Chapter 1: Getting Started with ANSYS

Go to the Next Chapter
Go to the Table of Contents for This Manual
Go to the Guides Master Index

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


1.1 Performing a Typical ANSYS Analysis

The ANSYS program has many finite element analysis capabilities, ranging from a simple, linear, static analysis to a complex, nonlinear, transient dynamic analysis. The analysis guide manuals in the ANSYS documentation set describe specific procedures for performing analyses for different engineering disciplines. The next few sections of this chapter cover general steps that are common to most analyses.

A typical ANSYS analysis has three distinct steps:

1.2 Building a Model

Building a finite element model requires more of an ANSYS user's time than any other part of the analysis. First, you specify a jobname and analysis title. Then, you use the PREP7 preprocessor to define the element types, element real constants, material properties, and the model geometry.

1.2.1 Specifying a Jobname and Analysis Title

This task is not required for an analysis, but is recommended.

1.2.1.1 Defining the Jobname

The jobname is a name that identifies the ANSYS job. When you define a jobname for an analysis, the jobname becomes the first part of the name of all files the analysis creates. (The extension or suffix for these files' names is a file identifier such as .DB.) By using a jobname for each analysis, you insure that no files are overwritten.

If you do not specify a jobname, all files receive the name FILE or file, depending on the operating system. You can change the default jobname as follows:

Command(s):

GUI:

Utility Menu>File>Change Jobname

The /FILNAME command is valid only at the Begin level. It lets you change the jobname even if you specified an initial jobname at ANSYS entry. However, the jobname applies only to files you open after using /FILNAME. Files opened before you use /FILNAME, such as the log file, Jobname.LOG, and error file Jobname.ERR, will still have the initial jobname.

1.2.1.2 Defining an Analysis Title

The /TITLE command (Utility Menu>File>Change Title), defines a title for the analysis. ANSYS includes the title on all graphics displays and on the solution output. You can issue the /STITLE command to add subtitles; these will appear in the output, but not in graphics displays.

1.2.1.3 Defining Units

The ANSYS program does not assume a system of units for your analysis. Except in magnetic field analyses, you can use any system of units so long as you make sure that you use that system for all the data you enter. (Units must be consistent for all input data.)

Using the /UNITS command, you can set a marker in the ANSYS database indicating the system of units that you are using. This command does not convert data from one system of units to another; it simply serves as a record for subsequent reviews of the analysis.

1.2.2 Defining Element Types

The ANSYS element library contains more than 100 different element types. Each element type has a unique number and a prefix that identifies the element category: BEAM4, PLANE77, SOLID96, etc. The following element categories are available:

BEAM
COMBINation
CONTACt
FLUID
HYPERelastic
INFINite
LINK
MASS
MATRIX
PIPE

PLANE
SHELL
SOLID
SOURCe
SURFace
TARGEt
USER
INTERface
VISCOelastic (or viscoplastic)

The element type determines, among other things:

BEAM4, for example, has six structural degrees of freedom (UX, UY, UZ, ROTX, ROTY, ROTZ), is a line element, and can be modeled in 3-D space. PLANE77 has a thermal degree of freedom (TEMP), is an eight-node quadrilateral element, and can be modeled only in 2-D space.

You must be in PREP7, the general preprocessor, to define element types. To do so, you use the ET family of commands (ET, ETCHG, etc.) or their GUI path equivalents; see the ANSYS Commands Reference for details. You define the element type by name and give the element a type reference number. For example, the commands shown below define two element types, BEAM4 and SHELL63, and assign them type reference numbers 1 and 2 respectively.

ET,1,BEAM4
ET,2,SHELL63
This table of type reference number versus element name is called the element type table. While defining the actual elements, you point to the appropriate type reference number using the TYPE command (Main Menu>Preprocessor> Create>Elements>Elem Attributes).

