Chapter 3: Solution

Go to the Next Chapter
Go to the Previous 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

3.1 What is Solution?

In the solution phase of the analysis, the computer takes over and solves the simultaneous equations that the finite element method generates. The results of the solution are:

nodal degree-of-freedom values, which form the primary solution
derived values, which form the element solution

The element solution is usually calculated at the elements' integration points. The ANSYS program writes the results to the database as well as to the results file (Jobname.RST, RTH, RMG, or .RFL).

Several methods of solving the simultaneous equations are available in the ANSYS program: frontal solution, sparse direct solution, Jacobi Conjugate Gradient (JCG) solution, Incomplete Cholesky Conjugate Gradient (ICCG) solution, Preconditioned Conjugate Gradient (PCG) solution, and an automatic iterative solver option (ITER). The frontal solver is the default, but you can select a different solver using one of the following:

Command(s):

EQSLV

GUI:

Main Menu>Preprocessor>Loads>Analysis Options
Main Menu>Solution>Analysis Options

3.2 Selecting a Solver

The following table provides general guidelines you may find useful in selecting which solver to use for a given problem.

Table 3-1 Solver selection guidelines

Solver

Typical
Applications

Model
Size

Memory
Use

Disk
Use

Frontal Solver (direct elimination solver)

When robustness is required (nonlinear analysis) or when memory is limited.

Under 50,000 DOFs

Low

High

Sparse Direct Solver
(direct elimination solver)

When robustness and solution speed are required (nonlinear analysis); for linear analysis where iterative solvers are slow to converge (especially for ill-conditioned matrices, such as poorly shaped elements).

10,000 to 500,000 DOFs
(more for shell & beam models).

Medium

High

PCG Solver (iterative solver)

When solution speed is crucial (linear analysis of large models).
Especially well suited for large models with solid elements.

50,000 to 1,000,000+ DOFs

High

Low

ICCG
(Iterative solver)

When solution speed is crucial in multiphysics applications. Handles models that are harder to converge in other iterative solvers (nearly indefinite matrices).

50,000 to 1,000,000+ DOFs

High

Low

JCG Solver (iterative solver)

When solution speed is crucial in "single-field" problems (thermal, magnetics, acoustics, and multiphysics)

50,000 to 1,000,000+ DOFs

Medium

Low

3.3 Using the Frontal Solver

The frontal solver does not assemble the complete global matrix. Instead, ANSYS performs the assembly and solution steps simultaneously as the solver processes each element. The method works as follows:

After the individual element matrices are calculated, the solver reads in the degrees of freedom (DOF) for the first element.
The program eliminates any degrees of freedom that can be expressed in terms of the other DOF by writing an equation to the .TRI file. This process repeats for all elements until all degrees of freedom have been eliminated and a complete triangularized matrix is left on the .TRI file.
The program then calculates the nodal DOF solution by back substitution, and uses the individual element matrices to calculate the element solution. Figure 3-1 shows the main steps in a frontal solution and the files produced at each step.

A term frequently mentioned in the context of a frontal solver is wavefront. The wavefront is the number of degrees of freedom retained by the solver during triangularization because they cannot yet be eliminated. As the solver processes each element and its degrees of freedom, the wavefront swells and shrinks, and finally becomes zero when all degrees of freedom have been processed. The highest value of the wavefront is called the maximum wavefront, and the averaged, root-mean-square value is called the RMS wavefront.

Figure 3-1 Typical steps and files in a frontal solution

The RMS wavefront of a model directly affects solution time: the smaller its value, the less CPU time required for solution. Before solution, therefore, you may wish to reorder the elements for a smaller wavefront. The ANSYS program does this automatically at the beginning of solution unless you have reordered the model yourself or have requested no reordering. (The ANSYS Modeling and Meshing Guide provides details about element reordering.) The maximum wavefront of a model directly affects memory requirements, in particular the amount of memory allocated for scratch data. See Chapter 19 for details about memory management.

3.4 Using the Sparse Direct Solver

The sparse direct solver is based on a direct elimination of equations as opposed to iterative solvers, where the solution is obtained through indirect means (that is, through iterative solution). Since the sparse direct solver is based on direct elimination, poorly conditioned matrices do not pose any difficulty in producing a solution.

Note-The sparse direct solver is not applicable to PSD spectrum analysis.

