Notes, Warnings and Errors: Solver Warnings

Description

The solvers generate warning messages in the form of:

*WARNING [XXX]: "Message"

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

Warnings indicate that something could be wrong in the model, that some data may be invalid and therefore needs to be ignored, or that certain details of the model may be irrelevant for the selected solver.

The solver continues to run after warnings are generated, however, it is recommended that all warning messages be inspected closely, understood and addressed by modifying the model where necessary.

List

[1]: Pre-load attributes are ignored by this solver - [TYPE] on [ELEMENT] XXXX is ignored.

The Harmonic Response and Spectral Response solvers do not support pre-load attributes (including thermal load, pre-stress, pre-strain and pre-tension) as harmonic or spectral loads - these are ignored as external loads. However, their effects in terms of stress softening/stiffening on a structure are included by the use of initial conditions in the Natural Frequency solver, which produces the mode shapes used by the Harmonic Response and Spectral Response solvers.

[2]: Table does not contain a point at (0,0) - table is ignored.

TABLE NAME: "XXXX"

For nonlinear materials, the stress-strain, moment-curvature, force-displacement and moment-rotation tables must have a point at (0,0). If the table that does not satisfy this condition, the solver gives this warning and the table is ignored.

[3]: Pre-load attribute on soil element ([Plate][Brick] XXXX) is ignored - not applicable to soil elements.

LOAD CASE: "XXXX"

Pre-stress and pre-strain attributes applied to soil elements are ignored. For soil analysis, the In-situ Stress attributes are used to define the initial conditions of the soil.

[4]: Plate XXXX has a negative support stiffness.

The support stiffness for plate edge and face supports must not be negative. This warning message will not generally occur because the Strand7 pre-processor checks these values before storing them in the model database.

[5]: Plate XXXX has a negative mass density.

Material mass density must be greater than zero. This warning message will not generally occur because the Strand7 pre-processor checks these values before storing them in the model database.

[6]: Node force/moment component at inactive degree of freedom (Node XXXX) is ignored.

LOAD CASE: "XXXX"

This warning indicates that a force or moment has been applied to a nodal degree of freedom that is fixed, inactive or not connected to elements. These force/moment components are ignored by the solver in the calculation of displacements, but are included in the nodal reaction results.

[7]: Mass matrix contains negative diagonals.

The mass matrix does not normally contain negative values on the diagonal unless the elements are very distorted or badly defined. The mesh should be inspected closely.

[8]: Thermal load on plate XXXX is ignored - not applicable to shear panel elements.

Shear panel elements do not support thermal load.

[9]: [Point force][Point moment] on beam XXXX is ignored - not applicable to [spring][cable][truss][cutoff bar][point contact][connection] elements.

Beam point forces and point moments are ignored when applied to certain beam element types.

[10]: [Point force][Point moment][Distributed force][Distributed moment] on beam XXXX is converted to equivalent nodal load.

LOAD CASE: "XXXX"

Concentrated and distributed loads applied to normal beam elements are converted to a consistent nodal load vector with appropriate force and moment components at the two ends (unless the Lumped Load option has been set in SOLVERS Parameters: ELEMENTS). When concentrated or distributed loads are applied to one of the other beam types, such as Truss or Spring, the applied load is approximated as equivalent point loads and/or moments at the nodes.

[11]: Temperature gradient on beam XXXX is ignored - applicable only to beam and straight pipe.

LOAD CASE: "XXXX"

The Beam Temperature Gradient attribute is only applicable to normal beam elements. If the attribute is applied to elements such as truss or spring-damper, it is ignored.

[12]: Modulus vs Temperature/Time Table treated as plastic type for creep material ([Beam][Plate][Brick] XXXX).

When an element uses a time dependent modulus via the assignment of a Factor vs Time table, or a temperature dependent modulus via the assignment of a Factor vs Temperature table, and the element also considers creep behaviour, only the Plastic option of the Temperature/Time table in the Common Properties: Nonlinear is valid. If the value has been set to Elastic, the solver gives this warning and changes the option to Plastic.

[13]: [Face normal pressure][Face shear][Face global pressure] on plate XXXX is ignored - not applicable to [plane stress][plane strain][axisymmetric] elements.

LOAD CASE: "XXXX"

Certain load attributes such as Plate Face Shear, are only applicable to plate/shell elements. If these attributes are applied to 2D elements such as plane stress, plane strain and axisymmetric elements, they are ignored.

[14]: Edge normal shear on plate XXXX is ignored - not applicable to [plane stress][plane strain][axisymmetric] elements.

LOAD CASE: "XXXX"

Certain load attributes such as Plate Normal Edge Shear, are only applicable to plate/shell elements. If these attributes are applied to 2D elements such as plane stress, plane strain and axisymmetric elements, they are ignored.

[15]: Temperature gradient on plate XXXX is ignored - applicable only to shell elements.

LOAD CASE: "XXXX"

The Plate Temperature Gradient attribute is only applicable to plate/shell elements. If the attribute is applied to 2D elements such as plane stress, plane strain and axisymmetric elements, it is ignored.

[16]: 3D membrane (Plate XXXX) might have failed.

If a 3D membrane element is placed in compression, it fails because it no longer has any lateral stiffness.

[17]: Maximum dynamic stiffness factor (YYYY) has been reached at point contact (Beam XXXX).

The scaling factor applied to a point contact element has reached the maximum allowable value. The limit value can be increased via Point contact maximum dynamic stiffness factor (>1). However, excessively large scaling factors usually signify a modelling error or an unattainable point contact element strain tolerance.

[18]: Face [convection][radiation] on plate XXXX is ignored - not applicable to axisymmetric elements.

Axisymmetric elements do not support the plate face heat transfer coefficients.

[19]: Shear panel internal angle (Plate XXXX) is invalid - results might not be reliable.

This warning message indicates that the angle at one or more corners of the quadrilateral is near zero degrees or near 180 degrees. In both cases the results will be unreliable. The mesh geometry should be checked and corrected if this warning is given.

[20]: Plate XXXX is excessively distorted - results might not be reliable.

Plate elements perform best when they are regular quadrilaterals (Quad4, Quad8, Quad9) or equilateral triangles (Tri3, Tri6). It is possible to generate a number of quadrilateral shapes for which the numerical integration procedures will fail: examples include the "bow-tie" element and elements with internal angles greater than 180 degrees. It is also possible that a well-shaped element becomes seriously distorted during the course of a geometry nonlinear analysis. This can occur when the element has buckled or has failed due to plastic or excessive deformation.

If this warning is given, the mesh should be checked and improved for the relevant elements.

[21]: Brick XXXX has a negative Jacobian - this could be due to excessive element distortion.

This warning message indicates that the element is excessively distorted, that it does not have a right hand local coordinate system, or that it is collapsed (i.e., element nodes are too close together or even at the same location). In the case of quadratic brick 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.

[22]: Shear panel (Plate XXXX) is warped.

The shear panel plate element does not support warping. If excessively warped, the results could be unreliable. The mesh geometry should be checked and corrected if this warning is given.

[23]: Material matrix for [plate][brick] property XXXX is singular.

For orthotropic plate and brick elements, the material matrix is generated by the solver. This warning message indicates that there are errors in the input data (e.g., a zero modulus). The material property data should be checked.

[24]: Cannot calculate surface normal at X nodes on plate YYYY - centroid normal will be used.

The surface normal on plate/shell elements is often required at every node. In the case where a unique normal direction cannot be calculated at a node, usually due to distorted elements, the centroid normal will be used instead.

[25]: Large plastic strain increment in [beam][plate][brick] XXXX.

This usually indicates that the amount of plastic strain generated within one load increment is excessive. If the solution fails to converge, the load step should be reduced.

[26]: Negative diagonal in global [stiffness][conductivity] matrix - (Node XXXX, [DX][DY][DZ][RX][RY][RZ]).

Negative diagonal ratio: XXXX

A negative diagonal in the stiffness matrix can indicate that the matrix is ill-conditioned or that a negative stiffness has been generated. For example, if a pre-stress is included, it is possible to generate a stress stiffness matrix, which when added to the normal stiffness matrix, generates a negative overall stiffness (i.e., the structure has buckled). The consequence of this depends on the analysis. This warning does not necessarily indicate a problem.

[27]: [Only XXXX eigenvalues [has][have] converged.][None of the requested eigenvalues has converged.]

This warning is given when not all of the requested eigenvalues in a linear buckling or natural frequency analysis have converged within the allowable limits.

[28]: Mass matrix is not positive definite.

This can occur if elements are significantly distorted such that the integration procedures generate a negative diagonal in the mass matrix used for natural frequency analysis. It may also occur in a well-defined model due to the Subspace eigenvalue extraction algorithm. As it is not usually possible to extract all the eigenvalues in a large structure, due to computing limitations, the Subspace algorithm iterates on a reduced set of degrees of freedom. In some situations, the chosen set of degrees of freedom may generate a singular mass matrix.

For the majority of cases, a singular mass matrix in an iteration of the Subspace procedure may become non-singular in a subsequent iteration and the problem will disappear. In more persistent cases, the number of modes requested should be changed, or the "Working Set" in the SOLVERS Parameters: EIGENVALUE increased.

[29]: Too many modes requested - at most, XXXX mode(s) can be determined.

This warning is given whenever the solver detects that the number of modes requested is greater than the number of independent displacements (degrees of freedom) in the model. This warning is different to Warning [61]: Too many modes are requested - number of modes is changed to XXXX., which instead compares the requested number with the number of active mass degrees of freedom (or active degrees of freedom in the geometric stiffness matrix for buckling analysis).

[30]: Yield criterion is set to von Mises due to assigned creep data. ([Beam][Plate][Brick] XXXX).

The creep laws that are not designated as Concrete Creep and Shrinkage laws are based on the von Mises equivalent stress criterion. If a creep analysis is performed and the element references both a von Mises creep law and a material nonlinear table that does not use the von Mises criterion (e.g., Tresca), the solver gives this warning and changes the material yield criterion to von Mises.

[31]: Beam XXXX is shorter than Default Minimum Dimension of XXXX.

The identified beam element has a length that is less than the minimum element dimension specified in SOLVERS Parameters: ELEMENTS.

[32]: Plate XXXX has a zero or negative Jacobian - this could be due to invalid element properties or excessive distortion.

This warning usually indicates that the element is collapsed (i.e., the nodes are too close together). In the case of quadratic elements, it may also indicate 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.

[33]: Effective concrete age has exceeded curve-fit time ([Beam][Plate][Brick] XXXX).

This could produce unexpected results, particularly for user-defined concrete creep.

When using the Creep: Concrete Creep and Shrinkage - Hyperbolic Law, the stress/temperature/strain relationship at any time instance is determined by a curve fitting technique using the parameters defined in the creep property definition (LAYOUTS: Creep) and the Curve Fit Time parameter specified in the SOLVERS Parameters: CREEP. The curve fitting technique involves the determination of a spring-damper system that represents the viscoelastic behaviour of the creep law (e.g., via Concrete Creep: Generalised Kelvin Chain or Concrete Creep: Generalised Maxwell Chain). This operation may generate different spring-damper systems depending on the time interval over which the curve fitting is performed. By allowing the Curve Fit Time parameter to be user definable, more accurate representations can be determined over the particular time interval of interest.

During the nonlinear material iterations to solve the creep equations, the effective time for any element is not necessarily the same as the real time used for the time stepping of the solution. Whenever the effective time exceeds the specified Curve Fit Time the solver gives this warning. If more accuracy is required over longer periods of time, the Curve Fit Time parameter can be increased, however, this may reduce accuracy during the early stages of creep. The curve Spacing Bias option may be used to bias more accuracy either towards the initial stages or final stages of creep, depending on the problem.

