# Error Message Database

This section is comprised of error messages in ascending numerical order.

## #1 through #99

### Error 41

`CBAR/CBEAM - Invalid Orientation Vector (zero length or parallel to the
element axis)`

This error may be printed when a
CBAR/CBEAM element in the model has an
invalid orientation vector. Orientation vector is used in conjunction with the
elemental X-axis to define the elemental Y- and Z-axes. Therefore, the
orientation vector should be non-zero in length and should not be parallel to
the elemental X-axis (line connecting `GA` and
`GB`).

- The orientation vector can be defined via
`X1`/`X2`/`X3`or`G0`. In the case of`X1`,`X2`,`X3`, make sure they are all not 0.0. If`G0`, then check to make sure`G0`is not set the same as`GA`. - Depending on the
`OFFT`field, verify the grid coordinate system of grid A (`GA`) and/or the definition of`X1`/`X2`/`X3`with regard to the basic system.

## #100 through #299

### Error 114

`Preloading in subcase # must come from a static subcase. Specified preloading
subcase # is not a static subcase`

Preloading currently is supported for only static loadcases in OptiStruct.

Check if the preloading is specified from a static load case as only preloading from static subcase is supported.

### Error 115

`Preloading not supported for nonlinear subcases`

Preloading can be defined as the pre-stress generated in the structure prior to the analysis of interest.

Preloading is supported only for linear subcases.

### Error 116

`Nested preloading not allowed but encountered in Subcase #. Preloading Subcase
# itself has preloading from Subcase #`

Preloading can be defined as the pre-stress generated in the structure prior to the analysis of interest. Preload/ Prestressing in OptiStruct is supported in linear static and nonlinear quasi-static loadcases with both large and small displacement types. Nested preloading is if Subcase C has preloading from Subcase B, which in turn has preloading from Subcase A.

Avoid nested preloading/prestressing loadcases.

### Error 118

`# AMSES/AMLS eigenvalue analysis may error out if preloading is higher than
first critical buckling load`

The first critical buckling load is load at which buckling occurs. If preload is higher than the critical buckling load, then there is a possibility that the structure might be already buckled due to the preload.

For any modal subcase (Modal frequency response analysis, Normal mode analysis), the preload should be less than the first critical buckling load.

### Error 153

`Exactly zero pivoting encountered during Numerical Factorization`

- Insufficiently constrained model
- Having rigid body mechanisms within the model
- Extremely ill-conditioned rigid element sets
- Extremely thin shells (as used for skinning) that have MID2/MID3
- Gap elements with extremely high stiffness (KA, especially KT or MU)

- MECHCHECK may be used to find the rigid body modes. To do
so, change the input to be an eigenvalue analysis and add
MECHCHECK. Warning: Results obtained with MECHCHECK cannot be used because the model is changed internally.
- Check the model and rerun the problem.

### Error 156

`No mode exists in the interval specified`

For any modal analysis, the range of frequency V1 and V2 or number of roots desired can be specified. If the specified range is small or the roots of the model do not exist in the range, then Error 162 occurs.

- Check the EIGRL card for the lower and upper bounds (V1 and V2) specified in the model.

### Error 157

`Error opening the scratch file <filepath>./filename.rs~.`

This error may be caused if sufficient disk space is unavailable on the machine or if access rights to open the file is not granted, or due to other system setup related issues. This also may possibly be caused by real time protection by antivirus.

- Use the TMPDIR I/O Options Entry,
`OS_TMP_DIR`

environment variable, or the`-tmpdirrun`

option to reference a scratch directory at a location with full read and write permissions. Additionally, make sure that the path where the job is run does not contain too many characters, which possibly goes beyond the allowable system limit. - Try to update the operating system, if running on Windows.
- Disable real time protection, and add an exception, for files with the extension .rs~ and OptiStruct related files (.fem, and so on).

### Error 160

`Gram-Schmidt reorthogonalization did not converge`

This error indicates that a massless mechanism may exist in the model. This is caused by ill-conditioning of the shifted matrix in Lanczos run. (example: zero lower bound specified for a model with rigid body modes).

- Run Normal Modes Analysis and look for Rigid Body Modes. If a Normal Modes Analysis run also fails, rerun the model using MECHCHECK (results of a MECHCHECK analysis are for testing purposes only and may be inaccurate).
- If massless mechanisms are found, additional constraints on the model may be required or the massless mechanisms may need to be removed for the model to run.