3.5 Using the Jacobi Conjugate Gradient (JCG) Solver

The JCG solver also starts with element matrix formulation, but the remaining steps are different. Instead of triangularizing the global matrix, the JCG solver assembles the full global matrix. The solver then calculates the DOF solution by iterating to convergence (starting with an assumed zero value for all DOF). Figure 3-2 summarizes these steps. The JCG solver is best suited for 3-D scalar field analyses that involve large, sparse matrices, for example a 3-D magnetic field analysis.

For some cases, the tolerance default value (set via the EQSLV,JCG command) of 1.0E-8 may be too restrictive, and may increase running time needlessly. The value 1.0E-5 may be acceptable in many situations.

The JCG solver is available only for static analyses, full harmonic analyses, or full transient analyses. (You specify these analysis types using the commands ANTYPE, STATIC, HROPT,FULL, or TRNOPT,FULL respectively.)

Figure 3-2 Typical steps and files in a JCG solution

With all conjugate gradient solvers, the user must be particularly careful to check that the model is appropriately constrained. No minimum pivot is calculated and the solver will continue to iterate if there is any rigid body motion possible.

3.6 Using the Incomplete Cholesky Conjugate Gradient (ICCG) Solver

The ICCG solver operates similarly to the JCG solver with the following exceptions:

The ICCG solver is more robust than the JCG solver for matrices that are not well-conditioned. Performance will vary with matrix conditioning, but in general ICCG performance compares to that of the JCG solver.
The ICCG solver uses a more sophisticated preconditioner than the JCG solver. Therefore, the ICCG solver requires approximately twice as much memory as the JCG solver.

The ICCG solver is available only for static analyses, full harmonic analyses [HROPT,FULL], or full transient analyses [TRNOPT,FULL]. (You specify the analysis type using the ANTYPE command.) The ICCG solver is useful for models that have sparse matrices, and is valid for elements with symmetric and unsymmetric matrices. The solver runs faster than the frontal solver for most problem sizes.

3.7 Using the Preconditioned Conjugate Gradient (PCG) Solver

The PCG solver operates similarly to the JCG solver, with four exceptions:

The PCG solver is usually about 4 to 10 times faster than the JCG solver for structural solid elements and about 10 times faster for shell elements. Savings increase with the problem size.
The PCG solver uses the .EMAT file shown in Figure 3-2 but not the .FULL file.
The JCG solver uses the diagonal of the global assembled matrix as a preconditioner. The PCG solver uses a more sophisticated preconditioner.
The PCG solver usually requires approximately twice as much memory as the JCG solver because it retains two matrices in memory:
- The preconditioner, which is almost the same size as the stiffness matrix
- The symmetric, non-zero part of the stiffness matrix.

You can use the /RUNST command (Main Menu>Run-Time Stats), to determine the space needed or the wavefront size. Special memory allocation is desirable. (See Chapter 19 for further information.)

The PCG solver usually requires less than 1/4 the disk file space used by the frontal solver. Savings increase with the problem size. The PCG solver usually runs faster than the frontal solver for large models (wavefront greater than about 1000).

The PCG solver is best suited for structural analysis. It is valid for elements with symmetric, sparse, definite or indefinite matrices. This solver is available only for static or steady-state analyses and transient analyses, or for subspace eigenvalue analyses (PowerDynamics).

The PCG solver primarily solves for displacements/rotations (in structural analysis), temperatures (in thermal analysis), etc. The accuracy of other derived variables (such as strains, stresses, flux, etc.) is dependent upon accurate prediction of primary variables.

Direct solvers (such as the frontal and sparse direct solvers) produce very accurate solution vectors. Indirect iterative solvers, such as the PCG solver, depend upon a convergence criterion specified by the user. Therefore, relaxation of the default tolerance may significantly affect the accuracy, especially of derived quantities.

The PCG solver is not recommended for problems with large numbers of constraint equations or for models with SHELL150 elements. For these types of problems, use the frontal solver. Also, the PCG solver does not support SOLID62 or MATRIX50 elements.

Note-When the PCG solver encounters an indefinite matrix, the solver will invoke an algorithm that handles indefinite matrices. If the indefinite PCG algorithm also fails (this happens when the equation system is ill-conditioned; for example, losing contact at a substep or plastic hinge developments), an outer Newton-Raphson loop will be triggered to perform a bisection. Normally the stiffness matrix will be better conditioned after bisection and the PCG solver can eventually solve all the nonlinear steps.

