Occasionally, you may need to restart an analysis after the initial run has been completed. Three different restart procedures are available:

The following examples illustrate instances where a restart may be necessary:

More load steps must be added to the analysis (multiframe restart).

There are additional loading conditions in a linear static analysis or additional portions of a time-history loading curve in a transient analysis (multiframe restart).

To recover from a convergence failure in a nonlinear analysis (multiframe restart).

To do a linear perturbation analysis (multiframe restart). See

*General Procedure for Linear Perturbation Analysis*for details.To generate load vectors, residual vectors, or enforced motion pseudo-static shapes for a subsequent mode-superposition analysis or spectrum analysis (modal analysis restart).

The multiframe restart can resume a job at any point in the analysis for which information is saved, allowing you to perform multiple analyses of a model and giving you more options for recovering from an abnormal termination. The program allows a multiframe restart for static and transient (full or mode-superposition method) analyses. Distributed ANSYS supports multiframe restarts for nonlinear static and full transient analyses, and for linear perturbation analyses.

The modal analysis restart can be used to do additional calculations after the eigensolution. Modal extraction typically requires more computing time than element loads generation, residual vector generation, and enforced static modes calculation. Reusing eigenmodes that have already been generated can save significant time in a downstream analysis.

You can also rerun a VT Accelerator analysis using information available from a previous run. Rerunning an analysis completed with VT Accelerator can reduce the number of iterations needed to obtain the solution for all load steps and substeps.

To perform a multiframe restart, the model must meet the following conditions:

The analysis type must be static (steady-state), harmonic (2-D magnetic only), or transient (full or mode-superposition method only). No other analysis types can be restarted.

At least one iteration must have been completed in the initial run.

The initial run should not have stopped abnormally (for example, a system level abort).

The initial analysis, which generated the restart files, and the restarted analysis must be performed with the same version of the ANSYS, Inc. software product.

For nonlinear static and full transient analyses, the program sets up the parameters for a multiframe restart by default.

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 the initial analysis, use the **RESCONTROL** command to set up the frequency at which restart files are saved
within each load step of the run.

When restarting 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 terminate a load step at the restart point (rescaling all loading)
and continue with the next load step.

The following example input shows how to set up the restart file parameters in an analysis then restart the analysis, continuing from a specified load step and substep.

/prep7 et,1,182,,, !Define nodes and elements mp,ex,1,10 mp,alpx,1,0.1 mp,alpy,1,0.1 mp,alpx,1,0.1 mp,nuxy,1,0.2 n,1 n,2,1 n,3,1,1 n,4,,1 n,5,2 n,6,2,1 e,1,2,3,4 e,2,5,6,3 finish /solu rescontrol,,all,1,5 !For all load steps, write the restart !file .Rnnn at every substep, but allow !a maximum of 5 restart files per load step nlgeom,on !Large strain analysis with temperature loadings nsubst,6,6,6 d,1,all d,2,uy outres,all,all bfe,1,temp,1,1 bfe,2,temp,1,5 solve rescontrol,file_summary !List information contained in all the !.Rnnn files for this job finish /post1 set,1,3 presol set,last presol finish /solu antyp,,rest,1,3 !Restart the analysis at load step 1, !substep 3 solve rescontrol,file_summary finish /post1 set,last presol finish /solu antype,,rest,1,3,endstep !End load step 1 at substep 3 !when time (load factor) = 0.5 !ldstep = 1, substep = 3, load solve !execute ENDSTEP, loads are !rescaled to time = 0.5 rescontrol,file_summary bfe,1,temp,1,2 !apply higher loads, bfe,2,temp,1,6 solve !execute solve to advance load !factor from previous !time = 0.5 to time = 1.5 /post1 set,last presol finish

The following example input shows how to terminate a load step at a particular substep, then continue with the next load step.

/solu antype,,rest,1,3,endstep !End load step 1 at substep 3 !when time (load factor) = 0.6125 !ldstep = 1, substep = 3, load solve !execute ENDSTEP, loads are !rescaled to time = 0.6125 rescontrol,file_summary bfe,1,temp,1,2 !apply higher loads, bfe,2,temp,1,6 solve !execute solve to advance load !factor from previous !time = 0.6125 to time = 1.6125 /post1 set,last presol finish

The following example input shows how to restart an analysis with old and new parameters.

