Release 11.0 Documentation for ANSYS
www.kxcad.net Home > CAE Index > ANSYS Index > Release 11.0 Documentation for ANSYS
The output from the solution consists of the nodal solution (or the primary degree of freedom solution) and the element solution (or the derived solution). Each of these solutions is described below. Solution output is written to the output file (Jobname.OUT, also known as the "printout"), the database, and the results file (Jobname.RST, Jobname.RTH, Jobname.RMG, or Jobname.RFL). The output file can be viewed through the GUI, while the database and results file data (sometimes called the "post data") can be postprocessed.
The output file contains the nodal DOF solution, nodal and reaction loads, and the element solutions, depending on the OUTPR settings. The element solutions are primarily the centroidal solution values for each element. Most elements have KEYOPTS to output more information (e.g. integration points).
The results file contains data for all requested [OUTRES] solutions, or load steps. In POST1, you issue the SET command to identify the load step you wish to postprocess. Results items for the area and volume elements are generally retrieved from the database by commands such as PRNSOL, PLNSOL, PRESOL, PLESOL, etc. The labels on these commands correspond to the labels shown in the input and output description tables for each element (such as "PLANE42 Input Summary" and Table 42.1: "PLANE42 Element Output Definitions" for PLANE42). For example, postprocessing the X-stress (typically labeled SX) is identified as item S and component X on the postprocessing commands. Coordinate locations XC, YC, ZC are identified as item CENT and component X, Y, or Z. Only items shown both on the individual command and in the element input/output tables are available for use with that command. An exception is EPTO, the total strain, which is available for all structural solid and shell elements even though it is not shown in the output description tables for those elements.
Generic labels do not exist for some results data, such as integration point data, all derived data for structural line elements (such as spars, beams, and pipes) and contact elements, all derived data for thermal line elements, and layer data for layered elements. Instead, a sequence number is used to identify these items (described below).
The nodal solution from an analysis consists of:
the degree of freedom (DOF) solution, such as nodal displacements, temperatures, and pressures
the reaction solution calculated at constrained nodes - forces at displacement constraints, heat flows at temperature DOF constraints, fluid flows at pressure DOF constraints, and so on.
The DOF solution is calculated for all active degrees of freedom in the model, which are determined by the union of all DOF labels associated with all the active element types. It is output at all degrees of freedom that have a nonzero stiffness or conductivity and can be controlled by OUTPR,NSOL (for printed output) and OUTRES,NSOL (for results file output).
The reaction solution is calculated at all nodes that are constrained (D, DSYM, etc.). Its output can be controlled by OUTPR,RSOL and OUTRES,RSOL.
For vector degrees of freedom and corresponding reactions, the output during solution is in the nodal coordinate system. If a node was input with a rotated nodal coordinate system, the output nodal solution will also be in the rotated coordinate system. For a node with the rotation θxy = 90°, the printed UX solution will be in the nodal X direction, which in this case corresponds to the global Y direction. Rotational displacements (ROTX, ROTY, ROTZ) are output in radians, and phase angles from a harmonic analysis are output in degrees.
The element output items (and their definitions) are shown along with the element type description. Not all of the items shown in the output table will appear at all times for the element. Normally, items not appearing are either not applicable to the solution or have all zero results and are suppressed to save space. However, except for the coupled-field elements PLANE223, SOLID226, and SOLID227, coupled-field forces appear if they are computed to be zero. The output is, in some cases, dependent on the input. For example, for thermal elements accepting either surface convection (CONV) or nodal heat flux (HFLUX), the output will be either in terms of convection or heat flux. Most of the output items shown appear in the element solution listing. Some items do not appear in the solution listing but are written to the results file.
Most elements have 2 tables which describe the output data and ways to access that data for the element. These tables are the "Element Output Definitions" table and the "Item and Sequence Numbers" tables used for accessing data through the ETABLE and ESOL commands.
The first table, "Element Output Definitions," describes possible output for the element. In addition, this table outlines which data are available for solution printout (Jobname.OUT and/or display to the terminal), and which data are available on the results file (Jobname.RST, Jobname.RTH, Jobname.RMG, etc.). It's important to remember that only the data which you request with the solution commands OUTPR and OUTRES are included in printout and on the results file, respectively. See Table 3.1: "BEAM3 Element Output Definitions" for a sample element output definitions table. As an added convenience, items in this table which are available through the Component Name method of the ETABLE command are identified by special notation (:) included in the output label. See The General Postprocessor (POST1) in the Basic Analysis Guide for more information. The label portion before the colon corresponds to the Item field on the ETABLE command, and the portion after the colon corresponds to the Comp field. For example, S:EQV is defined as equivalent stress, and the ETABLE command for accessing this data would be:
ETABLE,ABC,S,EQV
where ABC is a user-defined label for future identification on listings and displays. Other data having labels without colons can be accessed through the Sequence Number method, discussed with the "Item and Sequence Number" tables below.
