5.2. Reviewing Results in POST1

www.kxcad.net Home > CAE Index > ANSYS Index > Release 11.0 Documentation for ANSYS



Once the desired results data are stored in the database, you can review them through graphics displays and tabular listings. In addition, you can map the results data onto a path (for details, see Mapping Results onto a Path).

5.2.1. Displaying Results Graphically

Graphics displays are perhaps the most effective way to review results. You can display the following types of graphics in POST1:

  • Contour displays

  • Deformed shape displays

  • Vector displays

  • Path plots

  • Reaction force displays

  • Particle flow traces.

5.2.1.1. Contour Displays

Contour displays show how a result item (such as stress, temperature, magnetic flux density, etc.) varies over the model. Four commands are available for contour displays:

Command(s): PLNSOL
GUI: Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu
Command(s): PLESOL
GUI: Main Menu> General Postproc> Plot Results> Contour Plot> Element Solu
Command(s): PLETAB
GUI: Main Menu> General Postproc> Plot Results> Contour Plot> Elem Table
Command(s): PLLS
GUI: Main Menu> General Postproc> Plot Results> Line Elem Res

The PLNSOL command produces contour lines that are continuous across the entire model. Use either for primary as well as derived solution data. Derived solution data, which are typically discontinuous from element to element, are averaged at the nodes so that continuous contour lines can be displayed.

Sample contour displays of primary data (TEMP) and derived data (TGX) are shown below.

PLNSOL,TEMP             ! Primary data: degree of freedom TEMP

Figure 5.1  Contouring Primary Data with PLNSOL

If PowerGraphics is enabled, you can control averaging of derived data with the following:

Command(s): AVRES
GUI: Main Menu> General Postproc> Options for Outp
Utility Menu> List> Results> Options

Any of the above allows you to specify whether or not results will be averaged at element boundaries where material and/or real constant discontinuities exist. For more information, see "PowerGraphics".

Caution

If PowerGraphics is disabled, you cannot use the AVRES command to control averaging, and the averaging operation is performed at all nodes of the selected elements without regard to the attributes of the elements connected to them. This can be inappropriate in areas of material or geometric discontinuities. When contouring derived data (which are averaged at the nodes), be sure to select elements of the same material, same thickness (for shells), same element coordinate system orientation, etc.

PLNSOL,TG,X             ! Derived data: thermal gradient TGX

See the PLNSOL command description for further information.

Figure 5.2  Contouring Derived Data with PLNSOL

The PLESOL command produce contour lines that are discontinuous across element boundaries. Use this type of display mainly for derived solution data. For example:

PLESOL,TG,X

Figure 5.3  A Sample PLESOL Plot Showing Discontinuous Contours

The PLETAB command contours data stored in the element table. The Avglab field on the PLETAB command gives you the option of averaging the data at nodes (for continuous contours) or not averaging (the default, for having discontinuous contours). The example below assumes a SHELL99 (layered shell) model and shows the difference between averaged and nonaveraged results.

ETABLE,SHEARXZ,SMISC,9     ! Interlaminar shear (ILSXZ) at bottom of layer 2
PLETAB,SHEARXZ,AVG         ! Averaged contour plot of SHEARXZ

Figure 5.4  Averaged PLETAB Contours

PLETAB,SHEARXZ,NOAVG       ! Unaveraged (default) contour plot of SHEARXZ

Figure 5.5  Unaveraged PLETAB Contours

The PLLS command displays line element results in the form of contours. This command also requires data to be stored in the element table. This type of display is commonly used for shear and moment diagrams in beam analyses. The example below assumes a BEAM3 (2-D beam) model with KEYOPT(9) = 1:

ETABLE,IMOMENT,SMISC,6    ! Bending moment (MMOMZ) at end I, named IMOMENT
ETABLE,JMOMENT,SMISC,18   ! MMOMZ at end J, named JMOMENT
PLLS,IMOMENT,JMOMENT      ! Display results for IMOMENT, JMOMENT

Figure 5.6  Moment Diagram Using PLLS

PLLS simply draws a straight line between values at the I and J nodes of an element without any regard to how the result item varies along the element length. You can use a negative scaling factor to invert the plot.

Notes
  • You can produce isosurface contour displays by first setting Key on the /CTYPE command (Utility Menu> PlotCtrls> Style> Contours> Contour Style) to 1. See "The Time-History Postprocessor (POST26)" for more information about isosurfaces.

  • Averaged principal stresses: By default, principal stresses at each node are calculated from averaged component stresses. You can reverse this, so that principal stresses are first calculated per element, then averaged at the nodes. To do so, use the following:

    Command(s): AVPRIN
    GUI: Main Menu> General Postproc> Options for Outp
    Utility Menu> List> Results> Options

This method is not normally used, but can be useful in special circumstances. Averaging operations should not be done at nodal interfaces of differing materials.

  • Vector sum data: These follow the same practice as the principal stresses. By default, the vector sum magnitude (square root of the sum of the squares) at each node is calculated from averaged components. By using the AVPRIN command, you can reverse this, so that the vector sum magnitudes are first calculated per element, then averaged at the nodes.

  • Shell elements or layered shell elements: By default, results for shell or layered elements are assumed to be at the top surface of the shell or layer. To display results at the top, middle or bottom surface, use the SHELL command (Main Menu> General Postproc> Options for Outp). For layered elements, use the LAYER command (Main Menu> General Postproc> Options for Outp) to indicate layer number.

  • von Mises equivalent strains (EQV): The effective Poisson's ratio used in computing these quantities may be changed using the AVPRIN command.

    Command(s): AVPRIN
    GUI: Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu
    Main Menu> General Postproc> Plot Results> Contour Plot> Element Solu
    Utility Menu> Plot> Results> Contour Plot> Elem Solution

    Typically, you would set the effective Poisson's ratio to the input Poisson's ratio for elastic equivalent strain (item and component EPEL,EQV) and to 0.5 for inelastic strains (item and component EPPL,EQV or EPCR,EQV). For total strains (item and component EPTOT,EQV), you would typically use an effective Poisson's ratio between the input Poisson's ratio and 0.5. As an alternative, you can save the equivalent elastic strains using ETABLE with the effective Poisson's ratio equal to the input Poisson's ratio and save the equivalent plastic strains in another table using 0.5 as the effective Poisson's ratio, then combine the two table entries using SADD to obtain the total equivalent strain.

  • Effect of /EFACET: You may see different plots with different /EFACET settings when viewing continuous contour plots (PLNSOL). If you set /EFACET,1, the contour values for the intermediate locations are interpolated based on the average of the adjacent averaged corner node values. However, if you set /EFACET,2, the midside node values are first calculated within each element, based on the average of the adjacent unaveraged corner node values. The midside node values are then averaged together for a PLNSOL contour plot. If you issue /EFACET,4, ANSYS uses shape functions (except for higher order p-elements) to calculate results values at three subgrid points along each element edge. The subgrid values are first calculated within each element and are then averaged together for PLNSOL plots. Therefore, the contour values at the midside locations will differ with different /EFACET settings.

    In most cases, PLESOL contours will be the same regardless of /EFACET settings. However, you will see differences in PLESOL contour plots if you change /EFACET settings in conjunction with any RSYS setting other than KCN = 0. When a coordinate system other than global Cartesian is chosen (KCN = 1, 2, etc.), the results are first averaged in the global Cartesian coordinate system, and then the averaged results are transformed to the specified results coordinate system.

5.2.1.2. Deformed Shape Displays

You can use these in a structural analysis to see how the structure has deformed under the applied loads. To generate a deformed shape display, use one of the following:

Command(s): PLDISP
GUI: Utility Menu> Plot> Results> Deformed Shape
Main Menu> General Postproc> Plot Results> Deformed Shape

For example, you might issue the following PLDISP command:

PLDISP,1                ! Deformed shape superimposed over undeformed shape

Figure 5.7  A Sample PLDISP Plot

You can change the displacement scaling by issuing the /DSCALE command (Utility Menu> PlotCtrls> Style> Displacement Scaling).

Be aware that when you enter POST1, all load symbols are automatically turned off. These load symbols remain off if you subsequently re-enter the PREP7 or SOLUTION processors. If you turn the load symbols on in POST1, the resulting display will show the loads on the deformed shape.

5.2.1.3. Vector Displays

Vector displays use arrows to show the variation of both the magnitude and direction of a vector quantity in the model. Examples of vector quantities are displacement (U), rotation (ROT), magnetic vector potential (A), magnetic flux density (B), thermal flux (TF), thermal gradient (TG), fluid velocity (V), principal stresses (S), etc.