[34]: There [is][are] XXXX zero or negative eigenvalues - [this][these] could be due to buckling.

The Natural Frequency solver gives this warning whenever a negative or zero eigenvalue is encountered. A zero eigenvalue usually indicates a rigid body vibration mode, such as would be found for the frequency analysis of a structure with no restraints. A negative eigenvalue is usually the result of a frequency analysis that includes an initial condition from a previous static analysis; if the amount of compressive pre-load is sufficiently large, a negative eigenvalue will be generated, potentially indicating a buckled structure.

[35]: There [is][are] XXXX rigid body mode(s) according to eigenvalue analysis.

The presence of near-zero eigenvalues in a natural frequency analysis usually indicates a rigid body mode for the whole structure or a part of it that is disconnected and not restrained.

[36]: All natural frequencies are zero.

Check model and load case "XXXX".

This is usually encountered when the pre-load effects from the included initial condition in a natural frequency analysis are sufficiently large such that all modes are negative or zero. See also Warning [34]: There [is][are] XXXX zero or negative eigenvalues - [this][these] could be due to buckling.

[37]: All natural frequencies are zero - there should only be XXXX zero eigenvalue(s).

The number of zero eigenvalues should correspond to the number of rigid body modes. If these numbers are not consistent, it may mean that the structure has buckled due to excessive compressive stress, or that there are multiple unrestrained parts in the model. See also Warning [34]: There [is][are] XXXX zero or negative eigenvalues - [this][these] could be due to buckling.

[38]: All natural frequencies are zero - check model and/or increase shift value.

The shift can be used to determine frequency modes centred about that shift value. If a non-zero shift is used and all modes are still zero, this warning is given. Either increase the magnitude of the shift or check the structure for buckling. See also Warning [34]: There [is][are] XXXX zero or negative eigenvalues - [this][these] could be due to buckling.

[39]: All buckling load factors are zero.

This can occur if the load factors (eigenvalues) are smaller than the value designated as zero in SOLVERS Parameters: EIGENVALUE. In that case, all eigenvalues are rounded to zero.

[40]: Point Contact (Beam XXXX) has changed status.

This warning is given when the status of a point contact changes during the stress calculation phase of the solution, after the solution is deemed converged. It can mean that the solution is not fully converged and may require re-running with tighter tolerances.

[41]: There are XXXX zero natural frequencies, which is more than the number of rigid body modes.

This may be given as a summary warning in conjunction with Warning [34]: There [is][are] XXXX zero or negative eigenvalues - [this][these] could be due to buckling.

[42]: End Release at beam XXXX is ignored - not applicable to [cable][truss][cutoff bar][point contact][connection] elements.

End releases are supported only by normal beam and spring elements. If these are applied to types such as truss, the end releases are ignored.

[43]: Beam XXXX has an invalid reference node - the reference node is ignored.

If the node selected as the reference node in a Beam3 (i.e., the third node) is collinear or coincides with the end nodes on the beam, it is not possible to use such a node to define the beam's principal axis system. Therefore, the reference node is ignored and the axis system reverts to the default system (i.e., the beam becomes a Beam2 element).

[44]: Infinite response will be generated due to zero damping ratio for mode XXXX.

Usually this means that a harmonic response analysis has attempted to determine the structural response at a resonant frequency for a mode with zero damping. This is not valid as it causes a division by zero (i.e., infinite response). In that case, the solver will skip the corresponding frequency step. To predict the response of the structure at that frequency step, non-zero damping must be assigned to the mode.

[45]: Face support on plate XXXX is ignored - applicable only to shell and membrane plates.

Plate Attributes: Face Support are only applicable to plate/shell and 3D membrane elements. If face support attributes are applied to elements such as plane stress elements, the attributes are ignored.

[46]: Edge support on plate XXXX is ignored - not applicable to shear panel elements.

Plate Attributes: Edge Support are not applicable to shear panel elements, and if applied are ignored.

[47]: Response for modes marked with ** is set to zero, because zero damping ratios are assigned.

This is related to Warning [44]: Infinite response will be generated due to zero damping ratio for mode XXXX.. When an infinite response is generated for a mode, the solver gives a warning and sets the response contribution from that mode to zero.

[48]: Some damping ratios are greater than 0.1 - these might not be valid for narrow band PSD.

The assumptions made by the PSD option of the Spectral Response solver are only valid where damping ratios are less than 10%. If damping ratios greater than 10% are required, the Transient Dynamic solvers should be considered for the analysis.

[49]: A nonlinear solver should be used for analysis of cable elements - linear results might not be meaningful.

[The nominated cable inertia case is used for cable stiffness - this might not be valid for all load cases.]

The cable element introduces nonlinear geometry in the solution. Although it is possible to use the Linear Static solver for cable models, the cable stiffness used in the solution may not be accurate, especially if the nodes to which the cable connects are not fully fixed. Accurate evaluation of the cable stiffness requires a nonlinear analysis. More information can be found in the Cable Inertia Case section of SOLVERS Home: Case Dependence.

[50]: Not used.

[51]: Table contains insufficient valid data points - table is ignored.

TABLE NAME: "XXXX"

This warning is given when insufficient valid data points are found in a table. In most cases a table should contain more than a single point to be meaningful (e.g., to describe material nonlinear behaviour). For other uses (e.g., Factor vs Time, Factor vs Temperature), tables with a single point are allowed.

[52]: Table contains non-increasing X values - those points are ignored.

TABLE NAME: "XXXX"

This warning will be given for tables that are used to define material nonlinear behaviour such as stress-strain behaviour. In that case, if the table contains two or more points with the same X value, the solver ignores all but one of these duplicate values. For tables used for other purposes (e.g., a Factor vs Time table that scales a load case in a transient dynamic analysis) two points with the same X value are valid and acceptable.

[53]: Condensation has generated negative or zero stiffness for brick XXXX.

To enhance the performance of the Hexa8 brick element, additional internal degrees of freedom are added to the element. Those extra degrees of freedom are then condensed from the element matrix and their influence is added to the element's nodal degrees of freedom. This warning is given whenever the condensation of the internal degrees of freedom produces a negative or zero stiffness. Typical causes of this warning include distorted elements, incorrect material constants, or elements with excessively large aspect ratios.

[54]: [Point force][Point moment][Distributed force][Distributed moment] on beam XXXX is ignored - not applicable to cable elements.

LOAD CASE: "XXXX"

The only element loads supported by cable elements are: inertia loads due to global accelerations acting on the cable's self weight and/or non-structural mass attributes; globally directed distributed beam force attributes; thermal loads; pre-strain attributes. All other loads are ignored.

[55]: [Use of cable element might not be appropriate because vibration within the element is not considered.] [Use of cable element might not be appropriate because geometric nonlinearity is not considered.][Cable droop is defined by the nominated cable inertia load case.]

Cable elements (which are based on the geometrically nonlinear catenary formulation) are not directly supported in the Natural Frequency, Linear Buckling, Harmonic Response, Spectral Response and Linear Transient Dynamic solvers because the cable stiffness cannot be updated as its deformation changes. In these solvers, the cable stiffness is based on a fixed inertia load case selected for the solution, and it remains unchanged over the entire analysis sequence.

[56]: Insufficient disk space to store matrices - continuing without Sturm check.

If the Sturm Check has been requested in the Natural Frequency or Linear Buckling solvers, additional storage space is required for the backup of the stiffness matrix. If this space is not available at the time when the matrix is ready to be backed up, the solver gives this warning and continues without the Sturm check.

[57]: Plate XXXX has zero thickness.

The specified plate has a zero thickness, therefore it contributes no stiffness to the global matrix.

[58]: Initial OCR is less than 1.0 in Cam-Clay [plate][brick] property XXXX.

The Over Consolidation Ratio (OCR) should be greater than, or equal to 1.0. An OCR greater than 1.0 means that the soil has previously been loaded to a higher level of consolidation (compressive) stress than it is experiencing now.

[59]: Pre load on plate XXXX is ignored - not applicable to shear panel elements.

The shear panel plate element does not support pre-stress or pre-strain attributes.

[60]: [Mass participation factor(s) greater than 100%.]

[Translational mass participation factor(s) greater than 100%.]

[Rotational mass participation factor(s) greater than 100%.]

[Translational and rotational mass participation factors greater than 100%.]

This might be caused by modes that are not fully converged.

[Running Natural Frequency solver with smaller tolerance might avoid this.][Running Natural Frequency solver with smaller tolerance or with consistent mass might avoid this.]

In some situations, the Spectral Response solver may calculate a sum of mass participation ratios that exceeds 100%. This usually means that some of the included eigenvectors (i.e., mode shapes) are not fully converged. This also applies to harmonic response and natural frequency analyses.

[61]: Too many modes are requested - number of modes is changed to XXXX.

If the solver detects that the requested number of modes is greater than the number of active degrees of freedom, this warning message is given and the requested number is automatically reduced. For natural frequency analysis, the number of active degrees of freedom refers to the number of active mass degrees of freedom, whereas for linear buckling analysis, it refers to the number of active degrees of freedom in the geometric stiffness matrix. Note that this warning is different to WARNING [29]: Too many modes requested - at most, XXXX mode(s) can be determined., which considers only the stiffness degrees of freedom (not the mass matrix or geometric stiffness degrees of freedom).

[62]: Working set is not expanded - if convergence cannot be achieved, reduce number of requested modes.

To aid in the convergence of the eigenvalues, the solver expands the number of modes in the working set for the Subspace iteration procedure. For example, if 10 modes are requested, the solver may work with a set of 16 modes. If the number of independent modes in the structure is less than the number of modes requested plus the additional working set modes, the working set is only partially expanded, or not expanded at all.

[63]: Step XXXX has not converged within maximum allowable iterations.

For nonlinear analysis, there is a limit to the number of iterations within a single load step. If convergence cannot be achieved within this limit and SOLVERS Parameters: SUB-STEPPING is disabled, this warning is given and the solver continues with the next load step. In some situations, subsequent load steps may converge despite the non-convergence of a previous step. To reach convergence for some difficult to converge load steps, it may be necessary to reduce the load increment by increasing the number of load steps, or to enable SOLVERS Parameters: SUB-STEPPING to allow the solver to reduce the load step automatically.

[64]: Plate property XXXX has zero or near-zero transverse shear stiffness.

This warning applies to thick shell elements, which consider deformation due to transverse shear force. If the transverse shear stiffness is zero or near zero, unrealistic displacements may result. The plate property data should be checked.

[65]: Node restraints might not be sufficient to prevent rigid body motion.

The motion might be restrained by element supports, node stiffness or links.

Number of possible rigid body modes is XXXX (DOF LIST).

At the commencement of a structural solution, the solver attempts to detect the presence of any rigid body modes by investigating the nodal restraints. If nodal restraints are not sufficient to restrict rigid modes, the solver gives this warning. In some situations, such as when restraints are applied with respect to a UCS, or when links are present, the solver skips the detection of rigid body modes as it is not possible to establish these exist without assembling the global stiffness matrix. If rigid body motion is prevented by the presence of element support attributes, this warning is not applicable, even if it is given.

[66]: A positive shift (XXXX Hz) was used in Natural Frequency solver.

This might result in missing lower order modes.

For spectral and harmonic response (modal) analysis, it may be necessary to include the lowest modes of the structure in order to obtain an accurate response solution and a sufficient mass participation. If the natural frequency solution used for the modal analysis included a positive shift, some lower order modes may be missing from the set.

[67]: Maximum allowable rotational increment exceeded.

Largest rotation: XXXX deg. At Node XXXX.

