You can apply most loads either on the solid model (on keypoints, lines, and areas) or on the finite element model (on nodes and elements). For example, you can specify forces at a keypoint or a node. Similarly, you can specify convections (and other surface loads) on lines and areas or on nodes and element faces. No matter how you specify the loads, the solver expects all loads to be in terms of the finite element model. Therefore, if you specify loads on the solid model, the program automatically transfers them to the nodes and elements at the beginning of solution.
The following topics related to applying loads are available:
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 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.
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.
Notes About Solid-Model Loads
As mentioned earlier, solid-model loads are automatically transferred to the finite element model at the beginning of solution. If you mix solid model loads with finite-element model loads, couplings, or constraint equations, you should be aware of the following possible conflicts:
Transferred solid loads replace nodal or element loads already present, regardless of the order in which the loads were input. For example, DL,,,UX on a line overwrites any D,,,UX loads on the nodes of that line at transfer time. (DL,,,UX also overwrites D,,,VELX velocity loads and D,,,ACCX acceleration loads.)
Line or area symmetry or antisymmetry conditions (DL,,,SYMM, DL,,,ASYM, DA,,,SYMM, or DA,,,ASYM) often introduce nodal rotations that could effect nodal constraints, nodal forces, couplings, or constraint equations on nodes belonging to constrained lines or areas.
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.
The next few subsections discuss how to apply each category of loads - constraints, forces, surface loads, body loads, inertia loads, and coupled-field loads - and then explain how to specify load step options.
Table 2.1: DOF Constraints Available in Each Discipline shows the degrees of freedom that can be constrained in each discipline and the corresponding labels. Any directions implied by the labels (such as UX, ROTZ, AY, etc.) are in the nodal coordinate system. For a description of different coordinate systems, see the Modeling and Meshing Guide.
Table 2.2: Commands for DOF Constraints 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||Label|
For structural static and transient analyses, velocities and accelerations can be applied as finite element loads on nodes using the D command. Velocities can be applied in static or transient analyses; accelerations can only be applied in transient analyses. The labels for these loads are as follows:
|VELX, VELY, VELZ - translational velocities|
|OMGX, OMGY, OMGZ - rotational velocities|
|ACCX, ACCY, ACCZ - translational accelerations|
|DMGX, DMGY, DMGZ -rotational accelerations|
Although these are not strictly degree-of-freedom constraints, they are boundary conditions that act upon the translation and rotation degrees of freedom. See the D command for more information.
Table 2.2: Commands for DOF Constraints
Following are some of the GUI paths you can use to apply DOF constraints:
Use the DSYM command to apply symmetry or antisymmetry boundary conditions on a plane of nodes. The command generates the appropriate DOF constraints. See the Command Reference for the list of constraints generated.
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: Symmetry and Antisymmetry Boundary Conditions.) 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: Examples of Boundary Conditions. The DL and DA commands work in a similar fashion when you apply symmetry or antisymmetry
conditions on lines and 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 ( ):
*** 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.
To transfer constraints that have been applied to the solid model to the corresponding finite element model, use one of the following:
To transfer all solid model boundary conditions, use one of the following:
By default, if you repeat a DOF constraint on the same degree of freedom, the new specification replaces the previous one. You can change this default to add (for accumulation) or ignore with the DCUM command ( ). For example:
NSEL,... ! Selects a set of nodes D,ALL,UX,40 ! Sets UX = 40 at all selected nodes D,ALL,UX,50 ! Changes UX value to 50 (replacement) DCUM,ADD ! Subsequent D's to be added D,ALL,UX,25 ! UX = 50+25 = 75 at all selected nodes DCUM,IGNORE ! Subsequent D's to be ignored D,ALL,UX,1325 ! These UX values are ignored! DCUM ! Resets DCUM to default (replacement)
You can scale existing DOF constraint values as follows:
For example, if you want to scale only UX values and not any other DOF label, you can use the following commands:
DOFSEL,S,UX ! Selects UX label DSCALE,0.5 ! Scales UX at all selected nodes by 0.5 DOFSEL,ALL ! Reactivates all DOF labels
When scaling temperature constraints (TEMP) in a thermal analysis,
you can use the
TBASE field on the DSCALE command to scale the temperature offset from a base
temperature (that is, to scale |TEMP-
TBASE|) rather than the actual temperature values. The following figure
Figure 2.7: Scaling Temperature Constraints with DSCALE
The program transfers constraints that have been applied to the solid model to the corresponding finite element model in the following sequence:
In ascending area number order, DOF DA constraints transfer to nodes on areas (and bounding lines and keypoints).