To produce a vector display, use one of the following:

Command(s): PLVECT
GUI: Main Menu> General Postproc> Plot Results> Vector Plot> Predefined
Main Menu> General Postproc> Plot Results> Vector Plot> User-Defined

To scale the arrow lengths, use one of the following:

Command(s): /VSCALE
GUI: Utility Menu> PlotCtrls> Style> Vector Arrow Scaling

PLVECT,B                ! Vector display of magnetic flux density

Figure 5.8  PLVECT Vector Plot of Magnetic Field Intensity

You can also create your own vector quantity by specifying two or three components on the PLVECT command.

5.2.1.4. Path Plots

These are graphs that show the variation of a quantity along a predefined path through the model. To produce a path plot, you need to perform these tasks:

  1. Define path attributes using the PATH command (Main Menu> General Postproc> Path Operations> Define Path> Path Status> Defined Paths).

  2. Define the points of the path using the PPATH command (Main Menu> General Postproc> Path Operation> Define Path> Modify Path).

  3. Map the desired quantity on to the path using the PDEF command (Main Menu> General Postproc> Path Operations> Map onto Path)

  4. Use the PLPATH and PLPAGM commands (Main Menu> General Postproc> Path Operations> Plot Path Items) to display the results.

More details on this appear later in Mapping Results onto a Path.

5.2.1.5. Reaction Force Displays

These are similar to boundary condition displays and are activated using the labels RFOR or RMOM on the /PBC command. Any subsequent display (produced by commands such as NPLOT, EPLOT, or PLDISP) will include reaction force symbols at points where DOF constraints were specified. The sum of nodal forces for a DOF belonging to a constraint equation does not include the force passing through that equation. See the Theory Reference for ANSYS and ANSYS Workbench.

Like reactions, you can also display nodal forces using labels NFOR or NMOM on the /PBC command (Utility Menu> PlotCtrls> Symbols). These are forces exerted by an element on its node. The sum of these forces at each node is usually zero except at constrained nodes or at nodes where loads were applied.

By default, the force (or moment) values that are printed and plotted represent the total forces (sum of the static, damping, and inertial components). The FORCE command (Main Menu> General Postproc> Options for Outp) allows you to separate the total force into individual components.

5.2.1.6. Particle Flow and Charged Particle Traces

A particle flow trace is a special form of graphics display that shows how a particle travels in a flowing fluid. A charged particle trace is a graphics display that shows how a charged particle travels in an electric or magnetic field. See "Creating Geometric Results Displays" for more information on graphic displays and see "Animation" for information on particle trace animation. See the Theory Reference for ANSYS and ANSYS Workbench for simplifying assumptions on electromagnetic particle tracing.

A particle flow or charged particle trace requires two functions:

  1. The TRPOIN command (Main Menu> General Postproc> Plot Results> Flow Trace> Defi Trace Pt). Either defines a point on the path trajectory (starting point, ending point, or anywhere in between).

  2. The PLTRAC command (Main Menu> General Postproc> Plot Results> Flow Trace> Plot Flow Tra). Either produces the flow trace on an element display. Up to 50 points can be defined and plotted simultaneously.

A sample PLTRAC plot is shown below.

Figure 5.9  A Sample Particle Flow Trace

The Item and Comp fields on PLTRAC allow you to see the variation of a specified item (such as velocity, pressure, and temperature for a particle flow trace or electric potential for a charged particle trace). The variation of the item is displayed along the path trajectory as a color-contoured ribbon.

Figure 5.10  A Sample Charge Particle Trace in Electric and/or Magnetic Fields

Tracing a particle moving in a pure magnetic field might look like this:

The path of that particle moving through a pure electric field might look like this:

Plotting that same particle in the presence of both the electric and magnetic fields (with E normal to B) would then look like this:

Other commands are:

  • TRPLIS command (Main Menu> General Postproc> Plot Results> Flow Trace> List Trace Pt) - lists trace points.

  • TRPDEL command (Main Menu> General Postproc> Plot Results> Flow Trace> Dele Trace Pt) - deletes trace points.

  • TRTIME command (Main Menu> General Postproc> Plot Results> Flow Trace> Time Interval) - defines the flow trace time interval.

  • ANFLOW command (Utility Menu> PlotCtrls> Animate> Particle Flow) - generates an animated sequence of particle flow.

Notes
  • Three array parameters are created at the time of the particle trace: TRACPOIN, TRACDATA and TRACLABL. These array parameters can be used to put the particle velocity and the elapsed time into path form. The procedure to put the arrays into a path named PATHNAME is as follows:

    *get,npts,PARM,TRACPOIN,DIM,x
    PATH,PATHNAME,npts,9,1
    PAPUT,TRACPOIN,POINTS
    PAPUT,TRACDATA,TABLES
    PAPUT,TRACLABL,LABELS
    PRPATH,S,T_TRACE,VX_TRACE,VY_TRACE,VZ_TRACE,VS_TRACE
  • Particle flow traces occasionally stop for no apparent reason. This can occur in stagnant flow regions, near wall flow regions, or when a particle is tracking along an element edge. To resolve the problem, adjust the initial particle point slightly in the cross stream direction.

  • For charged particle traces, the variables Chrg and Mass input by the TRPOIN command (Main Menu> General Postproc> Plot Results> Flow Trace> Defi Trace Pt) have units of Coulombs and kilograms, respectively, in the MKS system.

  • The particle tracing algorithm could lead to an infinite loop. For example, a charged particle trace could lead to an infinite circular loop. To avoid infinite loops, the PLTRAC command argument MXLOOP sets a limiting value.

  • Charge particle tracing could be performed after an electrostatic analysis (using only electric field), or after a magnetostatic analysis using only magnetic field or coupled magnetic and electric fields. The latter case could be done using the electric field as a body load applied either with BFE,EF command or with LDREAD,EF command.

5.2.1.7. Cracking and Crushing Plots

If you have SOLID65 elements in your model, you can use the PLCRACK command (Main Menu> General Postproc> Plot Results> Crack/Crush) to determine which elements have cracked and/or crushed. Small circles will be shown where the concrete has cracked, and small octagons will be shown where the concrete has crushed (see Figure 5.11: "Concrete Beam with Cracks"). The cracking and crushing symbols are visible when a non-hidden, vector type of display is used. To specify such a device, issue the command /DEVICE,VECTOR,ON (Utility Menu> PlotCtrls> Device Options).

Figure 5.11  Concrete Beam with Cracks

5.2.2. Surface Operations

You can map any nodal results data onto a user defined surface in POST1. You can then perform mathematical operations on these surface results to calculate meaningful quantities, including total force or average stress for a cross section, net charge inside a closed volume, fluid mass flow rate, heat flow for a cross section, and more. You can also plot contours of the mapped results.

Surface operations are available both interactively (from the GUI), and via batch (command line operations). Each of the commands is referenced below; each process is found in the Main Menu> General Postproc> Surface Operations area of the GUI. A full complement of surface commands are provided to perform surface operations.

Table 5.4  Surface Operations

These POST1 commands are used to define an arbitrary surface and to develop results information for that surface.
SUCALCCreate new result data by operating on two existing result datasets on a given surface.
SUCRCreate a surface.
SUDELDelete geometry information as well as any mapped results for specified surface or for all selected surfaces.
SUEVALPerform operations on a mapped item and store result in a scalar parameter.
SUGETMove surface geometry and mapped results to an array parameter.
SUMAPMap results onto selected surface(s).
SUPLPlot specified result data on all selected surfaces or on the specified surface.
SUPRPrint surface information.
SURESUResume surface definitions from a specified file.
SUSAVESave surface definitions and result items to a file.
SUSELSelect a subset of surfaces
SUVECTPerform Operations between two mapped result vectors.

Note

You can define surfaces only in models containing 3-D solid elements. Shells, beams and 2-D element types are not supported. Surface creation will operate on selected, valid 3-D solid elements only and ignore other element types if they are present in your model.

The basic steps for surface operations are as follows:

  • Define the surfaces using the SUCR command.

  • Map the results data on the selected surfaces using the SUSEL and SUMAP commands.

  • Operate on the results using the SUEVAL, SUCALC and SUVECT commands.

Once your data is mapped on the surface, you can review the results using the graphical display and tabular listing capabilities found in the SUPL and SUPR commands.

Additional capabilities include archiving the surface data you create to a file or an array parameter, and recalling stored surface data. The following topics relate primarily to surface definition and usage.