This warning message is given during a geometry nonlinear analysis (both static and dynamic), whenever the rotation at any node exceeds a preset value. Because the nonlinear geometry solver needs to determine the rigid body rotation of any element between successive iterations, nodal rotation increments between load steps should be kept small. If convergence cannot be achieved, it may be necessary to reduce the load factors and/or increase the number of steps used, or employ one of the automatic sub-stepping options (SOLVERS Parameters: SUB-STEPPING (Static), SOLVERS Parameters: SUB-STEPPING (Time Based)).

[68]: Table contains decreasing Y values - those points are ignored for elastic-plastic analysis.

TABLE NAME: "XXXX"

This warning is given when an elastic-plastic material table contains decreasing Y values; softening in an elastic-plastic material analysis is not supported. Note that nonlinear elastic material tables do not have this restriction.

[69]: Maximum allowable plate element rotation exceeded (Plate XXXX).

This warning message indicates that the relative nodal rotation of the plate element has exceeded a preset amount. If convergence cannot be achieved, it may be necessary to reduce the load factors and/or increase the number of steps used, or employ one of the automatic sub-stepping options (SOLVERS Parameters: SUB-STEPPING (Static), SOLVERS Parameters: SUB-STEPPING (Time Based)).

[70]: Spring rotation (Beam XXXX) exceeds 5 degrees.

This warning is given in geometric nonlinear analysis when a spring with lateral stiffness rotates laterally by more than 5 degrees. The significance of this warning is that, unlike a beam element where the end displacements and rotations are coupled and therefore it is possible to separate rigid body rotation from the deformational displacements, in a spring element each stiffness and corresponding displacement is independent of the others, so it is not possible to update the direction of the lateral stiffness in the same way as it is done for beams. The message is not given for springs defined only with axial stiffness since the updated axial direction can always be determined.

[71]: [Nonlinear behaviour of contact cannot be predicted with a linear solution.] [Nonlinear behaviour of contact elements is ignored by this solver.]

All contact problems should be solved using a nonlinear solver. In a linear analysis, all point contact elements except for Zero Gap contact elements, are treated as truss elements and their stiffness is included in the matrix. Zero Gap contact elements are excluded in a linear analysis.

[72]: Plate XXXX is collapsed.

A collapsed plate can be due to a bad initial mesh or excessive distortions during a geometry nonlinear analysis. In either case, the results of such a mesh might not be reliable.

[73]: Internal angle is out of range in plate XXXX.

Because plate elements perform best when the internal angles of quadrilaterals are near 90 degrees and those of triangles are near 60 degrees, this warning is given for plate elements with internal angles exceeding a preset limit. The severity of this depends upon the plate angle and the location of the element in the mesh.

[74]: Table contains (X,Y) values with conflicting signs - those points are ignored.

TABLE NAME: "XXXX"

This warning is given when a data point in a material nonlinear table has conflicting signs (e.g., a Stress vs Strain table with positive stress corresponding to negative strain). Although the solver attempts to make sense of the table by ignoring these points, it is recommended that the table be corrected and the analysis re-run.

[75]: Offset at beam XXXX is ignored.

Offsets may only be applied to normal beam elements. If an offset is specified for one of the other beam types (e.g., truss or spring) the offset is ignored.

[76]: Off-diagonal terms in mass matrix due to [beam][plate] offsets are ignored - consistent mass should be used.

When offsets are applied to beam or plate elements in a dynamic analysis, the mass matrix cannot be a lumped diagonal matrix as off-diagonal terms are required to account for the interaction between translational and rotational inertia. If the lumped mass option has been selected for a dynamic analysis (e.g., natural frequency analysis) the off-diagonal terms are ignored and this warning message is given.

[77]: Global mass matrix is a zero matrix - no inertia effects will be included.

This warning is given by the Transient Dynamic solver whenever there is no mass in the system. Normally, a mass would be expected because the Transient Dynamic solver is solving dynamic equations of motion for which the inertia terms are an important part. Note that if there is no mass and no damping in the system, the solution effectively becomes a static solution.

[78]: [Shrink links are ignored or treated partially as Master-Slave links when using mode superposition.] [Shrink links are ignored or treated partially as Master-Slave links by this solver.]

Shrink Links may only be used in the Linear and Nonlinear Static solvers, and in the Transient solver with the full system option. If these links are used in the other solvers, they may be ignored or interpreted as Master-Slave links (e.g., in natural frequency analysis).

[79]: [Non-zero enforced displacements are ignored by this solver.] [Non-zero enforced displacements are ignored when using mode superposition.]

Non-zero enforced displacements may only be used in the Linear Static, Nonlinear Static, Quasi-static and Nonlinear Transient Dynamic solvers, as well as in the Linear Transient Dynamic solver with the full system option. They are ignored by all other solvers.

[80]: Thickness to length ratio of plate XXXX might be excessive due to relatively [small][large] thickness.

Quad4 plates used as plate/shell elements should maintain a reasonable thickness to edge length ratio. If the element is too thick or too thin, the automatic calculation of the drilling stiffness may generate values that are too small or too large. Unless the equation reduction fails, this may not be a serious problem in the mesh.

[81]: Global stiffness matrix might be singular.

Number of possible singularities detected = XXXX.

This warning message may be given at the conclusion of the Drilling and Singularity Check (see SOLVERS Parameters: ELEMENTS). If singularities are found, their locations (i.e., node numbers) and cause should be investigated by reading the log file before proceeding to review the mesh.

When a singularity is found at a node, a 3x3 nodal stiffness triplet is given. This triplet is a sub-matrix taken from the global stiffness matrix with its three rows and columns corresponding to the three translational or rotational degrees of freedom at that node. The singularity checking is performed based on the three eigenvalues of the sub-matrix. Existence of a negative eigenvalue implies a negative stiffness in a certain direction, while a zero eigenvalue means an unrestrained direction. Note that zero in this case means an eigenvalue that is small relative to the others (a parameter in the SOLVERS Parameters: ELEMENTS defines what 'small' is).

A negative stiffness is not physical, therefore a negative eigenvalue may indicate a serious problem with the mesh. Possible causes include distorted element geometry and invalid element material constants. Adjacent elements should also be checked.

If there is only one zero eigenvalue in the rotational stiffness sub-matrix, and a plate/shell element is connected to that node, the solver takes the corresponding direction as the axis of a drilling degree of freedom and adds a small amount of stiffness there to restrain the rotation about that axis. In this case, the warning message is not given.

If more than one zero eigenvalues are found in the rotational sub-matrix, or any in the translational sub-matrix, the solver assumes there is an error in the model. For these situations, the node's freedom conditions and the stiffness contributions from adjacent elements should be checked.

[82]: Negative convection coefficient applied to [beam][plate][brick] XXXX - absolute value will be used.

Negative convection coefficients are not valid in the heat transfer solvers. If applied, either directly or due to scaling by a Factor vs Time table during analysis, the absolute value will be used and this warning will be given.

[83]: Negative radiation coefficient applied to [beam][plate][brick] XXXX - absolute value will be used.

Negative radiation coefficients are not valid in the heat transfer solvers. If applied, either directly or due to scaling by a factor vs time table, the absolute value will be used and this warning will be given.

[84]: Bending thickness for nonlinear material element (Plate XXXX) is set equal to membrane thickness.

In material nonlinear analysis, the bending and membrane thickness values for a plate/shell must be the same. The solver enforces this by setting the bending thickness to be equal to the membrane thickness.

[85]: Not used.

[86]: Not used.

[87]: Mass for cable elements is lumped at nodes.

This warning is given whenever the mass matrix is required in a dynamic analysis involving cable elements. The total mass of a cable element is lumped to the nodes, which precludes the modelling of inertia (dynamic) effects along the cable. To include those effects, the cable can be modelled as a series of beam or truss or cable elements in order to distribute the nodal mass along the cable length.

[88]: Damping matrix for cable elements is lumped at nodes.

This warning is given whenever the damping matrix is required in a dynamic analysis involving cable elements. The damping effect of cable elements is lumped to the nodes, which precludes the modelling of viscous effects along the cable. To include those effects, the cable can be modelled as a series of beam or truss or cable elements in order to distribute the damping along the cable length.

[89]: Restart file cannot be opened.

This warning is given by the Nonlinear Static, Quasi-static and Nonlinear Transient Dynamic solvers in two situations:

1. A restart is requested and the restart file cannot be found or opened after the solver has been launched (note that if the restart file cannot be opened at solver launch time, the solver will not start). The restart file usually has the extension .SRF, .QRF or .DRF (depending on the solver type) and its creation is enabled from the Files tab of the solver dialog.
2. The solver is attempting to re-save the restart file but the save operation has failed.

[90]: [Minimum displacement scale has been reached - no further reduction will be applied to this [sub-step] [time step][increment].] [Minimum time step has been reached - no further reduction will be applied to this [sub-step][time step].] [Minimum load reduction factor has been reached - no further reduction will be applied to this [increment][sub-step].]

This warning is given by the Nonlinear Static, Quasi-static and Nonlinear Transient Dynamic solvers when Automatic Sub-Stepping has been enabled and the minimum load reduction factor has been reached. The load factor is progressively reduced in a non-convergent load step until convergence is achieved or the minimum load reduction factor has been reached. The minimum load reduction factor is specified in SOLVERS Parameters: SUB-STEPPING (Static) and SOLVERS Parameters: SUB-STEPPING (Time Based). If the minimum load reduction factor is reached and the solution has still not converged, the solver continues to iterate with these load factors until the maximum number of iterations has been reached.

[91]: Condensation has failed for [plate][brick] XXXX - bubble function not used.

This warning is given whenever the condensation of the internal degrees of freedom (bubble function) on a Quad4 or Hexa8 element produces a negative or zero stiffness. The extra internal degrees of freedom are included in these elements to enhance their performance. Typical causes of this warning include distorted elements or incorrect material constants. When condensation fails, the bubble function is not added.

[92]: Temporary files cannot be opened - automatic sub-stepping is disabled.

This warning may be given at the commencement or during the iterations in the Nonlinear Static, Quasi-static and Nonlinear Transient Dynamic solvers.

If the warning is given at the commencement, it means that a previously stored temporary file, required for a restart procedure, cannot be opened or cannot be found. The file names can be set and checked in the Files sub-tab of the SOLVERS tab (SOLVERS: Files). If the file cannot be found, the solution needs to start again from the beginning.

If the warning is given during the iteration procedure, it means that the temporary file cannot be saved. This can be caused by insufficient disk space or other file system issues such as a lost network connection when working on a network drive.

[93]: Mass matrix for released element (Beam XXXX) is approximate - refined mesh might be required.

This warning may be given by the natural frequency solver whenever a beam element includes an end release. The end release stiffness is calculated by the method of static condensation, which produces exact stiffness values at the ends of released beam elements. However, the mass matrix resulting from this condensation is approximate. In most cases the approximation does not greatly impact the natural frequency solution, but in some cases, particularly when both ends of the beam are released and the mode involves significant flexure of the single element, element subdivision may be required to achieve accurate results.

[94]: Shear modulus equation (a,b) for Cam-Clay [plate][brick] property XXXX is not valid.

This warning is given when the Cam-Clay equation for the shear modulus, defined as G = a + b*P, where P is the mean stress, produces invalid (i.e., negative) shear modulus.

[95]: Pipe radius for beam XXXX is ignored because it is too small.

When a curved pipe element has a pipe arc angle larger than 180 degrees, it will be treated as a straight element to avoid numerical errors.

[96]: Prescribed displacement component(s) at node XXXX cannot be enforced due to inactive degrees of freedom.

This warning is given if the prescribed displacements at a node are not consistent with the allowable degrees of freedom. A typical example is where the global freedoms in a particular direction are inactive (e.g., a plane strain problem, which has no global Z freedom) but a node contains a prescribed displacement in the Z direction. Another example might be a sector symmetry link applied to nodes that restrict the sector-symmetric movement.

[97]: Support on beam XXXX is ignored - applicable only to beam, pipe and user-defined beams.

