2.5. Applying Loads and Obtaining the Solution

You must define the analysis type and options, apply loads to the model, specify load step options, and initiate the finite element solution.

2.5.1. Defining the Analysis Type

During this phase of the analysis, you must first define the analysis type:

  • In the GUI, choose menu path Main Menu Solution> Analysis Type> New Analysis> Steady-state (static).

  • If this is a new analysis, issue the command ANTYPE,STATIC,NEW.

  • If you want to restart a previous analysis (for example, to specify additional loads), issue the command ANTYPE,STATIC,REST. You can restart an analysis only if the files Jobname.ESAV and Jobname.DB from the previous run are available.

2.5.2. Applying Loads

You can apply loads either on the solid model (keypoints, lines, and areas) or on the finite element model (nodes and elements). You can specify loads using the conventional method of applying a single load individually to the appropriate entity, or you can apply complex boundary conditions as tabular boundary conditions (see Applying Loads Using TABLE Type Array Parameters in the Basic Analysis Guide) or as function boundary conditions (see Using the Function Tool).

You can specify five types of thermal loads:

  • Constant Temperature (TEMP)

  • Heat Flow Rate (HEAT)

  • Convection (CONV)

  • Heat Flux (HFLUX)

  • Heat Generation Rate (HGEN)

2.5.2.1. Constant Temperature (TEMP)

These are DOF constraints usually specified at model boundaries to impose a known, fixed temperature. For SHELL131 and SHELL132 elements with KEYOPT(3) = 0 or 1, use the labels TBOT, TE2, TE3, . . ., TTOP instead of TEMP when defining DOF constraints.

2.5.2.2. Heat Flow Rate (HEAT)

These are concentrated nodal loads. Use them mainly in line-element models (conducting bars, convection links, etc.) where you cannot specify convections and heat fluxes. A positive value of heat flow rate indicates heat flowing into the node (that is, the element gains heat). If both TEMP and HEAT are specified at a node, the temperature constraint prevails. For SHELL131 and SHELL132 elements with KEYOPT(3) = 0 or 1, use the labels HBOT, HE2, HE3, . . ., HTOP instead of HEAT when defining nodal loads.


Note:  If you use nodal heat flow rate for solid elements, you should refine the mesh around the point where you apply the heat flow rate as a load, especially if the elements containing the node where the load is applied have widely different thermal conductivities. Otherwise, you may get an non-physical range of temperature. Whenever possible, use the alternative option of using the heat generation rate load or the heat flux rate load. These options are more accurate, even for a reasonably coarse mesh.


2.5.2.3. Convection (CONV)

Convections are surface loads applied on exterior surfaces of the model to account for heat lost to (or gained from) a surrounding fluid medium. They are available only for solids and shells. In line-element models, you can specify convections through the convection link element (LINK34).

You can use the surface-effect elements (SURF151, SURF152) to analyze heat transfer for convection/radiation effects. The surface-effect elements allow you to generate film coefficient calculations and bulk temperatures from FLUID116 elements and to model radiation to a point. You can also transfer external loads (such as from CFX) to ANSYS using these elements.

2.5.2.4. Heat Flux (HFLUX)

Heat fluxes are also surface loads. Use them when the amount of heat transfer across a surface (heat flow rate per area) is known. A positive value of heat flux indicates heat flowing into the element. Heat flux is used only with solids and shells. An element face may have either CONV or HFLUX (but not both) specified as a surface load. If you specify both on the same element face, ANSYS uses what was specified last.

2.5.2.5. Heat Generation Rate (HGEN)

You apply heat generation rates as "body loads" to represent heat generated within an element, for example by a chemical reaction or an electric current. Heat generation rates have units of heat flow rate per unit volume.

2.5.2.6. Commands Used to Apply Loads

Table 2.9: Thermal Analysis Load Types below summarizes the types of thermal analysis loads.

Table 2.9:  Thermal Analysis Load Types

Load TypeCategoryCmd FamilyGUI Path
Temperature (TEMP, TBOT, TE2, TE3, . . . TTOP)Constraints D Main Menu> Solution> Define Loads> Apply> Thermal> Temperature
Heat Flow Rate (HEAT, HBOT, HE2, HE3, . . . HTOP)Forces F Main Menu> Solution> Define Loads> Apply> Thermal> Heat Flow

Convection (CONV), 
Heat Flux (HFLUX)

Surface Loads SF
Main Menu> Solution> Define Loads> Apply> Thermal> Convection
Main Menu> Solution> Define Loads> Apply> Thermal> Heat Flux
Heat Generation Rate (HGEN)Body LoadsBF, BFE Main Menu> Solution> Define Loads> Apply> Thermal> Heat Generat

Table 2.10: Load Commands for a Thermal Analysis lists all the commands you can use to apply, remove, operate on, or list loads in a thermal analysis.