5.2.2.1. Defining the Surface

You define your surface using the SUCR command. This command creates your named surface (containing no more than eight characters), according to a specified category (plane, cylinder, or sphere), at a defined refinement level.

The surfaces you create fall into three categories:

  • A cross section you create based on the current working plane

  • A closed surface represented by a sphere at the current working plane origin, with a user-specified radius.

  • A cylindrical surface centered at the working plane origin, and extending infinitely in the positive and negative Z directions

For SurfType = CPLANE, nRefine refers to the number of points that define the surface. If SurfType = CPLANE, and nRefine = 0, the points reside where the cutting plane section cuts through the element. Increasing nRefine to 1 will subdivide each surface facet into 4 subfacets, thus increasing the number of points at which the results can be interpolated. nRefine can vary between 0 and 3. Increasing nRefine can have significant impact on memory and speed of surface operations.

/EFACET operations will add to this refinement, and values greater than 1 can amplify the effect of nRefine. An /EFACET setting greater than 1 divides the elements into subelements, and nRefine then refines the facets of the subelements.

For SurfType = SPHERE, and INFC, nRefine is the number of divisions along a 90° arc of the sphere (default is 90, Min = 10, Max = 90).

Each time you create a surface, the following predefined geometric items are computed and stored.

  • GCX, GCY, GCZ - global Cartesian coordinates at each point on the surface.

  • NORMX, NORMY, NORMZ - components of the unit normal at each point on the surface.

  • DA - contributory area of each point.

These items are used to perform mathematical operations with surface data (for instance, DA is required to calculate surface integrals). Once you create a surface, these quantities (using the predefined labels) are available for all subsequent math operations.

Issue SUPL,SurfName to display your defined surface. A maximum of 100 surfaces can exist within one model, and all operations (mapping results, math operations, etc.) will be carried out on all selected surfaces. You can use the SUSEL command to change the selected surface set.

See the SUCR command for more information of creating surfaces.

Note

When you define a cylinder (INFC), it is terminated at the geometric limits of your model. Also, any facet lying outside of those limits is discarded.

5.2.2.2. Mapping Results Data Onto a Surface

Once you define a surface, use the SUMAP command to map your data onto that surface. Nodal results data in the active results coordinate system is interpolated onto the surface and operated on as a result set. Your result sets can be made up of primary data (nodal DOF solution), derived data (stress, flux, gradients, etc.), FLOTRAN nodal results, and other results values.

You define your mapped data in the SUMAP command by supplying a name for the result set, and then specifying the type of data and the directional properties.

You can make the results coordinate system match the active coordinate system (used to define the path) by issuing the following pair of commands:

*GET,ACTSYS,ACTIVE,,CSYS
RSYS,ACTSYS

The first command creates a user-defined parameter (ACTSYS) that holds the value defining the currently active coordinate system. The second command sets the results coordinate system to the coordinate system specified by ACTSYS.

Results mapped on to a surface do not account for discontinuities (e.g., material discontinuities) but are based on the currently selected set of elements. Selecting the proper set of elements is critical to valid surface operations, and improper selection will either result in failed mapping, or produce invalid results.

To clear result sets from the selected surfaces (except GCX, GCY, GCZ, NORMX, NORMY, NORMZ, DA), issue SUMAP,RSetname,CLEAR. To form additional labeled result sets by operating on existing surface result sets, use the SUEVAL, SUVECT or SUCALC commands.

5.2.2.3. Reviewing Surface Results

You can use the SUPL command to visually display your surface results, or use the SUPR command to get a tabular listing.

SUPL of a single result set item is displayed as a contour plot on the selected surfaces. You can also obtain a vector plot (such as for fluid velocity vector) by using a special result set naming convention. If SetName is a "vector prefix" (i.e., if SetNameX, SetNameY, and SetNameZ exist), ANSYS will plot these vectors on the surface as arrows.

Example for vector plot:

  SUCREATE,SURFACE1,CPLANE     ! create a surface called "SURFACE1" 
SUMAP,VELX,V,X        ! map x,y,z velocities with VEL as prefix 
SUMAP,VELY,V,Y 
SUMAP,VELZ,V,Z 
SUPLOT,SURFACE1,VEL     ! this will result in a vector plot of velocities 
Display of facet outlines on the surface plots is controlled by /EDGE command similar to other postprocessing plots.

5.2.2.4. Performing Operations on Mapped Surface Result Sets

Three commands are available for mathematical operations among surface result sets:

  • The SUCALC command lets you add, multiply, divide, exponentiate and perform trigonometric operations on all selected surfaces.

  • The SUVECT command calculates the cross or dot product of two result vectors on all selected surfaces.

  • The SUEVAL command calculates surface integral, area weighted average, or sum of a result set on all selected surfaces. The result of this operation is an APDL scalar parameter.

5.2.2.5. Archiving and Retrieving Surface Data to a File

You can store your surface data in a file, so that when you leave POST1, it can be retrieved later. You use the SUSAVE command to store your data. Once you have saved the information for your surface, you use the SURESU command to retrieve it.

You can opt to archive all defined surfaces, all selected surfaces or only a specified surface. When you retrieve surface data, it becomes the currently active surface data. Any existing surface data is cleared.

The following input listings provides examples of archiving and retrieving operations.

/post1
! define spherical surface at WP origin, with a radius of 0.75 and 10 divisions per 90 degree arc
sucreate,surf1,sphere,0.75,10   
wpoff,,,-2                                ! offset working plane
! define a plane surface based on the intersection of working plane 
! with the currently selected elements
sucreate,surf2,cplane

susel,s,surf1           ! select surface 'surf1'
sumap,psurf1,pres   ! map pressure on surf1. Result set name "psurf1" 
susel,all                  ! select all surfaces
sumap,velx,v,x      ! map VX on both surfaces. Result set name "velx"
sumap,vely,v,y      ! map VY on both surfaces. Result set name "vely"
sumap,velz,v,z      ! map VZ on both surfaces. Result set name "velz"

supr                      ! global status of current surface data
supl,surf1,sxsurf1  !  contour plot result set sxsurf1
supl,all,velx,1          ! contour plot result set velx on all surfaces. Plot in context of all elements in 
model
supl,surf2,vel        ! vector plot of resultant velocity vector on surface "surf2"

suvect, vdotn,vel,dot,normal    !  dot product of velocity vector and surface normal
                                                 !  result is stored in result set "vdotn"
sueval, flowrate, INTG, vdotn         ! integrate "vdotn" over area to get apdl parameter "flow rate"
susave,all,file,surf                  ! Store defined surfaces in a file
finish

5.2.2.6. Archiving and Retrieving Surface Data to an Array Parameter

Writing surface data to an array allows you to perform APDL operations on your result sets. You use the SUGET command to write either the interpolated results data only (default), or the results data and the geometry data to your defined parameter. The parameter is automatically dimensioned and filled with data.

5.2.2.7. Deleting a Surface

Use the SUDEL command to delete one or more surfaces, along with the mapped results on those surfaces. You can choose to delete all surfaces, or choose to delete individual surfaces by name. Use the SUPR command to review the current list of surface names.

5.2.3. Integrating Surface Results

The INTSRF command (Main Menu> General Postproc> Nodal Calcs> Surface Integrl) allows you to integrate nodal results on a selected surface. You must first select the nodes on the surface where the nodal results are to be integrated.

You may use INTSRF to calculate lift and drag. If the surface is a fluid-solid interface, select only the fluid elements for integration. Then, select the nodes by using the EXT option on the NSEL command (Utility Menu> Select> Entities).

To use INTSRF to calculate lift and drag, you must specify a results coordinate system with the X-axis and Y-axis aligned in the direction of the incoming flow field and the direction of gravity, respectively. Then, the drag force is the force in the X-direction and the lift is the force in the Y-direction. You use INTSRF,PRES and INTSRF,TAUW to obtain the lift and drag forces, respectively. You can use INTSRF,FLOW to obtain both the lift and drag forces, separately. The outcome is written to the output (Jobname.OUT).

Integration results are in the active coordinate system (see the RSYS command). The type of results coordinate system must match the type used in the analysis. However, you may translate and rotate forces and moments as needed. You use the *GET command (Utility Menu> Parameters> Get Scalar Data) to retrieve the results.

5.2.4. Listing Results in Tabular Form

An effective way of documenting analysis results (for reports, presentations, etc.) is to produce tabular listings in POST1. Listing options are available for nodal and element solution data, reaction data, element table data, and more.

