Notes, Warnings and Errors: Solver Errors

Description

The solvers generate error messages in the form of:

*ERROR [XXX]: "Message"

Error messages are listed in the solver window and in the solver log file (see Results Interpretation: Solver Log File).

All error messages will immediately terminate the solvers, therefore, only one error message will ever appear in the solver window. When an error is generated, the solver attempts to identify the cause, gives a descriptive message and stops.

A class of error message that should never occur is given in the form of:

!INTERNAL: "Message"

If one of these is encountered, it should be reported to Strand7 Pty Limited by email:info@strand7.com, together with a copy of the model file that generated the error, if possible. This will help identify and rectify the issue.

List

[1]: Beam XXXX is collapsed.

The specified beam is considered to be collapsed when its length is less than the Minimum Dimension defined in the SOLVERS Parameters: ELEMENTS. This can occur either due to modelling errors or due to large element distortions in geometry nonlinear analysis. Note that zero-length Connection type beam elements may be used, since their stiffness is independent of their length.

[2]: Plate XXXX is collapsed or seriously distorted.

The specified plate is excessively distorted, either due to modelling errors or due to large element distortions in geometry nonlinear analysis. For quadratic elements, it may also mean that a mid-side node is too close to a corner node. Generally, mid-side nodes should be kept no closer than one third of the distance between the corner nodes.

[3]: Brick XXXX is collapsed or seriously distorted.

The specified brick is excessively distorted, either due to modelling errors or due to large element distortions in geometry nonlinear analysis. For quadratic elements, it may also mean that a mid-side node is too close to a corner node. Generally, mid-side nodes should be kept no closer than one third of the distance between the corner nodes.

[4]: Global stiffness matrix is singular.

This error occurs whenever singularities are found in the global stiffness matrix during the matrix decomposition phase. The log file should be investigated to determine which node and degree of freedom has generated the singularity. Some of the more common causes of a singular matrix include:

[5]: Link XXXX is collapsed or zero length.

This error occurs when a link that must have a finite length (e.g., a Pinned link) has been defined with zero length. Note that in staged analysis, a zero length link can be produced due to morphing. Some links are automatically replaced with equivalent links when their length becomes too small (e.g., Rigid Links are replaced with Master-Slave links). If the error occurs, the link should be replaced with a more appropriate one.

[6]: Not used.

[7]: Not used.

[8]: Zero/negative radius at plate XXXX.

For axisymmetric analysis, all nodes must have zero or positive X coordinates since these are used directly as the radius, which cannot be negative. This error indicates either that the model contains invalid data or (in nonlinear geometry analysis) excessive distortions have occurred such that nodes have crossed the Y (i.e., axisymmetric) axis.

[9]: Viscoelastic chain parameters could not be determined. ([Beam][Plate][Brick] XXXX).

When using the Creep: Concrete Creep and Shrinkage - Hyperbolic Law or the Creep: Concrete Creep and Shrinkage - User-Defined, viscoelastic chain parameters that describe the stress/strain relationship for any time instance, are determined by a curve fitting procedure. The success of this curve fitting procedure depends on the specification of suitable creep data in the creep property definition combined with appropriate curve fitting parameters in the SOLVERS Parameters: CREEP. If the curve fitting operation fails, this error is generated. The creep data and the curve fitting parameters in the SOLVERS Parameters: CREEP should be reviewed.

[10]: Invalid cable connection (Beam XXXX).

This error is generated whenever a reference system for a cable cannot be determined. This can occur when the two ends of the cable are on top of each other.

[11]: Not used.

[12]: Cam-Clay material failure at [plate][brick] XXXX.

[Normal consolidation line is almost parallel to swelling line][Incompatible/invalid property and/or initial data][Excessive strain (maximum strain component=XXXX)][Zero void ratio reached].

This error is generated when a Cam-Clay material model fails. If material failure can be attributed to a possible cause, additional information is given.

[13]: Solution has diverged.

This error is generated whenever a load step in a nonlinear analysis diverges and Automatic Load Stepping is not enabled (see SOLVERS Parameters: SUB-STEPPING (Static) and SOLVERS Parameters: SUB-STEPPING (Time Based)). Solution failure can be signalled by a number of events including the norm of the residual forces exceeding a specified value, the rotation increment at any node exceeding 180 degrees, plastic deformation divergence, etc. Any of the conditions that would trigger sub-stepping as described in Note[15]: Load increment reduced by XXXX% - <Reason for reduction>., Note[26]: Time step is reduced to XXXX - <Reason for reduction>. and Note[27]: Arc length has been reduced (Factor = XXXX) - <Reason for reduction>. will trigger a solution diverged error when Automatic Sub-stepping is not enabled.

[14]: Not used.

[15]: Zero equations have been generated - this solver requires as least one equation.

At least one node must have an active degree of freedom.

In order for the solver in question to proceed, at least one equation must be generated. If all nodes are constrained, no equations are generated and this error is produced. Although some solvers, such as the Linear Static solver, can solve models where all degrees of freedom are restrained, other solvers, such as the Natural Frequency solver, cannot.

[16]: Table, or extrapolation on table, crosses the horizontal axis ([Beam][Plate][Brick] XXX).

TABLE NAME: "XXXX"

This error can occur when tables used for nonlinear elastic materials contain negative gradients. Although a negative gradient for nonlinear elastic materials is allowed, positive strain must correspond to positive stress, and negative strain must correspond to negative stress. If this condition is not satisfied, either because the table physically crosses the horizontal axis (at some point not through the origin), or because the extrapolation of a negative gradient crosses the horizontal axis, this error is generated.