Table 2.10:  Load Commands for a Thermal Analysis

Load TypeSolid or FE ModelEntityApplyDeleteListOperateSettings
TemperatureSolid ModelKeypoints DK DKDELE DKLIST DTRAN -
"Finite ElementNodes D DDELE DLIST DSCALE DCUM, TUNIF
Heat Flow RateSolid ModelKeypoints FK FKDELE FKLIST FTRAN -
"Finite ElementNodes F FDELE FLIST FSCALE FCUM
Convection, Heat FluxSolid ModelLines SFL SFLDELE SFLLIST SFTRAN SFGRAD
"Solid ModelAreas SFA SFADELE SFALIST SFTRAN SFGRAD
"Finite ElementNodes SF SFDELE SFLIST SFSCALE SFGRAD, SFCUM
"Finite ElementElements SFE SFEDELE SFELIST SFSCALE SFBEAM, SFCUM, SFFUN, SFGRAD
Heat Generation RateSolid ModelKeypoints BFK BFKDELE BFKLIST BFTRAN -
"Solid ModelLines BFL BFLDELE BFLLIST BFTRAN -
"Solid ModelAreas BFA BFADELE BFALIST BFTRAN -
"Solid ModelVolumes BFV BFVDELE BFVLIST BFTRAN -
"Finite ElementNodes BF BFDELE BFLIST BFSCALE BFCUM
""Elements BFE BFEDELE BFELIST BFSCALE BFCUM

You access all loading operations (except List; see below) through a series of cascading menus. From the Solution Menu, you choose the operation (apply, delete, etc.), then the load type (temperature, etc.), and finally the object to which you are applying the load (keypoint, node, etc.).

For example, to apply a temperature load to a keypoint, follow this GUI path:

GUI:

Main Menu> Solution> Define Loads> Apply> Thermal> Temperature> On Keypoints

2.5.3. Using Table and Function Boundary Conditions

A general discussion of tabular boundary conditions is found in Applying Loads Using TABLE Type Array Parameters in the Basic Analysis Guide. Details specific to thermal analyses are described here.

For detailed information on defining table array parameters (both interactively and via command), see the ANSYS Parametric Design Language Guide.

There are no restrictions on element types.

Table 2.11: Boundary Condition Type and Corresponding Primary Variable lists the primary variables that can be used with each type of boundary condition in a thermal analysis.

Table 2.11:  Boundary Condition Type and Corresponding Primary Variable

Thermal Boundary ConditionCmd FamilyPrimary Variable
Fixed Temperature D TIME, X, Y, Z, NODE
Heat Flow F TIME, X, Y, Z, TEMP, NODE
Film Coefficient (Convection) SF TIME, X, Y, Z, TEMP, VELOCITY, ELEM, NODE
Bulk Temperature (Convections) SF TIME, X, Y, Z, ELEM, NODE
Heat Flux SF TIME, X, Y, Z, TEMP, ELEM, NODE
Heat Generation BF TIME, X, Y, Z, TEMP, ELEM
Uniform Heat GenerationBFUNIFTIME
Fluid Element (FLUID116 ) Boundary Condition
Flow Rate SFE TIME
Pressure D TIME, X, Y, Z

If you apply tabular loads as a function of temperature but the rest of the model is linear (e.g., includes no temperature-dependent material properties or radiation ), you should turn on Newton-Raphson iterations (NROPT,FULL) to evaluate the temperature-dependent tabular boundary conditions correctly.

An example of how to run a steady-state thermal analysis using tabular boundary conditions is described in Performing a Thermal Analysis Using Tabular Boundary Conditions.

For more flexibility defining arbitrary heat transfer coefficients, use function boundary conditions. For detailed information on defining functions and applying them as loads, see Using the Function Tool in the Basic Analysis Guide. Additional primary variables that are available using functions are listed below.