3.8 Using the Automatic Iterative (Fast) Solver Option

The Automatic Iterative Solver option [EQSLV,ITER] chooses an appropriate iterative solver (PCG, JCG, etc.) based on the physics of the problem being solved. When you use the Automatic Iterative Solver option you must input an accuracy level. The accuracy level is specified as an integer between 1 and 5 and is used for selecting the Iterative Solver tolerance for convergence checking. An accuracy level of 1 corresponds to the fastest setting (less number of iterations) and an accuracy level to 5 corresponds to the slowest setting (accurate, more number of iterations). ANSYS selects the tolerance based on the chosen accuracy level. For example:

For linear static or linear full transient structural analysis, an accuracy level of 1 corresponds to a tolerance of 1.0e-4 and an accuracy level of 5 corresponds to a tolerance of 1.0e-8.
For steady-state linear or nonlinear thermal analysis, an accuracy level of 1 corresponds to a tolerance of 1.0e-5 and and accuracy level of 5 corresponds to a tolerance of 1.0e-9.
For transient linear or nonlinear thermal analysis, an accuracy level of 1 corresponds to a tolerance of 1.0e-6 and an accuracy level of 5 corresponds to a tolerance of 1.0e-10.

This solver option is available only for linear static and linear full transient transient structural analysis and steady-state/transient linear or nonlinear thermal analysis.

Since the solver and tolerance are selected based on the physics and conditions of the problem being solved, it is recommended that this command be issued immediately before solving the problem (once the problem has been completely defined).

When the automatic iterative solver option is chosen and appropriate conditions have been met, neither the Jobname.EMAT nor Jobname.EROT files will be created for structural analysis and thermal analysis. This option is not recommended for thermal analysis involving phase change. When this option is chosen but the appropriate conditions have not been met, ANSYS uses the FRONTAL solver for the solution. A NOTE message is issued which informs you of the solver and tolerance used in the solution.

3.9 Obtaining the Solution

To initiate the solution, use one of the following:

Command(s):

SOLVE

GUI:

Main Menu>Solution>Current LS or Run FLOTRAN

Because the solution phase generally requires more computer resources that the other phases of an analysis, it is better suited to batch (background) mode than interactive mode.

The solver writes output to the output file (Jobname.OUT) and the results file. If you run the solution interactively, the output "file" is actually your screen (window). By using one of the following before issuing SOLVE, you can divert the output to a file instead of the screen:

Command(s):

/OUTPUT

GUI:

Utility Menu>File>Switch Output to>File or Output Window

Data written to the output file consist of the following:

Load summary information
Mass and moments of inertia of the model
Solution summary information
A final closing banner that gives total CPU time and elapsed time.
Data requested by the OUTPR output control command or its GUI counterpart

In interactive mode, much of the output is suppressed. The results file (Jobname.RST, RTH, RMG, or .RFL) contains all results data in binary form, which you can then review in the postprocessors.

Another useful file produced during solution is Jobname.STAT, which gives the status of the solution. You can use this file to monitor an analysis while it is running. It is particularly useful in iterative analyses such as nonlinear and transient analyses.

The SOLVE command calculates the solution for the load step data currently in the database.

3.10 Solving Multiple Load Steps

There are three ways to define and solve multiple load steps:

Load step file method
Array parameter method
Multiple SOLVE method.

3.10.1 Using the Load Step File Method

The load step file is a convenient method to use when you want to solve problems while you are away from your terminal or PC (for example, overnight). It involves writing each load step to a load step file (via the LSWRITE command or its GUI equivalent) and, with one command, reading in each file and obtaining the solution. See Chapter 2 for details about creating load step files.

To solve multiple load steps, issue the LSSOLVE command (Main Menu>Solution>From LS Files). LSSOLVE is actually a macro that reads in the load step files sequentially and initiates the solution for each load step. A sample command input for the load step file method is shown below:

/SOLU             	! Enter SOLUTION
...

!  Load Step 1:
D,...         	! Loads
SF,...
...
NSUBST,...        	! Load step options
KBC,...
OUTRES,...
OUTPR,...
...
LSWRITE         	! Writes load step file: Jobname.S01

!  Load Step 2:
D,...        	! Loads
SF,...
...
NSUBST,...        	! Load step options
KBC,...
OUTRES,...
OUTPR,...
...
LSWRITE          	! Writes load step file: Jobname.S02
...
...
LSSOLVE,1,2	! Initiates solution for load step files 1 and 2

See the ANSYS Commands Reference for a discussion of the NSUBST, KBC, OUTRES, OUTPR, LSWRITE and LSSOLVE commands.