[17]: Table contains invalid data and cannot be evaluated.

TABLE NAME: "XXXX"

Many table errors are automatically handled in the solvers. When it is not possible to handle a table error automatically, and the table cannot be ignored, this error is generated.

[18]: Total modal mass is zero.

This error is generated by the Spectral Response solver whenever the modal mass is zero for seismic excitation problems. The modal mass is found by multiplying the eigenvector (mode shape) by the mass matrix. A zero modal mass indicates that either the mass matrix (i.e., element mass density) is zero, or the eigenvector is null.

[19]: Not used.

[20]: [All eigenvalues are zero.] [All eigenvalues are zero - try a [non-zero][bigger] frequency shift or request fewer modes.]

This error is generated by the Natural Frequency and Linear Buckling solvers when all of the requested modes are zero. Note that a zero mode usually indicates a rigid body mode in the structure.

[21]: Mass matrix in Subspace is singular (Pivot = XXXX).

This error is generated whenever the mass matrix for a natural frequency analysis becomes singular. A singular mass matrix usually means zero mass in the Subspace matrix, which prevents the extraction of frequency modes. On the other hand, a zero global mass matrix is detected before the Subspace iteration commences.

[22]: Geometric stiffness matrix in Subspace is singular (Pivot = XXXX).

This is analogous to Error [21]: Mass matrix in Subspace is singular (Pivot = XXXX). but applies to the Linear Buckling solver. Just as the mass matrix used for natural frequency analysis can be singular, the geometric stiffness matrix used for buckling analysis can also be singular, preventing the extraction of the buckling factors.

[23]: Global mass matrix is a zero matrix - check material mass density and/or nodal mass.

At the completion of the stiffness and mass matrix assembly, a check is made of the total number of non-zero mass degrees of freedom in the system. If all entries are zero, it means that all the elements have no mass density, so a frequency analysis cannot be performed.

[24]: All entries in geometric stiffness matrix are zero.
Check element stresses in linear static analysis.

This is analogous to Error [23]: Global mass matrix is a zero matrix - check material mass density and/or nodal mass. but applies to the Linear Buckling solver. A geometric stiffness matrix with all zero entries means that the stresses/forces/moments in the elements are zero. For the Linear Buckling solver to proceed, non-zero entries are required in the geometric stiffness matrix.

[25]: Global matrix is too large to be solved.

This error is unlikely to occur for the vast majority of practical problems.

[26]: Solution has diverged - deformation at plate XXXX is too large.

This is applicable to nonlinear analysis, when the deformation of a plate element is too large. Large deformations can cause severely distorted elements resulting in the generation of an invalid stiffness matrix. A reduction in the load step size can often avoid the error.

[27]: Plate Edge Release error at plate XXXX - [invalid edge][condensation error].

This error is generated when plate edge release attributes generate a singularity in the procedure. This could be caused by attempting to release a collapsed edge, or an error in the matrix condensation process because too many edges have been released, or attempting to release a plate with no bending stiffness. In most cases, inspection of the element in question will reveal the cause of the error.

[28]: [Restart procedure has failed - restart file not compatible.][Restart procedure has failed - restart file does not contain the step to be used.][Restart procedure has failed - cannot find restart file.]

This is applicable to nonlinear analysis when the restart option is used (see SOLVERS: Files). Restarting usually requires reading a previously created solution file and associated restart file, both of which need to be consistent with the current model. If the temporary file is not consistent or cannot be found, the solution cannot restart. Therefore, this error can only occur if the initial solution file or restart file become unavailable after the solution restart has been launched (if the files are not available at launch time, the solution restart could not be launched).

[29]: Failure to establish starting vectors - refine mesh/replace links with rigid beam elements.

This error may appear in natural frequency or linear buckling analysis if appropriate starting vectors cannot be established. The starting vectors are degrees of freedom in the model automatically chosen by the solver as the best starting set for the eigenvalue extraction procedure.

[30]: Failure in file handling: "File name"

This error is related to the operating system. It indicates that a file, which the solver expects to use and which was available at solver launch time, can no longer be accessed.

[31]: Not used.

[32]: Not used.

[33]: Not used.

[34]: Not Used.

[35]: Not used.

[36]: [Plate][Brick] property XXXX (Cam-Clay), contains invalid data.

[Non-positive critical state line slope.][Non-positive normal consolidation line slope.][Non-positive swelling line slope.][Normal consolidation line slope must be greater than swelling line slope.][Invalid reference pressure (pr) for in-situ void ratio calculation.][Invalid reference void ratio (er) for in-situ void ratio calculation.][Invalid void ratio generated - check property data (er,pr) or assign void ratio as element attribute.]

This error is generated if any of the data in a Cam-Clay soil property is considered to be invalid.

[37]: Not used.

[38]: Restart procedure has failed due to element property changes [Number of Layers][Number of Gauss Points][MNL settings] ([Beam][Plate][Brick] XXXX).

In most cases, changes in property type cannot be made between restarts (e.g., a plate/shell element cannot be changed to a soil element). However, some changes are allowed (e.g., a 2D plane stress element can become a plate/shell element between restarts). If an unsupported property change has been made, this error will be generated together with information about the unsupported data changes. Note that the construction sequence option of the Nonlinear Static solver offers greater flexibility for changing types between restarts.

See Also