Sample Listing of PRESOL,ELEM

 PRINT ELEM ELEMENT SOLUTION PER ELEMENT
 ***** POST1 ELEMENT SOLUTION LISTING *****
  LOAD STEP     1  SUBSTEP=     1
  TIME=    1.0000         LOAD CASE=  0
 EL=     1  NODES=     1     3  MAT=  1                                                                                      BEAM3
 TEMP =    0.00    0.00    0.00    0.00
 LOCATION   SDIR        SBYT        SBYB    
  1 (I)   0.00000E+00  130.00     -130.00    
  2 (J)   0.00000E+00  104.00     -104.00    
 LOCATION   SMAX        SMIN     
  1 (I)    130.00     -130.00    
  2 (J)    104.00     -104.00    
 LOCATION  EPELDIR     EPELBYT     EPELBYB    
  1 (I)    0.000000    0.000004   -0.000004
  2 (J)    0.000000    0.000003   -0.000003
 LOCATION  EPTHDIR     EPTHBYT     EPTHBYB 
  1 (I)    0.000000    0.000000    0.000000
  2 (J)    0.000000    0.000000    0.000000
 EPINAXL =    0.000000
 EL=     2  NODES=     3     4  MAT=  1                                                                                      BEAM3
 TEMP =    0.00    0.00    0.00    0.00
 LOCATION   SDIR        SBYT        SBYB    
  1 (I)   0.00000E+00  104.00     -104.00    
  2 (J)   0.00000E+00  78.000     -78.000    
 LOCATION   SMAX        SMIN     
  1 (I)    104.00     -104.00    
  2 (J)    78.000     -78.000    
 LOCATION  EPELDIR     EPELBYT     EPELBYB    
  1 (I)    0.000000    0.000003   -0.000003
  2 (J)    0.000000    0.000003   -0.000003
 LOCATION  EPTHDIR     EPTHBYT     EPTHBYB 
  1 (I)    0.000000    0.000000    0.000000
  2 (J)    0.000000    0.000000    0.000000
 EPINAXL =    0.000000

5.2.4.1. Listing Nodal and Element Solution Data

To list specified nodal solution data (primary as well as derived), use either of the following:

Command(s): PRNSOL
GUI: Main Menu> General Postproc> List Results> Nodal Solution

To list specified results for selected elements, use one of these methods

Command(s): PRESOL
GUI: Main Menu> General Postproc> List Results> Element Solution

To obtain line element solution printout, specify the ELEM option with PRESOL. The program will list all applicable element results for the selected elements.

Sample Listing of PRNSOL,S
 PRINT S    NODAL SOLUTION PER NODE

 ***** POST1 NODAL STRESS LISTING *****                                       
 
  LOAD STEP=     5  SUBSTEP=     2                                             
   TIME=    1.0000      LOAD CASE=   0                                         
 
  THE FOLLOWING X,Y,Z VALUES ARE IN GLOBAL COORDINATES                         
 
   NODE    SX          SY          SZ          SXY         SYZ         SXZ     
      1   148.01     -294.54      .00000E+00 -56.256      .00000E+00  .00000E+00
      2   144.89     -294.83      .00000E+00  56.841      .00000E+00  .00000E+00
      3   241.84      73.743      .00000E+00 -46.365      .00000E+00  .00000E+00
      4   401.98     -18.212      .00000E+00 -34.299      .00000E+00  .00000E+00
      5   468.15     -27.171      .00000E+00  .48669E-01  .00000E+00  .00000E+00
      6   401.46     -18.183      .00000E+00  34.393      .00000E+00  .00000E+00
      7   239.90      73.614      .00000E+00  46.704      .00000E+00  .00000E+00
      8  -84.741     -39.533      .00000E+00  39.089      .00000E+00  .00000E+00
      9   3.2868     -227.26      .00000E+00  68.563      .00000E+00  .00000E+00
     10  -33.232     -99.614      .00000E+00  59.686      .00000E+00  .00000E+00
     11  -520.81     -251.12      .00000E+00  .65232E-01  .00000E+00  .00000E+00
     12  -160.58     -11.236      .00000E+00  40.463      .00000E+00  .00000E+00
     13  -378.55      55.443      .00000E+00  57.741      .00000E+00  .00000E+00
     14  -85.022     -39.635      .00000E+00 -39.143      .00000E+00  .00000E+00
     15  -378.87      55.460      .00000E+00 -57.637      .00000E+00  .00000E+00
     16  -160.91     -11.141      .00000E+00 -40.452      .00000E+00  .00000E+00
     17  -33.188     -99.790      .00000E+00 -59.722      .00000E+00  .00000E+00
     18   3.1090     -227.24      .00000E+00 -68.279      .00000E+00  .00000E+00
     19   41.811      51.777      .00000E+00 -66.760      .00000E+00  .00000E+00
     20  -81.004      9.3348      .00000E+00 -63.803      .00000E+00  .00000E+00
     21   117.64     -5.8500      .00000E+00 -56.351      .00000E+00  .00000E+00
     22  -128.21      30.986      .00000E+00 -68.019      .00000E+00  .00000E+00
     23   154.69     -73.136      .00000E+00  .71142E-01  .00000E+00  .00000E+00
     24  -127.64     -185.11      .00000E+00  .79422E-01  .00000E+00  .00000E+00
     25   117.22     -5.7904      .00000E+00  56.517      .00000E+00  .00000E+00
     26  -128.20      31.023      .00000E+00  68.191      .00000E+00  .00000E+00
     27   41.558      51.533      .00000E+00  66.997      .00000E+00  .00000E+00
     28  -80.975      9.1077      .00000E+00  63.877      .00000E+00  .00000E+00
 MINIMUM VALUES
 NODE        11           2           1          18           1           1
 VALUE   -520.81     -294.83      .00000E+00 -68.279      .00000E+00  .00000E+00
 MAXIMUM VALUES
 NODE         5           3           1           9           1           1
 VALUE    468.15      73.743      .00000E+00  68.563      .00000E+00  .00000E+00
 

5.2.4.2. Listing Reaction Loads and Applied Loads

You have several options in POST1 for listing reaction loads and applied loads. The PRRSOL command (Main Menu> General Postproc> List Results> Reaction Solu) lists reactions at constrained nodes in the selected set. The FORCE command dictates which component of the reaction data is listed: total (default), static, damping, or inertia. PRNLD (Main Menu> General Postproc> List Results> Nodal Loads) lists the summed element nodal loads for the selected nodes, except for any zero values.

Listing reaction loads and applied loads is a good way to check equilibrium. It is always good practice to check a model's equilibrium after solution. That is, the sum of the applied loads in a given direction should equal the sum of the reactions in that direction. (If the sum of the reaction loads is not what you expect, check your loading to see if it was applied properly.)

The presence of coupling or constraint equations can induce either an actual or apparent loss of equilibrium. Actual loss of load balance can occur for poorly specified couplings or constraint equations (a usually undesirable effect). Coupled sets created by CPINTF and constraint equations created by CEINTF or CERIG will in nearly all cases maintain actual equilibrium. Also, the sum of nodal forces for a DOF belonging to a constraint equation does not include the force passing through that equation, which affects both the individual nodal force and the nodal force totals. Other cases where you may see an apparent loss of equilibrium are: (a) 4-node shell elements where all 4 nodes do no lie in an exact flat plane, (b) elements with an elastic foundation specified, and (c) unconverged nonlinear solutions. See the Theory Reference for ANSYS and ANSYS Workbench.

Another useful command is FSUM. FSUM calculates and lists the force and moment summation for the selected set of nodes.

Command(s): FSUM
GUI: Main Menu> General Postproc> Nodal Calcs> Total Force Sum

Sample FSUM Output
 *** NOTE ***                          
 Summations based on final geometry and will not agree with solution     
  reactions.                                                             
 ***** SUMMATION OF TOTAL FORCES AND MOMENTS IN GLOBAL COORDINATES *****
  FX  =   .1147202    
  FY  =   .7857315    
  FZ  =   .0000000E+00
  MX  =   .0000000E+00
  MY  =   .0000000E+00
  MZ  =   39.82639    
 SUMMATION POINT=  .00000E+00  .00000E+00  .00000E+00

The NFORCE command provides the force and moment summation for each selected node, in addition to an overall summation.