Many element types have additional options, known as KEYOPTs, and are referred to as KEYOPT(1), KEYOPT(2), etc. For example, KEYOPT(9) for BEAM4 allows you to choose results to be calculated at intermediate locations on each element, and KEYOPT(3) for SHELL63 allows you to suppress extra displacement shapes. You can specify KEYOPTs using the ET command, the KEYOPT command (Main Menu>Preprocessor>Element Type> Add/Edit/Delete).

1.2.3 Defining Element Real Constants

Element real constants are properties that depend on the element type, such as cross-sectional properties of a beam element. For example, real constants for BEAM3, the 2-D beam element, are area (AREA), moment of inertia (IZZ), height (HEIGHT), shear deflection constant (SHEARZ), initial strain (ISTRN), and added mass per unit length (ADDMAS). Not all element types require real constants, and different elements of the same type may have different real constant values.

You can specify real constants using the R family of commands (R, RMODIF, etc.) or their equivalent menu paths; see the ANSYS Commands Reference for further information. As with element types, each set of real constants has a reference number, and the table of reference number versus real constant set is called the real constant table. While defining the elements, you point to the appropriate real constant reference number using the REAL command (Main Menu> Preprocessor>Create>Elements>Elem Attributes).

While defining real constants, keep these rules and guidelines in mind:

Command(s):

GUI:

Utility Menu>List>Elements>Attributes + RealConst
Utility Menu>List>Elements>Attributes Only
Utility Menu>List>Elements>Nodes + Attributes
Utility Menu>List>Elements>Nodes + Attributes + RealConst

Command(s):

GUI:

Utility Menu>List>Properties>All Real Constants
Utility Menu>List>Properties>Specified Real Const

Command(s):

GUI:

Utility Menu>PlotCtrls>Style>Size and Shape
Utility Menu>Plot>Elements

1.2.3.1 Creating Cross Sections

If you are building a model using BEAM188 or BEAM189, you can use the section commands (SECTYPE, SECDATA, etc. (Main Menu>Preprocessor>Sections> -Beam-Common Sects)) to define and use cross sections in your models. See Chapter 8 of the ANSYS Advanced Analysis Techniques Guide for information on how to use the Beam Tool to create cross sections.

1.2.4 Defining Material Properties

Most element types require material properties. Depending on the application, material properties may be:

As with element types and real constants, each set of material properties has a material reference number. The table of material reference numbers versus material property sets is called the material table. Within one analysis, you may have multiple material property sets (to correspond with multiple materials used in the model). ANSYS identifies each set with a unique reference number.

While defining the elements, you point to the appropriate material reference number using one of the following:

Command(s):

GUI:

Main Menu>Preprocessor>-Attributes->Define>Default Attribs

1.2.4.1 Using Material Library Files

Although you can define material properties separately for each finite element analysis, the ANSYS program enables you to store a material property set in an archival material library file, then retrieve the set and reuse it in multiple analyses. (Each material property set has its own library file.) The material library files also enable several ANSYS users to share commonly used material property data.

The material library feature offers you other advantages:

The next few paragraphs describe how to create and read material library files. For additional information, see the descriptions of the /MPLIB, MPREAD, and MPWRITE commands in the ANSYS Commands Reference.

1.2.4.2 Format of Material Library Files

Material library files are ANSYS command files. The file format supports both linear and nonlinear properties. You can reuse material library files because the commands in them are written so that, once you read a material property set into the ANSYS database, you can associate that set with any material number you wish.

1.2.4.3 Specifying a Default Read/Write Path for Material Library Files

Before you create any material library files, define a default read path and write path for those files:

Command(s):

GUI:

Main Menu>Preprocessor>Material Props>Material Library>Library Path

Note-The ANSYS-supplied material library is located at /ansys5x/matlib/.

In place of option, specify READ (to set the read path), WRITE (to set the write path), or STAT to see what read and write paths currently are in use. In place of PATH, specify the path to be used for material library files.