### Error 162

`No mode exists in the interval specified`

For any modal analysis, the range of frequency
`V1` and `V2` or number of roots desired
can be specified. If the specified range is small or the roots of the model do
not exist in the range, then Error 162 occurs.

- Check the EIGRL card for the lower and upper bounds
(
`V1`and`V2`) specified in the model.

### Error 163

`Too many vibration modes exist in the range of interest.`

This error happens as there are more than 500 eigenvalues calculated internally in the range of interest. The solver may require manual input to help targeting the frequency region of the desired modes.

- Narrow the range of interest by adjusting the lower and upper bounds.
- Fill the
`SHFSCL`entry in EIGRL card with the frequency of the (estimated) lowest mode.

### Error 164

`Too many buckling modes exist in the range of interest`

This error happens as there are more than 500 eigenvalues calculated internally in the range of interest. The solver may require manual input to help targeting the frequency region of the desired modes.

- Narrow the range of interest by adjusting the lower (V1) and upper (V2) bounds in the EIGRL card.
- Fill the
`SHFSCL`entry in EIGRL card with the frequency of the (estimated) lowest mode. Use of`SHFSCL`entry improves the performance of the buckling analysis especially when the applied load differs from the first buckling load by orders of magnitude.

### Error 165

`Gram-Schmidt re-orthogonalization did not converge.`

This error indicates that a massless mechanism may exist in the model, during Buckling Analysis

- Run Normal Modes Analysis and look for Rigid Body Modes. If any exist, there are massless mechanisms in the model.
- If a Normal Modes Analysis run also fails, rerun the model using MECHCHECK (results of a MECHCHECK analysis are for testing purposes only and may be inaccurate).
- If massless mechanisms are found, additional constraints on the model may be required or the massless mechanisms may need to be removed for the model to run.

### Error 166

`Three numerical factorizations in a row failed`

The error occurs when there are rigid body modes in the model in the buckling analysis.

- Small negative roots are usually computational zeros, indicating rigid body modes. Finite negative roots are an indication of modeling problems.
- It is recommended that
`V1`(lower bound in EIGRL card) not be set to zero when extracting rigid body modes. - Use a vibration eigenvalue loadcase to find the rigid body mode.

### Error 167

`Repeated factorization failure due to panel limitations on
pivoting`

This error occurs when panel size is small as the default panel size is internally determined based on the model. Zero diagonals in unpivoted factorization is caused due to singularities in stiffness matrix.

- Use card PARAM,
`PNLSIZ`to increase the panel size to the required value for the model. A larger panel size helps stabilize the factorization of an indefinite stiffness matrix. - Running Normal Modes Analysis or Linear Static Analysis by adding MECHCHECK helps detect the massless mechanisms.

### Error 168

`Repeated factorization failure encountering exact zero diagonals in unpivoted
factorization`

Zero diagonals in unpivoted factorization is caused due to singularities in stiffness matrix.

The stiffness matrix is solved by
formulation type `A`= LDLT; where
L is lower triangular matrix, D is
diagonal matrix and LT is lower triangular matrix transpose;
but, if the diagonal elements of the stiffness matrix reduce to zero, leading to
failure to solve the stiffness matrix. Therefore, the method of pivoting is used
to reduce the instabilities in the elimination method used to solve the
stiffness matrix.

- Running Normal Modes Analysis or Linear Static Analysis by adding MECHCHECK helps detect the massless mechanisms.
- Check the model for any modelling errors.

### Error 169

`Improperly posed generalized symmetric eigen problem - matrix specifying norm
must be positive (semi-)definite, but it is indefinite`

For Buckling Eigenvalue Analysis, the stiffness matrix should be positive definite.

- For pre-loaded buckling analysis, the pre-load may have already caused the structure to buckle.
- If determine the modeling issue (like connections, constraints, element quality) it is suggested to run a normal modes analysis.

### Error 173

`A dependent d.o.f. defined more than once in rigid element entry`

The degrees of freedom of the grid point is referenced as dependent by two different rigid elements. This causes double dependency.

Node (grid point) cannot be dependent on two rigid elements with same DOF.

User can try to recreate rigid elements connecting the node (grid point) with different DOF’s for each rigid element connecting the node. Example, connect the node with one rigid element having 123 dof’s and another rigid element with 456 dof’s.