Command(s): NFORCE
GUI: Main Menu> General Postproc> Nodal Calcs> Sum @ Each Node


Back To Top

Sample NFORCE Output
          ***** POST1 NODAL TOTAL FORCE SUMMATION *****
 LOAD STEP=     3  SUBSTEP=    43
  THE FOLLOWING X,Y,Z FORCES ARE IN GLOBAL COORDINATES
  NODE      FX         FY         FZ     
     1  -.4281E-01  .4212      .0000E+00
     2   .3624E-03  .2349E-01  .0000E+00
     3   .6695E-01  .2116      .0000E+00
     4   .4522E-01  .3308E-01  .0000E+00
     5   .2705E-01  .4722E-01  .0000E+00
     6   .1458E-01  .2880E-01  .0000E+00
     7   .5507E-02  .2660E-01  .0000E+00
     8  -.2080E-02  .1055E-01  .0000E+00
     9  -.5551E-03 -.7278E-02  .0000E+00
    10   .4906E-03 -.9516E-02  .0000E+00
 *** NOTE ***                            
 Summations based on final geometry and will not agree with solution     
  reactions.                                                             
 ***** SUMMATION OF TOTAL FORCES AND MOMENTS IN GLOBAL COORDINATES *****
  FX  =   .1147202    
  FY  =   .7857315    
  FZ  =   .0000000E+00
  MX  =   .0000000E+00
  MY  =   .0000000E+00
  MZ  =   39.82639    
 SUMMATION POINT=  .00000E+00  .00000E+00  .00000E+00

The SPOINT command defines the point (any point other than the origin) about which moments are summed.

GUI:
Main Menu> General Postproc> Nodal Calcs> Summation Pt> At Node
Main Menu> General Postproc> Nodal Calcs> Summation Pt> At XYZ Loc

5.2.4.3. Listing Element Table Data

To list specified data stored in the element table, use one of the following:

Command(s): PRETAB
GUI: Main Menu> General Postproc> Element Table> List Elem Table
Main Menu> General Postproc> List Results> Elem Table Data

To list the sum of each column in the element table, use the SSUM command (Main Menu> General Postproc> Element Table> Sum of Each Item).

Sample PRETAB and SSUM Output
***** POST1 ELEMENT TABLE LISTING *****                                      
 
   STAT    CURRENT     CURRENT     CURRENT 
   ELEM    SBYTI       SBYBI       MFORYI  
      1   .95478E-10 -.95478E-10 -2500.0    
      2  -3750.0      3750.0     -2500.0    
      3  -7500.0      7500.0     -2500.0    
      4  -11250.      11250.     -2500.0    
      5  -15000.      15000.     -2500.0    
      6  -18750.      18750.     -2500.0    
      7  -22500.      22500.     -2500.0    
      8  -26250.      26250.     -2500.0    
      9  -30000.      30000.     -2500.0    
     10  -33750.      33750.     -2500.0    
     11  -37500.      37500.      2500.0    
     12  -33750.      33750.      2500.0    
     13  -30000.      30000.      2500.0    
     14  -26250.      26250.      2500.0    
     15  -22500.      22500.      2500.0    
     16  -18750.      18750.      2500.0    
     17  -15000.      15000.      2500.0    
     18  -11250.      11250.      2500.0    
     19  -7500.0      7500.0      2500.0    
     20  -3750.0      3750.0      2500.0    
 MINIMUM VALUES
 ELEM        11           1           8
 VALUE   -37500.     -.95478E-10 -2500.0    
 MAXIMUM VALUES
 ELEM         1          11          11
 VALUE    .95478E-10  37500.      2500.0    
 SUM ALL THE ACTIVE ENTRIES IN THE ELEMENT TABLE  
 TABLE LABEL     TOTAL
 SBYTI     -375000.    
 SBYBI      375000.    
 MFORYI     .552063E-09

5.2.4.4. Other Listings

You can list other types of results with the following commands:

The PRVECT command (Main Menu> General Postproc> List Results> Vector Data) lists the magnitude and direction cosines of specified vector quantities for all selected elements.

The PRPATH command (Main Menu> General Postproc> List Results> Path Items) calculates and then lists specified data along a predefined geometry path in the model. You must define the path and map the data onto the path; see Mapping Results onto a Path.

The PRSECT command (Main Menu> General Postproc> List Results> Linearized Strs) calculates and then lists linearized stresses along a predefined path.

The PRERR command (Main Menu> General Postproc> List Results> Percent Error) lists the percent error in energy norm for all selected elements.

The PRITER command (Main Menu> General Postproc> List Results> Iteration Summry) lists iteration summary data.

5.2.4.5. Sorting Nodes and Elements

By default, all tabular listings usually progress in ascending order of node numbers or element numbers. You can change this by first sorting the nodes or elements according to a specified result item. The NSORT command (Main Menu> General Postproc> List Results> Sorted Listing> Sort Nodes) sorts nodes based on a specified nodal solution item, and ESORT (Main Menu> General Postproc> List Results> Sorted Listing> Sort Elems) sorts elements based on a specified item stored in the element table. For example:

NSEL,...                ! Selects nodes
NSORT,S,X               ! Sorts nodes based on SX
PRNSOL,S,COMP           ! Lists sorted component stresses

See the NSEL, NSORT, and PRNSOL command descriptions in the Commands Reference for further information.

Sample PRNSOL,S and Output after NSORT
PRINT S    NODAL SOLUTION PER NODE

  ***** POST1 NODAL STRESS LISTING *****                                       
 
  LOAD STEP=     3  SUBSTEP=    43                                             
   TIME=    6.0000      LOAD CASE=   0                                         
 
  THE FOLLOWING X,Y,Z VALUES ARE IN GLOBAL COORDINATES                         
 
   NODE    SX          SY          SZ          SXY         SYZ         SXZ     
    111  -.90547     -1.0339     -.96928     -.51186E-01  .00000E+00  .00000E+00
     81  -.93657     -1.1249     -1.0256     -.19898E-01  .00000E+00  .00000E+00
     51  -1.0147     -.97795     -.98530      .17839E-01  .00000E+00  .00000E+00
     41  -1.0379     -1.0677     -1.0418     -.50042E-01  .00000E+00  .00000E+00
     31  -1.0406     -.99430     -1.0110      .10425E-01  .00000E+00  .00000E+00
     11  -1.0604     -.97167     -1.0093     -.46465E-03  .00000E+00  .00000E+00
     71  -1.0613     -.95595     -1.0017      .93113E-02  .00000E+00  .00000E+00
     21  -1.0652     -.98799     -1.0267      .31703E-01  .00000E+00  .00000E+00
     61  -1.0829     -.94972     -1.0170      .22630E-03  .00000E+00  .00000E+00
    101  -1.0898     -.86700     -1.0009     -.25154E-01  .00000E+00  .00000E+00
      1  -1.1450     -1.0258     -1.0741      .69372E-01  .00000E+00  .00000E+00
 MINIMUM VALUES
 NODE         1          81           1         111         111         111
 VALUE   -1.1450     -1.1249     -1.0741     -.51186E-01  .00000E+00  .00000E+00
 MAXIMUM VALUES
 NODE       111         101         111           1         111         111
 VALUE   -.90547     -.86700     -.96928      .69372E-01  .00000E+00  .00000E+00

To restore the original order of nodes or elements, use the following:

Command(s): NUSORT
GUI: Main Menu> General Postproc> List Results> Sorted Listing> Unsort Nodes
Command(s): EUSORT
GUI: Main Menu> General Postproc> List Results> Sorted Listing> Unsort Elems

5.2.4.6. Customizing Your Tabular Listings

In some situations you may need to customize result listings to your specifications. The /STITLE command (which has no GUI equivalent) allows you to define up to four subtitles which will be displayed on output listings along with the main title. Other commands available for output customization are: /FORMAT, /HEADER, and /PAGE (also without GUI equivalents). They control such things as the number of significant digits, the headers that appear at the top of listings, the number of lines on a printed page, etc. These controls apply only to the PRRSOL, PRNSOL, PRESOL, PRETAB, and PRPATH commands.

5.2.5. Mapping Results onto a Path

One of the most powerful and useful features of POST1 is its ability to map virtually any results data onto an arbitrary path through your model. This enables you to perform many arithmetic and calculus operations along this path to calculate meaningful results: stress intensity factors and J-integrals around a crack tip, the amount of heat crossing the path, magnetic forces on an object, and so on. A useful side benefit is that you can see, in the form of a graph or a tabular listing, how a result item varies along the path.

Note

You can define paths only in models containing solid elements (2-D or 3-D) or shell elements. They are not available for line elements.

Three steps are involved in reviewing results along a path:

  1. Define the path attributes [PATH command].

  2. Define the path points [PPATH command].

  3. Interpolate (map) results data along the path [PDEF command].

Once the data are interpolated, you can review them using graphics displays [PLPATH or PLPAGM commands] and tabular listings or perform mathematical operations such as addition, multiplication, integration, etc. Advanced mapping techniques to handle material discontinuities and accurate computations are offered in the PMAP command (issue this command prior to PDEF).

