Notes, Warnings and Errors: Solver Notes

Description

The solvers generate informative notes in the form of:

*NOTE [XXX]: "Message"

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

Notes inform the user about decisions made by the solver, which the user might not have considered or might not have intended. They also remind the user about certain settings they may have selected for the analysis.

The solver continues to run after notes are generated.

List

[1]: Not used.

[2]: Iterative displacement is very small - displacement norm is regarded converged.

This note is given when every translational component of the displacement vector in the current iteration contains iterative displacements that are smaller than the Zero displacement parameter defined in SOLVERS Parameters: ITERATION (Structural). In that case it is assumed that the displacements are converged, irrespective of the current Displacement norm value.

[3]: More iterations required due to element bubble functions.

If the model contains elements with bubble functions (i.e., 2D Quad4 or 3D Hexa8) a solver restart may require an additional iteration to determine the bubble function displacements.

[4]: Not used.

[5]: Reference temperature for material temperature dependence is set to XXXX.

[This is the common Reference Temperature for XXXX load cases with nodal temperatures.][This is the lowest Reference Temperature in XXXX load cases with nodal temperatures.]

When multiple load cases containing temperature are considered simultaneously, as could occur in the Nonlinear Static, Quasi-static and Transient Dynamic solvers, a common reference temperature is determined. This does not change the applied thermal strain, only the reference point. Therefore, it can only affect material temperature dependency, which uses temperature, not temperature difference, to adjust temperature dependent material properties. A less ambiguous way to deal with this is to ensure that all the load cases use the same reference temperature and adjust the applied nodal temperature accordingly.

[6]: All diagonal terms in geometric stiffness matrix are zero.

The Linear Buckling solver assembles a geometric stiffness matrix based on the results of a previous static analysis. This geometric stiffness matrix will usually contain non-zero diagonals as long as the elements have some internal force/stress. If all of the diagonals in the geometric stiffness matrix are zero, but some of the off-diagonals are not zero, this note is given. Note that if the entire geometric stiffness matrix is zero, it usually means that the initial condition result case used for stress stiffening effects contains no elements with any internal force/stress. In that case, an error message is generated.

[7]: There are XXXX zero natural frequencies.

Zero natural frequencies usually relate to rigid body modes in an unrestrained structure. Normally there will be up to six zero frequency modes in an unrestrained 3D structure, and up to three in an unrestrained 2D structure (e.g. plane strain). If there are more in each case, it usually means that the model contains multiple unrestrained parts. For a typical restrained structure, there should be no zero frequency modes.

[8]: There are XXXX zero and YYYY very small natural frequencies.

Zero frequencies are as described in Note[7]: There are XXXX zero natural frequencies. These zero frequencies are seldom perfect zeros and are only set to zero if they are smaller than the Zero frequency parameter in SOLVERS Parameters: EIGENVALUE. In some cases, small frequencies that are slightly larger than Zero frequency are produced. In that case, this note alerts as to the possibility that these small frequencies might also be rigid body mode frequencies.

[9]: Not used.

[10]: Drilling degrees of freedom fixed = XXXX.

This note is given if the drilling suppression operation has suppressed some drilling degrees of freedom. See SOLVERS Parameters: ELEMENTS.

[11]: No singularities found.

This note is given if the drilling suppression operation has not suppressed any drilling degrees of freedom, and no other singularities were detected.

[12]: Table is assumed to be symmetric in tension/compression.

TABLE NAME: "XXXX"

If a nonlinear material table is defined only for the positive range (e.g., only for tensile strain), but the table needs to also be used in the negative range (e.g., for both tension and compression in a nonlinear elastic beam element), the table is assumed to act equally in compression and tension (by negating the data points on the compression side). To have the two sides of the table behave differently, both sides need to be defined.

[13]: More iterations required due to status or stiffness change in point contacts.

This note is given when the solution has converged in terms of both displacement and residual force norms, but the status or the stiffness of point contacts is still changing.

[14]: More iterations required due to status or stiffness change in beam supports.

This note is given when the solution has converged in terms of both displacement and residual force norms, but the status or the stiffness of compression-only beam supports is still changing.

[15]: Load increment reduced by XXXX% - <Reason for reduction>.

This note is given when the solver reduces the load increment. A reason for the reduction is also given.

[16]: Negative data in table is ignored for elastic-plastic analysis.

TABLE NAME: "XXXX"

This note is given when a material nonlinear table used for elastic-plastic analysis (e.g., a Stress vs Strain table) contains entries on the negative side of the range (e.g., negative strain) but the element cannot use the negative side. Note that some elasto-plastic situations (e.g. Beam Nonlinear Fibre Stress) can use both sides of the table.

[17]: Negative data in table is ignored for von Mises and Tresca criteria.

TABLE NAME: "XXXX"

This note is given when a Stress vs Strain table used for nonlinear material analysis contains entries in the negative side of the range (i.e., negative strain) but the table is used for von Mises or Tresca criteria. As these criteria are always positive quantities, negative entries in the tables are ignored.

[18]: [Step has not converged][Subspace iteration has not fully converged] - current convergence has been accepted by the user.

This note is given when the current step of a nonlinear analysis, or the current subspace iteration of a natural frequency or linear buckling analysis, has not yet converged but the user has chosen to accept the current results without iterating further (by clicking the icon on the SOLVERS: Solver Window).