In ascending area number order, SYMM and ASYM DA constraints transfer to nodes on areas (and bounding lines and keypoints).
In ascending line number order, DOF DL constraints transfer to nodes on lines (and bounding keypoints).
In ascending line number order, SYMM and ASYM DL constraints transfer to nodes on lines (and bounding keypoints).
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.
Changing the value of DK, DL, or DA constraints between solutions may produce many of these warnings at the 2nd or later solid BC transfer. These can be prevented if you delete the nodal D constraints between solutions using DADELE, DLDELE, and/or DDELE.
Table 2.3: "Forces" Available in Each Discipline shows a list of forces available in each discipline and the corresponding labels. Any directions implied by the labels (such as FX, MZ, CSGY, etc.) are in the nodal coordinate system. (See Coordinate Systems in the Modeling and Meshing Guide for a description of different coordinate systems.) Table 2.4: Commands for Applying Force Loads lists the commands to apply, list, and delete forces. Notice that you can apply them at nodes as well as keypoints.
Table 2.3: "Forces" Available in Each Discipline
Table 2.4: Commands for Applying Force Loads
Below are examples of some of the GUI paths to use for applying force loads:
By default, if you repeat a force at the same degree of freedom, the new specification replaces the previous one. You can change this default to add (for accumulation) or ignore by using one of the following:
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)
The FSCALE command allows you to scale existing force values:
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
The following table shows surface loads available in each discipline and their corresponding labels:
Table 2.5: Surface Loads Available in Each Discipline
|Surface Charge Density||CHRGS|
|All||Superelement Load Vector||SELV|
|Acoustic||Fluid-structure interaction (FSI) flag||FSI|
|Impedance or admittance coefficient||IMPD|
|Surface normal velocity or acceleration||SHLD|
|Maxwell surface flag or equivalent source surface||MXWF|
|Free surface flag||FREE|
|Exterior Robin radiation boundary flag||INF|
|Viscous-thermal boundary layer surface flag||BLI|
The following table shows the commands to apply, list, and delete surface loads. You can apply them at nodes and elements, as well as at lines and areas.
Table 2.6: Commands for Applying Surface Loads
Below are examples of some of the GUI paths to use for applying surface loads.
The 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 is used.
The program 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 (such as SHELL281) are applied on the nodal plane. KEYOPT(11) determines the location of the nodal plane within the shell. When using flat elements to represent doubly curved surfaces, values which should be a function of the active radius of the meridian be inaccurate.
To apply pressure loads on the lateral faces and the two ends of beam elements, use one of the following:
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.
The SFFUN command specifies a "function" of node number versus surface load to be used when you apply surface loads on nodes or elements.
It is useful when you want to apply nodal surface loads calculated elsewhere (by another software package, for instance). You should first define the function in the form of an array parameter containing the load values. The location of the value in the array parameter implies the node number. For example, the array parameter shown below specifies four surface load values at nodes 1, 2, 3, and 4, respectively.
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.
You can use either of the following to specify that a gradient (slope) is to be used for subsequently applied surface loads:
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, specify the following:
The type of load to be controlled (the
The coordinate system and coordinate direction in
which the slope is defined (
The coordinate location where the value of the load
(as specified on a subsequent surface load command) is in effect (
The slope (
For example, the hydrostatic pressure
(Lab = PRES) shown in Figure 2.9: Example of Surface Load Gradient is to be applied.
Its slope can be specified in the global Cartesian system (
SLKCN = 0) in the Y direction (
Sldir = Y). The pressure (specified on a subsequent SF command) is 500 at Y = 0 (
SLZER = 0),
and decreases by 25 units per length in the positive Y direction (
SLOPE = -25).
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
When specifying the gradient in a cylindrical coordinate system
SLKCN = 1, for example), keep some additional
points in mind. First,
SLZER is in degrees,
SLOPE is in units of load/degree.
Second, you need to follow two guidelines:
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,
SLZER should be between 0° and 360° if the singularity is at 0°
The following example illustrates why these guidelines are suggested. Consider a semicircle shell as shown in Figure 2.10: Tapered Load on a Cylindrical Shell, 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 θ coordinates of the shell range from -90° to +90°. The following commands 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°, tapering at 1 unit per degree SF,ALL,PRES,400 ! Pressure at all selected nodes: ! 400 at -90°, 490 at 0°, 580 at +90°.