/prep7 et,1,182 ! Build model n,1,0.0,0.0 n,2,0.0,0.5 n,3,0.0,1.0 n,4,1.0,0.0 n,5,1.0,0.5 n,6,1.0,1.0 e, 1,4,5,2 e, 2,5,6,3 mp,ex,1,1000.0 mp,nuxy,1,0.3 mp,alpx,1,1.e-4 d,1,all d,2,ux,0.0 d,3,ux,0.0 d,4,uy,0.0 *dim,ftbl,table,4,1,,time ! Make tabular point load ftbl(1,0)=1,2,3,4 ftbl(1,1)=2.5,5.0,7.5,10.0 nsel,all f,all,fx,%ftbl% ! Apply it to all nodes flist /solu rescont,,all,all ! Save all substeps for possible restart nlgeo,on time,4 deltim,1 outres,all,all solve ! Solve with point loads and the *.RDB file is saved ! at the moment. The parameterized tabular point load ! FTBL is also saved into *.RDB *dim,temtbl,table,4,1,,time ! Define table TEMTBL and use it for body load: temperature temtbl(1,0)=1,2,3,4 temtbl(1,1)=250,500.0,750,1000. ! bf,all,TEMP,%temtbl% ! May use this to apply the body load table ! bflist parsave,all,moreload ! Save all the APDL parameters and tables to file: moreload ! NOTE: *.RDB does not have information of table TEMTBL. fini /clear, nostart /solu antype,,restart,1,3,endstep ! Do restart ENDSTEP because we want to apply TEMTBL at ! TIME = 3.5 (LDSTEP=1,SUBSTEP=3) because we want to ! Apply the temperature load from TIME=3.5 onwards. ! Here, RESTART has resumed *.RDB database where the ! Table FTBL is saved. solve ! Activate ENDSTEP parresu,,moreload ! For further load step, we want to apply table TEMTBL ! as body force. NOTE: table TEMTBL is not in *.RDB. Therefore, ! we have to use PARRESU command. APDL file "moreload" is ! saved earlier. *status ! List all the ADPL information available at this point bf,all,TEMP,%temtbl% ! Apply temperature table load TEMTBL bflist time,4 ! Solve up to TIME = 4.0 because the load step ENDSTEP only ! carries up to TIME = 3.5 solve fini /post1 set,last prdis prrsol fini

The following example input demonstrates a restart after changing boundary conditions.

/prep7 et,1,21 r,1,1,1,1,1,1,1 n,1 e,1 fini /solu antyp,trans timint,off time,.1 nsub,2 kbc,0 d,1,ux,100 ! to apply initial velocity (IC command is preferred) solve timint,on ddele,1,ux ! this requires special handling by multi-frame restart ! if a reaction force exists at this dof, replace it with an equal ! force using the endstop option time,.2 nsub,5 rescontrol,define,all,1 ! request possible restart from any substep outres,nsol,1 solve fini /solu antyp,,restart,2,3 ! this command resumes the .rdb database created at the start of solution ! (restart from substep 3) d,1,ux,100 ! re-specify boundary condition deleted during solution solve fini /post26 nsol,2,1,ux prvar,2 ! results show constant velocity through restart finish

The following example input demonstrates
the use of a negative value input for * Ldstep* on the

`.Rnnn`

`Ldstep`

/prep7 mp,ex,1,10 mp,nuxy,1,0.3 mp,dens,1,0.5 n,1, n,2,1 n,3,1,1 n,4,0,1 n,5,2 n,6,2,1 n,7,3,0 n,8,3,1 nlist et,1,182 e,1,2,3,4 e,2,5,6,3 e,5,7,8,6 nsel,all d,1,all d,4,ux,0.01 finish /solu antype,static nlgeom,on nsubst,2,2,2 rescontrol,,-3,last ! For the next 11 loadsteps, write load history ! information to .ldhi file every 3rd loadstep *do,i,1,11 solve ! Solve for 11 loadsteps *enddo rescontrol,,-100,last ! For the next 1300 loadsteps, write load history ! information to .ldhi file every 100th loadstep *do,i,1,1300 solve ! Solve for another 1300 loadsteps *enddo finish /solu antype,,restart,,,pert ! Use the LAST possible restart point from ! the previous 1311 loadsteps ! to do a linear perturbation modal analysis perturb,modal solve,elform modopt,lanb,1 solve finish ! Completion of linear perturbation modal phase

The following example input shows how to delete a previously defined restart specification prior to adding a new one.

