Analysis record

This record describes the type of analysis, which should be performed. The analysis record can be splitted into optional meta-step input records (see below). Then certain attributes originally in analysis record can be specified independently for each meta-step. This is marked by adding “M” superscript to keyword. Then the attribute format is Keyword^M #(type).

The general format of this record can be specified using

  • “standard-syntax”
    nsteps #(in) [renumber #(in)] [profileopt #(in)] attributes #(string) [ninitmodules #(in)] [nmodules #(in)] [nxfemman #(in)]
  • “meta step-syntax”
    nmsteps #(in) [ninitmodules #(in)] [nmodules #(in)] [nxfemman #(in)]
    immediately followed by nmsteps meta step records with the following syntax:
    nsteps #(in) attributes #(string)
    The nmsteps parameter determines the number of “metasteps”. The meta step represent sequence of solution steps with common attributes. There is expected to be nmsteps subsequent metastep records. The meaning of meta step record parameters (or analysis record parameters in “standard syntax”) is following:
    • nsteps - determines number of subsequent solution steps within metastep.
    • renumber - Turns out renumbering after each time step. Necessary when Dirichlet boundary conditions change during simulation. Can also be turned out by the executeable flag -rn.
    • profileopt - Nonzero value turns on the equation renumbering to optimize the profile of characteristic matrix (uses Sloan algorithm). By default, profile optimization is not performed. It will not work in parallel mode.
    • attributes - contains the metastep related attributes of analysis (and solver), which are valid for corresponding solution steps within meta step. If used in standard syntax, the attributes are valid for all solution step.
    • ninitmodules - number of initialization module records for given problem. The initialization modules are specified after meta step section (or after analysis record, if no metasteps are present). Initialization modules allow to initialize the state variables by values previously computed by external software. The available initialization modules are described in section Initialization modules.
    • nmodules - number of export module records for given problem. The export modules are specified after initialization modules. Export modules allow to export computed data into external software for postprocessing. The available export modules are described in section Export modules.
    • nxfemman - 1 implies that an XFEM manager is created, 0 implies that no XFEM manager is created. The XFEM manager stores a list of enrichment items. The syntax of the XFEM manager record and related records is described in section Xfem manager record and associated records.
    • eetype - optional error estimator type used for the problem. Used for adaptive analysis, but can also be used to compute and write error estimates to the output files. See adaptive engineering models for details.

Not all of analysis types support the metastep syntax, and if not mentioned, the standard-syntax is expected. Currently, supported analysis types are

Structural Problems

StaticStructural

StaticStructural nsteps #(in) [deltat #(...)] [prescribedtimes #(...)] [stiffmode #(...)] [nonlocalext #(...)] [sparselinsolverparams #(...)]

Static structural analysis. Can be used to solve linear and nonlinear static structural problems, supporting changes in boundary conditions (applied load and supports). The problem can be solved under direct load or displacement control, indirect control, or by their arbitrary combination. Note, that the individual solution steps are used to describe the history of applied incremental loading. The load cases are not supported, for each load case the new analysis has to be performed. To analyze linear static problem with multiple load combinations, please use LinearStatic solver.

By default all material nonlinearities will be taken into account, geometrical not. To include geometrically nonlinear effect one must specify level of non-linearity in element records.

The sparselinsolverparams parameter describes the sparse linear solver attributes and is explained in section Sparse linear solver parameters. The optional parameter deltat defines the length of time step (equal to 1.0 by default). The times corresponding to individual solution times can be specified using optional parameter prescribedtimes, allowing to input array of discrete solution times, the number of solution steps is then equal to the size of this array. .

Linear static analysis

LinearStatics nsteps #(in) [sparselinsolverparams #(...)] [sparselinsolverparams #(...)]

Linear static analysis. Parameter nsteps indicates the number of loading cases. Problem supports multiple load cases, where number of load cases correspods to number of solution steps, individual load vectors are formed in individual time-steps. However, the static system is assumed to be the same for all load cases. For each load case an auxiliary time-step is generated with time equal to load case number.

The sparselinsolverparams parameter describes the sparse linear solver attributes and is explained in section Sparse linear solver parameters.

LinearStability

LinearStability nroot #(in) rtolv #(rn) [eigensolverparams #(...)]

Solves linear stability problem. Only first nroot smallest eigenvalues and corresponding eigenvectors will be computed. Relative convergence tolerance is specified using rtolv parameter.

The eigensolverparams parameter describes the sparse linear solver attributes and is explained in section Eigen value solvers.

EigenValueDynamic

EigenValueDynamic nroot #(in) rtolv #(rn) [eigensolverparams #(...)]

Represents the eigen value dynamic analysis. Only nroot smallest eigenvalues and corresponding eigenvectors will be computed. Relative convergence criteria is governed using rtolv parameter.

The eigensolverparams parameter describes the sparse linear solver attributes and is explained in section Eigen value solvers.