Other path operations you can perform include archiving paths or path data to a file or an array parameter and recalling an existing path with its data. The next few topics discuss path definition and usage.

5.2.5.1. Defining the Path

To define a path, you first define the path environment and then the individual path points. Decide whether you want to define the path by picking nodes, by picking locations on the working plane, or by filling out a table of specific coordinate locations. Then create the path by picking or by using both of the commands shown below or one of the following menu paths:

Command(s): PATH,
PPATH
GUI: Main Menu> General Postproc> Path Operations> Define Path> By Nodes
Main Menu> General Postproc> Path Operations> Define Path> On Working Plane
Main Menu> General Postproc> Path Operations> Define Path> By Location

Supply the following information for the PATH command:

  • A path name (containing no more than eight characters).

  • The number of path points (between 2 and 1000). Required only in batch mode, or when defining path points using the "By Location" option. When picking is used, the number of path points equals the number of picked points.

  • The number of sets of data which may be mapped to this path. (Four is the minimum; default is 30. There is no maximum.)

  • The number of divisions between adjacent points. (Default is 20; there is no maximum.)

  • When using the "By Location" option, a separate dialog box appears for defining path points (PPATH command). Enter the Global Cartesian coordinate values of the path points. The shape of the interpolated path geometry will follow the currently active CSYS coordinate system. Alternatively, you can specify a coordinate system for geometry interpolation (CS argument on the PPATH command).

Note

To see the status of path settings, choose the PATH,STATUS command.

The PATH and PPATH commands define the path geometry in the active CSYS coordinate system. If the path is a straight line or a circular arc, you need only the two end nodes (unless you want highly accurate interpolation, which may require more path points or divisions).

Note

If necessary, use the CSCIR command (Utility Menu> WorkPlane> Local Coordinate Systems> Move Singularity) to move the coordinate singularity point before defining the path.

To display the path you have defined, you must first interpolate data along the path (see Interpolating Data Along the Path). You then issue the /PBC,PATH,1 command followed by the NPLOT or EPLOT command. Alternatively, if you are using the GUI, choose Main Menu> General Postproc> Path Operations> Plot Paths to display the path on a node plot or choose Utility Menu> Plot> Elements followed by Main Menu> General Postproc> Path Operations> Plot Paths to display the path on an element plot. ANSYS displays the path as a series of straight line segments. The path shown below was defined in a cylindrical coordinate system:

Figure 5.12  A Node Plot Showing the Path

5.2.5.2. Using Multiple Paths

A maximum of 100 paths can exist within one model. However, only one path at a time can be the current path. To change the current path, choose the PATH,NAME command. Do not specify any other arguments on the PATH command. The named path will become the new current path.

5.2.5.3. Interpolating Data Along the Path

The following commands are available for this purpose:

Command(s): PDEF
GUI: Main Menu> General Postproc> Path Operations> path operation
Command(s): PVECT
GUI: Main Menu> General Postproc> Path Operations> Unit Vector

These commands require that the path be defined first.

Using the PDEF command, you can interpolate virtually any results data along the path in the active results coordinate system: primary data (nodal DOF solution), derived data (stresses, fluxes, gradients, etc.), element table data, FLOTRAN nodal results data, and so on. The rest of this discussion (and in other documentation) refers to an interpolated item as a path item. For example, to interpolate the thermal flux in the X direction along a path, the command would be as follows:

PDEF,XFLUX,TF,X

The XFLUX value is an arbitrary user-defined name assigned to the path item. TF and X together identify the item as the thermal flux in the X direction.

Note

You can make the results coordinate system match the active coordinate system (used to define the path) by issuing the following pair of commands:

*GET,ACTSYS,ACTIVE,,CSYS
RSYS,ACTSYS

The first command creates a user-defined parameter (ACTSYS) that holds the value defining the currently active coordinate system. The second command sets the results coordinate system to the coordinate system specified by ACTSYS.

5.2.5.4. Mapping Path Data

POST1 uses {nDiv(nPts-1) + 1} interpolation points to map data onto the path (where nPts is the number of points on the path and nDiv is the number of path divisions between points [PATH]). When you create the first path item, the program automatically interpolates the following additional geometry items: XG, YG, ZG, and S. The first three are the global Cartesian coordinates of the interpolation points and S is the path length from the starting node. These items are useful when performing mathematical operations with path items (for instance, S is required to calculate line integrals). To accurately map data across material discontinuities, use the DISCON = MAT option on the PMAP command (Main Menu> General Postproc> Path Operations> Define Path> Path Options).

To clear path items from the path (except XG, YG, ZG, and S), issue PDEF,CLEAR. To form additional labeled path items by operating on existing path items, use the PCALC command (Main Menu> General Postproc> Path Operations>operation).

The PVECT command defines the normal, tangent, or position vectors along the path. A Cartesian coordinate system must be active for this command. For example, the command shown below defines a unit vector tangent to the path at each interpolation point.

PVECT,TANG,TTX,TTY,TTZ

TTX, TTY, and TTZ are user-defined names assigned to the X, Y, and Z components of the vector. You can use these vector quantities for fracture mechanics J-integral calculations, dot and cross product operations, etc. For accurate mapping of normal and tangent vectors, use the ACCURATE option on the PMAP command. Issue the PMAP command prior to mapping data.

5.2.5.5. Reviewing Path Items

To obtain a graph of specified path items versus path distance, use one of the following:

Command(s): PLPATH
GUI: Main Menu> General Postproc> Path Operations> Plot Path Item

To get a tabular listing of specified path items, use one of the following:

Command(s): PRPATH
GUI: Main Menu> General Postproc> List Results> Path Items

You can control the path distance range (the abscissa) for PLPATH and PRPATH (Main Menu> General Postproc> Path Operations> Path Range) or the PRANGE command. Path defined variables may also be used in place of the path distance for the abscissa item in the path display.

You can use two other commands, PLSECT (Main Menu> General Postproc> Path Operations> Linearized Strs) and PRSECT (Main Menu> General Postproc> List Results> Linearized Strs), to calculate and review linearized stresses along a path defined by the first two nodes on the PPATH command. Typically, you use them in pressure vessel applications to separate stresses into individual components: membrane, membrane plus bending, etc. The path is defined in the active display coordinate system.

You can display a path data item as a color area contour display along the path geometry. The contour display offset from the path may be scaled for clarity. To produce such a display, use either of the following:

Command(s): PLPAGM
GUI: Main Menu> General Postproc> Plot Results> Plot Path Items> On Geometry

5.2.5.6. Performing Mathematical Operations among Path Items

Three commands are available for mathematical operations among path items:

The PCALC command (Main Menu> General Postproc> Path Operations> operation) lets you add, multiply, divide, exponentiate, differentiate, and integrate path items.

The PDOT command (Main Menu> General Postproc> Path Operations> Dot Product) calculates the dot product of two path vectors.

The PCROSS command (Main Menu> General Postproc> Path Operations> Cross Product) calculates the cross product or two path vectors.

5.2.5.7. Archiving and Retrieving Path Data to a File

If you wish to retain path data when you leave POST1, you must store it in a file or an array parameter so that you can retrieve it later. You first select a path or multiple paths and then write the current path data to a file:

Command(s): PSEL
GUI: Utility Menu> Select> Paths
Command(s): PASAVE
GUI: Main Menu> General Postproc> Path Operations> Archive Path> Store> Paths in file

To retrieve path information from a file and store the data as the currently active path data, use the following:

Command(s): PARESU
GUI: Main Menu> General Postproc> Path Operations> Archive Path> Retrieve> Paths from file

You can opt to archive or fetch only the path data (data mapped to path (PDEF command) or the path points (defined by the PPATH command). When you retrieve path data, it becomes the currently active path data (existing active path data is replaced). If you issue PARESU and have multiple paths, the first path from the list becomes the currently active path.

Sample input and output are shown below.