1.2.4.4 Creating (Writing) a Material Library File

To create an archival material library file, perform these steps:

1. To tell the ANSYS program what system of units you are using, issue the /UNITS command. For example, to specify the international system of units, you would issue the command /UNITS,SI. You cannot access the /UNITS command directly from the GUI.

2. Define a material property using the MP command (Main Menu> Preprocessor>Material Props>Isotropic). To do so, you must specify a material number and at least one material property value (for example, magnetic permeability or MURX).

3. From the PREP7 preprocessor, issue the command shown below:

MPWRITE,Filename,,,LIB,MAT
Issuing MPWRITE writes the material data specified by material number MAT into the named file in the current working directory. (If you previously specified a material library write path by issuing the /MPLIB command (Main Menu> Preprocessor>Material Props>Material Library>Library Path), ANSYS writes the file to that location instead.)

Naming conventions for a material library file are as follows:

1.2.4.5 Reading a Material Library File

To read a material library file into the ANSYS database, perform these steps:

1. Use the /UNITS command or its GUI equivalent to tell the ANSYS program what system of units you are using.

Note-The default system of units for ANSYS is SI. The GUI lists only material library files with the currently active units.

2. Specify a new material reference number or an existing number that you wish to overwrite:

Command(s):

GUI:

Main Menu>Preprocessor>Create>Elements>Elem Attributes

Caution: Overwriting an existing material in the ANSYS database deletes all of the data associated with it.

3. To read the material library file into the database, use one of the following:

Command(s):

GUI:

Main Menu>Preprocessor>Material Props>Material Library>Import Library

1.2.4.6 Linear Material Properties

Linear material properties can be constant or temperature-dependent, and isotropic or orthotropic. To define constant material properties (either isotropic or orthotropic), use one of the following:

Command(s):

GUI:

Main Menu>Preprocessor>Material Props>property type

You also must specify the appropriate property label; for example EX, EY, EZ for Young's modulus, KXX, KYY, KZZ for thermal conductivity, and so forth. For isotropic material you need to define only the X-direction property; the other directions default to the X-direction value. For example:

MP,EX,1,2E11     ! Young's modulus for material ref. no. 1 is 2E11
MP,DENS,1,7800   ! Density for material ref. no. 1 is 7800
MP,KXX,3,43      ! Thermal conductivity for material ref. no 1 is 43
Besides the defaults for Y- and Z-direction properties (which default to the X-direction properties), other material property defaults are built in to reduce the amount of input. For example, Poisson's ratio (NUXY) defaults to 0.3, shear modulus (GXY) defaults to EX/2(1+NUXY)), and emissivity (EMIS) defaults to 1.0. See the ANSYS Elements Reference for details.

You can choose constant, isotropic, linear material properties from a material library available through the GUI. Young's modulus, density, coefficient of thermal expansion, Poisson's ratio, thermal conductivity and specific heat are available for 10 materials in four unit systems.

Caution: The property values in the material library are provided for your convenience. They are typical values for the materials you can use for preliminary analyses and non-critical applications. As always, the user is responsible for all data input to the ANSYS program.

To define temperature-dependent material properties, you can use the MP command in combination with the MPTEMP or MPTGEN command (Main Menu> Preprocessor>Material Props>property type and Main Menu>Preprocessor> Material Props>Temp Table or Main Menu>Preprocessor>Material Props> Generate Temp). You also can use the MPTEMP and MPDATA commands (Main Menu>Preprocessor>Material Props>Temp Table or Main Menu> Preprocessor>Material Props>Prop Table). The MP command allows you to define a property-versus-temperature function in the form of a polynomial. The polynomial may be linear, quadratic, cubic, or quartic:

Cn are the coefficients and T is the temperature. You enter the coefficients using the C0, C1, C2, C3, and C4 arguments on the MP command. If you specify just C0, the material property is constant; if you specify C0 and C1, the material property varies linearly with temperature; and so on. When you specify a temperature-dependent property in this manner, the program internally evaluates the polynomial at discrete temperature points with linear interpolation between points (that is, piece-wise linear representation) and a constant-valued extrapolation beyond the extreme points. You must use the MPTEMP or MPTGEN command before the MP command for second and higher-order properties to define appropriate temperature steps.