[19]: Global acceleration in X direction is taken as acceleration in radial direction.

When a model contains axisymmetric elements, the global acceleration in the X direction will be regarded as the acceleration in the radial direction.

[20]: Not used.

[21]: Not used.

[22]: More iterations required due to status or stiffness change in plate supports.

This note is given when the solution has converged in terms of both displacement and residual force norms, but the status or the stiffness of compression-only plate supports is still changing.

[23]: More iterations required due to status or stiffness change in brick supports.

This note is given when the solution has converged in terms of both displacement and residual force norms, but the status or the stiffness of compression-only brick supports is still changing.

[24]: More iterations required due to status or stiffness change in cutoff bars.

This note is given when the solution has converged in terms of both displacement and residual force norms, but the status or the stiffness of cutoff bars is still changing.

[25]: Table defines linear material (E0 = XXXX).

TABLE NAME: "XXXX"

When a table with only two points is assigned to a material, the material will remain linear and elastic. Its stiffness is defined by the slope of the line connecting the two points.

[26]: Time step is reduced to XXXX - <Reason for reduction>.

If automatic time stepping is enabled, and this is triggered during the solution, the solver gives this note. A reason for the reduction is also given.

[27]: Arc length has been reduced (Factor = XXXX) - <Reason for reduction>.

This note is given when Displacement Control (Arc Length) has been enabled and the arc length needs to be reduced. A reason for the reduction is also given.

[28]: Number of equations changed to XXXX due to changes in restraints and/or links.

During the nonlinear analysis of a structural model containing links, orientation changes in the links can affect the number of dependent/independent equations from load step to load step, which in turn can affect the total number of equations required in the global matrix.

[29]: More iterations required due to material nonlinearity.

This note is given when the solution has converged in terms of both displacement and residual force norms, but material yielding in one or more elements has only just been detected.

[30]: [Both applied and residual forces are very small - force norm is regarded converged.][Residual force is very small - force norm is regarded converged.]

This note is given when the maximum residual force at any node is smaller than the Zero Force parameter entered in the SOLVERS Parameters: ITERATION (Structural), but the Residual Norm Tolerance has not been satisfied. In that case, the Residual Norm Tolerance is ignored. This note is the force counterpart to Note[2]: Iterative displacement is very small - displacement norm is regarded converged.

[31]: Solution terminated because total rotation magnitude exceeds set limit of XXXX deg.

This note is given when the nonlinear static solver terminates due to the maximum nodal rotations exceeding the user-specified limit (see SOLVERS Parameters: SUB-STEPPING (Static)).

[32]: More iterations required due to cable elements.

This note is given when the solution has converged in terms of both displacement and residual force norms, but one or more cable elements has not yet converged.

[33]: Spring elements with end release attributes are treated as springs with effective stiffness.

This note is given when a spring element has an end release assigned. Unlike the beam elements, spring elements with end release are replaced with a new spring of the equivalent released stiffness.

[34]: More iterations required due to displacement scaling.

This note is given when the solution has converged in terms of both displacement and residual force norms, but due to displacement scaling, not all of the externally applied load has been applied to the model.

[35]: More iterations required because no eigenvector has converged.

This note is given when the eigenvalues of a natural frequency or linear buckling analysis have converged while the eigenvectors (mode shapes) have not yet converged solution, and the user has requested that iterations be added to ensure eigenvector convergence (see SOLVERS Parameters: EIGENVALUE).

[36]: Linear elastic modulus calculated as XXXX in table.

This note is given to inform the user as to the gradient through the origin of a stress-strain table used for material nonlinear analysis. This gradient is used as the elastic modulus for the material.

[37]: PCG solution has been accepted by the user.

This note is given when the iterative PCG solver has not yet converged but the user has accepted the unconverged result.

[38]: [Link forces not added to node reaction calculations.][Link flux not added to node flux calculations.]

This note is given to inform the user that the link nodal forces and moments in a structural analysis, or the link nodal flux in a heat transfer analysis, have not been added as nodal reactions. At those nodes, the reactions will be reported as non-zero, being equivalent to the missing reactions from the links, unless other reaction components have also been excluded.

[39]: Damping forces not added to node reaction calculations.

This note is given in a transient dynamic analysis to inform the user that the equivalent nodal forces due to external damping have not been added as nodal reactions. At those nodes, the reactions will be reported as non-zero, being equivalent to the missing reactions from the external damping forces, unless other reaction components have also been excluded.

[40]: Inertia forces not added to node reaction calculations.

This note is given in a transient dynamic analysis to inform the user that the equivalent nodal forces due to mass inertia have not been added as nodal reactions. At those nodes, the reactions will be reported as non-zero, being equivalent to the missing reactions from the node inertia forces, unless other reaction components have also been excluded.

[41]: Inertia relief forces not added to node reaction calculations.

This note is given in a linear static analysis for Inertia Relief freedom cases to inform the user that the equivalent inertia relief nodal forces, i.e., the forces that the solver adds to balance the other applied loads, have not been added as nodal reactions. At those nodes, the reactions will be reported as non-zero, being equivalent to the missing reactions from the inertia relief forces, unless other reaction components have also been excluded.

[42]: Displacement scaling is reduced to XXXX%

If automatic sub-stepping with displacement scaling is enabled, and this is triggered during the solution, the solver gives this note to inform the user as to the current reduction factor.