3.10.2 Using the Array Parameter Method

This method, mainly intended for transient or nonlinear static (steady-state) analyses, requires knowledge of array parameters and do-loops, which are part of APDL (ANSYS Parametric Design Language). See the APDL Programmer's Guide for information about APDL. The array parameter method involves building tables of load versus time using array parameters and is best explained by the following example.

Figure 3-3 Examples of time-varying loads

Suppose that you have a set of time-varying loads such as the ones shown above. There are three load functions, so you need to define three array parameters. All three array parameters must be of type TABLE. The force function has five points, so it needs a 5x1 array; the pressure function needs a 6x1 array; and the temperature function needs a 2x1 array. Notice that all three arrays are one-dimensional. The load values are entered in column 1 and the time values are entered in column zero. (The zeroth column and zeroth row, which normally contain index numbers, must be changed and filled with a monotonically increasing set of numbers if you define the array parameter as a TABLE.)

To define the three array parameters, you first need to declare their type and dimensions. To do so, use either of the following:

Command(s):

*DIM

GUI:

Utility Menu>Parameters>Array Parameters>Define/Edit

For example:

*DIM,FORCE,TABLE,5,1
*DIM,PRESSURE,TABLE,6,1
*DIM,TEMP,TABLE,2,1

You can now use either the array parameter editor (Utility Menu> Parameters>Array Parameters>Define/Edit) or a set of "=" commands to fill these arrays. The latter method is shown below.

FORCE(1,1)=100,2000,2000,800,100	! Force values in column 1
FORCE(1,0)=0,21.5,50.9,98.7,112  	! Corresponding time values in column 0
FORCE(0,1)=1		 	! Zeroth row
PRESSURE(1,1)=1000,1000,500,500,1000,1000
PRESSURE(1,0)=0,35,35.8,74.4,76,112
PRESSURE(0,1)=1
TEMP(1,1)=800,75
TEMP(1,0)=0,112
TEMP(0,1)=1

You have now defined the load histories. To apply these loads and obtain the solution, you need to construct a do-loop (using the commands *DO and *ENDDO) such as the one shown below:

TM_START=1E-6               ! Starting time (must be > 0)
TM_END=112                  ! Ending time of the transient
TM_INCR=1.5                 ! Time increment
*DO,TM,TM_START,TM_END,TM_INCR    ! Do for TM from TM_START to TM_END in
                                  !  steps of TM_INCR
   TIME,TM                  ! Time value
   F,272,FY,FORCE(TM)       ! Time-varying force (at node 272, FY)
   NSEL,...                 ! Select nodes on pressure surface
   SF,ALL,PRES,PRESSURE(TM) ! Time-varying pressure
   NSEL,ALL                 ! Activate all nodes
   NSEL,...                 ! Select nodes for temperature specification
   BF,ALL,TEMP,TEMP(TM)     ! Time-varying temperature
   NSEL,ALL                 ! Activate all nodes
   SOLVE                    ! Initiate solution calculations
*ENDDO

See the ANSYS Commands Reference for discussions of the *DO, TIME, F, NSEL, SF, BF and *ENDDO commands.

You can change the time increment (TM_INCR parameter) very easily with this method. With other methods, changing the time increment for such complex load histories would be quite cumbersome.

3.10.3 Using the Multiple SOLVE Method

This method is the most straightforward. It involves issuing the SOLVE command after each load step is defined. The main disadvantage, for interactive use, is that you have to wait for the solution to be completed before defining the next load step. A typical command stream for the multiple SOLVE method is shown below:

/SOLU
...
! Load step 1:
D,...
SF,...
...
SOLVE	! Solution for load step 1

! Load step 2
F,...
SF,...
...
SOLVE	! Solution for load step 2
Etc.

3.11 Terminating a Running Job

You can terminate a running ANSYS job, if necessary, with the help of system functions such as a system break, issuing a kill signal, or deleting the entry in the batch queue. For nonlinear analyses, however, this is not the preferred method, because a job terminated in this manner cannot be restarted.

To terminate a nonlinear analysis "cleanly" on a multitasking operating system, create an abort file, named Jobname.ABT (or, on some case-sensitive systems, jobname.abt), containing the word nonlinear on the first line, starting in column 1. At the start of an equilibrium iteration, if the ANSYS program finds such a file in the working directory, the analysis will be stopped and can be restarted at a later time.

Note-If commands are being read using a file specified via the /INPUT command (Main Menu>Preprocessor>Material Props>Material Library, or Utility Menu> File>Read Input from), the abort file will terminate the solution, but the program will continue to read commands from the specified input file. Thus, any postprocessing commands included in the input file will execute.