In some cases there is more than one label which can be used after the colon, in which case they are listed and separated by commas. The Definition column defines each label and, in some instances, also lists the label used on the printout, if different. The O column indicates those items which are written to the output window and/or the output file. The R column indicates items which are written to the results file and which can be obtained in postprocessing.
Many elements also have a table, or set of tables, that list the Item and sequence number required for data access using the Sequence Number method of the ETABLE command. See The General Postprocessor (POST1) in the Basic Analysis Guide for an example. The number of columns in each table and the number of tables per element vary depending on the type of data available and the number of locations on the element where data was calculated. For structural line elements, for example, the KEYOPT(9) setting will determine the number of locations (intermediate points) along the element where data is to be calculated.
For example, assume we want to determine the sequence number required to access the member moment in the Z direction (MMOMZ) for a BEAM3 element. Assume also that the data we want to obtain is at end J, and that KEYOPT(9) = 1, that is, data has also been calculated at one intermediate location. See Table 3.4: "BEAM3 Item and Sequence Numbers (KEYOPT(9) = 3)" for a sample item and sequence numbers table. Locate MMOMZ under the "Name" column. Notice that the Item is listed as SMISC. SMISC refers to summable miscellaneous items, while NMISC refers to nonsummable miscellaneous items (see the Basic Analysis Guide for more details). Follow across the row until you find the sequence number, 18, in the J column. The correct command to move MMOMZ at end J for BEAM3 (KEYOPT(9) = 1) to the element table is:
ETABLE,ABC,SMISC,18
ABC is a user-defined label for later identification on listings and displays.
Pressure output for structural elements shows the input pressures expanded to the element's full tapered-load capability. See the SF, SFE, and SFBEAM commands for pressure input. For example, for element type PLANE42, which has an input load list of "Pressures: Face 1 (J-I), Face 2 (K-J), Face 3 (L-K), Face 4 (I-L)," the output PRESSURE line expands the pressures to P1(J), P1(I); P2(K), P2(J); P3(L), P3(K); and P4(I), P4(L). P1(J) should be interpreted as the pressure for load key 1 (the pressure normal to face 1) at node J; P1(I) is load key 1 at node I; etc. If the pressure is input as a constant instead of tapered, both nodal values of the pressure will be the same. Beam elements which allow an offset from the node have addition output labeled OFFST. To save space, pressure output is often omitted when values are zero. Similarly, other surface load items (such as convection (CONV) and heat flux (HFLUX)), and body load input items (such as temperature (TEMP), fluence (FLUE), and heat generation (HGEN)), are often omitted when the values are zero (or, for temperatures, when the T-TREF values are zero).
Output such as stress, strain, temperature, etc. in the output listing is given at the centroid (or near center) of the element. The location of the centroid is updated if large deflections are used. The output quantities are calculated as the average of the integration point values (see the Theory Reference for ANSYS and ANSYS Workbench). The component output directions for vector quantities correspond to the input material directions which, in turn, are a function of the element coordinate system. For example, the SX stress is in the same direction as EX. In postprocessing, ETABLE may be used to compute the centroidal solution of each element from its nodal values.
Surface output is available in the output listing on certain free surfaces of solid elements. A free surface is a surface not connected to any other element and not having any DOF constraint or nodal force load on the surface. Surface output is not valid on surfaces which are not free or for elements having nonlinear material properties. Surface output is also not valid for elements deactivated [EKILL] and then reactivated [EALIVE]. Surface output does not include large strain effects.
The surface output is automatically suppressed if the element has nonlinear material properties. Surface calculations are of the same accuracy as the displacement calculations. Values are not extrapolated to the surface from the integration points but are calculated from the nodal displacements, face load, and the material property relationships. Transverse surface shear stresses are assumed to be zero. The surface normal stress is set equal to the surface pressure. Surface output should not be requested on condensed faces or on the zero-radius face (center line) of an axisymmetric model.