Beam supports are only applicable to the normal beam elements, pipe elements and user-defined beams. If a support attribute is applied to other beam element types such as truss or spring, it is ignored.

[98]: Partial end release on spring element (Beam XXXX) is ignored in material nonlinear analysis.

[Release of translation in axial direction.] [Release of rotation about axial direction.]

The beam end release attribute cannot be used to release material nonlinear spring elements.

[99]: Material temperature ignored for user-defined creep law - nominal temperature (XXXX) will be used. Set Property Temperature Dependence to <Combined Temperature> in solver options to consider temperature dependence.

For user-defined creep, in which one or more Strain vs Time tables are used to define the stress-strain-temperature-time relationship, the Property Temperature Dependence option in SOLVERS Home: Case Dependence should be set to <Combined Temperature> as this is required to correctly define the temperature distribution at each time step. If this has not been set, a nominal temperature is assumed for the element (this is the equivalent of 25 degrees Celsius for models with units, or zero for models that do not use units).

[100]: 2D element (Plate xxx) is not in XY-plane - projection onto XY-plane will be used.

Plane stress, plane strain and axisymmetric analysis requires that the elements be flat and located on the global XY-plane at Z=0. If the element is warped, or not parallel to the XY-plane, the projection of the element onto the XY-plane will be used. However, the model data should be corrected in preference to relying on the projection. To model a plane stress element in 3D, the 3D membrane element can be used.

[101]: [Beam][Plate][Brick] XXXX has no thermal damping - check material density and specific heat.

For transient heat analysis, the coefficient of specific heat (Cp), multiplied by the mass density of the material, defines the thermal damping in the system, and is usually required for such analysis. This warning is given if either Cp or mass density are zero for the indicated beam.

[102]: Not used.

[103]: Not used.

[104]: Time now (XXXX) has exceeded the last time step in transient heat solution.

Temperature distribution at last step of the heat solution will be used from now on.

This warning is applicable to transient dynamic and quasi-static analysis that uses a previously generated transient heat solution to define the temperature time history. This message is given when time in the structural solution exceeds the total time of the heat solution. The structural solver will then use the temperature distribution of the last step in the heat solution for all the remaining time steps.

[105]: Translational end release attributes on beam XXXX generate a singular element - respective stiffness ignored.

When translational end release is applied to both ends of a beam element and in the same principal axis direction, the element will have no stiffness in that particular direction. In that case the respective end releases are ignored and the corresponding stiffness of the element is set to zero. The applied end release attributes should be checked.

[106]: Torsional end release attributes on beam XXXX generate a singular element - torsional stiffness ignored.

When torsional end release is applied to both ends of a beam element, the element will have no torsional stiffness at the nodes. In that case the torsional end releases are ignored and the torsional stiffness of the element is set to zero. The applied end release attributes should be checked.

[107]: End release attributes on beam XXXX generate a singular element - bending and shear stiffness ignored.

When translational and rotational end releases are applied to both ends of a beam element, the element may have no bending stiffness in one or both principal planes. In that case the end releases are ignored and the lateral stiffness of the element is set to zero. The applied end release attributes should be checked.

[108]: [Plate][Brick] property XXXX contains invalid rubber constants.

This warning is given if the rubber constants yield a negative shear modulus or Poisson's ratio.

[109]: Thermal strain is too large in [plate][brick] XXXX.

This warning is given when thermal strain applied to a plate or brick element in geometry nonlinear analysis is close to, or greater than, unity. The solver will use the applied value, however, if the solution fails to converge, the load step may need to be reduced and the validity of such a large thermal strain reconsidered.

[110]: Pre-strain is too large in [plate][brick] XXXX.

This warning is given when pre-strain applied to a plate or brick element in geometry nonlinear analysis is close to, or greater than, unity. The solver will use the applied value, however, if the solution fails to converge, the load step may need to be reduced and the validity of such a large pre-strain reconsidered.

[111]: Off-diagonal entries in mass matrix are ignored for rotational mass at node XXXX.

When a rotational mass in a UCS that is not parallel to the global Cartesian system is applied to a node in a dynamic analysis, the mass matrix cannot be a lumped (diagonal) matrix as off-diagonal terms may be required to account for the interaction of inertia about two or more axis directions. If the lumped mass option has been selected for a dynamic analysis (e.g., natural frequency analysis) the off-diagonal terms of rotational mass are ignored and this warning is given.

[112]: Translational damper at node XXXX is ignored - applicable only to nonlinear transient and full-system linear transient.

Node Translational Damping attributes are used only in the Linear (full-system) and Nonlinear Transient Dynamic solvers. Those attributes are ignored by all other solvers.

[113]: Subspace dimension was reduced to XXXX.

During the Subspace iteration of an eigenvalue problem, the dimension of the Subspace may be reduced due to the removal of base vectors. The most likely reasons for base vector removal are that there are fewer independent modes than the current dimension of the Subspace, or that a very large eigenvalue has appeared in an iteration (base vectors corresponding to very large eigenvalues are removed according to the Max eigenvalue ratio setting under SOLVERS Parameters: EIGENVALUE).

[114]: Number of modes calculated is reduced to XXXX.

[This may be caused by buckling or negative stiffness.] [This may be caused by buckling, negative stiffness or the presence of links.]

When the Subspace dimension is reduced and is less than the number of requested modes, the number of calculated modes will no longer be the same as that requested, so this warning is given.

[115]: Compression-only option of support on [beam][plate][brick] XXXX is ignored by this solver.

[Use Nonlinear Static solver.] [Use Nonlinear Transient solver.]

Beam, plate and brick support attributes have a Compression-Only option, which is applicable only in the Nonlinear Static, Quasi-static and Nonlinear Transient Dynamic solvers. In all other solvers, the support attribute is assumed to act equally in tension and in compression.

[116]: Not used.

[117]: Transverse shear deformation in beam XXXX is not considered in material nonlinear or creep analysis.

The thick beam element is limited to linear material analysis. When a nonlinear material or creep property is included in the analysis of a beam element, thin beam theory is used and the shear deformation is ignored.

[118]: [Lateral end release at beam XXXX is ignored - not supported in geometric nonlinear analysis.][Lateral end release at beam XXXX is ignored.]

In geometry nonlinear analysis, translational end release attributes applied in the lateral directions of beams are ignored. Axial end releases are supported in geometry nonlinear analysis. Some beam element types do not support lateral releases at all.

[119]: Temperature gradient on plate XXXX is ignored - applicable only to shell elements.

LOAD CASE: "XXXX"

For plate elements that are not plate/shell types, temperature gradient attributes are ignored.

[120]: Axial strain in beam XXXX is greater than 5.0%.

It is assumed that the axial strain of the beam element remains small in geometry nonlinear analysis. When the strain is greater than 5%, this warning is given.

[121]: Node [translational][rotational] mass components at node XXXX are ignored due to restraint conditions.

This warning is given when applied nodal masses are ignored due to the node restraints.

[122]: [Warping][Current Warping] ratio for plate XXXX is YYY.

This warning is given whenever the warping ratio of a Quad4 plate/shell element exceeds 10%. For geometry nonlinear analysis, a flat element may become warped during the solution; in that case, the second message is given. Where the warping ratio is exceeded on the initial mesh, the element geometry near the warped plates should be revised and the amount of warping reduced, if possible.

[123]: Nonlinear behaviour of cutoff bars is ignored by this solver.

Use nonlinear solver with material nonlinearity enabled.

To include the nonlinear behaviour of cutoff bars (i.e., to consider the tensile and compressive force limits), the Nonlinear Static, the Quasi-static or the Nonlinear Transient Dynamic solver must be run. Note that the nonlinear status of cutoff bars, as determined by the nonlinear solvers, can be used as initial conditions in the Linear Buckling and Natural Frequency solvers.

[124]: [Change(s) to load factors for increment XXXX detected.] [Change(s) to load factors for increments XXXX and/or YYYY detected.]

This warning is given at the commencement of a nonlinear solution restart, if the load factors for the previously solved increments have changed from those in the previous run.

[125]: Point contact (Beam XXXX) is ignored because initial stiffness is zero.

For a point contact element to be included in the analysis, it must have a non-zero initial stiffness. The Dynamic Stiffness option can adjust the stiffness only by scaling an initial stiffness.

[126]: Pre-tension on point contact (Beam xxx) is ignored - not applicable to point contact elements.

LOAD CASE: "XXXX"

Pre-tension attributes are not applicable to point contact elements. Note that Normal Gap point contact elements do support pre-strain attributes as a way of controlling their activation points.

[127]: Table contains invalid data - table is ignored.

TABLE NAME: "XXXX"

This warning is given when an elastic-plastic material table contains invalid data such that no meaningful use can be made of the table data. In that case, the table is ignored and the element reverts to being a linear one.

[128]: There [is one][are XXXX] converged eigenvalue(s) with unconverged eigenvector(s).

This warning is given when an eigenvalue (frequency or buckling load factor) has converged, but its eigenvector (mode shape) has not. Although it applies to both the Natural Frequency and the Linear Buckling solvers, it is mostly relevant for a natural frequency analysis. For a natural frequency analysis, if only the frequency is required, the warning can usually be ignored. However, if the results of the natural frequency analysis are required for mode superposition analysis (e.g., harmonic or spectral response analysis) it is important to also have converged mode shapes. To help obtain converged mode shapes, the options under SOLVERS Parameters: EIGENVALUE can be adjusted.

[129]: Strain for plate element (Plate XXXX) is too large.

Strain in thickness direction is out of range.

This warning is given when the Green's strain in the thickness direction of 3D membrane and plane stress elements approaches or is less than -0.5 in geometric nonlinear analysis. As this strain value is obtained by forcing the corresponding stress component to zero, the calculated value may be out of range when the in-plane strain in the element is very large.

[130]: All loads on material nonlinear beams are treated as lumped loads.

Element loads such as Beam Distributed Force and Beam Point Force attributes applied to beam elements with nonlinear material behaviour, are treated as lumped loads. This includes:

• Beam elements with Moment vs Curvature tables.
• Beam elements with fibre Stress vs Strain tables.
• Beam elements with creep material.
• Beam elements with Modulus vs Time or Modulus vs Temperature tables and the Temperature/Time nonlinearity set to Plastic.
• Beam elements for which support attributes are switched to the Lumped option by the solver (see WARNING [242]: Loads on beam XXXX converted to lumped loads due to support.).

"Treated as lumped" means that the element load is converted into nodal loads; usually only the nodal force components of the load are applied to the element, whilst the moment components are ignored. As the load is now nodal rather than element based, the internal force/moment distribution in the beam will always be linear between the nodes, and the shear force will be constant, irrespective of the applied load (i.e., there is now no body load). For a suitably refined mesh, which is normally required for nonlinear analysis anyway, treating these loads as lumped will produce an acceptable piecewise approximation to the member forces and moments.

[131]: Axial direction of compression-only cutoff bar (Beam XXXX) has reversed.

This warning is given during the stressing phase of a geometry nonlinear analysis if a compression-only cutoff bar is found to be carrying tension.

[132]: Axial direction of tension-only cutoff bar (Beam XXXX) has reversed.

This warning is given during the stressing phase of a geometry nonlinear analysis if a tension-only cutoff bar is found to be carrying compression.

[133]: Initial mean stress is tensile in [plate][brick] XXXX - value is ignored.

In-situ stress, initial fluid (pore) pressure or OCR data might be invalid.

Cam-Clay materials require a compressive mean stress in order to generate a stiffness matrix. If significant tensile stresses are generated in a Cam-Clay material, the element, and hence the solution, may fail.

[134]:Support for beam XXXX is modelled as lumped due to very high support/beam stiffness ratio.