/prep7 et,1,182 ! Build the model mp,ex,1,3e9 mp,nuxy,1,0.3 mp,dense,1,2500 n,1, n,2,1 n,3,1,1 n,4,0,1 n,5,2 n,6,2,1 n,7,3,0 n,8,3,1 nlist e,1,2,3,4 e,2,5,6,3 e,5,7,8,6 nall nsel,s,loc,x,0 d,all,all,0 nsel,all save finish /solu antype,static ! Perform a static analysis nlgeom,on ! Large deflection is on nsel,s,loc,x,3 f,all,fx,50 allsel,all nsubst,5,5,5 rescontrol,define,-3,last ! For the next 10 loadsteps, write load history ! information to .ldhi file every 3rd loadstep *do,i,1,10 ! solve for 10 loadsteps solve *enddo rescontrol,delete,-3 ! Delete previous RESCONTROL command rescontrol,define,last,last ! For the next 10 loadsteps, write load history ! information to .ldhi file for the last loadstep only *do,i,1,10 ! solve for another 10 loadsteps solve *enddo rescontrol,file_summary ! Print the substeps and load step information for all .Xnnn files ! The .Xnnn files saved for loadsteps: 3, 6, 9, 20 ! The .ldhi file saved for loadsteps: 2,3,5,6,8,9,19,20 finish

**Note:** If you are using the Solution Controls dialog box to do a static or full transient analysis, you can specify
basic multiframe restart options on the dialog's **Sol'n Options** tab. These options include the maximum number of restart files that
you want to write for a load step, as well as how frequently you want
the files to be written. For an overview of the Solution
Controls dialog box, see *Using Special Solution Controls for Certain Types of Structural
Analyses*. For details about how to set options
on the Solution Controls dialog box, access
the dialog box ( ), select the tab that you are interested in, and click the button.

The following files are necessary to do a multiframe restart:

**Jobname.RDB**- This is a database file saved automatically at the first iteration of the first load step, first substep of a job. This file provides a complete description of the solution with all initial conditions, and remains unchanged regardless of how many restarts are done for a particular job. When running a job, you should input all information needed for the solution - including parameters (APDL), components, and mandatory solution setup information - before you issue the first**SOLVE**. If you do not specify parameters before issuing the first**SOLVE**command, the parameters are not saved in the**.RDB**file. In this case, you must use**PARSAV**before you begin the solution and**PARRES**during the restart to save and restore the parameters. If the information stored in the**.RDB**file is not sufficient to perform the restart, you must input the additional information in the restart session before issuing the**SOLVE**command.**Jobname.LDHI**- This is the load history file for the specified job. It is an ASCII file (similar to files created by**LSWRITE**) that contains all loading and boundary conditions for specified load steps, including parameters that may be required for tabular loads and boundary conditions. The frequency at which load history information is written is determined by the**RESCONTROL**command. In general, you need the loading and boundary conditions for two contiguous load steps because of the ramped load conditions for a restart.The loading and boundary conditions are stored for the FE mesh. Loading and boundary conditions applied to the solid model are transferred to the FE mesh before being stored in

**Jobname.LDHI**. During a multiframe restart, the program reads the loading and boundary conditions for the restart load step from this file (similar to an**LSREAD**command).By default, the load history information is written to

**Jobname.LDHI**only for the last load step. For analyses that involve many load steps, this saves disk space and speeds up overall solution time. Alternatively, you can specify the frequency that load step information is written to**Jobname.LDHI**by inputting a negative number for theargument of the`Ldstep`

**RESCONTROL**command.The

**Jobname.LDHI**file is modified at the end of each specified load step. You cannot modify this file because any modifications may cause an unexpected restart condition.**Jobname.R**- For nonlinear static and full transient analyses. This file contains element saved records similar to the`nnn`

**.ESAV**or**.OSAV**files. This file also contains all solution commands and status for a particular substep of a load step. All of the**.R**files are saved at the converged state of a substep so that all element saved records are valid. If a substep does not converge, no`nnn`