  • Tsurf (TS) (element surface temperature for SURF151 or SURF152 elements)

  • Density (material property DENS)

  • Specific heat (material property C)

  • Thermal conductivity (material property KXX)

  • Thermal conductivity (material property KYY)

  • Thermal conductivity (material property KZZ)

  • Viscosity (material property VISC)

  • Emissivity (material property EMIS)

2.5.4. Specifying Load Step Options

For a thermal analysis, you can specify general options, nonlinear options, and output controls.

Table 2.12:  Specifying Load Step Options

OptionCommandGUI Path
General Options
Time TIME Main Menu> Solution> Load Step Opts> Time/Frequenc> Time-Time Step
Number of Time Steps NSUBST Main Menu> Solution> Load Step Opts> Time/Frequenc> Time and Substps
Time Step Size DELTIM Main Menu> Solution> Load Step Opts> Time/Frequenc> Time-Time Step
Stepped or Ramped Loads KBC Main Menu> Solution> Load Step Opts> Time/Frequenc> Time-Time Step
Nonlinear Options
Max. No. of Equilibrium Iterations NEQIT Main Menu> Solution> Load Step Opts> Nonlinear> Equilibrium Iter
Automatic Time Stepping AUTOTS Main Menu> Solution> Load Step Opts> Time/Frequenc> Time-Time Step
Convergence Tolerances CNVTOL Main Menu> Solution> Load Step Opts> Nonlinear> Convergence Crit
Solution Termination Options NCNV Main Menu> Solution> Load Step Opts> Nonlinear> Criteria to Stop
Line Search Option LNSRCH Main Menu> Solution> Load Step Opts> Nonlinear> Line Search
Predictor-Corrector Option PRED Main Menu> Solution> Load Step Opts> Nonlinear> Predictor
Output Control Options
Printed Output OUTPR Main Menu> Solution> Load Step Opts> Output Ctrls> Solu Printout
Database and Results File Output OUTRES Main Menu> Solution> Load Step Opts> Output Ctrls> DB/Results File
Extrapolation of Results ERESX Main Menu> Solution> Load Step Opts> Output Ctrls> Integration Pt

2.5.5. General Options

General options include the following:

  • The TIME option.

    This option specifies time at the end of the load step. Although time has no physical meaning in a steady-state analysis, it provides a convenient way to refer to load steps and substeps.

    The default time value is 1.0 for the first load step and 1.0 plus the previous time for subsequent load steps.

  • The number of substeps per load step, or the time step size.

    A nonlinear analysis requires multiple substeps within each load step. By default, the program uses one substep per load step.

  • Stepped or ramped loads.

    If you apply stepped loads, the load value remains constant for the entire load step.

    If you ramp loads (the default), the load values increment linearly at each substep of the load step.

  • Monitor Results in Real Time

    The NLHIST command allows you to monitor results of interest in real time during a solution. Before starting the solution, you can request nodal data such as temperatures or heat flows. You can also request element nodal data such as thermal gradients and fluxes at specific elements to be graphed. The result data are written to a file named Jobname.nlh. Nodal results and contact results are monitored at every converged substep while element nodal data are written as specified via the OUTRES setting. You can also track results during batch runs. To execute, either:

    • Access the ANSYS Launcher and select File Tracking from the Tools menu.

      Or...

    • Type nlhist182 in the command line.

    Use the supplied file browser to navigate to your Jobname.nlh file, and click on it to invoke the tracking utility. You can use this utility to read the file at any time, even after the solution is complete.

    To use this option, use either of these methods:

    Command(s): NLHIST
    GUI: Main Menu> Solution> Results Tracking

2.5.6. Nonlinear Options

Specify nonlinear load step options if nonlinearities are present. Nonlinear options include the following:

  • Number of equilibrium iterations.

    This option specifies the maximum allowable number of equilibrium iterations per substep. The default value of 25 should be enough for most nonlinear thermal analyses.

  • Automatic time stepping.

    For nonlinear problems, automatic time stepping determines the amount of load increment between substeps, to maintain solution stability and accuracy.

  • Convergence tolerances.

    ANSYS considers a nonlinear solution to be converged whenever specified convergence criteria are met. Convergence checking may be based on temperatures, heat flow rates, or both. You specify a typical value for the desired item (VALUE field in the CNVTOL command) and a tolerance about the typical value (TOLER field). The convergence criterion is then given by VALUE x TOLER. For instance, if you specify 500 as the typical value of temperature and 0.001 as the tolerance, the convergence criterion for temperature is 0.5 degrees.