At -90°, the pressure value is 400 (as specified), increasing as θ increases by a slope of 1 unit per degree, to 490 at 0° and 580 at +90°.
You might think to specify 270°, rather than -90°, for SLZER, as follows:
SFGRAD,PRES,11,Y,270,1 ! Slope the pressure in the theta direction ! of C.S. 11. Specified pressure in effect ! at 270°, tapering at 1 unit per degree SF,ALL,PRES,400 ! Pressure at all selected nodes: ! 400 at -90°, 490 at 0°, 580 at +90°
As shown on the left in Figure 2.11: Violation of Guideline 2 (left) and Guideline 1 (right), however,
specifying 270° results in a tapered load much different than
the one intended. This behavior occurs because the singularity is
still located at 180° (the θ coordinates still range from
-90° to +90°), but SLZER is not between -180° and +180°. As a result, the program
uses a load value of 400 at 270°, and a slope of 1 unit per degree
to calculate the applied load values of 220 at +90°, 130 at 0°,
and 40 at -90°. Avoid this behavior by following the second guideline,
that is, specifying
SLZER to be a value
between ±180° when the singularity is at 180°, and
between 0° and 360° when the singularity is at 0°.
Suppose that you change the singularity location to 0°, thereby satisfying the second guideline (270° is then between 0° and 360°). But then the θ 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° SFGRAD,PRES,11,Y,270,1 ! Slope the pressure in the theta direction ! of C.S. 11. Specified pressure in effect ! at 270°, tapering at 1 unit per degree SF,ALL,PRES,400 ! Pressure at all selected nodes: ! 400 at 270°, 490 at 360°, 220 at +90° ! and 130 at 0°
Again, the program uses a load value of 400 at 270° and a slope of 1 unit per degree to calculate the applied load values of 400 at 270°, 490 at 360°, 220 at 90°, and 130 at 0°. Violating Guideline 1 cause a singularity in the tapered load itself, as shown on the right in Figure 2.11: Violation of Guideline 2 (left) and Guideline 1 (right). Due to node discretization, the actual load applied not change as abruptly at the singularity as it is shown in the figure. Instead, the node at 0° have the load value of, in the case shown, 130, while the next node clockwise (say, at 358°) have a value of 488.
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 SURF153 with face 3 loading or SURF154 with face 4 loading.
By default, if you repeat a surface load at the same surface, the new specification replaces the previous one. You can change this default to add (for accumulation) or ignore using one of the following:
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.
To transfer surface loads that have been applied to the solid model to the corresponding finite element model, use one of the following:
Occasionally, you may need to apply a surface load that the element type you are using does not accept. For example, you may need to apply uniform tangential (or any non-normal or directed) pressures on structural solid elements, radiation specifications on thermal solid elements, etc. In such cases, you can overlay the surface where you want to apply the load with surface effect elements and use them as a "conduit" to apply the desired loads. Currently, the following surface effect elements are available: SURF151 and SURF153 for 2-D models and SURF152, SURF154, SURF156, and SURF159 for 3-D models.
The following table shows all body loads available in each discipline and their corresponding labels:
Table 2.7: Body Loads Available in Each Discipline
|Thermal||Heat Generation Rate||HGEN|
|Volume Charge Density||CHRGD|
|Diffusion||Diffusing Substance Generation Rate||DGEN|
|Acoustic||Mass source or mass source rate||JS|
|Velocity or acceleration||VELO|
The following table shows the commands to apply, list, and delete body loads. You can apply them at nodes, elements, keypoints, lines, areas, and volumes.
Table 2.8: Commands for Applying Body Loads
Below are examples of some of the GUI paths to use for applying body loads:
Note: Body loads you specify on nodes are independent of those specified on elements. For a given element, the program 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.
The BFE command specifies body loads on an element-by-element basis. However, you can specify body loads at several locations on an element, requiring multiple load values for one element. The locations used vary from element type to element type, as shown in the examples that follow. The defaults (for locations where no body loads are specified) also vary from element type to element type. Therefore, be sure to refer to the element documentation online or in the Element Reference before you specify body loads on elements.
For 2-D and 3-D solid elements (PLANEnnn and SOLIDnnn), the locations for body loads are usually the corner nodes.