3.12 Restarting an Analysis

Sometimes you may need to restart an analysis after the initial run has been completed. For instance, you may want to add more load steps to the analysis. These may be additional loading conditions in a linear static analysis or additional portions of a time-history loading curve in a transient analysis. Or, you may need to recover from a convergence failure in a nonlinear analysis.

3.12.1 Requirements for Restarting an Analysis

The model must meet the following conditions to restart an analysis:

The analysis type must be either static (steady-state), harmonic (2-D magnetic only), or transient (full method only). No other analysis can be restarted.
At least one iteration must have been completed in the initial run.
The initial run should not have stopped due to a "killed" job, system break, or system crash.

The following files must be available from the initial run:
- Jobname.DB - the database file saved after solution but before POST1 postprocessing. You should save the file after solution completion because many solution variables are set after the solution process starts. Save the file before you enter POST1 because during postprocessing, the SET command (or the equivalent GUI path) overwrites existing boundary conditions in memory with those from the results file. A subsequent SAVE command will then store these boundary conditions. (For non-converged solutions, the database file is saved automatically; see the note below.)

Jobname.EMAT - element matrices (if created).

Jobname.ESAV or .OSAV - Element saved data (.ESAV) or old element saved data (.OSAV). Jobname.OSAV is required only if the .ESAV file is missing, incomplete, or otherwise corrupted because of a diverging solution; because the displacement limit was exceeded; or because of a negative pivot (see Table 3-2). It is written if KSTOP is set to 1 (default) or 2 on the NCNV command, or if automatic time stepping is active. If the .OSAV file is required, you must rename it as Jobname.ESAV before restarting the analysis.
Results file - This file is not required, but if it is available, results from the restart run will be appended to it with the proper, sequential load step and substep numbers. If the initial run terminated because the number of results sets on the results file were exceeded, you will need to rename the initial results file to a different name before restarting. To do so, either issue the /ASSIGN command (Utility Menu>File>ANSYS File Options).

Note-If the program terminates due to non-convergence, time limits, the abort file (Jobname.ABT), or other program-detected failure, the database is automatically saved, and the solution output (Jobname.OUT) will list the files and other information required for restarting. See also Table 3-2 for a list of termination causes and the element saved data file needed to restart.

In interactive mode, an existing database file is first written to a backup file (File.DBB). In batch mode, an existing database file is replaced by the current database information with no backup.

Table 3-2 Restart information for nonlinear analyses

Cause of Termination

Element Saved Data File

Required Corrective Action

Normal (i.e., no errors)

Jobname.ESAV

Add more load steps at the end of your job.

Non-convergence

Jobname.OSAV

Define a smaller time step, change the adaptive descent option, or take other action to enhance convergence. Rename Jobname.OSAV as Jobname.ESAV before restarting.

Non-convergence due to insufficient equilibrium iterations

Jobname.ESAV

If the solution was converging, allow more equilibrium equations (NEQIT command)

Cumulative iteration limit exceeded (NCNV command)

Jobname.ESAV

Increase ITLIM on NCNV command.

Time limit exceeded (NCNV)

Jobname.ESAV

None (simply restart the analysis).

Displacement limit exceeded (NCNV)

Jobname.OSAV

(Same as for non-convergence.)

Negative pivot

Jobname.OSAV

(Same as for non-convergence.)

Jobname.ABT
� if solution was converging
� if solution was diverging

Jobname.ESAV
Jobname.OSAV

Make whatever changes are necessary to address the behavior that caused you to voluntarily terminate the analysis.

"Full" results file (more than 1000 substeps)
Time steps output.

Jobname.ESAV

Could indicate a problem - check settings on CNVTOL, DELTIM, and NSUBST, or KEYOPT(7) for contact elements. Or, specify larger number of results allowed on results file [/CONFIG,NRES] before solution or reduce the number of results to be output. Also rename results file (/ASSIGN)

"Killed" job (system break), system crash, or system time-limit exceeded

Not applicable

No restart is possible.

3.12.2 Procedure for Restarting an Analysis

The procedure to do a restart analysis is as follows:

1. Enter the ANSYS program and specify the same jobname that was used in the initial run. (To do so, issue the /FILNAME command (Utility Menu>File>Change Jobname)).

2. Resume the database file (RESUME command (Utility Menu>File> Resume Jobname.db)), then enter the SOLUTION processor (/SOLU command (Main Menu>Solution)).