The hyperbolic shape functions used to model the exact beam Winkler support can only be used in a linear analysis and when the ratio of the support stiffness to the beam's lateral stiffness is sufficiently small. If the ratio becomes too large this warning is given and the support formulation reverts to a lumped equivalent stiffness at the nodes. To obtain better results, the relevant beams should be subdivided.

[135]: Transverse shear deformation in beam XXXX is not considered due to support.

For beam elements with support attributes, the shear area is ignored.

[136]: Conflicting prescribed displacement component(s) found at node XXXX.

These cannot be simultaneously enforced.

This warning can be given by the Linear Transient solver in situations where multiple freedom cases are included and the same node/dof combination has non-zero prescribed displacements in more than one freedom set, or where one freedom set fixes the dof while another enforces a non-zero value. The Linear Transient solver cannot enforce these so (usually) only the first encountered freedom case will be satisfied. Multiple freedom cases can be used in the Linear Transient solver as long as the same node/dof does not have these conflicts. In the Nonlinear Transient Dynamic solver, the enforced displacements from different freedom sets are added together at each time step, so this restriction does not apply.

[137]: Support for beam XXXX is modelled as lumped due to material nonlinearity.

Subdivide beam element to obtain better results.

This is applicable to nonlinear material analysis. The formulation of beam elements with a support attribute is based on hyperbolic shape functions provided a linear material is used (Winkler foundation). For a nonlinear material beam, the support is modelled using equivalent springs lumped at the nodes.

[138]: Element viscous damping in string groups is ignored.

Truss elements in string groups do not support the viscous damping option if Property Damping has been selected in SOLVERS Home: Damping/Added Damping

[139]: Pre-tension on cable (Beam XXXX) is ignored - cable elements do not support pre-tension - use pre-strain.

LOAD CASE: "XXXX"

The Pre-tension attribute is ignored by cable elements. To impose a pre-tension on cable elements, the Cable Free Length attribute or the Pre-strain attribute should be used. When a Cable Free Length attribute is not assigned, the cable length is assumed to be equal to the distance between the two nodes (cord distance). By assigning a free length that is less than the cord distance, a pre-tension is effectively applied. When a Pre-strain attribute is applied, the free length of the cable is adjusted according to the Pre-strain attribute.

[140]: Pipe radius for beam XXXX is ignored - attribute supported only by pipe elements.

The Pipe Radius attribute is applicable only to pipe elements. It will be ignored if applied to other beam element types.

[141]: Radius for beam XXXX is invalid - this element will be treated as straight.

A radius is invalid if it is smaller than half of the distance between the two end nodes of a curved beam element (i.e., pipe). An invalid radius attribute is ignored in the solution and the element is treated as straight.

[142]: Distributed force on curved element (Beam XXXX) is applied over full length.

LOAD CASE: "XXXX"

Distributed forces on curved elements (i.e., pipes) are assumed to be over their full length. If a distributed force is applied over only part of the element length, an equivalent force is applied, uniformly distributed over the full length of the element. To apply a distributed force over a partial length of a curved pipe element, the element should be subdivided.

[143]: Curved element (Beam XXXX) is released in element's local system.

For curved beam elements (i.e., pipes), end release attributes refer to the default principal axis system of the element, not the curvilinear system; a translational end release in the 3 axis direction may still produce an axial force in the 3 axis direction of the element.

[144]: Support on curved element (Beam xxx) is modelled as lumped.

Subdivide element to obtain better results.

Beam support attributes applied to curved beams (i.e., pipes), are treated as equivalent springs lumped at the nodes. To get more accurate results, a subdivided mesh may be required.

[145]: Refined mesh might be required for curved element (Beam XXXX).

In linear static analysis, a circular curved beam can be accurately represented with one element (when the angle of the arc is less than 180 degrees). In natural frequency and linear buckling analysis a curved beam should be represented with multiple elements. If the angle of an element is larger than 45 degrees, this warning is given.

[146]: Strain for plate XXXX is bigger than 10% - results might not be reliable.

Small strain is assumed unless the material is rubber. If any normal strain component exceeds 10%, this warning is given.

[147]: Linearly distributed force on pipe element (Beam XXXX) is replaced with a uniformly distributed force.

Distributed force on curved elements must be uniform over the full length of the element. If a linearly distributed force has been applied, it is replaced with an equivalent uniformly distributed force. To apply linearly varying distributed force over a curved pipe element, the element should be subdivided.

[148]: Takeup element (Beam XXXX) will be treated as a spring - nonlinear solver should be used.

A Takeup Gap point contact element may introduce nonlinearity into a solution. If such an element is used in a linear analysis, the element is treated as a spring, and this warning is given.

[149]: Large creep strain increment in [beam][plate][brick] XXXX.

This warning usually indicates that the amount of creep strain generated within one time step is too large. If the solution fails to converge, the time step should be reduced.

[150]: Table does not describe a valid Takeda material model - table is ignored.

TABLE NAME: "XXXX"

The Takeda model is defined with either a three-segment or a six-segment curve (table). If only the positive quadrant is defined (i.e., the same behaviour is assumed for both compression and tension), the table must consist of three segments, with the first point passing through (0,0). If both positive and negative quadrants are defined (i.e., different behaviour is assumed for tension and compression), the table must consist of six segments (i.e., seven points with the first three points in the negative quadrant, the fourth point at (0,0), and the last three points in the positive quadrant). If the table does not satisfy these requirements, this warning is given and the table is ignored.

[151]: Inputs for Rayleigh damping factors are invalid - Rayleigh damping is excluded.

The mass and stiffness coefficients (Alpha, Beta) for Rayleigh damping can be specified directly or calculated using two frequencies and corresponding damping ratios. If the latter option is used, and the Alpha and Beta coefficients cannot be evaluated, Rayleigh damping is excluded and this warning is given (see Special Topics: Damping).

[152]: Off-diagonal terms for torsional part of beam mass matrix are ignored - consistent mass should be used.

The contribution to the mass matrix for torsional rotation may contain off-diagonal terms if the element's axial direction is not aligned with one of the global coordinate axes. When the lumped (diagonal) mass matrix is used, the off-diagonal terms cannot be considered and therefore this warning is given.

[153]: Not used.

[154]: Zero modulus/shear modulus not allowed for pipe elements (Beam XXXX).

The elastic and shear moduli for pipe elements must be positive (and non-zero) because the element's stiffness matrix is determined by inverting a compliance matrix. If this requirement is not met, the corresponding element will be ignored in the solution and this warning is given.

[155]: Off-diagonal terms in mass matrix due to constraint equations ignored - use consistent mass to include.

When links are used in a model, mathematical relationships are imposed between two or more degrees of freedom. If any of these mathematical relationships impose a constraint between translational and rotational degrees of freedom, the effective mass matrix may not be a diagonal matrix once the dependent degrees of freedom are eliminated. If the lumped mass option has been selected for a dynamic analysis (e.g., natural frequency analysis) the off-diagonal terms generated by the link equations are ignored and this warning is given.

[156]: All modal loads are zero for current case.

For spectral response analysis, all response results will be zero if the modal loads are all zero. This warning is given in that case.

[157]: Significant round-off error detected for the linear equation solution - check model and results.

When the nodal balance is checked at the end of the solution by performing a residuals check (SOLVERS Parameters: GENERAL), this warning is given if the error ratio is larger than 1%.

[158]: Distributed moment on beam XXXX is ignored - not applicable to [spring][cable][truss][cutoff bar][point contact][connection] elements.

LOAD CASE: "XXXX"

A Beam Distributed Moment attribute can only be applied to normal beams, straight pipes, and user-defined beam types. For the other types of beam elements, this attribute will be ignored.

[159]: [Plate][Brick] property XXXX contains zero bulk modulus.

This warning is given for rubber materials in nonlinear analysis when the rubber property has a zero bulk modulus. Although mathematically valid, a zero bulk modulus is unexpected for a rubber material.

[160]: Null base excitation vector - all response for this case will be zero.

This warning is given when the base excitation vector defined for the Spectral Response solver or Harmonic Response solvers is a null vector for a particular case.

[161]: Pipe pressure on beam XXXX is ignored - applicable only to pipe elements.

LOAD CASE: "XXXX"

This warning is given when a pipe pressure attribute has been applied to a beam element that is not a pipe.

[162]: Pipe temperature on beam XXXX is ignored - applicable only to pipe elements.

LOAD CASE: "XXXX"

This warning is given when a pipe temperature attribute has been applied to a beam element that is not a pipe.

[163]: Thickness of plate XXXX could be too big for its curvature, or the element may be excessively distorted.

This warning is given when a plate/shell element has a thickness that is considered to be too big for its curvature. This is especially relevant to Tri6, Quad8 and Quad9 elements that are not flat, but may also apply to Quad4 elements that are warped. The warning can also be given for excessively distorted curved elements even if their thickness is not excessive.

[164]: Material matrix for [plate][brick] property XXXX is invalid or not positive definite.

This warning is given when the material matrix for a plate or brick property is invalid. This typically arises for orthotropic, anisotropic and user-defined materials that have material parameters or matrices that do not satisfy the requirements. This warning is also given when the material matrix is defined as a compliance matrix, which needs to be inverted to produce a stiffness matrix; if the compliance matrix cannot be inverted or its inversion produces a matrix that is not positive definite, the warning is given.

[165]: Not used.

[166]: Viscous Damping for Spring-Damper (Beam XXXX) is ignored.

This warning message is given when viscous damping has been specified for spring-damper elements and a transient solver is not used.

[167]: For material nonlinear analysis, all segments must be of the same property.

Nonlinear behaviour for String Group XXXX will be ignored.

To consider material nonlinearity in a String Group, all segments (i.e., all grouped truss elements) must be of the same property.

[168]: For material nonlinear analysis of String Group XXXX, average temperature will be used for determining temperature dependent material parameters.

This warning is given when a string group uses elements whose modulus is temperature dependent but the temperature along the string is not constant. String groups require the same modulus over all segments (i.e., all truss elements) in the group.

[169]: Tetrahedral element (Brick XXXX) is excessively distorted - results might not be reliable.

This warning is generated when any of Brick Dihedral Angle Ratio, Mixed Product or Det(Jacobian) is outside a preset value.

[170]: Node restraint conditions [and/or links] might prevent free inertial movement(s) in [DX][DY][DZ][RX][RY][RZ].

For inertia relief analysis, the model must be unrestrained in the directions specified by the inertia relief freedom case (Special Topics: Inertia Relief Analysis). This warning is given when the required rigid body motion modes are prevented by node restraints and/or links.

[171]: [Redundant link XXXX is ignored.][Redundant link/restraint conditions detected adjacent to node XXXX.]

[This usually means that a link cluster is over-constrained.][Only one node should have a fixed temperature on a rigid link cluster.]

This warning is given when redundant link/restraint conditions are detected by the solver. The link cluster might have too many, or incompatible, restraints. The redundant conditions are ignored.

[172]: Contradicting link/restraint conditions detected adjacent to node XXXX.
[This usually means that a link cluster is over-constrained.][Only one node should have a fixed temperature on a rigid link cluster.]

This warning is given when contradicting link/restraint conditions are detected by the solver. The solver selects one of the conditions. For example, if restraints are applied at the ends of a rigid link to stretch the link, the restraints contradict the condition of rigidity in the link. Although the solver proceeds, the model should be corrected.

[173]: Pre-tension on pipe (Beam XXXX) is ignored because the element is curved.

LOAD CASE: "XXXX"

Pre-tension attributes are not applicable to curved pipe elements. Pre-strain attributes may be used.

[174]: Element mass in string groups is ignored.

As all elements in a string group are assumed to be massless, mass density values in the element's property set are ignored.

[175]: Pre-stress/pre-strain attribute is applied as mean pre-stress in fluid element ([Plate][Brick] XXXX).