Figure 2.12: BFE Load Locations
For 2-D and 3-D Solids
For shell elements (SHELLnnn), the locations for body loads are usually the "pseudo-nodes" at the top and bottom planes, as shown below.
Figure 2.13: BFE Load Locations for Shell Elements
Line elements (BEAMnnn, LINKnnn, PIPEnnn, etc.) are similar to shell elements; the locations for body loads are usually the pseudo-nodes at each end of the element.
Figure 2.14: BFE Load Locations for Beam and Pipe Elements
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.
You can use the BFK command to apply body loads at keypoints. If you specify loads at the corner keypoints of an area or a volume, all load values must be equal for the loads to be transferred to the interior nodes of the area or volume. If you specify unequal load values, they are transferred (with linear interpolation) to only the nodes along the lines that connect the keypoints. Figure 2.15: Transfers to BFK Loads to Nodes illustrates this:
You can use the BFK command to specify table names at keypoints. If you specify table names at the corner keypoints of an area or a volume, all table names must be equal for the loads to be transferred to the interior nodes of the area or volume.
Figure 2.15: Transfers to BFK Loads to Nodes
You can use the BFL, BFA, and BFV commands to specify body loads on lines, areas, and volumes of a solid model, respectively. Body loads on lines of a solid model are transferred to the corresponding nodes of the finite element model. Body loads on areas or volumes of a solid model are transferred to the corresponding elements of the finite element model.
The BFUNIF command specifies a uniform body load at all nodes in the model. Most often, you use this command or path to specify a uniform temperature field; that is, a uniform temperature body load in a structural analysis or a uniform starting temperature in a transient or nonlinear thermal analysis. This is also the default temperature at which the program evaluates temperature-dependent material properties.
Another way to specify a uniform temperature is as follows:
By default, if you repeat a body load at the same node or same element, the new specification replaces the previous one. You can change this default to ignore using one of the following:
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.
To transfer body loads that have been applied to the solid model to the corresponding finite element model, use one of the following:
You can scale existing body load values using these commands:
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.
Every element have its body loads determined by the corresponding solid body load. Any BFK's present 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 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 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 transfer to area elements, (5) BFV loads on an attached volume that did NOT transfer to volume elements, (6) directly defined BF loads, or (7) BFUNIF loads.
In "Case C" situations, the following conflicts can arise:
The program transfers body loads that have been applied to the solid model to the corresponding finite element model in the following sequence:
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.
Changing the value of BFK, BFL, BFA, or BFV constraints between solutions may produce many of these warnings at the 2nd or later solid BC transfer. These can be prevented if you delete the nodal BF loads between solutions using BFVDELE, BFADELE, BFLDELE, and/or BFDELE.
Use the following commands for inertia loads:
Figure 2.16: Inertia Loads Commands
|Whole structure||Component-based||Vector in the global (X,Y,Z)|
There are no specific commands to list or delete inertia loads. To list them, issue STAT, INRTIA. To remove an inertia load, 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. The CMACEL command is similar to the ACEL command, except that the translational acceleration applies to a component and not the whole structure.
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.
You can also use the CMOMEGA and CMDOMEGA commands to specify the rotational velocity and acceleration effects for element components you define. You either specify an axis and the scalar vector quantity, or define the three components of the rotational value and the point in space you are considering. You can use these commands for Element components only.
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 program requires you to use consistent units for mass. If you are accustomed to the U. S. Customary 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 only be used in a static analysis.
No angular velocity or angular acceleration is applied.
Gravitational acceleration is unity (g = 1.0).
A handy way to specify density so that you can use it readily in either a "convenient," weight-density form or "consistent," mass-density form is to define a parameter for gravitational acceleration, g:
Table 2.9: 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|
Ocean loading includes the effects of
waves, current, drag, and buoyancy. Loading is input globally via
the ocean family
of commands (OC
xxxxxx). Ocean loading is supported in static, full
transient (TRNOPT,FULL), and full harmonic (HROPT,FULL) analyses.