3. Indicate that this is a restart analysis (by issuing the command ANTYPE,,REST (Main Menu>Solution>Restart)).

4. Replot the geometry for the analysis (using one of the plot commands (APLOT, EPLOT (Utility Menu>Plot> Replot)).

5. Specify revised or additional loads as needed. Modified ramped loads start from their previous values. Newly applied ramped loads are ramped from zero; newly applied body loads start from initial values. Deleted loads which are reapplied are treated as new, not modified, loads. Surface and body loads to be deleted should be ramped to zero or to the initial value, so that the Jobname.ESAV and Jobname.OSAV files are consistent with the database.

Be sure to take whatever corrective action is necessary if you are restarting from a convergence failure. 6. Specify whether the triangularized matrix (Jobname.TRI) is to be reused, using one of the following:

Command(s):

KUSE

GUI:

Main Menu>Preprocessor>Loads>Other>Reuse Tri Matrix
Main Menu>Solution>Other>Reuse Tri Matrix

KUSE

Jobname

ANSYS Theory Reference

KUSE

Sometimes, you may have to analyze the same model for different constraint conditions, for instance a quarter-symmetry model with symmetry-symmetry (SS), symmetry-antisymmetry (SA), antisymmetry-symmetry (AS), and antisymmetry-antisymmetry (AA) conditions. In such a situation, keep the following points in mind:

All four cases (SS, SA, AS, AA) require a new triangularized matrix.
You can keep copies of the Jobname.TRI files for the various cases and use them as appropriate.
You can use substructuring (with the constrained nodes as master DOF) to minimize computing time. (See Chapter 5 of the ANSYS Advanced Analysis Techniques Guide.)

7. Initiate the restart solution by issuing the SOLVE command. (See Section 3.9 for details.)

8. Repeat steps 4, 5, and 6 for additional load steps, if any. Or use the load step file method to create and solve multiple load steps. Use the following commands:

Command(s):

LSWRITE

GUI:

Main Menu>Preprocessor>Loads>Write LS File
Main Menu>Solution>Write LS File

Command(s):

LSSOLVE

GUI:

Main Menu>Solution>From LS Files

9. Postprocess as desired, then exit the ANSYS program.

A sample restart input listing is shown below.

!  Restart run:
/FILNAME,...	! Jobname
RESUME
/SOLU
ANTYPE,,REST	! Specify restart of previous analysis
!
! Specify new loads, new load step options, etc. 
! Take appropriate corrective action for nonlinear analyses.
!
SAVE
SOLVE	! Initiate restart solution
SAVE	! Optional SAVE for possible subsequent restart
FINISH
!
! Postprocess as desired
!
/EXIT,NOSAV

3.12.3 Restarting a Nonlinear Analysis From an Incompatible Database

Sometimes, postprocessing is performed prior to a restart. If you issue SET and SAVE commands during this postprocessing, the boundary conditions in your database might be altered and become inconsistent with those needed for a restart. By default, the program saves your file automatically when you exit. At the end of solution, the boundary conditions for the last load step are stored in the database memory. (The database contains only one set of boundary conditions.)

A SET command in POST1 (other than SET,LAST) reads the boundary conditions for the specified results into the database, and overwrites the database stored in memory. If you subsequently save your file or exit, ANSYS overwrites the boundary conditions in the database file with the D's and F's from the current results file. However, to perform a restart which ramps boundary conditions from the last solved substep, you need the boundary conditions for the last successfully solved load substep.

3.12.3.1 Re-establishing Boundary Conditions

To re-establish the correct boundary conditions for the restart, first run a "dummy" load step. The procedure is as follows:

1. Rename Jobname.OSAV as Jobname.ESAV.

2. Enter the ANSYS program and specify the same jobname that was used in the initial run. (To do so, issue the /FILNAME command (Utility Menu>File>Change Jobname)).

3. Resume the database file (RESUME command (Utility Menu> File>Resume Jobname.db)), then enter the SOLUTION processor (/SOLU command (Main Menu>Solution)).

4. Indicate that this is a restart analysis by issuing the command ANTYPE,,REST (Main Menu>Solution>Restart).

5. Re-specify boundary conditions from the last substep that was successfully solved. One substep is sufficient since the solution will converge immediately.

6. Issue a SOLVE command (Main Menu>Solution>Current LS or Main Menu>Solution>Run FLOTRAN).

7. Apply final loads and load step options as desired. You will need to adjust the number of substeps (or time step size) if this load step is a "continuation" of the previous (before the dummy) load step. Time step numbering may be altered from your initial intent. Use a small time increment in step 6 if you need to preserve the time step numbering (such as for a transient analysis).