NlDEIDynamic

NlDEIDynamic nsteps #(in) dumpcoef #(rn) [deltaT #(rn)]

Represents the direct explicit nonlinear dynamic integration. The central difference method with diagonal mass matrix is used, damping matrix is assumed to be proportional to mass matrix, \(\boldsymbol{C} = \mathrm{dumpcoef} * \boldsymbol{M}\), where \(\boldsymbol{M}\) is diagonal mass matrix. Parameter nsteps specifies how many time steps will be analyzed. deltaT is time step length used for integration, which may be reduced by program in order to satisfy solution stability conditions. Parameter reduct is a scaling factor (smaller than 1), which is multiplied with the determined step length adjusted by the program. If deltaT is reduced internally, then nsteps is adjusted so that the total analysis time remains the same.

The parallel version has the following additional syntax:
&\(\langle\)[nonlocalext]\(\rangle\)&

DEIDynamic

DEIDynamic nsteps #(in) dumpcoef #(rn) [deltaT #(rn)]

Represent the linear explicit integration scheme for dynamic problem solution. The central difference method with diagonal mass matrix is used, damping matrix is assumed to be proportional to mass matrix, \(\boldsymbol{C} = \mathrm{dumpcoef} * \boldsymbol{M}\), where \(\boldsymbol{M}\) is diagonal mass matrix. deltaT is time step length used for integration, which may be reduced by program in order to satisfy solution stability conditions. Parameter nsteps specifies how many time steps will be analyzed.

DIIDynamic

DIIDynamic nsteps #(in) deltaT #(rn) [ddtscheme #(in)] [gamma #(rn)] [beta #(rn)] [eta #(rn)] [delta #(rn)] [theta #(rn)]

Represents direct implicit integration of linear dynamic problems. Solution procedure described in Solution procedure described in K. Subbaraj and M. A. Dokainish, A SURVEY OF DIRECT TIME-INTEGRATION METHODS IN COMPUTATIONAL STRUCTURAL DYNAMICS - II. IMPLICIT METHODS, Computers & Structures Vol. 32. No. 6. pp. 1387-1401, 1989.

Parameter ddtscheme determines integration scheme, as defined in src/oofemlib/timediscretizationtype.h (TD_ThreePointBackward=0 (default), TD_TwoPointBackward = 1, TD_Newmark = 2, TD_Wilson = 3, TD_Explicit = 4).

Parameters beta and gamma determine the stability and acuracy of the integration algorithm, both have zero values as default. For gamma=0.5 and beta = l/6, the linear acceleration method is obtained. Unconditional stability is obtained, when \(2\beta \ge \gamma \ge 1/2\). The dafault values are beta=0.25 and gamma=0.5. The Wilson-theta metod requires additional theta parameter with default value equal to 1.37. The damping is assumed to be modeled as Rayleigh damping \(\boldsymbol{C} = \eta \boldsymbol{M} + \delta \boldsymbol{K}\).

IncrementalLinearStatic

IncrementalLinearStatic endOfTimeOfInterest #(rn) prescribedTimes #(ra)

Represents incremental linear static problem. The problem is solved as series of linear solutions and is intended to be used for solving linear creep problems or incremental perfect plasticity.

Supports the changes of static scheme (applying, removing and changing boundary conditions) during the analysis.

Response is computed in times defined by prescribedTimes array. These times should include times, when generally the boundary conditions are changing, and in other times of interest. (For linear creep analysis, the values should be uniformly distributed on log-time scale, if no change in loading or boundary conditions). The time at the end of interested is specified using endOfTimeOfInterest parameter.

NonLinearStatic

NonLinearStatic
Non-linear static analysis. The problem can be solved under direct load or displacement control, indirect control, or by their arbitrary combination. By default all material nonlinearities will be included, geometrical not. To include geometrically nonlinear effect one must specify level of non-linearity in element records. There are two different ways, how to specify the parameters - the extended and standard syntax.

Extended syntax

The extended syntax uses the “metastep” concept and has the following format:

NonLinearStatic [nmsteps #(in)] nsteps #(in) [contextOutputStep #(in)] [sparselinsolverparams #(string)] [nonlinform #(in)] <[nonlocstiff #(in)]> <[nonlocalext]> <[loadbalancing]>

This record is immediately followed by metastep records with the format described below. The analysis parameters have following meaning

  • nmsteps - determines the number of “metasteps”, default is 1.
  • nsteps - determines number of solution steps.
  • contextOutputStep - causes the context file to be created for every contextOutputStep-th step and when needed. Useful for postprocessing.
  • The sparselinsolverparams parameter describes the sparse linear solver attributes and is explained in section Sparse linear solver parameters.
  • nonlinform - formulation of non-linear problem. If == 1 (default), total Lagrangian formulation in undeformed original shape is used (first-order theory). If == 2, the equlibrated displacements are added to original ones and updated in each time step (second-order theory).
The metastep record has the following general syntax:
nsteps #(in) [controlmode #(in)] [deltat #(rn)] [stiffmode #(in)] [refloadmode #(in)] solverParams #() [sparselinsolverparams #(string)] [donotfixload #()]