The second way to define temperature-dependent material properties is to use a combination of MPTEMP and MPDATA commands. MPTEMP (or MPTGEN) defines a series of temperatures, and MPDATA defines corresponding material property values. For example, the following commands define a temperature-dependent enthalpy for material 4:

MPTEMP,1,1600,1800,2000,2325,2326,2335   ! 6 temperatures (temps 1-6)
MPTEMP,7,2345,2355,2365,2374,2375,3000   ! 6 more temps (temps 7-12)
MPDATA,ENTH,4,1,53.81,61.23,68.83,81.51,81.55,82.31     ! Corresponding
MPDATA,ENTH,4,7,84.48,89.53,99.05,112.12,113.00,137.40  ! enthalpy values
If an unequal number of property data points and temperature data points are defined, the ANSYS program uses only those locations having both points defined for the property function table. To define a different set of temperatures for the next material property, you should first erase the current temperature table by issuing MPTEMP (without any arguments) and then define new temperatures (using additional MPTEMP or MPTGEN commands).

The MPPLOT command (Main Menu>Preprocessor>Material Props>Graph) displays a graph of material property versus temperature. Figure 1-1 shows a plot of the enthalpy-temperature curve defined in the example above. The MPLIST command (Main Menu>Preprocessor>Material Props>List), lists material properties.

Figure 1-1 A sample MPPLOT display

Below are some notes about temperature-dependent material properties:

MPTEMP,7,2340           ! Modifies location 7, retains other locations
MPDRES,ENTH,4           ! Associates ENTH for material 4 with new temps
The reason for the MPDRES command is this: Whenever you define a temperature-dependent property, the temperature-property data pairs are immediately stored in the database. Modifying the temperature data points affects only material properties that are subsequently defined, not what is already stored. The MPDRES command forces modification of what is already stored in the database. Two additional fields on MPDRES allow you to modify a stored property and store it under a new label or a new material reference number.

The MPTRES command (Main Menu>Preprocessor>Material Props>Restore Temps) allows you to replace the current temperature table with that of a previously defined material property in the database. You can then use the previous temperature data points for another property.

For temperature-dependent thermal expansion coefficients (ALPX, ALPY, ALPZ), if the base temperature for which they are defined (the definition temperature) differs from the reference temperature (the temperature at which zero thermal strains exist, defined by MP,REFT or TREF), then use the MPAMOD command to convert the data to the reference temperature. For GUI paths equivalent to this command, see the MPAMOD description in the ANSYS Commands Reference.

The ANSYS program takes temperature-dependent material properties into account during solution when element matrices are formulated. The program first calculates the temperature at the center of each element (or, for thermal elements, at the integration points of each element), determines the corresponding material property value by linear interpolation of the property-temperature table, and then uses this value to formulate the element matrices. If an element's temperature falls below or above the defined range of tabular data, then the defined extreme minimum or maximum value, respectively, is assumed for the material property outside the defined range.

You can save linear material properties (whether they are temperature-dependent or constant) to a file or restore them from a text file. (See Section 1.2.4 for a discussion of material library files.) You also can use either of the following to write both linear and nonlinear material properties to a file:

Command(s):

GUI:

Main Menu>Preprocessor>Archive Model>Write

Note-If you are using the CDWRITE command in any of the ANSYS-derived products (ANSYS/Emag, ANSYS/Thermal, etc.), you must edit the Jobname.CDB file that CDWRITE creates to remove commands which are not available in the derived product. You must do this before reading the Jobname.CDB file.