8. Continue the procedure as outlined in Section 3.12.

3.13 Exercising Partial Solution Steps

When you initiate a solution, the ANSYS program goes through a predefined series of steps to calculate the solution; it formulates element matrices, triangularizes matrices, and so on. Another SOLUTION command, PSOLVE, (Main Menu>Solution>Partial Solu) allows you to exercise each such step individually, completing just a portion of the solution sequence each time. For example, you can stop at the element matrix formulation step and go down a different path to perform inertia relief calculations. Or, you can stop at the Guyan reduction step (matrix reduction) and go on to calculate reduced eigenvalues.

Some possible uses of the PSOLVE approach are listed below.

You can use it as a restart tool. For instance, you can start from the .EMAT file and perform a different analysis.
You can use it to perform a prestressed modal analysis of a large deflection static solution.
You can use the results of an intermediate solution step (such as the triangularized matrix) as input to another software package or user-written program.
If you are interested just in inertia relief calculations or some such intermediate result, the PSOLVE approach is useful. See the ANSYS Structural Analysis Guide for more information.

3.14 Estimating Run Time and File Sizes

For "small to moderately sized" ANSYS models with little added analysis complexity, most users will simply initiate the solution as indicated previously in this chapter. However, for larger models, or for analyses with complicated nonlinear options, you may feel more comfortable knowing what to expect before initiating solution. For example, how long will your analysis take to solve and how much disk space will you need before you run it? How much memory will your analysis need? While there is no exact method of predicting these quantities, the ANSYS program can estimate them in its RUNSTAT module.

The RUNSTAT module is a processor, or routine, of its own. You can enter it by issuing the /RUNSTAT (Main Menu>Run-Time Stats) command at the Begin level.

The RUNSTAT module estimates run times and other statistics based on information in the database. Therefore, you must define the model geometry (nodes, elements, etc.), loads and load options, and analysis options before you enter RUNSTAT. It is best to use RUNSTAT immediately before solving.

3.14.1 Estimating Run Time

To estimate the run time, the ANSYS program needs your computer's performance information: MIPS (millions of instructions per second), MFLOPs (millions of floating point operations per second), etc. To obtain this information, use the RSPEED command (Main Menu>Run-Time Stats>System Settings).

If you do not know such details about your computer, you can execute the macro SETSPEED, which issues the appropriate RSPEED command for you. For more information about the SETSPEED macro, see Section 3.7 of the ANSYS Operations Guide.

The other piece of information needed to estimate the total run time is the number of iterations (or load steps in a linear, static analysis) for the analysis. To get this information, use either method shown below:

Command(s):

RITER

GUI:

Main Menu>Run-Time Stats>Iter Setting

To obtain an estimate of run time, use one of the following:

Command(s):

RTIMST

GUI:

Main Menu>Run-Time Stats>Individual Stats

Based on information supplied by the RSPEED and RITER commands and the model information in the database, the RTIMST command gives you a run time estimate.

3.14.2 Estimating File Size

The RFILSZ command estimates the size of the following files: .ESAV, .EMAT, .EROT, .TRI, .FULL, .RST, .RTH, .RMG, and .RFL. The GUI equivalent for RFILSZ is the same as for RTIMST. The estimate of the results files is based on one set of results (one substep). You will need to multiply it by the estimated number of results written for the actual results file sizes.

3.14.3 Estimating Memory Requirements

The RWFRNT command (Main Menu>Run-Time Stats>Individual Stats) gives wavefront estimates and memory requirements for solution. You can then request that amount of memory using the ANSYS work space entry option. (See Chapter 19 for more information about memory management.) The RWFRNT command automatically reorders the elements if no reordering has previously been done.

Other RUNSTAT commands are RSTAT, which gives model statistics (node and element information); RMEMRY, which gives memory statistics; and RALL (Main Menu>Run-Time Stats>All Statistics), which is a convenience command that executes the RSTAT, RWFRNT, RTIMST, and RMEMRY commands. The GUI equivalent for all these commands except for RALL is Main Menu>Run-Time Stats>Individual Stats.

3.15 Singularities

A singularity exists in an analysis whenever an indeterminate or non-unique solution is possible. A negative or zero equation solver pivot value will yield such a solution. In some instances, it may be desirable to continue the analysis, even though a negative or zero pivot value is encountered. You can use the PIVCHECK command to specify whether or not to stop the analysis when this occurs.