where

  • controlmode - determines the type of solution control used for corresponding meta step. if == 0 then indirect control will be used to control solution process (arc-length method, default). if == 1 then direct displacement or load control will be used (Newton-Raphson solver). In the later mode, one can apply the prescribed load increments as well as control displacements.
  • deltaT - is time step length. If not specified, it is set equal to 1,0. Each solution step has associated the corresponding intrinsic time, at which the loading is generated. The deltaT determines the spacing between solution steps on time scale.
  • stiffMode - If == 0 (default) then tangent stiffness will be used at new step beginning and whenever numerical method will ask for stiffness update. If == 1 the use of secant tangent will be forced. The secant stiffness will be used at new step beginning and whenever numerical method will ask for stiffness update. If == 2 then original elastic stiffness will be used during the whole solution process.
  • The refloadmode parameter determines how the reference force load vector is obtained from given totalLoadVector and initialLoadVector. The initialLoadVector describes the part of loading which does not scale. Works only for force loading, other non-force components (temperature, prescribed displacements should always given in total values). If refloadmode is 0 (rlm_total, default) then the reference incremental load vector is defined as totalLoadVector assembled at given time. If refloadmode is 1 (rlm_inceremental) then the reference load vector is obtained as incremental load vector at given time.
  • solverParams - parameters of solver. The solver type is determined using controlmode.
  • The sparselinsolverparams parameter describes the sparse linear solver attributes and is explained in section Sparse linear solver parameters.
  • By default, reached load at the end of metastep will be maintained in subsequent steps as fixed, non scaling load and load level will be reset to zero. This can be changed using keyword donotfixload, which if present, causes the loading to continue, not resetting the load level. For the indirect control the reached loading will not be fixed, however, the new reference loading vector will be assembled for the new metastep.
The direct control corresponds to controlmode=1 and the Newton-Raphson solver is used. Under the direct control, the total load vector assembled for specific solution step represents the load level, where equilibrium is searched. The implementation supports also displacement control - it is possible to prescribe one or more displacements by applying “quasi prescribed” boundary condition(s). The load level then represents the time, where the equilibrium has been found. The Newton-Raphson solver parameters (solverParams) for load-control are:
maxiter #(in) [minsteplength #(in)] [minIter #(in)] [manrmsteps #(in)] [ddm #(ia)] [ddv #(ra)] [ddltf #(in)] [linesearch #(in)] [lsearchamp #(rn)] [lsearchmaxeta #(rn)] [lsearchtol #(rn)] [nccdg #(in) ccdg1 #(ia) ccdgN #(ia) ] rtolv #(rn) [rtolf #(rn)] [rtold #(tn)] [initialGuess #(rn)] where
  • maxiter determines the maximum number of iterations allowed to reach equilibrium. If equilibrium is not reached, the step length (corresponding to time) is reduced.
  • minsteplength parameter is the minimum step length allowed.
  • minIter - minimum number of iterations which always proceed during the iterative solution.
  • If manrmsteps parameter is nonzero, then the modified N-R scheme is used, with the stiffness updated after manrmsteps steps.
  • ddm is array specifying the degrees of freedom, which displacements are controlled. Let the number of these DOFs is N. The format of ddm array is 2*N dofman1 idof1 dofman2 idof2 … dofmanN idofN, where the dofmani is the number of i-th dof manager and idofi is the corresponding DOF number.
  • ddv is array of relative weights of controlled displacements, the size should be equal to N. The actual value of prescribed dofs is defined as a product of its weight and the value of load time function specified using ddltf parameter (see below).
  • ddltf number of load time function, which is used to evaluate the actual displacements of controlled dofs.
  • linesearch nonzero value turns on line search algorithm. The lsearchtol defines tolerance (default value is 0.8), amplification factor can be specified using lsearchamp parameter (should be in interval \((1,10)\)), and parameter lsearchmaxeta defines maximum limit on the length of iterative step (allowed range is \((1.5,15)\)).
  • nccdg allows to define one or more DOF groups, that are used for evaluation of convergence criteria. Each DOF is checked if it is a member of particular group and in this case its contribution is taken into account when evaluating the convergence criteria for that group. By default, if nccdg is not specified, one group containing all DOF types is created. The value of nccdg parameter defines the number of DOF type groups. For each group, the corresponding DOF types need to be specified using ccdg# parameter, where ’#’ should be replaced by group number (numbering starts from 1). This array contains the DofIDItem values, that identify the physical meaning of DOFs in the group. The values and their physical meaning is defined by DofIDItem enum type (see src/oofemlib/dofiditem.h for reference).
  • rtolv determines relative convergence norm (both for displacement iterative change vector and for residual unbalanced force vector). Optionally, the rtolf and rtold parameters can be used to define independent relative convergence crteria for unbalanced forces and displacement iterative change. If the default convergence criteria is used, the parameters rtolv,rtolf, and rtold are real values. If the convergence criteria DOF groups are used (see bellow the description of nccdg parameter) then they should be specified as real valued arrays of nccdg size, and individual values define relative convergence criteria for each individual dof group.