**.R**file is written for that substep. Instead, an`nnn`

**.R**file from a previously converged substep is written. However, if the current substep number is 1, the`nnn`

**.R**file will be from the last substep of the previous load step.`nnn`

**Jobname.M**- For mode-superposition transient analysis. This file contains the modal displacements, velocities, and accelerations records and solution commands for a single substep of a load step`nnn`

**Note for Distributed ANSYS **For Distributed ANSYS, the **Jobname.RDB** and **Jobname.LDHI** files
contain data for the entire model and are required on the master process
only. The **Jobname** files contain
only the data for the domain on which they were created and are required
on the master and slaves processes. The

`X`

.R`nnn`

`nnn`

`X`

`X`

Multiframe restart has the following limitations for a nonlinear static analysis, a nonlinear full transient analysis, or a linear full transient analysis:

Material properties or elements cannot be changed during a restart.

The factorized matrix cannot be reused (

**KUSE**). A new stiffness matrix and the related**.LN22**file is regenerated.The

**.R**file does not save the`nnn`

**EKILL**and**EALIVE**commands. If**EKILL**or**EALIVE**commands are required in the restarted session, they must be issued again.The database file (

**Jobname.DB**) saved by the user (**SAVE**command) is not used by the restart. The**Jobname.RDB**file, which is a database file saved automatically by the program at the start of the first substep of the first load step, is used by the restart.The

**.RDB**file saves only the database information available at the first substep of the first load step. If other information is input after the first load step and that information is needed for the restart, it must be input again in the restart session. This situation often occurs when parameters are used (APDL); issue the**PARSAV**command to save the parameters during the initial run, and**PARRES**restore them in the restart. The situation also occurs when changing element REAL constants values; in this case, reissue the**R**command during the restart session.A restart cannot occur at the equation solver level (for example, the PCG iteration level). The job can only be restarted at a substep level (either transient or Newton-Raphson loop).

An analysis cannot be restarted with a load step number larger than 9999.

Multiframe restart does not support the arc-length method (

**ARCLEN**command).All loading and boundary conditions are stored in the

**Jobname.LDHI**file. Upon restart, removing or deleting solid modeling loading and boundary conditions does not remove these conditions from the finite element model. Loading and boundary conditions must be removed directly from nodes and elements.To terminate a nonlinear analysis "cleanly" on a multitasking operating system, create an abort file named

**Jobname.ABT**in the working directory (or on some case-sensitive systems,**jobname.abt**). This file should contain the word*nonlinear*in the first column of the first line. If the program locates this file at the start of an equilibrium iteration, the analysis stops and can be restarted at a later time.Nested

***DO**loops are not supported for restarts.The first time step of a restarted transient solution using the HHT algorithm (

**TRNOPT**) uses the Newmark algorithm. Subsequent time steps use the HHT algorithm.For the case of distributed memory parallel processing, you must use Distributed ANSYS prior to and during the restart, and the core count must be consistent. See

*Restarts in Distributed ANSYS*in the*Parallel Processing Guide*for a more detailed description of how to perform restarts in Distributed ANSYS.

Use the following procedure to restart an analysis:

Enter the program and specify the same jobname that was used in the initial run. To do so, issue the

**/FILNAME**command ( ). Enter the SOLUTION processor using**/SOLU**( ).Determine the load step and substep at which to restart by issuing

**RESCONTROL**, FILE_SUMMARY. This command prints the substep and load step information for all**.R**files in the current directory.`nnn`

Resume the database file and indicate that this is a restart analysis by issuing

**ANTYPE**,,REST,,`LDSTEP`

,`SUBSTEP`

( ).`Action`

Specify revised or additional loads as needed. Be sure to take whatever corrective action is necessary if you are restarting from a convergence failure.

Initiate the restart solution by issuing the

**SOLVE**command. (See*Obtaining the Solution*for details.) You must issue the**SOLVE**command when taking any restart action, including ENDSTEP or RSTCREATE.Postprocess as desired, then exit the program.

If the files **Jobname.LDHI** and **Jobname.RDB** exist, the **ANTYPE**,,REST
command:

Resumes the database

**Jobname.RDB**Rebuilds the loading and boundary conditions from the

**Jobname.LDHI**fileRebuilds the solution commands and status from the

**.R**file, or from the`nnn`

**.M**file in the case of a mode-superposition transient analysis.`nnn`

At this point, you can enter other commands to overwrite input
restored by the **ANTYPE** command.