The default value for the PIVCHECK command is ON. With PIVCHECK set to ON, a linear static analysis (in batch mode only) stops when a negative or zero pivot value is encountered. The message "NEGATIVE PIVOT VALUE" or "PIVOTS SET TO ZERO" is displayed. If PIVCHECK is set to OFF, the pivots are not checked. Set PIVCHECK to OFF if you want your batch mode linear static analysis to continue in spite of a zero or negative pivot value. The PIVCHECK setting has no effect for nonlinear analyses, since a negative or zero pivot value can occur for a valid analysis. When PIVCHECK is set to OFF, ANSYS automatically increases any pivot value smaller than machine "zero" to a value between 10 and 100 times that machine's "zero" value. Machine "zero" is a tiny number the machine uses to define "zero" within some tolerance. This value varies for different computers (1e-15).

The following conditions may cause singularities in the solution process:

Insufficient constraints.
Nonlinear elements in a model (such as gaps, sliders, hinges, cables, etc.). A portion of the structure may have collapsed or may have "broken loose."
Negative values of material properties, such as DENS or C, specified in a transient thermal analysis.
Unconstrained joints. The element arrangements may cause singularities. For example, two horizontal spar elements will have an unconstrained degree of freedom in the vertical direction at the joint. A linear analysis would ignore a vertical load applied at that point. Also, consider a shell element with no in-plane rotational stiffness connected perpendicularly to a beam or pipe element. There is no in-plane rotational stiffness at the joint. A linear analysis would ignore an in-plane moment applied at that joint.
Buckling. When stress stiffening effects are negative (compressive) the structure weakens under load. If the structure weakens enough to effectively reduce the stiffness to zero or less, a singularity exists and the structure has buckled. The "NEGATIVE PIVOT VALUE--" message will be printed.
Zero Stiffness Matrix (on row or column). Both linear and nonlinear analyses will ignore an applied load if the stiffness is exactly zero.

Go to the beginning of this chapter

Solver	Typical Applications	Model Size	Memory Use	Disk Use
Frontal Solver (direct elimination solver)	When robustness is required (nonlinear analysis) or when memory is limited.	Under 50,000 DOFs	Low	High
Sparse Direct Solver (direct elimination solver)	When robustness and solution speed are required (nonlinear analysis); for linear analysis where iterative solvers are slow to converge (especially for ill-conditioned matrices, such as poorly shaped elements).	10,000 to 500,000 DOFs (more for shell & beam models).	Medium	High
PCG Solver (iterative solver)	When solution speed is crucial (linear analysis of large models). Especially well suited for large models with solid elements.	50,000 to 1,000,000+ DOFs	High	Low
ICCG (Iterative solver)	When solution speed is crucial in multiphysics applications. Handles models that are harder to converge in other iterative solvers (nearly indefinite matrices).	50,000 to 1,000,000+ DOFs	High	Low
JCG Solver (iterative solver)	When solution speed is crucial in "single-field" problems (thermal, magnetics, acoustics, and multiphysics)	50,000 to 1,000,000+ DOFs	Medium	Low

Cause of Termination	Element Saved Data File	Required Corrective Action
Normal (i.e., no errors)	Jobname.ESAV	Add more load steps at the end of your job.
Non-convergence	Jobname.OSAV	Define a smaller time step, change the adaptive descent option, or take other action to enhance convergence. Rename Jobname.OSAV as Jobname.ESAV before restarting.
Non-convergence due to insufficient equilibrium iterations	Jobname.ESAV	If the solution was converging, allow more equilibrium equations (NEQIT command)
Cumulative iteration limit exceeded (NCNV command)	Jobname.ESAV	Increase ITLIM on NCNV command.
Time limit exceeded (NCNV)	Jobname.ESAV	None (simply restart the analysis).
Displacement limit exceeded (NCNV)	Jobname.OSAV	(Same as for non-convergence.)
Negative pivot	Jobname.OSAV	(Same as for non-convergence.)
Jobname.ABT � if solution was converging � if solution was diverging	Jobname.ESAV Jobname.OSAV	Make whatever changes are necessary to address the behavior that caused you to voluntarily terminate the analysis.
"Full" results file (more than 1000 substeps) Time steps output.	Jobname.ESAV	Could indicate a problem - check settings on CNVTOL, DELTIM, and NSUBST, or KEYOPT(7) for contact elements. Or, specify larger number of results allowed on results file [/CONFIG,NRES] before solution or reduce the number of results to be output. Also rename results file (/ASSIGN)
"Killed" job (system break), system crash, or system time-limit exceeded	Not applicable	No restart is possible.