### Error 174

`A dependent d.o.f. defined more than once in an MPC set`

When a node (grid-point) in an MPC set (equation) is referenced as dependent dof more than once.

To avoid double dependency issues with MPC
sets, their dependent degrees-of-freedom may be converted to independent
degrees-of-freedom when conversion is necessary for the model to run. This
conversion can be used if the dependent degree-of-freedom of a rigid element is
a dependent degree-of-freedom of another constraint equation (may come from an
MPC equation or another rigid element). This conversion from dependent to
independent degrees-of-freedom is done automatically when
PARAM, `AUTOMSET`, YES
is specified in the input data.

### Error 175

`A dependent d.o.f. defined more than once in an MPC set and rigid
elements`

When a node (grid-point) in an MPC set (equation) is referenced as dependent dof more than once or it is also referenced by a rigid element along with being referenced in a MPC set.

To avoid double dependency issues with MPC
sets, their dependent degrees-of-freedom may be converted to independent
degrees-of-freedom when conversion is necessary for the model to run. This
conversion can be used if the dependent degree-of-freedom of a rigid element is
a dependent degree-of-freedom of another constraint equation (may come from an
MPC equation or another rigid element). This conversion from dependent to
independent degrees-of-freedom is done automatically when
PARAM, `AUTOMSET`, YES
is specified in the input data.

### Error 176

`A dependent d.o.f. of rigid elements is constrained in an SPC set`

SPC applied on the node (grid-point) with dependent DOF specified for the rigid element.

Select the independent node (grid-point) and avoid the dependent dof of the rigid element.

### Error 177

`A dependent d.o.f. of an MPC set is constrained in an SPC set`

A dependent DOF of an MPC set is constrained in an SPC set.

Select the different node (grid-point) and avoid the dependent dof of the MPC set.

### Error 179

`The dependent d.o.f’s of multi-point constraints produces a singular
matrix`

In MPC set, if one grid point is made to be dependent on grid point two and grid point two is dependent on grid point three and then making the grid point three dependent on grid point one causes the grid point one dependent on itself or creating the circular dependency in MPC constraint set.

Circular dependency in MPC set should be avoided by selecting the dependent DOF appropriately.

### Error 273

`Available Working Storage Insufficient`

This error can occur in a run with insufficient working storage (RAM).

- Try to force in-core solution using
`-corein`

. - Disable dynamic memory allocation and set the total allowable static RAM
using
`-fixlen`

.

## #300 through #599

### Error 312

`In static load case # the compliance is negative or large xxx.
Optimization/buckling analysis cannot be performed due to
possible rigid body mode`

Large compliance means the model has huge displacements compared to model size. This error occurs when a model is under constrained or incorrect material property definition or contact definitions are incorrect or missing.

There is a possibility of rigid body mode in the model which can lead to negative or large static compliance. Check the model for constrains, material properties assigned, and contacts & contact definitions are defined appropriately.

### Error 326

`<cmdname>RBE3</cmdname> element # cannot support a x-force -
check element data.`

This error indicates that the independent degrees of freedom of the RBE3 are not able to transmit forces applied in the X direction in a model containing improperly constrained RBE3 elements.

- Find all RBE3 elements in the model and look for improperly constrained independent grid points.
- If the forces are not transmitted in the X direction,
add component 1 to the list of degrees of freedom
(
`Ci`field) for the independent grids on the improperly constrained RBE3.

### Error 338

`Singularity during Gaussian elimination for rearranging constraint
equations in RBE3 element part xxx`

This error occurs probably because the
`UM` DOF do not remove all six
rigid body modes.

`UM` DOF options
for RBE3 elements lets user apply a SPC
to the dependent DOF on the RBE3 element.
This is done by taking nodes from the independent set and
typing them back into the MPC to allow the dependent node to
be constrained.

- PARAM,
`AUTOMSET`, YES option instead of`UM`option manually for RBE3. - From OptiStruct 2018.0
version onwards, by default the
PARAM,
`AUTOMSET`, YES is switched on.

### Error 339

`The dependent d.o.f. is constrained by grid or spc
data`

SPC applied on the node (grid-point) with dependent DOF specified for the rigid element.

The dependent node is constrained with SPCs which is not valid. Instead, constrain the independent node.