**Note:** The
loading and boundary conditions restored from the **Jobname.LDHI** are for the FE mesh. The solid model loading and boundary conditions
are not stored on the **Jobname.LDHI**.

After the job is restarted, the files are affected in the following ways:

The

**.RDB**file is unchanged.All information for load steps and substeps past the restart point is deleted from the

**.LDHI**file. Information for each new load step is then appended to the file.All of the

**.R**or`nnn`

**.M**files that have load steps and substeps earlier than the restart point remain unchanged. Those files containing load steps and substeps beyond the restart point are deleted before the restart solution begins in order to prevent file conflicts.`nnn`

For nonlinear static and full transient analyses, the results file (

**.RST**) is updated according to the restart. All results from load steps and substeps later than the restart point are deleted from the file to prevent conflicts, and new information from the solution is appended to the end of the results file.For a mode-superposition transient analysis, the reduced displacements file

**.RDSP**is updated according to the restart. All results from load steps and substeps later than the restart point are deleted from the file to prevent conflicts, and new information from the solution is appended to the end of the reduced displacements file.

When a job is started from the beginning again (first substep,
first load step), all of the restart files (**.RDB**, **.LDHI**, and **.R** or

`nnn`

`nnn`

You can issue the command **ANTYPE**,,REST,* LDSTEP*,

`SUBSTEP`

The following example input shows how to create a results file for a particular substep in an analysis.

! Restart run: /solu antype,,rest,1,3,rstcreate !Create a results file from load !step 1, substep 3 outres,all,all !Store everything into the results file outpr,all,all !Optional for printed output solve !Execute the results file creation finish /post1 set,,1,3 !Get results from load step 1, !substep 3 prnsol finish

After solving a modal analysis to obtain the eigensolution, you can restart the modal analysis to perform the following calculations:

An eigensolution is not calculated in the restart phase.

The symmetric eigensolvers (LANB, LANPCG, SNODE, and SUBSP on
the **MODOPT** command) support all of the above calculations
during a modal analysis restart. The complex eigensolvers support
only some of the above calculations during a restart, as described
below:

The damped eigensolver (

**MODOPT**,DAMP) only supports mode expansion.The QR Damped eigensolver (

**MODOPT**,QRDAMP) only supports mode expansion when complex solutions are requested (= ON on the`Cpxmod`

**MODOPT**command). When complex solutions are not requested (= OFF), this eigensolver supports mode expansion and multiple load vector generation.`Cpxmod`

The unsymmetric eigensolver (

**MODOPT**,UNSYM) supports mode expansion and multiple load vector generation.

For a modal analysis restart, the database must contain the
model data as well as the modal solution data. The model in the database
must match the initial model used to solve the first modal solution.
In addition, the following files must be available: mode file (**Jobname.MODE**, as well as **Jobname.LMODE** if the unsymmetric eigensolver was used with **MODOPT**,UNSYM,,,,,,BOTH), EMAT file (**Jobname.EMAT**), ESAV file (**Jobname.ESAV**), and database (**Jobname.DB**).

New elements can be added in the restart session to define the load vectors. These new elements must have no mass or stiffness characteristics that could affect the eigenvalues obtained from the original modal analysis. Examples of such elements include:

Surface elements without density (SURF153, SURF154, SURF156).

Follower elements (FOLLW201) with KEYOPT(1) = 1 (constant direction load).

Contact elements using the multipoint constraint (MPC) approach to define surface-based constraints. The loads must be applied to the pilot node. Please refer to Surface-Based Constraints in the Mechanical APDL Contact Technology Guide for more information.

During each restart solution, the load vectors generated will
replace those generated during the previous modal solution (which
may be the original modal analysis or a modal analysis restart). See *Example 5.8: Modal Analysis Restart* for a detailed example of this procedure.

The following restrictions apply to modal analysis restart:

A modal analysis cannot be restarted if residual vectors (

**RESVEC**command) are calculated during the first analysis.Modal analysis restart is not supported for cyclic symmetry analysis.

The following example demonstrates a typical command sequence for a modal analysis restart.

