Chapter 1: Getting Started with ANSYS

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

A typical ANSYS analysis has three distinct steps:

• Build the model.
• Apply loads and obtain the solution.
• Review the results.

1.2 Building a Model

1.2.1 Specifying a Jobname and Analysis Title

1.2.1.1 Defining the Jobname

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:

• By using the initial jobname entry option when you enter the ANSYS program, either via the launcher or on the ANSYS execution command. For details, see the ANSYS Operations Guide.
• From within the ANSYS program, you can use either of the following:

/FILNAME

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

1.2.1.3 Defining Units

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

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:

• The degree-of-freedom set (which in turn implies the discipline-structural, thermal, magnetic, electric, quadrilateral, brick, etc.)
• Whether the element lies in two-dimensional or three-dimensional 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

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

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:

• When using one of the R commands, you must enter real constants in the order shown in Table 4.n.1 for each element type in the ANSYS Elements Reference.
• For models using multiple element types, use a separate real constant set (that is, a different REAL reference number) for each element type. The ANSYS program issues a warning message if multiple element types reference the same real constant set. However, a single element type may reference several real constant sets.
• To verify your real constant input, use the RLIST and ELIST commands, with RKEY=1 (shown below). RLIST lists real constant values for all sets. The command ELIST,,,,,1 produces an easier-to-read list that shows, for each element, the real constant labels and their values.

ELIST

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):

RLIST

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

• For line and area elements that require geometry data (cross-sectional area, thickness, diameter, etc.) to be specified as real constants, you can verify the input graphically by using the following commands in the order shown:

/ESHAPE and EPLOT

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

ANSYS displays the elements as solid elements, using a rectangular cross-section for link and shell elements and a circular cross-section for pipe elements. The cross-section proportions are determined from the real constant values.

1.2.3.1 Creating Cross Sections

1.2.4 Defining Material Properties

• Linear or nonlinear
• Isotropic, orthotropic, or anisotropic
• Constant temperature or temperature-dependent.

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

Command(s):

MAT

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

1.2.4.1 Using Material Library Files

The material library feature offers you other advantages:

• Because the archived contents of material library files are reusable, you can use them to define other, similar material property sets quickly and with fewer errors. For example, suppose that you have defined material properties for one grade of steel and want to create a material property set for another grade of steel that is slightly different. You can write the existing steel material property set to a material library file, read it back into ANSYS under a different material number, and then, within ANSYS, make the minor changes needed to define properties for the second type of steel.
• Using the /MPLIB command (Main Menu>Preprocessor>Material Props> Material Library>Library Path), you can define a material library read and write path. Doing this allows you to protect your material data resources in a read-only archive, while giving ANSYS users the ability to write their material data locally without switching paths.
• You can give your material library files meaningful names that reflect the characteristics of the data they contain. For example, the name of a material library file describing properties of a steel casting might be STEELCST.SI_MPL. (See Section 1.2.4.4 for an explanation of file naming conventions.)
• You can design your own directory hierarchy for material library files. This enables you to classify and catalog the files by material type (plastic, aluminum, etc.), by units, or by any category you choose.

1.2.4.2 Format of Material Library Files

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

Command(s):

/MPLIB,option,PATH

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

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

Filename is the name to assign to the material library file. Issue MPWRITE (Main Menu>Preprocessor> Material Props>Material Library>Export Library) and specify the filename for the material library file.

Naming conventions for a material library file are as follows:

• The name of the file is the name you specify on the MPWRITE command. If you do not specify a filename, the default name is JOBNAME.
• The extension of a material library filename follows the pattern .xxx_MPL, where xxx identifies the system of units for this material property sets. For example, if the system of units is the CGS system, the file extension is .CGS_MPL. The default extension, used if you do not specify a units system before creating the material library file, is .USER_MPL. (This indicates a user-defined system of units.)

1.2.4.5 Reading a Material Library File

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):

MAT

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):

MPREAD,Filename...LIB

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

The LIB argument supports a file search hierarchy. The program searches for the named material library file first in the current working directory, then in your home directory, then in the read path directory specified by the /MPLIB command, and finally in the ANSYS-supplied directory /ansys5x/matlib. If you omit the LIB argument, the programs searches only in the current working directory.

1.2.4.6 Linear Material Properties

Command(s):

MP

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

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:

C_n 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

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:

• To modify a property data point on an existing curve, simply redefine the desired data point by issuing MPDATA with the appropriate location number. For example, to change the ENTH value in location 6 of the above enthalpy-temperature curve from 82.31 to 83.09, the command would be MPDATA,ENTH,4,6,83.09
• To modify a temperature data point on an existing curve, you need two commands: MPTEMP with the appropriate location number to specify the new temperature value, and MPDRES (Main Menu>Preprocessor> Material Props>Modify Temps) to associate the new temperature table with the material property. For example, to change the temperature in location 7 of the above enthalpy-temperature curve from 2345 to 2340, the commands would be:

MPTEMP,7,2340           ! Modifies location 7, retains other locations
MPDRES,ENTH,4           ! Associates ENTH for material 4 with new temps

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):

CDWRITE,MAT

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

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

Command(s):

TBPLOT, TBLIST

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

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

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

1.2.6.1 Defining the Analysis Type and Analysis Options

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

1.2.6.2 Applying Loads

DOF Constraints
Forces
Surface Loads
Body Loads
Inertia Loads
Coupled-field Loads

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

1.2.6.4 Initiating the Solution

Command(s):

SOLVE

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):

LSSOLVE

Main Menu>Solution>From LS Files

Chapter 3 discusses this and other solution-related topics.

1.2.7 Review the Results

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