Pre-loads in fluid elements must be hydrostatic. If different values of pre-stress or pre-strain have been applied in different directions, the mean value is applied in all directions instead.

[176]: There are errors in global acceleration/angular data for this axisymmetric model.

Correction(s) have been made to maintain symmetry in loading condition.

Only axisymmetric deformation can be modelled in an axisymmetric analysis, and therefore inertia force components (global accelerations) causing other deformations are ignored.

[177]: Seismic analysis with axisymmetric elements is not meaningful - no accelerations are applied.

As axisymmetric deformation is not possible for an equivalent static seismic analysis, axisymmetric models cannot be used with seismic load cases. The global seismic accelerations in those load cases are ignored.

[178]: Pipe radius on beam XXXX is ignored because it is too large - pipe angle < 0.0001 deg.

When a curved pipe element has a very small pipe angle (i.e., very large relative radius), it is treated as a straight element to avoid numerical errors.

[179]: Both tension and compression limits are zero for cutoff bar (Beam XXXX).

When both tension and compression limits of a cutoff bar are zero, the element will have no axial strength in a material nonlinear analysis. In that case the stiffness of the element is ignored.

[180]: Nonlinear behaviour of cutoff bars is ignored in this solution.

To consider such behaviour, set nonlinear material option.

This warning is given during a nonlinear static, quasi-static or nonlinear transient dynamic analysis if the nonlinear material option is not set. This option must be set to include the nonlinear behaviour of cutoff bars.

[181]: Mass participation factors reported above might be approximate because of the link(s) used.

[The response determined is not affected.]

In models containing links, the mass participation factors calculated could be approximate, if:

• there is a coupling between the translational and rotational mass attached to the links (or link clusters); and
• one of the dependent translational degrees of freedom in the link (or link cluster) is restrained.

This is related to the solver's processing of links via constraint equations and to the choice of dependent and independent degrees of freedom. Due to the decomposition of the matrix of constraints, one or more mass degrees of freedom may be removed from the matrix as it is represented as a function of other degrees of freedom. If the removed degrees of freedom are translational degrees of freedom, the mass participation factors calculated will be approximate.

However, irrespective of the mass participation factors given, in a spectral or harmonic response solution the accuracy of all the other results is not affected.

[182]: End release rotation at beam XXXX is larger than 45 degrees.

This warning is given in geometric nonlinear analysis whenever the end release rotation at the end of a released beam element exceeds 45 degrees. Very large rotations in an iteration of a nonlinear geometric analysis can lead to numerical instability and non-convergence.

[183]: There are XXXX translational and YYYY rotational singularities suppressed.

Check restraints, element property data and connectivity.

The solver will terminate whenever a singularity in the global stiffness matrix is detected, unless the option Suppress All Singularities has been set in the SOLVERS Parameters: GENERAL. If the option is set, this warning is given for all detected and suppressed singularities.

[184]: Pre-consolidation pressure (PC0) is less than in-situ stress for [plate][brick] XXXX - PC0 reset to in-situ stress.

This warning is given when the pre-consolidation pressure (PC0) is less than the in-situ stress. As PC0 should be higher than the in-situ stress, it is set equal to the in-situ stress if it is found to be less.

[185]: Support for beam XXXX is modelled as lumped to consider compression-only attribute.

Subdivide element to obtain better results.

Support attributes on beam elements are normally modelled using the Beam on Elastic Foundation (Winkler) theory, which produces a consistent stiffness matrix for the element and gives exact results even for a single element on an elastic support. When the support attribute is set as compression-only, and a nonlinear solver is used, the elastic support is replaced by equivalent springs lumped at the nodes.

[186]: Restraint condition has changed at node XXXX.

Re-run Natural Frequency solver to get consistent results.

When a natural frequency solution uses the results of a static solution (linear or nonlinear) as its initial conditions (e.g., to include stress stiffening), the same degrees of freedom should be active in both solutions. If they are not, this warning is given.

[187]: [Stress-Strain table is ignored for tapered beam XXXX.][Moment-Curvature tables are ignored for tapered beam XXXX.][Stress-Strain and Moment-Curvature tables are ignored for tapered beam XXXX.]

To consider material nonlinearity in tapered beams, select nonlinear fibre stress beam in property set.

Tapered beam elements do not support the Use Moment vs Curvature tables for bending option specified in the beam property set. If a tapered beam uses this option, and the property set references stress-strain and/or moment-curvature tables, the tables are ignored and the element becomes a tapered beam with linear material. To consider moment-curvature tables, the taper attribute on the element should be removed and the element subdivided with a different cross section and moment-curvature table assigned to each untapered element. Alternatively, the tapered beam can be modelled using the fibre stress option instead of the moment-curvature option.

[188]: Coupling between axial force and bending moments is ignored in beam XXXX - not considered by nonlinear moment-curvature beams.

When moment-curvature tables are used in material nonlinear analysis of beam elements, the principal element stiffness directions (axial, bending in plane 1, bending in plane 2) are all considered to be uncoupled (i.e., independent of each other). To consider coupling, the beam can be modelled using the fibre stress option instead of the moment-curvature option.

[189]: Normal component of plate point force on plate XXXX is ignored - not applicable to [plane stress][plane strain][axisymmetric] elements.

LOAD CASE: "XXXX"

When applying plate point force attributes, which may be defined in 3D, to 2D plate elements (plane stress, plane strain, axisymmetric), only the components in the global XY plane are considered; the out-of-plane component is ignored.

[190]: Plate point moment on plate XXXX is ignored - applicable only to shell elements.

LOAD CASE: "XXXX"

The plate point moment attribute may be applied only to plate/shell elements. If applied to 2D plate elements (plane stress, plane strain, axisymmetric), it is ignored.

[191]: Soil element ([Plate][Brick] XXXX) is used without nonlinear material (MNL) solver option - results might not be correct.

The soil material model is a nonlinear material model. If it is used in material linear analysis, only an initial linear stiffness is assigned and this warning is given.

[192]: Large strain in [plate][brick] XXXX. (Maximum strain component = YYYY).

The Cam-Clay material model is a small-strain, nonlinear material model. If it is used in geometric nonlinear analysis and the strains exceed preset values, this warning is given as results might not be meaningful.

[193]: Geometric nonlinearity is ignored for beam XXXX - not applicable to connection elements.

Connection elements do not support geometric nonlinearity and their lengths have no effect on the stiffness. If they are used in a geometric nonlinear analysis the initial orientation of the element is used no matter how large the displacements become, and this warning is given.

[194]: Non-structural mass normal offset for [beam][plate][brick] XXXX is ignored - mass is projected onto the [beam][plate][brick] in the normal direction.

This warning is given when the in-plane component of the offset in a non-structural mass attribute can be accommodated in the mass matrix while the normal component cannot. This is usually the case for elements that do not include rotational degrees of freedom. For example, for brick elements the offset can only act on the surface of the brick; if the offset includes a component normal to the surface of the brick that component is set to zero and this warning is given.

[195]: Soil fluid bulk modulus (required by undrained soil material) is much lower than bulk modulus of water.

This warning is given if the soil fluid bulk modulus is much lower than the bulk modulus of water. This usually indicates an error in the units used for bulk modulus.

[196]: [Global acceleration should be non-zero when fluid elements are included in the model.] [Global acceleration has not been correctly defined for fluid element (Plate XXXX).]

[For axisymmetric elements, the direction must be global Y.] [For plane strain elements, the direction must be either global X or global Y.]

When fluid elements are used, gravity must be defined correctly because the direction of gravity determines the surface tension contribution (3D brick surfaces and 2D plate edges). For brick elements, gravity must be applied in one of the global XYZ directions. For plane strain elements, it must be applied in either global X or global Y. For axisymmetric elements, it must be applied in global Y, which corresponds to the axisymmetric Z axis. If these conditions are not satisfied, the results might not be meaningful.

[197]: Table contains duplicate X values - [one or more points are removed] [average Y value is used], but this could produce unexpected results.

TABLE NAME: "XXXX"

If a table contains multiple points with the same X value, the way the Y value is interpolated depends on the purpose of the table. For stress-strain, moment-curvature and other tables used for nonlinear elastic materials, only the first point in the set of duplicate points will be kept in the table; subsequent duplicates are removed from the table and therefore this can affect the intended behaviour. For tables that define relationships such as temperature vs time, factor vs position and so on, the average of a pair of duplicate points is used for the interpolation of values coinciding with duplicate X values. Tables with duplicate X values are ambiguous and should be replaced with tables that define a unique Y value over the full range of X values. See Special Topics: How Solvers Use Tables.

[198]: Not used.

[199]: Geometric nonlinearity is ignored for beam XXXX - not applicable to curved pipe elements.

Curved pipe elements do not support geometric nonlinearity. If they are used in a geometric nonlinear analysis the initial orientation of the element is used no matter how large the displacements become, and this warning is given.

[200]: Beam stiffness factors are ignored for beam XXXX - not applicable to nonlinear elements.

The beam stiffness factors are applicable only to linear material analysis.

[201]: Beam stiffness factors on beam XXXX are ignored - not applicable to [spring][cable][truss][cutoff bar][point contact] elements.

The beam stiffness factors are not applicable to all beam element types.

[202]: Torsional stiffness of truss elements is ignored when they are part of a string group (String Group XXXX).

Truss elements are normally used as tension-compression elements, however they also support torsional stiffness when both the shear modulus and the torsion constant are defined and the appropriate option is set in the property set. Truss elements may also be assigned to a string group for modelling string-like behaviour analogous to a string passing through a series of pulleys. When truss elements are part of a string group, the torsional stiffness is ignored.

[203]: Projected distributed force on curved element (Beam XXXX) is applied approximately - refined mesh might be required.

LOAD CASE: "XXXX"

When projected distributed loads are applied to curved beam elements (pipes), the equivalent nodal loads determined could be approximate, depending on the orientation of the element. To check for convergence and accuracy of the solution, the element should be subdivided.

[204]: PCG solution not fully converged within maximum allowable iterations [- cases converged = XXXX of YYYY].

When the PCG option is used, the iterative nature of the solution is such that some load cases might not have converged within the allowable number of iterations. When this occurs, this warning is given. Convergence might be achieved by increasing the number of iterations and re-running the analysis.

[205]: Normal component of plate global edge pressure on plate XXXX is ignored.

When applying plate global edge pressure attributes to 2D plate elements (plane stress, plane strain, axisymmetric), only the components in the global XY plane are considered; the out-of-plane component is ignored.

[206]: PCG option not available for this solver - direct sparse option will be used.

The PCG solver is not available for some of the solvers (e.g., the Natural Frequency and Linear Buckling solvers).

[207]: Calculation of effective time for creep strain hardening has not converged ([Beam][Plate][Brick] XXXX).

Approximate value for effective time will be used.

The creep strain-hardening material model assumes that creep rates are a function of stress, accumulated creep strain and temperature. The numerical implementation of this material model requires the calculation of an effective time that accounts for these various factors. If the calculation of the effective time does not converge, an approximate value for the effective time will be used.

[208]: [Plate][Brick] XXXX contains invalid (er,pr) data for void ratio calculation.

Void ratio set to er=XXXX.

If invalid data has been defined for void ratio calculations, a valid void ratio is automatically assigned and this warning is given.

[209]: Insufficient RAM for efficient PCG solution (Require XXXX MB. Allocated YYYY MB).

If the amount of RAM required for an efficient PCG solution cannot be allocated, this warning is given and the solver continues by using the hard drive as temporary storage. This will usually impact run time significantly.

[210]: Zero diagonal in global matrix.

A zero diagonal has been detected in the global stiffness matrix during the PCG solution.

[211]: Non-structural mass offset for [beam][plate][brick] XXXX is ignored in element mass matrix.