For 3-D solid elements, the face coordinate system has the x-axis in the same general direction as the first two nodes of the face, as defined with pressure loading. The exact direction of the x-axis is on the line connecting the midside nodes or midpoints of the two opposite edges. The y-axis is normal to the x-axis, in the plane of the face.
Table 2.1: "Output Available through ETABLE" lists output available through the ETABLE command using the Sequence Number method (Item = SURF). See the appropriate table (4.xx.2) in the individual element descriptions for definitions of the output quantities.
Table 2.1 Output Available through ETABLE
| Element Dimensionality | |||
|---|---|---|---|
| snum | 3-D | 2-D | Axisymm |
| 1 | FACE | FACE | FACE |
| 2 | AREA | AREA | AREA |
| 3 | TEMP | TEMP | TEMP |
| 4 | PRES | PRES | PRES |
| 5 | EPX | EPPAR | EPPAR |
| 6 | EPY | EPPER | EPPER |
| 7 | EPZ | EPZ | EPZ |
| 8 | EPXY | 0 | EPSH [1] |
| 9 | SX | SPAR | SPAR |
| 10 | SY | SPER | SPER |
| 11 | SZ | SZ | SZ |
| 12 | SXY | 0 | 0 |
| 13 | 0 | 0 | 0 |
| 14 | 0 | 0 | SSH [1] |
| 15 | S1 | S1 | S1 |
| 16 | S2 | S2 | S2 |
| 17 | S3 | S3 | S3 |
| 18 | SINT | SINT | SINT |
| 19 | SEQV | SEQV | SEQV |
If an additional face has surface output requested, then snum 1-19 are repeated as snum 20-38.
Convection heat flow output may be given on convection surfaces of solid thermal elements. Output is valid on interior as well as exterior surfaces. Convection conditions should not be defined on condensed faces or on the zero-radius face (center line) of an axisymmetric model.
Integration point output is available in the output listing with certain elements. The location of the integration point is updated if large deflections are used. See the element descriptions in the Theory Reference for ANSYS and ANSYS Workbench for details about integration point locations and output. Also the ERESX command may be used to request integration point data to be written as nodal data on the results file.
The term element nodal means element data reported for each element at its nodes. This type of output is available for 2-D and 3-D solid elements, shell elements, and various other elements. Element nodal data consist of the element derived data (e.g. strains, stresses, fluxes, gradients, etc.) evaluated at each of the element's nodes. These data are usually calculated at the interior integration points and then extrapolated to the nodes. Exceptions occur if an element has active (nonzero) plasticity, creep, or swelling at an integration point or if ERESX,NO is input. In such cases the nodal solution is the value at the integration point nearest the node. See the Theory Reference for ANSYS and ANSYS Workbench for details. Output is usually in the element coordinate system. Averaging of the nodal data from adjacent elements is done within POST1.
These are an element's loads (forces) acting on each of its nodes. They are printed out at the end of each element output in the nodal coordinate system and are labeled as static loads. If the problem is dynamic, the damping loads and inertia loads are also printed. The output of element nodal loads can be controlled by OUTPR,NLOAD (for printed output) and OUTRES,NLOAD (for results file output).
Element nodal loads relate to the reaction solution in the following way: the sum of the static, damping, and inertia loads at a particular degree of freedom, summed over all elements connected to that degree of freedom, plus the applied nodal load (F or FK command), is equal to the negative of the reaction solution at that same degree of freedom.
For information about nonlinear solution due to material nonlinearities, see the Theory Reference for ANSYS and ANSYS Workbench. Nonlinear strain data (EPPL, EPCR, EPSW, etc.) is always the value from the nearest integration point. If creep is present, stresses are computed after the plasticity correction but before the creep correction. The elastic strains are printed after the creep corrections.
A 2-D solid analysis is based upon a "per unit of depth" calculation and all appropriate output data are on a "per unit of depth" basis. Many 2-D solids, however, allow an option to specify the depth (thickness). A 2-D axisymmetric analysis is based on a full 360°. Calculation and all appropriate output data are on a full 360° basis. In particular, the total forces for the 360° model are output for an axisymmetric structural analysis and the total convection heat flow for the 360° model is output for an axisymmetric thermal analysis. For axisymmetric analyses, the X, Y, Z, and XY stresses and strains correspond to the radial, axial, hoop, and in-plane shear stresses and strains, respectively. The global Y axis must be the axis of symmetry, and the structure should be modeled in the +X quadrants.