    For temperatures, ANSYS compares the change in nodal temperatures between successive equilibrium iterations ( ΔT = Ti -Ti-1) to the convergence criterion. Using the above example, the solution is converged when the temperature difference at every node from one iteration to the next is less than 0.5 degrees.

    For heat flow rates, ANSYS compares the out-of-balance load vector to the convergence criterion. The out-of-balance load vector represents the difference between the applied heat flows and the internal (calculated) heat flows.

  • Termination settings for unconverged solutions.

    If ANSYS cannot converge the solution within the specified number of equilibrium iterations, ANSYS either stops the solution or moves on to the next load step, depending on what you specify as the stopping criteria.

  • Line search.

    This option enables ANSYS to perform a line search with the Newton-Raphson method.

  • Predictor-corrector option.

    This option activates the predictor-corrector option for the degree of freedom solution at the first equilibrium iteration of each substep.

2.5.6.1. Tracking Convergence Graphically

As a nonlinear thermal analysis proceeds, ANSYS computes convergence norms with corresponding convergence criteria each equilibrium iteration. Available in both batch and interactive sessions, the Graphical Solution Tracking (GST) feature displays the computed convergence norms and criteria while the solution is in process. By default, GST is ON for interactive sessions and OFF for batch runs. To turn GST on or off, use either of the following:

Command(s): /GST
GUI: Main Menu> Solution> Load Step Opts> Output Ctrls> Grph Solu Track

Figure 2.6: Convergence Norms below shows a typical GST display.

Figure 2.6:  Convergence Norms

Convergence Norms

Displayed by the Graphical Solution Tracking (GST) Feature


2.5.7. Output Controls

The third class of load step options enables you to control output. The options are as follows:

  • Control printed output.

    This option enables you to include any results data in the printed output file (Jobname.OUT).

  • Control database and results file output

    This option controls what data ANSYS writes to the results file (Jobname.RTH).

  • Extrapolate results.

    Use this option to review element integration point results by copying them to the nodes instead of extrapolating them. (Extrapolation is the default.)

2.5.8. Defining Analysis Options

Next, you define the analysis options. Possible options include:

  • Select an equation solver. You can specify any of these values:

    • Sparse solver (default for static and full transient analyses)

    • Jacobi Conjugate Gradient (JCG) solver

    • Incomplete Cholesky Conjugate Gradient (ICCG) solver

    • Preconditioned Conjugate Gradient solver (PCG)

    To select an equation solver, use either of the following:

    Command(s): EQSLV
    GUI: Main Menu> Solution> Analysis Type> Analysis Options
  • Specify a temperature offset. This is the difference in degrees between absolute zero and the zero of the temperature system being used. The offset temperature is included internally in the calculations of pertinent elements (such as elements with radiation effects or creep capabilities). It allows you to input temperatures in degrees Celsius (instead of kelvin) or degrees Fahrenheit (instead of Rankine), and then postprocess temperatures in like fashion. For more information, see Radiation.

    To specify the offset temperature, use either of the following:

    Command(s): TOFFST
    GUI: Main Menu> Solution> Analysis Type> Analysis Options

Sometimes you may need to restart an analysis after the initial run has been completed. A multiframe restart allows you to save analysis information at many substeps during a run, then restart the run at one of those substeps. Before running your initial analysis, you should use the RESCONTROL command to set up the frequency at which restart files are saved within each load step of the run.

To set the controls for a multiframe restart, issue the following:

Command(s): RESCONTROL
GUI: Main Menu> Solution> Load Step Opts> Nonlinear> Restart Control

If your analysis contains material nonlinearities, results from a restart may be different than results from a single run because the stiffness matrices are always recreated in a restart run, but may or may not be in a single run (depending on the behavior resulting from the THOPT,REFORMTOL setting).

2.5.9. Saving the Model

After you have specified the load step and analysis options, you should save a backup copy of the database to prevent your model from being lost if your computer system should fail. Should you ever need to retrieve your model, do so via either of the following:

Command(s): RESUME
GUI: Utility Menu> File> Resume Jobname.db
Utility Menu> File> Resume from

2.5.10. Solving the Model

To start the solution, use either of the following:

Command(s): SOLVE
GUI: Main Menu> Solution> Solve> Current LS

When you need to restart a job, use the ANTYPE command to specify the restart point and type of restart. You can continue the job from the restart point (making any corrections necessary), or you can terminate a load step at the restart point (rescaling all of the loading) then continue with the next load step.


Release 18.2 - © ANSYS, Inc. All rights reserved.