  • initialGuess is an optional parameter with default vaue 0, for which the first iteration of each step starts from the previously converged state and applies the prescribed displacement increments. This can lead to very high strains in elements connected to the nodes with changing prescribed displacements and the state can be far from equilibrium, which may results into slow convergence and strain localization near the boundary. If initialGuess is set to 1, the contribution of the prescribed displacement increments to the internal nodal forces is linearized and moved to the right-hand side, which often results into an initial solution closer to equilibrium. For instance, if the step is actually elastic, equilibrium is fully restored after the second iteration, while the default method may require more iterations.
The indirect solver corresponds to controlmode=0 and the CALM solver is used. The value of reference load vector is determined by refloadmode parameter mentioned above at the first step of each metastep. However, the user must ensure that the same value of reference load vector could be obtained for all solution steps of particular metastep (this is necessary for restart and adaptivity to work). The corresponding meta step solver parameters (solverParams) are:
Psi #(rn) MaxIter #(in) stepLength #(rn) [minStepLength #(in)] [initialStepLength #(rn)] [forcedInitialStepLength #(rn)] [reqIterations #(in)] [maxrestarts #(in)] [minIter #(in)] [manrmsteps #(in)] [hpcmode #(in)] [hpc #(ia)] [hpcw #(ra)] [linesearch #(in)] [lsearchamp #(rn)] [lsearchmaxeta #(rn)] [lsearchtol #(rn)] [nccdg #(in) ccdg1 #(ia) … ccdgN #(ia)] rtolv #(rn) [rtolf #(rn)] [rtold #(rn)] [pert #(ia)] [pertw #(ra)] [rpa #(rn)] [rseed #(in)] where
  • Psi - CALM \(\Psi\) control parameter. For \(\Psi\) = 0 displacement control is applied. For nonzero values the load control applies together with displacement control (ALM). For large \(\Psi\) load control apply.
  • MaxIter - determines the maximum number of iteration allowed to reach equilibrium state. If this limit is reached, restart follows with smaller step length.
  • stepLength - determines the maximum value of arc-length (step length).
  • minStepLength - minimum step length. The step length will never be smaller. If convergence problems are encountered and step length cannot be decreased, computation terminates.
  • initialsteplength - determines the initial step length (the arc-length). If not provided, the maximum step length (determined by stepLength parameter) will be used as the value of initial step length.
  • forcedInitialStepLength - When simulation is restarted, the last predicted step length is used. Use forcedInitialStepLength parameter to override the value of step length. This parameter will also override the value of initial step length set by initialsteplength parameter.
  • reqIterations - approximate number of iterations controlled by changing the step length.
  • maxrestarts - maximum number of restarting computation when convergence not reached up to MaxIter.
  • minIter - minimum number of iterations which always proceed during the iterative solution. reqIterations are set to be the same, MaxIter are increased if lower.
  • manrmsteps - Forces the use of accelerated Newton Raphson method, where stiffness is updated after manrmsteps steps. By default, the modified NR method is used (no stiffness update).
  • hpcmode Parameter determining the alm mode. Possible values are: 0 - (default) full ALM with quadratic constrain and all dofs, 1 - (default, if hpc parameter used) full ALM with quadratic constrain, taking into account only selected dofs (see hpc param), 2 - linearized constrain in displacements only, taking into account only selected dofs with given weight (see hpc and hpcw parameters).
  • hpc - Special parameter for Hyper-plane control, when only selected DOFs are taken account in ALM step length condition. Important mainly for material nonlinear problems with strong localization. This array selects the degrees of freedom, which displacements are controlled. Let the number of these DOFs be N. The format of ddm array is 2*N dofman1 idof1 dofman2 idof2 … dofmanN idofN, where the dofmani is the number of i-th dof manager and idofi is the corresponding DOF number.
  • hpcw Array of DOF weights in linear constraint. The dof ordering is determined by hpc parameter, the size of the array should be N.
  • linesearch nonzero value turns on line search algorithm. The lsearchtol defines tolerance, amplification factor can be specified using lsearchamp parameter (should be in interval \((1,10)\)), and parameter lsearchmaxeta defines maximum limit on the length of iterative step (allowed range is \((1.5,15)\)).
  • nccdg allows to define one or more DOF groups, that are used for evaluation of convergence criteria. Each DOF is checked if it is a member of particular group and in this case its contribution is taken into account when evaluating the convergence criteria for that group. By default, if nccdg is not specified, one group containing all DOF types is created. The value of nccdg parameter defines the number of DOF type groups. For each group, the corresponding DOF types need to be specified using ccdg# parameter, where ’#’ should be replaced by group number (numbering starts from 1). This array contains the DofIDItem values, that identify the physical meaning of DOFs in the group. The values and their physical meaning is defined by DofIDItem enum type (see src/oofemlib/dofiditem.h for reference).
  • rtolv determines relative convergence norm (both for displacement iterative change vector and for residual unbalanced force vector). Optionally, the rtolf and rtold parameters can be used to define independent relative convergence crteria for unbalanced forces and displacement iterative change. If the default convergence criteria is used, the parameters rtolv,rtolf, and rtold are real values. If the convergence criteria DOF groups are used (see bellow the description of nccdg parameter) then they should be specified as real valued arrays of nccdg size, and individual values define relative convergence criteria for each individual dof group.
  • pert Array specifying DOFs that should be perturbed after the first iteration of each step. Let the number of these DOFs be M. The format of ddm array is 2*M dofman1 idof1 dofman2 idof2 … dofmanN idofN, where the dofmani is the number of i-th dof manager and idofi is the corresponding DOF number.
  • pertw Array of DOF perturbations. The dof ordering is determined by pert parameter, the size of the array should be M.
  • rpa Amplitude of random perturbation that is applied to each DOF.
  • rseed Seed for the random generator that generates random perturbations.