1.2.4.7 Nonlinear Material Properties

Nonlinear material properties are usually tabular data, such as plasticity data (stress-strain curves for different hardening laws), magnetic field data (B-H curves), creep data, swelling data, hyperelastic material data, etc. The first step in defining a nonlinear material property is to activate a data table using the TB command (Main Menu>Preprocessor>Material Props>Data Tables> Define/Activate). For example, TB,BH,2 activates the B-H table for material reference number 2.

To enter the tabular data, use the TBPT command (Main Menu>Preprocessor> Material Props>Data Tables>Edit Active). For example, the following commands define a B-H curve:

TBPT,DEFI,150,.21
TBPT,DEFI,300,.55
TBPT,DEFI,460,.80
TBPT,DEFI,640,.95
TBPT,DEFI,720,1.0
TBPT,DEFI,890,1.1
TBPT,DEFI,1020,1.15
TBPT,DEFI,1280,1.25
TBPT,DEFI,1900,1.4
You can verify the data table through displays and listings using the following:

Command(s):

GUI:

Main Menu>Preprocessor>Material Props>Data Tables>Graph
Main Menu>Preprocessor>Material Props>Data Tables>List

Figure 1-2 shows a sample TBPLOT (of the B-H curve defined above):

Figure 1-2 A sample TBPLOT display

1.2.4.8 Anisotropic Elastic Material Properties

Some element types accept anisotropic elastic material properties, which are usually input in the form of a matrix. (These properties are different from anisotropic plasticity, which requires different stress-strain curves in different directions.) Among the element types that allow elastic anisotropy are SOLID64 (the 3-D anisotropic solid), PLANE13 (the 2-D coupled-field solid), SOLID5 and SOLID98 (the 3-D coupled-field solids).

The procedure to specify anisotropic elastic material properties resembles that for nonlinear properties. You first activate a data table using the TB command (with Lab=ANEL) and then define the terms of the elastic coefficient matrix using the TBDATA command. Be sure to verify your input with the TBLIST command. See Section 2.5 of the ANSYS Elements Reference manual and the appropriate element descriptions for more information.

1.2.5 Creating the Model Geometry

Once you have defined material properties, the next step in an analysis is generating a finite element model-nodes and elements-that adequately describes the model geometry. The graphic below shows some sample finite element models:

Figure 1-3 Some sample finite element models

There are two methods to create the finite element model: solid modeling and direct generation. With solid modeling, you describe the geometric shape of your model, then instruct the ANSYS program to automatically mesh the geometry with nodes and elements. You can control the size and shape of the elements that the program creates. With direct generation, you "manually" define the location of each node and the connectivity of each element. Several convenience operations, such as copying patterns of existing nodes and elements, symmetry reflection, etc. are available.

Details of the two methods and many other aspects related to model generation-coordinate systems, working planes, coupling, constraint equations, etc.-are described in the ANSYS Modeling and Meshing Guide.

1.2.6 Apply Loads and Obtain the Solution

In this step, you use the SOLUTION processor to define the analysis type and analysis options, apply loads, specify load step options, and initiate the finite element solution. You also can apply loads using the PREP7 preprocessor.

1.2.6.1 Defining the Analysis Type and Analysis Options

You choose the analysis type based on the loading conditions and the response you wish to calculate. For example, if natural frequencies and mode shapes are to be calculated, you would choose a modal analysis. You can perform the following analysis types in the ANSYS program: static (or steady-state), transient, harmonic, modal, spectrum, buckling, and substructuring.

Not all analysis types are valid for all disciplines. Modal analysis, for example, is not valid for a thermal model. The analysis guide manuals in the ANSYS documentation set describe the analysis types available for each discipline and the procedures to do those analyses.

Analysis options allow you to customize the analysis type. Typical analysis options are the method of solution, stress stiffening on or off, and Newton-Raphson options.

To define the analysis type and analysis options, use the ANTYPE command (Main Menu>Preprocessor>Loads>New Analysis or Main Menu> Preprocessor>Loads>Restart) and the appropriate analysis option commands (TRNOPT, HROPT, MODOPT, SSTIF, NROPT, etc.). For GUI equivalents for the other commands, see their descriptions in the ANSYS Commands Reference.