## #600 through #999

### Error 703

`Number of design variables = #, Number of constraints = #, Error
code from optimizer = #. The optimizer failed to find a
solution of the optimization problem at the current
iteration`

This is an error inside the optimizer.

- Try to switch to a different optimizer using DOPTPRM,OPTMETH.
- Contact OS support to report this issue with a copy of the exact error reported.

### Error: Programming Error - Generic

Generic

This error occurs if there is a Programming Error in OptiStruct.

- Contact OptiStruct support

### Error 711

`An unconstrained rigid body rotation in the rigid
element.`

The RBAR has some of the DOF in 456 directions unconstrained (123 DOF is dependent on the DOF of solid element its connected). When RBAR connects two solid grids, it is free to rotate along its axis as solid element has DOF only in 123 directions.

- Consider the RBAR with only DOF in 123.
- Add the SPC at the solid element node (solid grid) with 456 DOF arrested.

### Error 712

`An unconstrained rigid body rotation in the rigid element. This
RBAR is free to rotate about its axis.`

The RBAR has DOF’s in 456 directions unconstrained and can rotate about its axis.

- Consider the RBAR with only DOF in 123.
- Add the SPC at element nodes with 456 constrain to arrest 456 DOF.

### Error 713

`An unconstrained rigid body rotation in the rigid element. This
RBE2 is free to rotate about its axis.`

The RBE2 has DOF’s in 456 directions unconstrained and connected to an element with nodes (grid point) having DOF only in 123 directions.

- Consider the RBE2 with only DOF in 123.
- Add the SPC at element nodes with 456 constrain to arrest 456 DOF.

### Error 723

`An invalid rigid element. This RBE2 is not connected with any
structural element`

The one or both ends of the rigid element is/are not connected to any node(s) associated with the structural element. This causes one or more ends of the RBE2 element to be free.

Check for any rigid elements or rigid element chains with ends that are not connected to any grid point (nodes) associated with structural element.

### Error 811

`Buckling analysis with inertia relief not supported `

Buckling analysis with inertia relief is not possible because the eigenvalues/ eigenvectors are dof dependent and unpredictable. In the inertia relief analysis, boundary conditions are used only to restrain the rigid body motion and external loads are balanced by the set of translational and rotational accelerations. The stiffness matrix becomes positive semi-definite and thus leads to singularity in buckling with inertia relief.

Do not perform buckling analysis with inertia relief.

### Error 814

`Solver cannot compute zero eigenvalues for a buckling subcase. The
model probably has rigid body mode`

If the eigenvalue is zero then the buckling load computes to zero which would give an error.

Check the model for rigid body modes by running modal analysis to check for rigid body modes in the model.

### Error 831

`Optimization problem is too big to be solved by the MFD/SQP
optimizer. Number of design variables = #. Number of
retained constraints = #. Please, use the 64-bit integer
version of OptiStruct by adding "-i64" solver script
option.`

Optimization problem is too large with large number of design variables and constraints.

Use the 64-bit integer version of
OptiStruct by adding
"`-i64`

" solver script option. This
can help solve the larger model or higher number of design
variables under consideration.

## #1000 through #5999

### Error 1813

`Buckling responses can only be used in free-sizing or topology optimization of
shells with non-zero T0, composites with non-zero DOPTPRM TMINPLY, composites
with minimum LAMTHK/PLYTHK, or when the design properties are excluded from
buckling analysis through the EXCLUDE command`

This error can occur in a Free-Size or Topology buckling optimization run when the base thickness value is set in the T0 field on the PSHELL Bulk Data Entry.

- LAMTHK
- Indicates that laminate thickness constraints are applied
- PLYTHK
- Indicates that ply thickness constraints are applied

- For Free-Size Buckling Optimization, the base thickness value should be set
in the
`T0`field on the DSIZE Bulk Data Entry. - For Topology Buckling Optimization, the base thickness value should be set
in the
`T0`field on the`TMIN`continuation line in the DTPL Bulk Data Entry. - Composites should have non -zero ply thickness defined for DOTTPRM, TMINPLY card.

### Error 1832

`Blank ATTB on DRESP1 card part xxx. ATTB cannot be blank for responses used in
modal frequency response optimization when the number of loading frequencies is
not known beforehand (i.e. FREQ3, FREQ4 or FREQ5 cards are used) and when the
number of modes on the EIGRL card is not explicitly specified.`

This error occurs when `ATTB` on
DRESP1 card is blank for modal frequency response
optimization.