The following ocean-loading input groups are available:
Basic (required for any ocean loading)
Current (optional, for applying drift current)
Wave (optional, for applying a wave state)
Zone (optional, for applying local ocean effects)
All ocean loading requires specifying the linear acceleration
of the global Cartesian reference frame (ACEL,
ACEL_Y = 0.0, and
ACEL_Z = acceleration due
Ocean-loading support is available for the following current-technology elements:
|SURF154||3-D Structural Surface Effect|
|LINK180||3-D Spar (or Truss)|
|BEAM188||3-D 2-Node Beam|
|BEAM189||3-D 3-Node Beam|
|PIPE288||3-D 2-Node Pipe|
|PIPE289||3-D 3-Node Pipe|
For more information, see the following related topics:
A coupled-field analysis usually involves applying results data from one analysis as loads in a second analysis. For example, you can apply the nodal temperatures calculated in a thermal analysis as body loads in a structural analysis (for thermal strain). Similarly, you can apply magnetic forces calculated in a magnetic field analysis as nodal forces in a structural analysis. To apply such coupled-field loads, use one of the following:
See the Coupled-Field Analysis Guide for details about how to use this command in different types of coupled-field analyses.
For constraints, surface loads, body loads, and Y-direction accelerations, you define loads exactly as they would be for any nonaxisymmetric model. However, for concentrated forces the procedure is a little different. For these quantities, input load values of force, moment, etc. are on a "360° basis." That is, the load value is entered in terms of total load around the circumference. For example, if an axisymmetric axial load of 1500 pounds per inch of circumference were applied to a 10” diameter pipe (Figure 2.17: Concentrated Axisymmetric Loads), the total load of 47,124 lb. (1500*2 π*5 = 47,124) would be applied to node N as follows:
Axisymmetric results are interpreted in the same fashion as their corresponding input loads. That is, reaction forces, moments, etc. are reported on a total load (360°) basis.
Axisymmetric harmonic elements require that their loads be supplied in a form that the program can interpret as a Fourier series. The MODE command ( or ), together with other load commands (D, F, SF, etc.), is required for these elements. See the Command Reference for details.
Specify a sufficient number of constraints to prevent unwanted rigid-body motions, discontinuities, or singularities. For example, for an axisymmetric model of a solid structure such as a solid bar, a lack of UX constraint along the axis of symmetry can potentially allow spurious "voids" to form in a structural analysis. (See Figure 2.18: Central Constraint for Solid Axisymmetric Structure.)
If an applied load acts on a degree of freedom which offers no resistance to it (that is, perfectly zero stiffness), the program ignores the load.
You can specify initial state as a loading parameter for a structural analysis in ANSYS. Initial state loading is valid for static or full transient analyses (either linear or nonlinear), and for modal, buckling and harmonic analyses. Initial state must be applied in the first load step of an analysis.
Initial state is also available in Distributed ANSYS.
For more information, see Initial State.
To apply loads using TABLE parameters, you use the appropriate loading commands or menu paths for your analysis. However, instead of specifying an actual value for a particular load, you specify the name of a table array parameter. Not all boundary conditions support tabular loads; please refer to the documentation on the specific loads you are working with to determine if tabular loads are supported.
Note: When defining
loads via commands, you must enclose the table name in % symbols:
tabname%. For example, to specify a table
of convection values, you would issue a command similar to the following:
If your data cannot be conveniently expressed as a table, you may want to use function boundary conditions. See Using the Function Tool.
If working interactively, you can define a new table at the time you apply the loads by selecting the "new table" option. You be asked to define the table through a series of dialog boxes. You can also define a table before you apply loads by choosing the menu path *DIM command. Tabular loads can be defined in both the global Cartesian (default) or a local coordinate system you define with the LOCAL command (only Cartesian, spherical and cylindrical coordinate systems are valid). If working in batch mode, you need to define the table before issuing any of the loading commands., or by using the
When you define the table array parameter, you can define various primary variables, depending on the type of analysis you are doing. Table 2.10: Boundary Condition Type and Corresponding Primary Variable lists boundary conditions and their associated primary variables for supported types of analyses. Additional primary variables are available using function boundary conditions. See Using the Function Editor for more information. Primary variables are shown as the valid labels used by the *DIM command. You can apply tabular loads according to a local coordinate system defined via LOCAL, and specified in *DIM.
When defining the tables, the primary variables must be in ascending order in the table indices (as in any table array).