/post1
path,radial,2,30,35     ! Define path name, No. points, No. sets, No. divisions
ppath,1,,.2             ! Define path by location
ppath,2,,.6
pmap,,mat               ! Map at material discontinuities
pdef,sx,s,x             ! Interpret radial stress
pdef,sz,s,z             ! Interpret hoop stress
plpath,sx,sz            ! Plot stresses
pasave                  ! Store defined paths in a file
finish
/post1
paresu                  ! retrieve path data from file
plpagm,sx,,node         ! plot radial stresses on the path
finish

5.2.5.8. Archiving and Retrieving Path Data to an Array Parameter

Writing path data to an array is useful if you want to map a particle flow or charged particle trace onto a path (PLTRAC). If you wish to retain path data in an array parameter, use the command or one of the GUI paths shown below to write current path data to an array variable:

Command(s): PAGET, PARRAY, POPT
GUI: Main Menu> General Postproc> Path Operations> Archive Path> Retrieve> Path from array
Main Menu> General Postproc> Path Operations> Archive Path> Retrieve> Paths from file

To retrieve path information from an array variable and store the data as the currently active path data, use one of the following:

Command(s): PAPUT, PARRAY, POPT
GUI: Main Menu> General Postproc> Path Operations> Archive Path> Store> Path in array
Main Menu> General Postproc> Path Operations> Archive Path> Store> Paths from file

You can opt to archive or fetch only the path data (data mapped to path (PDEF command) or the path points (defined by the PPATH command). The setting for the POPT argument on PAGET and PAPUT determines what is stored or retrieved. You must retrieve path points prior to retrieving path data and labels. When you retrieve path data, it becomes the currently active path data (existing active path data is replaced).

Sample input and output are shown below.

/post1
path,radial,2,30,35     ! Define path name, No. points, No. sets, No. divisions
ppath,1,,.2             ! Define path by location
ppath,2,,.6
pmap,,mat               ! Map at material discontinuities
pdef,sx,s,x             ! Interpret radial stress
pdef,sz,s,z             ! Interpret hoop stress
plpath,sx,sz            ! Plot stresses
paget,radpts,points     ! Archive path points in array "radpts"
paget,raddat,table      ! Archive path data in array "raddat"
paget,radlab,label      ! Archive path labels in array "radlab"
finish
/post1
*get,npts,parm,radpts,dim,x  ! Retrieve number of points from array "radpts"
*get,ndat,parm,raddat,dim,x  ! Retrieve number of data points from array "raddat"
*get,nset,parm,radlab,dim,x  ! Retrieve number of data labels form array "radlab"
ndiv=(ndat-1)/(npts-1)       ! Calculate number of divisions
path,radial,npts,ns1,ndiv    ! Create path "radial" with number of sets ns1>nset
paput,radpts,points          ! Retrieve path points
paput,raddat,table           ! Retrieve path data
paput,radlab,labels          ! Retrieve path labels
plpagm,sx,,node              ! Plot radial stresses on the path
finish

Figure 5.13  A Sample PLPATH Display Showing Stress Discontinuity at a Material Interface

Figure 5.14  A Sample PLPAGM Display

5.2.5.9. Deleting a Path

To delete one or more paths, use one of the following:

Command(s): PADELE, DELOPT
GUI: Main Menu> General Postproc> Path Operations> Delete Path
Main Menu> General Postproc> Path Operations> Delete Path

You can opt to delete all paths or choose a path to delete by name. To review the current list of path names, issue the command PATH,STATUS.

5.2.6. Estimating Solution Error

One of the main concerns in a finite element analysis is the adequacy of the finite element mesh. Is the mesh fine enough for good results? If not, what portion of the model should be remeshed? You can get answers to such questions with the ANSYS error estimation technique, which estimates the amount of solution error due specifically to mesh discretization. This technique is available only for linear structural and linear/nonlinear thermal analyses using 2-D or 3-D solid elements or shell elements.

In the postprocessor, the program calculates an energy error for each element in the model. The energy error is similar in concept to the strain energy. The structural energy error (labeled SERR) is a measure of the discontinuity of the stress field from element to element, and the thermal energy error (TERR) is a measure of the discontinuity of the heat flux from element to element. Using SERR and TERR, the ANSYS program calculates a percent error in energy norm (SEPC for structural percent error, TEPC for thermal percent error).

Note

Error estimation is based on stiffness and conductivity matrices that are evaluated at the reference temperatures (TREF). Error estimates, therefore, can be incorrect for elements with temperature-dependent material properties if those elements are at a temperature that is significantly different than TREF.

In many cases, you can significantly increase program speed by suppressing error estimation. This improved performance is most evident when error estimation is turned off in a thermal analysis. Therefore, you may want to use error estimation only when needed, such as when you wish to determine if your mesh is adequate for good results.

You may turn error estimation off issuing ERNORM,OFF (Main Menu> General Postproc> Options for Outp). By default, error estimation is active. Since the value set by the ERNORM command is not saved on Jobname.DB, you will need to reissue ERNORM,OFF if you wish to again deactivate error estimation after resuming an analysis .

In POST1 then, you can list SEPC and TEPC for all selected elements using the PRERR command (Main Menu> General Postproc> List Results> Percent Error). The value of SEPC or TEPC indicates the relative error due to a particular mesh discretization. To find out where you should refine the mesh, simply produce a contour display of SERR or TERR and look for high-error regions.

Using this error estimation technique, you can set up an automated scheme whereby the mesh is automatically refined in high-error regions. This is called adaptive meshing. See "Adaptive Meshing" in the Advanced Analysis Techniques Guide. For theoretical details about error estimation, see the Theory Reference for ANSYS and ANSYS Workbench.

5.2.7. Using the Results Viewer to Access Your Results File Data

The following links correspond to the three basic control areas on the Results Viewer:

For the Main Menu, see The Results Viewer Main Menu
For the Toolbar, see The Results Viewer Toolbar
For the Step/Sequence Data Access Control, see The Results Viewer Step/Sequence Data Access Controls

Figure 5.15  The Results Viewer

When you enter POST1, the available operations for the PGR data are “Results Viewer” or “Write PGR File.” The “Write PGR File” options are explained above. Choosing the Results Viewer disables much of the standard ANSYS GUI functionality. Many of these operations are not available because of PowerGraphics limitations. However, a good deal of the POST1 functionality is contained in the Result Viewer menu structure, and in the right and middle mouse button context sensitive menus that are accessible when you use the Results Viewer. The Results Viewer is described in the following paragraphs.

The ANSYS Results Viewer is a compact toolbar for viewing your analysis results. Although it is designed to display the information in your PGR file, you can use it to access any data you have stored in a valid results file (*.RST, *.RFL, *.RTH, *.RMG, etc.). When you open the Results Viewer, it accesses the PGR file you created for your current analysis, if one exists. You also have the option to open other PGR or results files. Because the viewer can access your results data without loading the entire database file, it is an ideal location from which to compare data from many different analyses.

Even if you have loaded other PGR or results files, you are still able to return to your original analysis. You can either reload the original PGR or results file from the current analysis before closing the Results Viewer, or after closing the Results Viewer, issue the PGRAPH,ON,S command, where S is the job name for your current analysis.

5.2.7.1. The Results Viewer Layout

There are three basic control areas on the Results Viewer: The Main Menu, The Toolbar and The Step/Sequence Data Access Control. Each of these areas is described below.

5.2.7.1.1. The Results Viewer Main Menu

The Main Menu is located along the top of the Results Viewer and provides access to the File, Edit, View and Help menus. The following functions can be accessed from each of these headings.

Figure 5.16  The Results Viewer File Menu

File -
Open Results -

You can open any PGR file, or any results file (*.RST, *.RFL, *.RTH, *.RMG, etc.) from any location on your file system.

List Result Information -

This selection displays a list of all results data included in the current file, and information about the current sequence for a PGR file.

Write Results -

You can use the data from your results file to create a new PGR file. This selection brings up the PGR File options dialog box and allows you to specify the creation of a new PGR file from any results file.

Save Animation -

Save an animation file (*.anim, *.avi) to a specified location. Animations created from the Results Viewer are not stored in the PGR file and are not written to the data base.

Close -

This option closes the Results Viewer and reverts back to the standard ANSYS GUI. If you have opened the results or PGR file from another analysis, you should return to your original file before closing the Results Viewer.

Edit -

You can select subsets of the model based on model attributes (material, element type, real ID, and element component). This selection leads to a specialized PGR menu that allows you to select from a list of material identifications, element types, element component designations and real constant values. For the results files, this brings up the appropriate “Element Select” widget, or picking window.

Figure 5.17  The Results Viewer View Menu

View -
Real Data -

You can display the real data from your analysis in the graphics window. This selection is grayed out when only real data exists for your analysis.

Imaginary Data -

You can display the imaginary data for you analysis in the graphics window. This selection is grayed out when no valid imaginary data exists.

Expanded Model -

You can perform all of the periodic/cyclic, modal cyclic and axisymmetric expansions that are available from the /EXPAND command.