Member force output is available with most structural line elements. The listing of this output is activated with a KEYOPT described with the element and is in addition to the nodal load output. Member forces are in the element coordinate system and the components correspond to the degrees of freedom available with the element. For example, member forces printed for BEAM3 would be MFORX, MFORY, MMOMZ.
For BEAM3, BEAM4, BEAM44, BEAM54, SHELL61, PIPE16, PIPE17, PIPE18, PIPE20, PIPE59, and PIPE60, the signs of their member forces at all locations along the length of the elements are based on force equilibrium of the member segment from end I to that location. For example, for the simple one-element cantilever beam loaded as shown, the tensile force and the bending moments are positive at all points along the element, including both ends.
Failure criteria are commonly used for orthotropic materials. They can be input using either the FC commands or the TB commands. The FC command input is used in POST1. The TB command input is used directly in the composite elements and is described below.
The failure criteria table is started by using the TB command (with Lab = FAIL). The data table is input in two parts:
the failure criterion keys
the failure stress/strain data.
Data not input are assumed to be zero. See the Theory Reference for ANSYS and ANSYS Workbench for an explanation of the predefined failure criteria. The six failure criterion keys are defined with the TBDATA command following a special form of the TBTEMP command [TBTEMP,,CRIT] to indicate that the failure criterion keys are defined next. The constants (C1-C6) entered on the TBDATA command are:
Table 2.2 Orthotropic Material Failure Criteria Data
| Constant | Meaning | ||||
|---|---|---|---|---|---|
| 1 | Maximum Strain Failure Criterion - Output
as FC1 (uses strain constants 1-9)
| ||||
| 2 | Maximum Stress Failure
Criterion - Output as FC2 (uses stress constants 10-18) Options are the same as for constant 1, except subroutine is USRFC2. | ||||
| 3 | Tsai-Wu Failure Criterion - Output as FC3 (uses
constants 10-21)
| ||||
| 4-6 | User-defined Failure
Criteria - Output as FC4 TO FC6
|
The failure data, which may be temperature-dependent, must be defined with the TBDATA command following a temperature definition on the TBTEMP command. Strains must have absolute values less than 1.0. Up to six temperatures (NTEMP = 6 maximum on the TB command) may be defined with the TBTEMP commands. The constants (C1-C21) entered on the TBDATA command (6 per command), after each TBTEMP command, are:
Constant - (Symbol) - Meaning
1 - (
)
- Failure strain in material x-direction in tension (must be positive).
2 - (
)
- Failure strain in material x-direction in compression (default = -) (may not be positive).
3 - (
)
- Failure strain in material y-direction in tension (must be positive).
4 - (
)
- Failure strain in material y-direction in compression (default = -) (may not be positive).
5 - (
)
- Failure strain in material z-direction in tension (must be positive).
6 - (
)
- Failure strain in material z-direction in compression (default = -) (may not be positive).
7 - (
)
- Failure strain in material x-y plane (shear) (must be positive).
8 - (
)
- Failure strain in material y-z plane (shear) (must be positive).
9 - (
)
- Failure strain in material x-z plane (shear) (must be positive).
10 - (
)
- Failure stress in material x-direction in tension (must be positive).
11 - (
)
- Failure stress in material x-direction in compression (default = -) (may not be positive).
12 - (
)
- Failure stress in material y-direction in tension (must be positive).
13 - (
)
- Failure stress in material y-direction in compression (default = -) (may not be positive).
14 - (
)
- Failure stress in material z-direction in tension (must be positive).
15 - (
)
- Failure stress in material z-direction in compression (default = -) (may not be positive).
16 - (
)
- Failure stress in material x-y plane (shear) (must be positive).
17 - (
)
- Failure stress in material y-z plane (shear) (must be positive).
18 - (
)
- Failure stress in material x-z plane (shear) (must be positive).
19 - (
)
- x-y coupling coefficient for Tsai-Wu Theory (default = -1.0).
20 - (
)
- y-z coupling coefficient for Tsai-Wu Theory (default = -1.0).
21 - (
)
- x-z coupling coefficient for Tsai-Wu Theory (default = -1.0).
Tsai-Wu coupling coefficients must be between
-2.0 and 2.0. Values between -1.0 and 0.0 are recommended. For 2-D analysis,
set , , , and to
a value several orders of magnitude larger than , , or ; and
set Cxz and Cyz to zero.
See the TB command for a listing of the elements that can be used with the FAIL material option.
See Specifying Failure Criteria in the Structural Analysis Guide for more information on this material option.