Standard syntax

In this case, all parameters (for analysis as well as for the solver) are supplied in analysis record. The default meta step is created for all solution steps required. Then the meta step attributes are specified within analysis record. The format of analysis record is then following
NonLinearStatic nsteps #(in) [nonlocstiff #(in)] [contextOutputStep #(in)] [controlmode #(in)] [deltat #(rn)``] rtolv #(rn) [stiffmode #(in)] lstype #(in) smtype #(in) solverParams #() [nonlinform #(in)] <[nonlocstiff #(in)]> <[nonlocalext]> <[loadbalancing]

The meaning of parameters is the same as for extended syntax.

Parameter lstype allows to select the solver for the linear system of equations. Parameter smtype allows to select the sparse matrix storage scheme. The scheme should be compatible with the solver type. See section Sparse linear solver parameters for further details.

Adaptive linear static

Adaptlinearstatic nsteps #(in) [sparselinsolverparams #(...)] [meshpackage #(in)] errorestimatorparams #(...)

Adaptive linear static analysis. Multiple loading cases are not supported. Due to linearity of a problem, the complete reanalysis from the beginning is done after adaptive remeshing. After first step the error is estimated, information about required density is generated (using mesher interface) and solution terminates. If the error criteria is not satisfied, then the new mesh and corresponding input file is generated and new analysis should be performed until the error is acceptable. Currently, the available error estimator for linear problems is Zienkiewicz-Zhu. Please note, that adaptive framework requires specific functionality provided by elements and material models. For details, see element and material model manuals.

  • Parameter nsteps indicates the number of loading cases. Should be set to 1.
  • The sparselinsolverparams parameter describes the sparse linear solver attributes and is explained in section Sparse linear solver parameters.
  • The meshpackage parameter selects the mesh package interface, which is used to generate information about required mesh density for new remeshing. The supported interfaces are explained in section Mesh generator interfaces. By default, the T3d interface is used.
  • The errorerestimatorparams parameter contains the parameters of Zienkiewicz Zhu Error Estimator. These are described in section Error estimators and indicators.

Adaptive nonlinear static

Adaptnlinearstatic Nonlinearstaticparams #() [equilmc #(in)] [meshpackage #(in)] [eetype #(in)] errorestimatorparams #(...)

Represents Adaptive Non-LinearStatic problem. Solution is performed as a series of increments (loading or displacement). The error is estimated at the end of each load increment (after equilibrium is reached), and based on reached error, the computation continues, or the new mesh densities are generated and solution stops. Then the new discretization should be generated. The truly adaptive approach is supported, so the computation can be restarted from the last step (see section Running the code), solution is mapped to new mesh (separate solution step) and new load increment is applied. Of course, one can start the analysis from the very beginning using new mesh. Currently, the available estimators/indicators include only linear Zienkiewicz-Zhu estimator and scalar error indicator. Please note, that adaptive framework requires specific functionality provided by elements and material models. For details, see element and material model manuals.

  • Set of parameters Nonlinearstaticparams are related to nonlinear analysis. They are described in section NonLinearStatic.
  • Parameter equilmc determines, whether after mapping of primary and internal variables to new mesh the equilibrium is restored or not before new load increment is applied. The possible values are: 0 (default), when no equilibrium is restored, and 1 forcing the equilibrium to be restored before applying new step.
  • The meshpackage parameter selects the mesh package interface, which is used to generate information about required mesh density for new remeshing. The supported interfaces are explained in section Mesh generator interfaces. By default, the T3d interface is used.
  • Parameter eetype determines the type of error estimator/indicator to be used. The parameters errorestimatorparams represent set of parameters corresponding to selected error estimator. For description, follow to section Error estimators and indicators.

Free warping analysis

FreeWarping nsteps #(in)

Free warping analysis computes the deplanation function of cross section with arbitrary shape. It is done by solving the Laplace’s equation with automatically generated boundary conditions corresponding to the free warping problem.

This type of analysis supports only TrWarp elements and WarpingCS cross sections. One external node must be defined for each warping cross section. The coordinates of this node can be arbitrary but this node must be defined with parametr DofIDMask 1 24 and one boundary condition which represents relative twist acting on corresponding warping cross section. No additional loads make sence in free warping analysis.

Parameter nsteps indicates the number of loading cases. Series of loading cases is maintained as sequence of time-steps. For each load case an auxiliary time-step is generated with time equal to load case number. Load vectors for each load case are formed as load vectors at this auxiliary time.

Transport Problems

Stationary transport problem

StationaryProblem nsteps #(in) [sparselinsolverparams #(...)] [exportfields #(ia)]

Stationary transport problem. Series of loading cases is maintained as sequence of time-steps. For each load case an auxiliary time-step is generated with time equal to load case number. Load vectors for each load case are formed as load vectors at this auxiliary time. The sparselinsolverparams parameter describes the sparse linear solver attributes and is explained in section Sparse linear solver parameters.