Attributes -

The attributes of your model can be accessed according to the conventions in the /PNUM command.

Help -

Selecting help directs you to the list of PGR commands and documentation links located at the beginning of this section. You can then navigate to the appropriate area of the documentation.

5.2.7.1.2. The Results Viewer Toolbar

The Results Viewer toolbar is located across the middle of the Results Viewer. You can choose the type of results data to plot, and designate how the information should be plotted. You can also query results data from the graphics display, create animations, generate results listings, plot or generate file exports of your screen contents, or open the HTML Report Generator to construct a report on the results data.

Figure 5.18  The Results Viewer Toolbar

Element Plot

The first item on the toolbar is the element plot icon. This is the only model display available.

Result Item Selector

This drop down menu allows you to choose from the various types of data. The choices displayed may not always be available in your results file.

Plot Type Selector

You left mouse click and hold down on this button and it produces a “fly out” that allows you to access the four types of results plots available - Nodal, Element, Vector and Trace.

Query Results

You use the query tool to retrieve results data directly from selected areas in the graphics window. The ANSYS picking menu is displayed, allowing you to select multiple items. The information is displayed only for the current view.

Animate Results

You can create animations based on the information you have included in the PGR file. Because this information is created as a separate file, it is not saved within the PGR file. You must save the individual animations using the Results Viewer's Main Menu, Save Animation function.

List Results

The list results button creates a text listing of all of the nodal results values for the selected sequence number and result item. . You can print this data directly, or save it to a file for use in other applications.

Image Capture

You can plot the contents of the graphics window directly to a post script enabled printer, capture the contents to another window that is created automatically, or port the contents to an exportable graphics file in any one of the following popular formats:

PNG - Portable Network Graphics
EPS - Encapsulated Post Script
JPEG - Joint Photographic Exchange Group
WRL - Virtual Reality Meta Language
EPSI - Encapsulated Postscript with TIFF Preview
BMP - Windows Bitmap
WMF - Windows Metafile
EMF - Windows Enhanced Metafile
For Windows (PC) use, you must have a postscript enabled printer installed in order to obtain these export formats. If a postscript printer is not installed, file export is not available.

Report Generator

This function opens the ANSYS Report Generator. You use the report generator to capture your screen contents, animations, and result listings, and save them to a report assembly tool. This tool allows you to organize the data and add text in order to assemble a complete report. For more information on the ANSYS Report Generator, see "The Report Generator" later in this manual for more information on the Report Generator.

5.2.7.2. The Results Viewer Step/Sequence Data Access Controls

When you access a PGR file or a results file, the data is presented according to the sequential data sets of your original analysis. These data sets correspond to a specific time, load step, and substep of your analysis. Data is also stored in a separate sequence when you append the PGR file, or perform additional loading during an existing analysis. You use the following controls to access these different result sets.

NOTE: When you append data to your PGR file, it may disrupt the normal chronological format of the standard ANSYS results file. Time related data access functions may not always be presented in a linear chronological format in your PGR file.

Figure 5.19  The Results Viewer Step/Sequence Data Access Controls

The Data Sequence Slider Bar

The slider bar directly under the Results Viewer Toolbar corresponds to the individual data sequences that are available for the current results file. Each tick mark along the slider represents a data set. The data sequence number is displayed in the text box at the far right of the series of boxes below the slider. You can move to any data set either by moving the slider, or by entering the sequential number of the data set in the box.

Note

Because PGR data is not added chronologically during append operations, the sequential order of the data sets corresponds to when the data is written, not to the time within the actual analysis.

The Play and Stop Buttons

You use these buttons to move through the selected data sequence according to the defined load steps or substeps. The play button will step you through each of the data sets and when the final (maximum) set is reached, begin moving incrementally back down.

Time

This text box displays the time for each data set.

Load Step

Each individual load step number is displayed. You can enter a valid load step number here and that load step will be displayed.

Substep

Each individual load substep number is displayed. You can enter a valid substep number here and that substep will be displayed.

Sequence

The result sets are written sequentially to the results file during an analysis. This displays the sequence number from the results file. You also create additional sequences when you append the PGR file or add new loading data to your original analysis.

5.2.7.3. The Results Viewer Context Sensitive Menus

When you enter the Results Viewer, the rest of the ANSYS GUI is disabled. This prevents conflicts between the limited data available in PGR mode, and the functionality that can be accessed from the other GUI areas. Many of the functions you will need to deal with the results data have been moved to “context sensitive” menus that you access via the right and middle mouse buttons.

The Results Viewer places your cursor in “picking mode” anytime you place the cursor in the graphics window. This allows you to select data sets and other screen operations dynamically, many times without accessing the ANSYS Picking Menu. For the Results Viewer, the standard ANSYS method of using the right mouse button to alternate between picking and unpicking has been moved to the middle mouse button. The middle mouse button allows you to change between picking and unpicking. You can choose the mode of picking desired (selection of points on the working plane, selection of existing entities in the selected set and selection of points on the screen). You can also access entity filters to limit those entities that can be selected. For the two-button PC mouse, the middle button functions are activated by using the SHIFT-RIGHT MOUSE combination.

The right mouse button is used for context menus. These menus present choices that are applicable to the current selection. If you select “Screen Picking,” you will get a legend data context menu if the cursor is over a legend item, and the graphics window context menu anywhere else.

If you select “WP Picking,” and no points have been selected, you will get the legend or graphics context menus. If you have already selected points on the working plane, you will get a context menu that is applicable to the type of analysis you are performing (a FLOTRAN analysis will present a trace point selection menu, etc.). If you select “Entity Picking,” and no entities are selected, you will get the standard Graphics and Legend context menus. If you have selected entities, you will get a context menu that is applicable to the current type of analysis.

Graphics Window Context Menu

The following items are available from the context menu you get when you right mouse click anywhere in the graphics window except over the legend information.

Figure 5.20  Graphics Window Context Menu

Replot -

Replots the screen and integrates any changes you have made.

Display WP -

Toggles the Working Plane display (triad, grid, etc.) on and off.

Erase Displays -

Toggles screen refreshes according to /ERASE - /NOERASE command functionality.

Capture Image -

You can plot the contents of the graphics window directly to a printer, capture the contents to another window that is created automatically, or port the contents to an exportable graphics file in any one of the following popular formats:

PNG - Portable Network Graphics
EPS - Encapsulated Post Script
JPEG - Joint Photographic Exchange Group
WRL - Virtual Reality Meta Language
EPSI - Encapsulated Postscript with TIFF Preview
BMP - Windows Bitmap
WMF - Windows Metafile
EMF - Windows Enhanced Metafile
For Windows (PC) use, you must have a postscript-enabled printer installed in order to obtain these export formats. If a postscript printer is not installed, file export is not available.

Annotation -

You can choose between either static (2-D), or dynamic (3-D) annotations, and you can toggle your annotations on and off.

Display Legend -

Toggles the legend display on and off

Cursor Mode -

When the Results Viewer is selected, the Cursor Mode option allows you to switch between modes of picking, that include: Pointer, Working Plane, and Entities.

View -

Provides a drop-down list of view options: Isometric, Oblique, Front, Right, Top, Back, Left, and Bottom.

Fit -

Fits the extents of the model in the graphics area.

Zoom Back -

Returns to the previous zoom setting.

Window Properties -

You can access limited legend and display property control, along with a number of viewing angle, rotational setting and magnification controls. The Legend Settings allow you to select which legend items will be displayed, and to specify their location in the graphics window. The Display Settings let you specify Hidden, Capped or Q-Slice displays, and to modify the Z-buffering options, including smoothing and directional light source functions or 3-D options.

Graphics Properties -

This selection refers to those settings which affect all windows specified in a multi-window layout (/WINDOW) along with access to the Working Plane Settings and Working Plane Offset widgets, and the Window Layout controls dialog boxes.

Legend Area Context Menus

The legend area context menus will vary according to the location of your cursor in the legend, and the content of the legend data already being displayed. Right mouse clicking on the legend data provides control of the legend information, while clicking on the logo provides control of the date display and other miscellaneous functions. Clicking on the contour legend area provides a complete set of menus to customize your contour legend.

The legend setting and font control menus can be accessed from any of the legend context menus.

5.2.7.4. Associated PGR Commands

The following links lead to the commands associated with creating, appending and reading your PGR file:

Solution Commands

PGWRITE and POUTRES.

POST1 Commands

POUTRES, PGSAVE, PGRAPH, PGRSET, and PGSELE