To offset non-structural mass attributes normal to the surface of an element, the element must support rotational degrees of freedom at its nodes because the offset operation accounts for the offset by coupling translational and rotational degrees of freedom. If the element does not support rotational degrees of freedom (e.g., a 3D membrane element), the offset is ignored and this warning is given.

[212]: Not used.

[213]: Average temperature used for thermal expansion in fluid element ([Beam][Plate][Brick] XXXX).

Similarly to pre-load attributes, thermal expansion in fluid elements may be applied only in an average way. The average nodal thermal strain will be applied over the whole element when node temperature is included.

[214]: Default range for number of viscoelastic units could not be accommodated. The number of viscoelastic units used is XXXX.

The solver parameters for creep analysis (SOLVERS Parameters: CREEP) provide the solver with a hint as to the range (min/max) of viscoelastic units to be used to represent the required creep law behaviour. If the number of units used by the solver is outside the range, this warning is given.

[215]: Nonlinear behaviour of soil [cannot be predicted with a linear solution][is ignored by this solver].

Use [Nonlinear Static][Nonlinear Transient] solver to consider nonlinear soil behaviour.

This warning is given whenever a solver that does not consider material nonlinearity is used to run a model with soil elements, or a solver that can consider material nonlinearity is run with the MNL option not set.

[216]: Pre-strain effect of in-situ stress on soil elements is ignored by this solver.

The in-situ stress attributes are ignored by all the linear solvers as the pre-strain effect of soil elements cannot be considered in a linear analysis. A nonlinear solver should be used to consider the effect.

[217]: Friction model for point contact (Beam XXXX) set to Rectangular because one of the friction coefficients is zero.

The elliptical yield surface of a friction model cannot be defined with only one non-zero friction coefficient.

[218]: Invalid Pipe Flexibility Factor in beam property XXXX is ignored.

The Flexibility Factor for pipe elements must be greater than zero. Zero or negative values will be ignored (i.e., a Flexibility Factor of 1.0 will be used unless it is greater than zero).

[219]: Prescribed displacement component(s) at node XXXX reference(s) two or more different UCS.

The restraint is converted to global Cartesian because the components could generate a conflict.

This warning is given when enforced displacement attributes from multiple freedom cases applied simultaneously reference conflicting UCS. For example, in general it is not possible to satisfy both a Cartesian and a cylindrical UCS. The enforced displacements and their UCS should be reviewed and made consistent.

[220]: Calculation of effective time for creep strain hardening has failed ([Beam][Plate][Brick] XXXX).

Time hardening model will be used for current iteration.

The creep strain-hardening material model assumes that creep rates are a function of stress, accumulated creep strain and temperature. The numerical implementation of this material model requires the calculation of an effective time that accounts for these various factors. If the calculation of this effective time fails, the solver will temporarily revert to a time-hardening model. A failure to calculate an effective time for the strain-hardening model could be due to sudden changes in stress levels or extremely high creep strain rates, and may indicate that smaller time steps are required.

[221]: Zero inertial accelerations were generated for case XXXX.

This warning is given by the Inertia Relief option of the Linear Static solver whenever the applied loads are self-balancing or when the solution of the matrix that calculates the accelerations fails.

[222]: Response variable: XXXX is ignored - not supported by the selected element ([Beam][Plate][Brick] XXXX).

This warning is given by the Load Influence solver whenever a response variable applied to an element is not supported (e.g., moment response on plane stress element).

[223]: Laminate plate property XXXX has zero transverse shear stiffness. Transverse shear stiffness has been assigned as equivalent isotropic values.

This warning is given when laminates are used in thick plate/shell analysis (Quad8, Quad9, Tri6) and the transverse shear stiffness is calculated to be zero. The thicknesses of the plies and their transverse shear terms (e.g., the G13 and G23 moduli) should be checked for errors. Equivalent isotropic values will be used when this warning is given.

[224]: Plate property XXXX has zero transverse shear stiffness.

This warning is given when non-isotropic thick plate/shells (Quad8, Quad9, Tri6) are used (laminates excluded) and the transverse shear stiffness is zero. For thick plate/shell elements, a zero transverse shear stiffness is not allowed, so a value corresponding to an equivalent isotropic material is used. The thickness and transverse shear modulus terms in the property data should be checked.

[225]: [Node][Beam][Plate][Brick] XXXX is below the reference elevation - its seismic mass is ignored.

CASE NAME: "XXXX"

This warning is given when elements at or below the reference elevation are detected in a Seismic Load Case. Masses at or below the reference elevation are included in the calculation of the total structural mass. The product of total mass of the structure, the gravity and the base shear factor will yield the total amount of lateral load (seismic base shear). The total lateral load is only distributed and applied to the elements that are above the reference point. That is, seismic mass below the reference elevation does not generate lateral force. For a consistent model with seismic loading, the reference elevation should be the same as the elevation of the restrained nodes; in this case, there is no ambiguity about the mass.

[226]: Global matrix contains large pivot ratios - this could indicate an ill-conditioned problem.

Pivots are diagonal entries in the stiffness matrix that are used as quotients during the factorisation process. If the ratio between the largest and the smallest pivot is greater than 1E16, this warning is given since such large ratios usually indicate an ill-conditioned matrix. The pivots are reported in the solver log file.

[227]: Elastic-plastic table contains gradients larger than E0 - one or more points are ignored.

TABLE NAME: "XXXX"

For elastic-plastic type material tables, the largest gradient must be through the origin (i.e., E0). If the gradient anywhere else is greater than E0, the table is automatically modified to remove those higher gradients, and this warning is given. The automatic adjustment of the table usually produces reasonable results for the case where only small violations of the gradient requirement exist. However, it is better to correct the table so that the analysis does not need to rely on this automatic modification.

[228]: [Support for beam XXXX is modelled approximately due to geometric nonlinearity and/or staging - refined mesh might be required.] [Support for beam XXXX is modelled approximately due to geometric nonlinearity in initial solution - refined mesh might be required.]

In nonlinear geometry analysis (and staged analysis), support attributes applied to beam elements do not use the exact Winkler formulation. Instead, an approximate support stiffness is modelled based on the beam element's cubic shape functions. To check for convergence and accuracy of the solution, the element should be subdivided.

[229]: Minimum arc length has been reached - no further reduction will be applied to this sub-step.

This warning is given when Displacement Control (Arc Length) is used and the minimum arc length reduction factor has been reached. The minimum arc length reduction factor is specified in SOLVERS Parameters: SUB-STEPPING (Static). If the minimum arc length reduction factor is reached and the solution has still not converged, the solver continues to iterate at this arc length level until the maximum number of iterations has been reached.

[230]: [Link type] (Link XXXX) might be inhibited by fixed nodal [restraints - this could also affect convergence][temperatures].

This warning is given in situations where links are connected to nodes with restraints that inhibit the intended behaviour of the link. This can result in ill-conditioning in geometry nonlinear analysis and could also impact on the convergence. For example, a pinned link parallel to the global X axis with DX fixed at both ends is effectively a redundant link in geometric linear analysis; in geometric nonlinear analysis it can be the source of ill-conditioning. When the link is in its initial orientation, it is not possible to formulate constraint equations since the only active degrees of freedom on the link (DX in this case) are not available in the global matrix (since it is horizontal, the link behaviour cannot be described in terms of its DY degrees of freedom). If during subsequent iterations the link nodes move such that the link is no longer parallel to the global X axis, it is theoretically possible to formulate equations on the link in terms of the DY degrees of freedom. However, as the link is rigid, it will attempt to iterate back to its original length during the iteration process, and as it gets closer to its initial (horizontal) orientation, the DY coefficients in the link equations approach zero. There are many similar situations that could occur.

[231]: Not used.

[232]: Data in user defined creep table might be invalid - negative gradient found.

This warning is given when the user-defined creep tables describe a relationship such that an increase in temperature or an increase in stress reduces the creep rate. This is not an expected behaviour for typical engineering materials so usually it means that there is an error in the tables defining the user-defined creep.

[233]: Pre-strain on point contact (Beam XXXX) is ignored - not applicable to [Zero Gap][Takeup Gap] type.

Zero Gap and Takeup Gap contact elements do not support pre-strain attributes.

[234]: Pre-strain z-component on plate XXXX is ignored - only applicable to axisymmetric plates.

This warning is given when the applied local z pre-strain attribute is invalid. This attribute is applicable only to axisymmetric elements.

[235]: Pre-stress z-component on plate XXXX is ignored - applicable only to plane strain and axisymmetric elements.

This warning is given when the applied local z pre-stress attribute is invalid. This attribute is applicable only to plane strain and axisymmetric elements.

[236]: Lateral [translational][rotational][translational and rotational] degrees of freedom have been suppressed for beam XXXX.

This warning is given when a truss, spring or cutoff bar is parallel to one of the global axes and is lacking lateral support. Those lateral degrees of freedom, including rotations, are automatically suppressed to avoid singularity in linear analysis. For example if a properly connected truss element is subdivided into two, the intermediate node will form a pinned connection; if the intermediate node is not connected to other elements for lateral support, all relevant degrees of freedom are suppressed at that node, and this warning is given. This suppression is not performed for geometric nonlinear analysis.

[237]: Default freedom conditions appear to be over-constrained - one or more elements might require additional freedoms.

Some element types require specific degrees of freedom to function properly. For example plate/shell elements require rotations to bend into shape and therefore all six global degrees of freedom should be generally available. If these required degrees of freedom are globally restrained under CASES: Freedom Cases, this warning is given.

[238]: Enforced displacements applied in a spherical or toroidal UCS.

When both DT and DP are enforced, results might be dependent on load step (or sub-step) size.

This warning is given in nonlinear geometry problems whenever enforced displacements are defined on a spherical or toroidal UCS and both DT (theta-translation) and DP (phi-translation) are enforced. In these coordinate systems, the order of displacements is important. For example in a spherical system where R=1000 mm, translating along the equator by a single 500 mm arc increment, followed by translating towards one of the poles by a single 500 mm arc increment, will reach a coordinate of (T=28.65 deg, P=28.65 deg). Translating in five equal increments of 100 mm in both azimuth and polar directions will result in a different final coordinate of (T=29.55 deg, P=28.65 deg). This is because as the incline angle increases the azimuthal movement of the same amount covers a wider angle.

[239]: Excessive drilling moment detected at plate XXXX.

This warning is given when the drilling rotation of Tri3 shell elements is too large due to an attempt to transfer a point moment via the drilling degree of freedom. This can happen in linear buckling analysis, and in natural frequency analysis with initial conditions specified. A common cause of this is when a beam or a link is connected normal to the Tri3 element and the moment transferred is too large for the element's in-plane behaviour to accommodate. The moment is usually better transferred via a cluster of beams in the plane of the plate.

[240]: Reduced integration has been used in plate element XXXX - this could lead to unexpected behaviour.

This warning is given when the reduced integration option is used for plane stress, plane strain or axisymmetric plate elements. In certain situations, reduced integration may improve convergence in material nonlinear analysis but it may also potentially produce singular models.

[241]: Nonlinear material (MNL) status is different to the initial file - this could lead to unexpected behaviour.

This warning is given when the solution restarts into the same solution type but the nonlinear material MNL setting has been changed. For example, this can occur when restarting a nonlinear static solution with MNL turned on from a nonlinear static initial condition file that was solved with MNL turned off. This may produce unexpected results.

[242]: Loads on beam XXXX converted to lumped loads due to support.