Table 2.10: Boundary Condition Type and Corresponding Primary Variable
|Boundary Condition||Primary Variable||Command |
TIME, X, Y, Z
D,,(TEMP, TBOT, TE2, TE3, . . ., TTOP)
TIME, X, Y, Z, TEMP
F,,(HEAT, HBOT, HE2, HE3, . . ., HTOP)
Film Coefficient (Convection)
TIME, X, Y, Z, TEMP, VELOCITY
Bulk Temperature (Convection)
TIME, X, Y, Z
TIME, X, Y, Z, TEMP
TIME, X, Y, Z, TEMP
Uniform Heat Generation
TIME or FREQ, X, Y, Z, TEMP
D,(UX, UY, UZ, ROTX, ROTY, ROTZ)
TIME or FREQ, X, Y, Z, TEMP
Forces and Moments
TIME or FREQ, X, Y, Z, TEMP, SECTOR
F,(FX, FY, FZ, MX, MY, MZ)
Fluid Mass Flow Rate
TIME or FREQ, X, Y, Z, TEMP, SECTOR
TIME or FREQ, X, Y, Z, TEMP, SECTOR
TIME, X, Y, Z, TEMP
TIME or FREQ, X, Y, Z
TIME or FREQ, X, Y, Z
Superelement Load Vector
TIME, X, Y, Z
TIME, X, Y, Z
TIME, X, Y, Z
|High-Frequency Electromagnetic Analyses|
TIME, X, Y, Z
TIME, X, Y, Z
TIME, X, Y, Z
TIME, X, Y, Z
|Diffusion Flow Rate|
TIME, X, Y, Z
TIME, X, Y, Z, TEMP
|Diffusion Substance Generation|
TIME, X, Y, Z, TEMP
See the *DIM command for more information on defining your labels.
VELOCITY label refers to the
magnitude of the velocity degrees of freedom or the computed fluid
velocity in FLUID116 elements.
Table 2.11: Real Constants and Corresponding Primary Variable for SURF151, SURF152, and FLUID116
Contact elements (CONTA171, CONTA172, CONTA173, CONTA174, CONTA175, CONTA176, CONTA177, and CONTA178) also support table parameter input for some real constants. For a complete list of these real constants and their associated primary variables, see Table 3.2: Real Constants and Corresponding Primary Variables for CONTA171-CONTA177 in the Contact Technology Guide and Table 178.2: Real Constants and Corresponding Primary Variables for CONTA178 in CONTA178. The following two primary variables are used exclusively with contact element real constants:
PRESSURE - contact pressure. The index values associated with PRESSURE are positive for compression and negative for tension.
GAP - geometrical contact gap/penetration. The index values associated with GAP are positive for closed penetration and negative for an open gap.
If you need to specify a variable other than one of the primary variables listed, you can do so by defining an independent parameter. To specify an independent parameter, you define an additional table for the independent parameter. That table must have the same name as the independent parameter, and can be a function of either a primary variable or another independent parameter. You can define as many independent parameters as necessary, but all independent parameters must relate to a primary variable.
For example, consider a convection coefficient (HF) that varies as a function of rotational speed (RPM) and temperature (TEMP). The primary variable in this case is TEMP. The independent parameter is RPM, which varies with time. In this scenario, you need two tables: one relating RPM to TIME, and another table relating HF to RPM and TEMP.
*DIM,SYCNV,TABLE,3,3,,RPM,TEMP SYCNV(1,0)=0.0,20.0,40.0 SYCNV(0,1)=0.0,10.0,20.0,40.0 SYCNV(0,2)=0.5,15.0,30.0,60.0 SYCNV(0,3)=1.0,20.0,40.0,80.0 *DIM,RPM,TABLE,4,1,1,TIME RPM(1,0)=0.0,10.0,40.0,60.0 RPM(1,1)=0.0,5.0,20.0,30.0 SF,ALL,CONV,%SYCNV%
When defining the tables, the independent variables must be in ascending order in the table indices (as in any table array).
For convenience, you can multiply table parameters by constants, add one table to another, and add a constant increment for offset. To do so, use the *TOPER command ( ). The two tables must have the same dimensions and must have the same variable names for the rows and columns. The tables must also have identical index values for rows, columns, etc.
If you use table array parameters to define boundary conditions, you may want to verify that the correct table and the correct values from the table were applied. You can do so in several ways:
You can look in the Output window. If you apply tabular boundary conditions on finite element or solid model entities, the name of the table, not the numerical value, is echoed in the Output window.
You can list boundary conditions. If you list the boundary conditions during /PREP7, table names are listed. Longer table names may be truncated. However, if you list boundary conditions during any of the solution or postprocessing phases at a particular entity or time point, the actual numerical value at the location or time is listed.