If the present problem is used within the context of staggered-like analysis, the temperature field obtained by the solution can be exported and made available to any subsequent analyses. For example, temperature field obtained by present analysis can be taken into account in subsequent mechanical analysis. To allow this, the temperature must be “exported”. This can be done by adding array exportfields. This array contains the field identifiers, which tell the problem to register its primary unknowns under given identifiers. See file field.h. Then the subsequent analyses can get access to exported fields and take them into account, if they support such feature.

Transient transport problem

TransientTransport nsteps #(in) deltaT #(rn) or dTfunction #(in) or prescribedtimes #(ra) alpha #(rn) [initT #(rn)] [lumped] [keeptangent] [exportfields #(ia)]

Nonlinear implicit integration scheme for transient transport problems. The generalized midpoint rule (sometimes called \(\alpha\)-method) is used for time discretization, with alpha parameter, which has limits \(0\le\alpha\le1\). For \(\alpha=0\) explicit Euler forward method is obtained, for \(\alpha=0.5\) implicit trapezoidal rule is recovered, which is unconditionally stable, second-order accurate in \(\Delta t\), and \(\alpha=1.0\) yields implicit Euler backward method, which is unconditionally stable, and first-order accurate in \(\Delta t\). deltaT is time step length used for integration, nsteps parameter specifies number of time steps to be solved. It is possible to define dTfunction with a number referring to corresponding time function, see section Time functions records. Variable time step is advantageous when calculating large time intervals.

The initT sets the initial time for integration, 0. by default. If lumped is set, then the stabilization of numerical algorithm using lumped capacity matrix will be used, reducing the initial oscillations. See section Stationary transport problem for an explanation on exportfields.

This transport problem supports sets and changes in number of equations. It is possible to impose/remove Dirichlet boundary conditions during solution.

Transient transport problem - linear case - obsolete

NonStationaryProblem nsteps #(in) deltaT #(rn) | deltaTfunction #(in) alpha #(rn) [initT #(rn)] [lumpedcapa] [sparselinsolverparams #(..)] [exportfields #(ia)] [changingProblemSize]

Linear implicit integration scheme for transient transport problems. The generalized midpoint rule (sometimes called \(\alpha\)-method) is used for time discretization, with alpha parameter, which has limits \(0\le\alpha\le1\). For \(\alpha=0\) explicit Euler forward method is obtained, for \(\alpha=0.5\) implicit trapezoidal rule is recovered, which is unconditionally stable, second-order accurate in \(\Delta t\), and \(\alpha=1.0\) yields implicit Euler backward method, which is unconditionally stable, and first-order accurate in \(\Delta t\). deltaT is time step length used for integration, nsteps parameter specifies number of time steps to be solved. It is possible to define deltaTfunction with a number referring to corresponding time function, see section Time functions records. Variable time step is advantageous when calculating large time intervals. It is strongly suggested to use nonlinear transport solver due to stability reasons, see section Transient transport problem.

The initT sets the initial time for integration, 0 by default. If lumpedcapa is set, then the stabilization of numerical algorithm using lumped capacity matrix will be used, reducing the initial oscillations. See section Stationary transport problem for an explanation on exportfields.

This linear transport problem supports changes in number of equations. It is possible to impose/remove Dirichlet boundary conditions during solution. This feature is enabled with changingProblemSize, which ensures storing solution values on nodes (DoFs) directly. If the problem does not grow/decrease during solution, it is more efficient to use conventional solution strategy and the parameter should not be mentioned.

Note: This problem type requires transport module and it can be used only when this module is included in your oofem configuration.

Transient transport problem - nonlinear case - obsolete

NlTransientTransportProblem nsteps #(in) deltaT #(rn) | deltaTfunction #(in) alpha #(rn) [initT #(rn)] [lumpedcapa #()] [nsmax #(in)] rtol #(rn) [manrmsteps #(in)] [sparselinsolverparams #(...)] [exportfields #(ia)] [changingProblemSize]

Implicit integration scheme for transient transport problems. The generalized midpoint rule (sometimes called \(\alpha\)-method) is used for time discretization, with alpha parameter, which has limits \(0\le\alpha\le1\). For \(\alpha=0\) explicit Euler forward method is obtained, for \(\alpha=0.5\) implicit trapezoidal rule is recovered, which is unconditionally stable, second-order accurate in \(\Delta t\), and \(\alpha=1.0\) yields implicit Euler backward method, which is unconditionally stable, and first-order accurate in \(\Delta t\). See matlibmanual.pdf for solution algorithm.

deltaT is time step length used for integration, nsteps parameter specifies number of time steps to be solved. For deltaTfunction and initT see section Transient transport problem - linear case - obsolete. Parameter maxiter determines the maximum number of iterations allowed to reach equilibrium (default is 30). Norms of residual physical quantity (heat, mass) described by solution vector and the change of solution vector are determined in each iteration. The convergence is reached, when the norms are less than the value given by rtol. If manrmsteps parameter is nonzero, then the modified N-R scheme is used, with the left-hand side matrix updated after manrmsteps steps. nsmax maximum number of iterations per time step, default is 30. If lumpedcapa is set, then the stabilization of numerical algorithm using lumped capacity matrix will be used, reducing the initial oscillations.