You can specify either a new analysis or a restart, but a new analysis is the choice in most cases. Restarts are available only for static (steady-state), harmonic (2-D magnetic only), and transient analyses. The various analysis guides discuss details of restarts. You cannot change the analysis type and analysis options after the first solution.

A sample input listing for a structural transient analysis is shown below. Remember that the discipline (structural, thermal, magnetic, etc.) is implied by the element types used in the model.

ANTYPE,TRANS
TRNOPT,FULL
SSTIF,ON
NLGEOM,ON
Once you have defined the analysis type and analysis options, the next step is to apply loads. Some structural analysis types require other items to be defined first, such as master degrees of freedom and gap conditions. The ANSYS Structural Analysis Guide describes these items where necessary.

1.2.6.2 Applying Loads

The word loads as used in this manual includes boundary conditions (constraints, supports, or boundary field specifications) as well as other externally and internally applied loads. Loads in the ANSYS program are divided into six categories:

You can apply most of these loads either on the solid model (keypoints, lines, and areas) or the finite element model (nodes and elements). For details about the load categories and how they can be applied on your model, see Chapter 2 in this manual.

Two important load-related terms you need to know are load step and substep. A load step is simply a configuration of loads for which you obtain a solution. In a structural analysis, for example, you may apply wind loads in one load step and gravity in a second load step. Load steps are also useful in dividing a transient load history curve into several segments.

Substeps are incremental steps taken within a load step. You use them mainly for accuracy and convergence purposes in transient and nonlinear analyses. Substeps are also known as time steps-steps taken over a period of time.

Note-The ANSYS program uses the concept of time in transient analyses as well as static (or steady-state) analyses. In a transient analysis, time represents actual time, in seconds, minutes, or hours. In a static or steady-state analysis, time simply acts as a counter to identify load steps and substeps.

1.2.6.3 Specifying Load Step Options

Load step options are options that you can change from load step to load step, such as number of substeps, time at the end of a load step, and output controls. Depending on the type of analysis you are doing, load step options may or may not be required. The analysis procedures in the analysis guide manuals describe the appropriate load step options as necessary. See Chapter 2 for a general description of load step options.

1.2.6.4 Initiating the Solution

To initiate solution calculations, use either of the following:

Command(s):

GUI:

Main Menu>Solution>Current LS
Main Menu>Solution>
solution_method

When you issue this command, the ANSYS program takes model and loading information from the database and calculates the results. Results are written to the results file (Jobname.RST, Jobname.RTH, Jobname.RMG, or Jobname.RFL) and also to the database. The only difference is that only one set of results can reside in the database at one time, while you can write all sets of results (for all substeps) to the results file.

You can solve multiple load steps in a convenient manner:

Command(s):

GUI:

Main Menu>Solution>From LS Files

Chapter 3 discusses this and other solution-related topics.

1.2.7 Review the Results

Once the solution has been calculated, you can use the ANSYS postprocessors to review the results. Two postprocessors are available: POST1 and POST26.

You use POST1, the general postprocessor, to review results at one substep (time step) over the entire model or selected portion of the model. The command to enter POST1 is /POST1 (Main Menu>General Postproc), valid only at the Begin level. You can obtain contour displays, deformed shapes, and tabular listings to review and interpret the results of the analysis. POST1 offers many other capabilities, including error estimation, load case combinations, calculations among results data, and path operations.

You use POST26, the time history postprocessor, to review results at specific points in the model over all time steps. The command to enter POST26 is /POST26 (Main Menu>TimeHist Postpro), valid only at the Begin level. You can obtain graph plots of results data versus time (or frequency) and tabular listings. Other POST26 capabilities include arithmetic calculations and complex algebra. Details of POST1 and POST26 capabilities and how to use them are described in chapters later in this document.


Go to the beginning of this chapter