/filnam,case1 /prep7 et,1,plane182 ! 2D PLANE182 elements mp,ex,1,2.0e11 ! Material Properties mp,dens,1,7800 mp,nuxy,1,0.3 rect,0,4,0,2 ! Rectangular area esize,0.5 type,1 mat,1 amesh,1 ! Mesh area with PLANE182 elements allsel,all nsel,s,loc,x,0 d,all,all,0 ! Fix the model at location X=0 nsel,all finish /com, /com, First Modal solve /com, /solu antype,modal modopt,lanb,20,0,20000 ! Use Block Lanczos, extract 20 modes in frequency range of 0 to 20000 nsel,s,loc,x,4 f,all,fx,10e5 ! First load vector (FX) nsel,all solve ! First modal solve save,case1,db finish /clear,nostart /filname,case1 resume,,db finish /com, /com, Adding New elements /com, /prep7 et,2,surf153 ! 2D Structural effect element keyopt,2,4,1 ! No midside node mp,dens,2,0 ! Density set to zero so it won't affect modal analysis results type,2 mat,2 lmesh,2 allsel,all finish /com, /com, Modal Restart Analysis /com, /solu antype,modal,restart ! Restart previous modal solve to define new load vectors fdele,all,fx ! Delete previously defined load modcontrol,on ! Generate multiple load vectors mxpand,20,,,yes ! Expand modes esel,s,type,,2 sfe,all,1,pres,0,20000 ! First load vector (SFE) overwrites the load vector generated allsel,all ! in the first modal solve (FX) solve ! First solve in modal anlayiss restart sfedele,all,1,pres,0 ! Delete previously defined load nsel,s,loc,x,2 nsel,r,loc,y,2 f,all,fy,-10e5 ! Second load vector (FY) allsel,all solve ! Second solve in modal anlayiss restart finish /com, /com, MSUP harmonic analysis by scaling the loads generated in modal solve /com, /solu antype,harmonic ! Perform Harmonic analysis hropt,msup,20 fdele,all,fy ! Delete loads defined in the modal analysis fdele,all,fx sfedele,all,1,pres,0 outres,all,all hrout,on harfrq,315,325 ! Excitation frequency nsubs,20,20,20 ! Number of substeps kbc,1 lvscale,0.5,1 ! Scale the first load vector (SFE) lvscale,0.0,2 ! Do not scale the second load vector (FY) solve finish /com, /com, Expansion of MSUP harmonic results /com, /solu expass,on outres,all,all numexp,all,,,yes ! Expand results for all substeps and calculate element results solve finish /com, /com, Time history post processing of displacement and reaction force results /com, /post26 n1=node(4,2,0) n2=node(0,0,0) nsol,2,n1,u,x,ux1 rforce,3,n2,f,x,fx1 prvar,2,3 finish

Once you have performed an analysis using the VT Accelerator option
[**STAOPT**,VT or **TRNOPT**,VT], you
may rerun the analysis; the number of iterations required to obtain
the solution for all load steps and substeps is greatly reduced. You
can make the following types of changes to the model before rerunning:

Modified or added/removed loads (constraints may not be changed, although their value may be modified)

Materials and material properties

Section and real constants

Geometry, although the mesh connectivity must remain the same (i.e. the mesh may be morphed)

VT Accelerator allows you to effectively perform parametric studies of nonlinear and transient analyses in a cost-effective manner (as well as to quickly re-run the model, which is typically necessary to get a nonlinear model operational).

When rerunning a VT Accelerator analysis, the following files must be available from the initial run:

**Jobname.DB**– the database file. It may be modified as listed in the previous section.**Jobname.ESAV**– Element saved data**Jobname.RSX**– Variational Technology results file

The procedure for rerunning a VT Accelerator analysis is as follows:

Enter the program and specify the same jobname that was used in the initial run with

**/FILNAME**).Resume the database file using

**RESUME**( ) and make any modifications to the data.Enter the SOLUTION processor using

**/SOLU**( ), and indicate that this is a restart analysis by issuing**ANTYPE**,,VTREST ( ).Because you are re-running the analysis, you must reset the load steps and loads. If resuming a database saved

*after*the first load step of the initial run, you must delete the loads and redefine the loads from the first load step.Initiate the restart solution by issuing the

**SOLVE**command. See*Obtaining the Solution*for details.Repeat steps 4, 5, and 6 for the additional load steps, if any.