This warning is given in the following situations:

• Very high support to beam bending stiffness ratio is detected (Warning[134]:Support for beam XXXX is modelled as lumped due to very high support/beam stiffness ratio.).
• Nonlinear material is considered for beams with support (Warning[137]: Support for beam XXXX is modelled as lumped due to material nonlinearity.).
• Curved beam element with support is used (Warning[144]: Support on curved element (Beam xxx) is modelled as lumped.).
• Compression-only beam support is used (Warning[185]: Support for beam XXXX is modelled as lumped to consider compression-only attribute.).
• Beam element with support is used in nonlinear geometry or in staged analyses (Warning[228]: [Support for beam XXXX is modelled approximately due to geometric nonlinearity and/or staging - refined mesh might be required.] [Support for beam XXXX is modelled approximately due to geometric nonlinearity in initial solution - refined mesh might be required.]).
• The beam is a user-defined beam (Warning[243]: Support on user-defined beam (Beam XXXX) is modelled as lumped.).
• Tapered beam element with support is used (Warning[245]: Support on tapered element (Beam XXXX) is modelled as lumped.).
• Bending stiffness (EI) of the element is zero.

Loads on beam elements with support will be converted to lumped loads. The beam element should be subdivided to improve the accuracy of the results.

[243]: Support on user-defined beam (Beam XXXX) is modelled as lumped.

The Winkler formulation is not available for user-defined beams. The support is modelled as lumped springs at the nodes.

[244]: Geometric nonlinearity is ignored for user-defined beam elements (Beam XXXX).

User-defined beam elements do not support geometric nonlinearity. If they are used in a geometric nonlinear analysis the initial orientation of the element is used no matter how large the displacements become, and this warning is given.

[245]: Support on tapered element (Beam XXXX) is modelled as lumped.

Subdivide beam element to obtain better results.

The Winkler formulation is not available for tapered beams. The support is modelled as lumped springs at the nodes.

[246]: Table for shrinkage strain does not pass through (0,0) - shrinkage will be offset by value at time=0.

TABLE NAME: "XXXX"

Shrinkage strain for concrete creep materials must be zero at time = 0. If it is not, the values in the table are offset by the value at time=0.

[247]: Too many modes might have been requested - very small mass terms have been included in working set.

Fewer modes should be requested, or mesh should be refined if more modes are required.

The total number of mass degrees of freedom in the mass matrix dictates the maximum number of frequency modes that can be calculated, and therefore the maximum size of the Subspace. A mass degree of freedom is deemed to be one that has a non-zero mass entry in the diagonal of the mass matrix. In some cases, due to numerical round-off, mass matrix diagonals that should be zero produce very small positive values. It can be difficult to filter these from the real mass terms. If the Subspace is artificially expanded on the basis of these very small (practically zero) mass terms, the iterative procedure may not be efficient and may even fail to converge. If this warning is given, the mesh should be refined, or the number of modes requested should be reduced.

[248]: Support for beam XXXX is modelled approximately due to lumped loads - refined mesh might be required.

If lumped loads have been requested for beam elements (see SOLVERS Parameters: ELEMENTS) or they have been set for the element automatically for any reason, support stiffness on the element cannot be modelled using the exact Winkler formulation, and therefore it reverts to an approximate representation with springs lumped at nodes. To check for convergence and accuracy of the solution, the element should be subdivided.

[249]: Temperature effects generate infinite creep stiffness in [beam][plate][brick] XXXX - creep or temperature data might be invalid.

When temperature effects are included in concrete creep materials, the creep rate will be modified according to the parameters presented in the Concrete Creep and Shrinkage - Temperature Effects. If the temperature dependency equation cannot be evaluated, this warning is given.

[250]:[Radius difference at nodes of sector-symmetry link (Link XXXX) exceeds 0.1%.]

[Local Z axis difference at nodes of sector-symmetry link (Link XXXX) exceeds 0.1%.]

The corresponding positions at two ends of a sector-symmetry link should be exactly on the respective sectors, they should have the same radius and the same Z ordinates. If the radii or the Z ordinates of the two ends differ by more than 0.1%, this warning is given.

[251]: Number of links is different to number contained in restart file - this might invalidate link results in previous steps.

For a restart, the model must contain the same number of nodes, beams, plates and bricks as were contained in the model that produced the restart file. An exception is made for links to allow for the possibility of adding or removing links in the continuing analysis. If this feature is used, extra care is required to ensure that the changing number of links from result case to result case does not produce unwanted effects.

[252]: Shear centre offsets in beam XXXX are ignored due to support.

When a beam element uses a support attribute, the shear centre on the cross section is ignored.

[253]: Offset at plate XXXX is ignored.

Plate offsets are applicable only to plate/shell elements. If applied to other plate types, the offset is ignored and this warning is given.

[254]: Bubble function not used in brick XXXX due to high element aspect ratio.

The performance of the Hexa8 brick elements in structural analysis is enhanced by the addition of extra internal degrees of freedom, known as the bubble function degrees of freedom. Before the element stiffness matrix can be added to the global stiffness matrix, the bubble degrees of freedom are condensed and their influence is added to the nodes of the element. During the condensation process, a matrix is inverted. If the matrix inversion cannot be undertaken due to a high element aspect ratio, the bubble function is not added to the element and this warning is given.

[255]: Bubble function in brick XXXX might not be accurate due to high element aspect ratio.

The performance of the Hexa8 brick elements in structural analysis is enhanced by the addition of extra internal degrees of freedom, known as the bubble function degrees of freedom. Before the element stiffness matrix can be added to the global stiffness matrix, the bubble degrees of freedom are condensed and their influence is added to the nodes of the element. During the condensation process, a matrix is inverted. If the matrix inversion process involves large pivot ratios indicating an ill-conditioned matrix due to a high element aspect ratio, the bubble function is still added to the element and this warning is given.

[256]: [Beam][Plate][Brick] XXXX is partially below the reference elevation - some of its seismic mass is ignored.

This is similar to Warning[225]: [Node][Beam][Plate][Brick] XXXX is below the reference elevation - its seismic mass is ignored. except that it applies when the element is partially below the reference elevation. Seismic mass below the reference elevation does not generate lateral force.

[257]: UCS directions for [restraint at node][material axes at brick][mass at node][stiffness at node][damper at node][influence at node][influence at brick][end 1 of beam][end 2 of beam][one or more nodes on link] are undefined - directions revert to global Cartesian.

For non-Cartesian coordinate systems, directions can be undefined at singular points (for example, at the poles of a spherical coordinate system). In that case, the axes revert to the global Cartesian directions.

[258]: Current yield criterion for beam property XXXX is different to the criterion in the initial file.

This could produce invalid results.

This warning is given when a nonlinear material beam uses a different yield criterion to that used to produce the initial conditions file.

[259]: In linear analysis, thermal load on cable elements cannot be applied (Beam XXXX).

In linear analysis, temperature effects normally add the element forces to the load case that produce the equivalent element strain. For cable elements the temperature effects in linear analysis are not used to produce load. They are used only to establish an effective cable length so that its stiffness, under the action of gravity, can be determined for addition to the global stiffness matrix.

[260]: In linear analysis, pre-strain on cable elements is used only to change the cable free length (Beam XXXX).

This is the pre-strain equivalent of Warning[259]: In linear analysis, thermal load on cable elements cannot be applied (Beam XXXX).

[261]: Global distributed force on cable (Beam XXXX) is converted to equivalent uniform load.

Cable elements support uniformly distributed force applied in the global axis directions. If a non-uniformly distributed force is applied, the average uniformly distributed force is applied instead, and this warning is given.

[262]: Non-uniform distributed mass on cable (Beam XXXX) is converted to equivalent uniform mass.

Cable elements support uniformly distributed mass applied along their length. If a non-uniformly distributed mass is applied, the average uniformly distributed mass is applied instead, and this warning is given.

[263]: Initial temperature at node XXXX is not consistent with initial temperature on all nodes of the link.

When links are used in heat transfer analysis, a link cluster enforces the same temperature at all nodes of the cluster (unless a multi-point link with a constant term is used). If the initial node temperatures at the nodes of the link cluster are not all the same, the distribution is not consistent with the condition imposed by the links. The inconsistent initial conditions will not be maintained as the cluster must produce the same temperature at each node during the analysis.

[264]: Pre-curvature on non-bending plate XXXX is ignored.

Plate pre-curvature attributes are applicable only to plate/shell elements. If applied to other plate types, the attribute is ignored and this warning is given.

[265]: Pre-curvature on beam XXXX is ignored - attribute applies only to beam and straight pipe.

Beam pre-curvature attributes are applicable only to normal beams and straight pipes. If applied to other beam types, the attribute is ignored and this warning is given.

[266]: Global matrix contains excessively large pivots - this could indicate an ill-conditioned problem.

If this warning is given it is likely that there has been a numerical overflow during the factorisation of the global stiffness matrix. The model, all element properties and tables should be checked. If the analysis is a nonlinear one, it is likely that divergence has occurred somewhere (such as the stiffness of Dynamic Stiffness Point Contacts becoming excessively large).

[267]: No freedom cases have been included - this could produce global rigid body motion.

This warning is given by the Nonlinear Static and Quasi-static solvers when no freedom cases have been included in the load table (see SOLVERS: Load (Nonlinear Static) and SOLVERS: Load (Quasi-static)). This will almost always produce an unstable problem that is unlikely to converge.

[268]: Inertia relief accelerations do not balance applied loads precisely - check applied loads and restraints.

For inertia relief analysis, a vector of global linear and angular accelerations is calculated that, when applied to the mass matrix, produces a load vector whose resultant balances the resultant of the applied loads. In most cases, this procedure produces sufficiently well balanced loads such that the total summation vector is near zero (see Special Topics: Inertia Relief Analysis). This warning is given when the total summation vector is not near zero, which could indicate that the model does not enable the required free body movements to be represented (e.g., there are spurious restraints or node stiffness attributes or element support attributes).

[269]: Combination generation failed - generate the combinations from the post-processor.

The Linear Static solver allows for the linear load case combination file to be generated during the execution of the solver, instead of as an operation performed by the post-processor when opening the result file (see SOLVERS: Load (Linear Static and Load Influence)). If the solver combination procedure fails, the combinations should be attempted using the post-processor as this will provide additional diagnostic messages.

[270]: [Plate stiffness factors are ignored for nonlinear element (Plate XXXX).][ Plate stiffness factors are ignored for rubber element (Plate XXXX).][ Plate stiffness factors are ignored for non-isotropic element (Plate XXXX)]. Mass factors are considered.

The plate stiffness factors attribute is applicable only to linear isotropic plate elements. If applied to other plate element types, they are ignored and this warning is given.

[271]: Lower bound has been exceeded in table - [a zero value will be used][an extrapolated value will be used][end value will be used].

This warning is given whenever the evaluation of a table is required at an X value lower than the minimum X value defined in the table. See Special Topics: How Solvers Use Tables.

[272]: Upper bound has been exceeded in table - [a zero value will be used][an extrapolated value will be used][end value will be used].

This warning is given whenever the evaluation of a table is required at an X value higher than the maximum X value defined in the table. See Special Topics: How Solvers Use Tables.

[273]: Table range does not cover [Solver Defaults] Creep Curve Fit Time - end values will be used.

This warning is given when the creep definition is not defined over the full Creep Curve Fit Time specified in SOLVERS Parameters: CREEP Either of the two should be adjusted to make them consistent.

[274]: Table missing strain value at time zero - point at (0,0) is assumed.

When Strain vs Time tables are used to define creep material behaviour, they should have a point at (0,0) - that is, creep strain is zero at time zero. If the point is missing, the solver will automatically insert it. However, the data should be reviewed and corrected.

[275]: Node temperature attributes are ignored by this solver in terms of load excitation.

The Harmonic Response and Spectral Response solvers do not support nodal temperature as harmonic or spectral loads - these are ignored as external loads. However, their effects in terms of stress softening/stiffening on a structure are included by the use of an initial conditions file in the Natural Frequency solver.

See Also

• Notes, Warnings and Errors