You can look at the graphical display. Where tabular
boundary conditions were applied, the table name and any appropriate
symbols (face outlines, arrows, etc.) can be displayed using the standard
graphic display capabilities (/PBC, /PSF, etc.), provided that table numbering is on (/PNUM,
You can look at the numerically-substituted table
of values (/PNUM,
SVAL) in POST1.
You can retrieve a value of a table parameter at any given combination of variables using the *STATUS command ( ).
An example of how to run a steady-state thermal analysis using tabular boundary conditions is described in Performing a Thermal Analysis Using Tabular Boundary Conditions.
This example shows how to run an analysis using a 5-D table. Note that 4- and 5-D tables cannot be defined interactively; you must use the command method.
This problem consists of a thermal-stress analysis with a pressure that varies as a function of (x,y,z,time,temp). The table and table values are first defined. The table is applied as a pressure boundary condition to the faces of a rectangular beam. Time and temperature are prescribed for two load steps and solved.
/batch,list /title, Illustrate use of 5D table for SF command (pressure) loading !!!! !!!! !!!! create 5D table for applied pressure X1=2 !!!! X dimensionality Y1=2 !!!! Y dimensionality Z1=10 !!!! Z dimensionality D4=5 !!!! time dimensionality D5=5 !!!! temperature dimensionality len=10 !!!! cantilever beam length wid=1 !!!! cantilever beam width hth=2 !!!! cantilever beam height *dim,xval,array,X1 !!!! create 1D arrays to load 5D table xval(1)=0,20 !!!! variations per dimension same *dim,yval,array,Y1 !!!! but give different values on each yval(1)=0,20 !!!! book and shelf *dim,zval,array,10 zval(1)=10,20,30,40,50,60,70,80,90,100 *dim,tval,array,5 tval(1)=1,.90,.80,.70,.60 *dim,tevl,array,5 tevl(1)=1,1.20,1.30,1.60,1.80 *dim,ccc,tab5,X1,Y1,Z1,D4,D5,X,Y,Z,TIME,TEMP *taxis,ccc(1,1,1,1,1),1,0,wid !!! X-Dim *taxis,ccc(1,1,1,1,1),2,0,hth !!! Y-Dim *taxis,ccc(1,1,1,1,1),3,1,2,3,4,5,6,7,8,9,10 !!! Z-Dim *taxis,ccc(1,1,1,1,1),4,0,10,20,30,40 !!! Time *taxis,ccc(1,1,1,1,1),5,0,50,100,150,200 !!! Temp *do,ii,1,2 *do,jj,1,2 *do,kk,1,10 *do,ll,1,5 *do,mm,1,5 ccc(ii,jj,kk,ll,mm)=(xval(ii)+yval(jj)+zval(kk))*tval(ll)*tevl(mm) *enddo *enddo *enddo *enddo *enddo /prep7 block,,wid,,hth,,len !!!! create beam volume et,1,5 !!!! use SOLID5 esize,0.5 !!!! element size mshkey,1 !!!! mapped mesh vmesh,all mp,ex,1,1e7 !!!! material properties mp,nuxy,1,.3 mp,kxx,1,1 nsel,s,loc,z,0 !!!! fix end of beam d,all,all fini save !!!! save problem for future restart /solu antyp,trans timint,off asel,u,loc,z,0 sfa,all,1,pres,%ccc% !!!! apply pressure to all selected areas alls time,1e-3 !!!! first solution at time = "0" nsub,1 outres,all,all !!!! output everything to results file d,all,temp,0 !!!! for first problem, temp = 0 solve time,30 !!!! second solution, time=30 d,all,temp,150 !!!! second solution, temp=150 solve finish /post1 /view,1,1,1,1 /psf,press,norm,3,0,1 /pbc,all,0 set,1,1 /title, Pressure distribution; time=0, temp=0 eplot set,2,1 /title, Pressure distribution; time=30, temp=150 eplot finish
The following plots illustrate the pressure distribution for the two load cases.
Note the difference in the pressure load in the second load case.
You can use components and assemblies to apply loads to portions of the mode:
For related information, see Using Components and Assemblies.
Apply loads to portions of the model using a component as follows:
The SF command specifies the film coefficient
of 10 on nodes in the component (
All nodes in the component are retrieved regardless of the entity
cmpALLSEL,BELOW,ALL SF,ALL,CONV, 10