See the Section Stationary transport problem for an explanation on exportfields. The meaning of changingProblemSize is given in Section Transient transport problem - linear case - obsolete.

Note: This problem type requires transport module and it can be used only when this module is included in your oofem configuration.

Fluid Dynamic Problems

Transient incompressible flow - CBS Algorithm

CBS nsteps #(in) deltaT #() [theta1 #(in)] [theta2 #(in)] [cmflag #(in)] [scaleflag #(in) lscale #(in) uscale #(in) dscale #(in)] [lstype #(in)] [smtype #(in)]

Solves the transient incompressible flow using algorithm based on Characteristics Based Split (CBS, for reference see O.C.Zienkiewics and R.L.Taylor: The Finite Element Method, 3rd volume, Butterworth-Heinemann, 2000). At present, only semi-implicit form of the algorithm is available and energy equation, yielding the temperature field, is not solved. Parameter nsteps determines number of solution steps. Parameter deltaT is time step length used for integration. This time step will be automatically adjusted to satisfy integration stability limits \(\Delta t \le {\frac{h}{\vert\boldsymbol{u}\vert}}\) and \(\Delta t \le {\frac{h^2}{2\nu}}\), if necessary. Parameters theta1 and theta2 are integration constants, \(\theta_1, \theta_2 \in \langle{\frac12}, 1\rangle\). If cmflag is given a nonzero value, then consistent mass matrix will be used instead of (default) lumped one.

The characteristic equations can be solved in non-dimensional form. To enable this, the scaleflag should have a nonzero value, and the following parameters should be provided: lscale, uscale, and dscale representing typical length, velocity, and density scales.

Parameter lstype allows to select the solver for the linear system of equations. Parameter smtype allows to select the sparse matrix storage scheme. The scheme should be compatible with the solver type. See section Sparse linear solver parameters for further details.

Transient incompressible flow SUPG/PSPG Algorithm

SUPG nsteps #(in) deltaT #(rn) rtolv #(rn) [atolv #(rn)] [stopmaxiter #(in)] [alpha #(rn)] [cmflag #(in)] [deltatltf #(in)] [miflag #(in)] [scaleflag #(in) lscale #(in) uscale #(in) dscale #(in)] [lstype #(in)] [smtype #(in)]

Solves the transient incompressible flow using stabilized formulation based on SUPG and PSPG stabilization terms. The stabilization provides stability and accuracy in the solution of advection-dominated problems and permits usage of equal-order interpolation functions for velocity and pressure. Furthermore, stabilized formulation significantly improves convergence rate in iterative solution of large nonlinear systems of equations.

By changing the value \(\alpha\), different methods from “Generalized mid-point family” can be chosen, i.e., Forward Euler (\(\alpha=0\)), Midpoint rule (\(\alpha=0.5\)), Galerkin (\(\alpha=2/3\)), and Backward Euler (\(\alpha=1\)). Except the first one, all the methods are implicit and require matrix inversion for solution. Some results form an energy method analysis suggest unconditional stability for \(\alpha\ge 0.5\) for the generalized mid-point family. As far as accuracy is concerned, the midpoint rule is to be generally preferred.

Parameter nsteps determines number of solution steps. Parameter deltaT is time step length used for integration. Alternatively, the load time function can be used to determine time step length for particular solution step. The load time function number is determined by parameter deltatltf and its value evaluated for solution step number should yield the step length.

Parameters rtolv and atolv allow to specify relative and absolute errors norms for residual vector. The equilibrium iteration process will stopped when both error limits are satisfied or when the number of iteration exceeds the value given by parameter stopmaxiter.

If cmflag is given a nonzero value, then consistent mass matrix will be used instead of (default) lumped one.

The algorithm allows to solve the flow of two immiscible fluids in fixed spatial domain (currently only in 2d). This can be also used for solving free surface problems, where one of the fluids should represent air. To enable multi-fluid analysis, user should set parameter miflag. The supported values are described in section Material interfaces. Please note, that the initial distribution of reference fluid volume should be provided as well as constitutive models for both fluids.

The characteristic equations can be solved in non-dimensional form. To enable this, the scaleflag should have a nonzero value, and the following parameters should be provided: lscale, uscale, and dscale representing typical length, velocity, and density scales.

Parameter lstype allows to select the solver for the linear system of equations. Parameter smtype allows to select the sparse matrix storage scheme. Please note that the present algorithm leads to a non-symmetric matrix. The scheme should be compatible with the solver type. See section Sparse linear solver parameters for further details.

Transient incompressible flow (PFEM Algorithm)

PFEM nsteps #(in) deltaT #(rn) material #(in) cs #(in) pressure #(in) [mindeltat #(rn)] [maxiter #(in)] [rtolv #(rn)] [rtolp #(rn)] [alphashapecoef #(rn)] [removalratio #(rn)] [scheme #(in)] [lstype #(in)] [smtype #(in)]

Solves the transient incompressible flow using particle finite element method based on the Lagrangian formulation of Navier-Stokes equations.

Mesh nodes are represented by PFEMParticles (see pfemparticles), which can freely move and even separate from the main domain. To integrate governing equations in each solution step, a temporary mesh, built from particles, is needed. The mesh is rebuilt from scratch in each solution step to prevent large distortion of elements. Paramters cs and material assign types from cross section and material record to created elements. Thus, the problem is defined without any elements in the input file.

