Main Menu>Preprocessor>Loads>Nonlinear> Convergence Crit Main Menu>Solution>Nonlinear>Convergence Crit	Specifies convergence tolerances
NCNV	Main Menu>Preprocessor>Loads>Nonlinear> Criteria to Stop Main Menu>Solution>Nonlinear>Criteria to Stop	Provides options for terminating analyses

2.7.4 Output Controls

Table 2-14 Output controls commands

Command	GUI Menu Paths	Purpose
OUTRES	Main Menu>Preprocessor>Loads> Output Ctrls>DB/Results File Main Menu>Solution>Output Ctrls>DB/Results File	Controls what ANSYS writes to the database and results file and how often it is written.
OUTPR	Main Menu>Preprocessor>Loads> Output Ctrls>Solu Printout Main Menu>Solution>Output Ctrls>Solu Printout	Controls what is printed (written to the solution output file, Jobname.OUT) and how often it is written.

The example below illustrates using OUTRES and OUTPR:

OUTRES,ALL,5	! Writes all data every 5th substep
OUTPR,NSOL,LAST	! Prints nodal solution for last substep only

OUTRES,ALL,10
OUTRES,NSOL,5

OUTRES,NSOL,5
OUTRES,ALL,10

A third output control command, ERESX, allows you to review element integration point values in the postprocessor.

Command(s):

ERESX

Main Menu>Preprocessor>Loads>Output Ctrls>Integration Pt
Main Menu>Solution>Output Ctrls>Integration Pt

By default, the ANSYS program extrapolates nodal results that you review in the postprocessor from integration point values for all elements except those with active material nonlinearities (for instance, non-zero plastic strains). By issuing ERESX,NO, you can turn off the extrapolation and instead copy integration point values to the nodes, making those values available in the postprocessor. Another option, ERESX,YES, forces extrapolation for all elements, whether or not they have active material nonlinearities.

2.7.5 Biot-Savart Options

Table 2-15 Biot-Savart commands

Command	GUI Menu Paths	Purpose
BIOT	Main Menu>Preprocessor>Loads>Magnetics> Biot-Savart Main Menu>Solution>Magnetics>Biot-Savart	Calculates the magnetic source field intensity due to a selected set of current sources.
EMSYM	Main Menu>Preprocessor>Loads>Magnetics> Copy Sources Main Menu>Solution>Magnetics>Copy Sources	Duplicates current sources that exhibit circular symmetry.

The ANSYS Electromagnetic Field Analysis Guide explains the use of these commands where appropriate.

2.7.6 Spectrum Options

2.8 Creating Multiple Load Step Files

The LSWRITE command writes the load step file (one file per load step, identified as Jobname.S01, Jobname.S02, Jobname.S03, etc.). Use one of these methods:

Command(s):

LSWRITE

Main Menu>Preprocessor>Loads>Write LS File
Main Menu>Solution>Write LS File

After all load step files are written, you can use one action command to read in the files sequentially and obtain the solution for each load step (see Chapter 3).

The sample set of commands shown below defines multiple load steps:

/SOLU               	! Enter SOLUTION
...
!  Load Step 1:
D,...       	! Loads
SF,...
...
NSUBST,...        	! Load step options
KBC,...
OUTRES,...
OUTPR,...
...
LSWRITE         	! Writes load step file: Jobname.S01

!  Load Step 2:
D,...        	! Loads
SF,...
...
NSUBST,...        	! Load step options
KBC,...
OUTRES,...
OUTPR,...
...
LSWRITE          	! Writes load step file: Jobname.S02
...

Some notes about the load step file:

• The load step data are written to the file in terms of ANSYS commands.

• The LSWRITE command does not capture changes to real constants (R) or material properties (MP).
• The LSWRITE command automatically transfers solid-model loads to the finite element model, so all loads are written in the form of finite-element load commands. In particular, surface loads are always written in terms of SFE (or SFBEAM) commands, regardless of how they were applied.
• To modify data on load step file number n, issue the command LSREAD,n to read in the file, make the desired changes, and then issue LSWRITE,n (which will overwrite the old file n). You can also directly edit the load step file using your system editor, but this is generally not recommended. The GUI equivalents of the LSREAD command are:

Main Menu>Preprocessor>Loads>Read LS File
Main Menu>Solution>Read LS File

• The LSDELE command allows you to delete load step files from within the ANSYS program. The GUI equivalents of LSDELE are:

Main Menu>Preprocessor>Loads>Operate>Delete LS Files
Main Menu>Solution>Operate>Delete LS Files

• Another useful load step related command is LSCLEAR, which allows you to delete all loads and reset all load step options to their defaults. You can use it, for example, to "clean up" the load step data before reading in a load step file for modifications.

GUI equivalents for LSCLEAR are:

Main Menu>Preprocessor>Loads>Delete>All Load Data>data type
Main Menu>Preprocessor>Loads>Reset Options
Main Menu>Preprocessor>Loads>Settings>Reset Factors
Main Menu>Solution>Reset Options
Main Menu>Solution>Settings>Reset Factors

Go to the beginning of this chapter