Mesh is generated using Delaunay triangulation and Alpha shape technique for the identification of the free surface. The parameter alphashapecoef should reflect initial distribution of PFEMParticles. Value approximately equal to 1,5-multiple of shortest distance of two neighboring particles has been found well. On the free surface the zero-pressure boundary condition is enforced. This must be defined in boundary condition record under the number defined by pressure.

Parameter scheme controls whether the equation system for the components of the auxiliary velocity is solved explicitly (0) or implicitly (1). The last is the default option.

Parameter nsteps determines number of solution steps. Parameter deltaT is time step length used for integration. To ensure numerical stability, step length is adapted upon mesh geometry and velocity of paricular nodes. To avoid to short time length a minimal size can be defined by mindeltat. Alternatively prescribing limit removalratio of the element edge length too close particles can be removed from solution.

Optional parameters rtolv and rtolp allow to specify relative norms for velocity and pressure difference of two subsequent iteration step. Default values are 1.e-8. By default maximal 50 iterations are performed, if not specified by maxiter.

Parameter lstype allows to select the solver for the linear system of equations. Parameter smtype allows to select the sparse matrix storage scheme. Please note that the present algorithm leads to a non-symmetric matrix. The scheme should be compatible with the solver type. See section Sparse linear solver parameters for further details.

Coupled Problems

Staggered Problem

StaggeredProblem (nsteps #(in) deltaT #(rn)) \(|\) timeDefinedByProb #(in) prob1 #(s) prob2 #(s) [stepMultiplier #(rn)]

Represent so-called staggered analysis. This can be described as an sequence of sub-problems, where the result of some sub-problem in the sequence can depend on results of previous sub-problems in sequence. Typical example is heat transfer analysis followed by mechanical analysis taking into account the temperature field generated by the heat transfer analysis. Similar analysis can be done when coupling moisture transport with concrete drying strain.

The actual implementation supports only sequence of two sub-problems. The sub-problems are described using sub-problem input files. The syntax of sub-problem input file is the same as for standalone problem. The only addition is that sub-problems should export their solution fields so that they became available for subsequent sub-problems. See the Section Stationary transport problem.

The subproblem input files are described using prob1 and prob2 parameters, which are strings containing a path to sub-problem input files, the prob1 contains input file path of the first sub-problem, which runs first for each solution step, the prob2 contains input file path of the second sub-problem.

There are two options how to control a time step sequence. The first approach uses timeDefinedByProb which uses time sequence from the corresponding subproblem. The subproblem may specify arbitrary loading steps and allows high flexibility. The second approach uses the staggered problem to take control over time. Therefore any sub-problem time-stepping parameters are ignored (even if they are required by sub-problem input syntax) and only staggered-problem parameters are relevant. deltaT is than a time step length used for integration, nsteps parameter specifies number of time steps to be solved. stepMultiplier multiplies all times with a given constant. Default is 1.

Note: This problem type is included in transport module and it can be used only when this module is configured. Note: All material models derived from StructuralMaterial base will take into account the external registered temperature field, if provided.

FluidStructure Problem

FluidStructureProblem nsteps #(in) deltaT #(rn) prob1 #(s) prob2 #(s) [maxiter #(in)] [rtolv #(rn)] [rtolp #(rn)]

Represents a fluid-structure analysis based on StaggeredProblem but providing iterative synchronization of sub-problems. The implementation uses the the PFEM model Transient incompressible flow (PFEM Algorithm) for the fluid part. For the structural part a full dynamic analysis using implicit direct integration DIIDynamic DIIDynamic is considered.

The coupling of both phases is based on the idea of enforcing compatibility on the interface. Special fluid particle are attached to every structural node on the interface that can be hit by the fluid. These special particles have no degrees of freedom associated, so no equations are solved on them. However, their movement is fully determined by associated structural nodes. Their velocities governed by the solid part affect the fluid equation naturally.

This iterative procedure is based on the so-called Dirichlet-Neumann approach. Dirichlet boundary conditions are the prescribed velocities on the fluid side of the interface, whereas applied forces on the structural side represent the Neumann boundary conditions.

The convergence criterion is based on the difference of the pressure and velocity values on the interface from the subsequent iterative steps. Once they are smaller than prescribed tolerance, the iteration is terminated and solution can proceed to the next step.

The subproblem input files are described using prob1 and prob2 parameters, which are strings containing a path to sub-problem input files, the prob1 contains input file path of the first sub-problem, which runs first for each solution step, the prob2 contains input file path of the second sub-problem. The time step sequence is controlled by the number of steps nsteps and the time step length deltaT.

Optional parameters rtolv and rtolp allow to specify relative norms for velocity and pressure differnce of two subsequent iteration step. Default values are 1.e-3. By default maximal 50 iterations are performed, if not specified by maxiter.

Note: This problem type is included in PFEM module and it can be used only when this module is configured.

DummyEngngModel

Dummy nnmodules #(in)

Represents a dummy model, whch is not capable to perform any analysis. Its intended use is to invoke the configured export modules, so that the problem geometry can be exported without requiring to actually solve the problem.