The value `ATTB` field on
DRESP1 should be specified as number of loading
frequencies is not known and number of modes on EIGRL card is
not specified.

### Error 1837

`LOWFQ/HIGHFQ options are defined on <name1> card part.10002. Those options
are only valid for frequency response and local buckling optimization. For local
buckling optimization, only LOWFQ is allowed.`

LOWFQ and HIGHFQ are used in DRESP1 to specify the A response or a set of responses that are the result of a design analysis iteration.

LOWFQ
and HIGHFQ defines the Frequency Range within which the
responses are determined. Additionally, the `ATTB` field can be
used to specify functions to calculate combined responses over the frequency
range.

Check the model for type of optimization responses and attributes selected for optimization consideration as LOWFQ/HIGHFQ options are valid only for frequency response and local buckling optimization.

### Error 1859

`Discrete optimization is not available for topology, topography or free-sizing
optimization`

Discrete optimization (discrete design variables) is not available for topology, topography or free sizing optimization.

For topology, topography or free sizing optimization continuous design variables can be used.

### Error 1862

`Reliability-based optimization cannot be used without random design variables
or random parameters`

Reliability-based Design Optimization (RBDO) is an optimization method that can be used to provide optimum designs in the presence of uncertainty.

Random Design Variables and/or Random Parameters are used to define the structural design space in OptiStruct.

- Check if Random Design Variables has been defined using
`RAND`continuation lines on the DESVAR Bulk Data Entry. - Check if Random Parameters has been defined using RANP definition.

### Error 1868

`DOPTPRM, BKLOCAL2 has to be non-zero positive value for local buckling
optimization feature`

DOPTPRM card is used to define design optimization parameters by overriding the defaults.

DOPTPRM, BKLOCAL2 is Bulk Data Entry which is used to specify the maximum number of elements to represent the buckling zone for local modes.

Use of the zero or negative value for the DOPTPRM, BKLOCAL2 causes input error in the solver as it cannot interpret the maximum number of elements to represent the buckling zone.

### Error 1908

`Case Control data LOAD=** is not referenced by any bulk data relevant for used
subcase type. Run terminated because of error(s) in the input data`

Referenced Bulk Data does not have relevant loading for the defined loadstep.

- Check the model for the loadstep if all the load collectors are assigned as required for the analysis being performed.
- Check if the selected load collectors have defined loads in them and the referenced Bulk Data has relevant loading for defined loadsteps.

### Error 2790

`AMSES/AMLS cannot be used for buckling analysis of subcase #. Please use EIGRL
for buckling analysis.`

AMSES and AMLS are not supported for buckling analysis.

- Both AMLS and AMSES parameters cannot be defined for buckling analysis. They are typically used for modal frequency response and modal transient response analysis.
- Instead, use EIGRL entry (which uses LANCZOS method) for buckling analysis.

### Error 2920

`Buckling subcase with MFLUID is not supported because mass effect is not
accounted in Buckling analysis. Please remove MFLUID card from the control
section. `

The MFLUID command can be used in the Subcase Information section to select the parameters and damp elements and activate the calculation of virtual fluid mass. MFLUID may be requested for normal modes, complex eigenvalue, frequency response, or transient response analysis.

Buckling analysis does not account for the mass effect.

Remove MFLUID card from the control section.

### Error 3002

`The first point (X1,Y1) specified on the <cmdname>TABLES1</cmdname>
entry is not located at the origin`

This error can occur in a run wherein the
TABLES1 entry, that does not begin at the origin is
referenced by a MATS1 Bulk Data Entry on the
`TID` field, and if the `TYPSTRN` field on
the MATS1 entry is set to
0.

- The
`TYPSTRN`=0 setting indicates that the`TID`curve on TABLES1 entry defines the stress-strain curve in terms of the total strain. However, the TABLES1 entry does not start at the origin, which corresponds to plastic strain definition. Therefore, you can set the`TYPSTRN`field equal to 1, which utilizes the plastic strain based data for MATS1. - If you want to use total strain data instead, then use a minimum of three data-pairs on the TABLES1 entry, with one entry beginning at the origin.

### Error 3016

`Only two pairs of data on <cmdname>TABLES1</cmdname> Bulk Data Entry.
The minimum number of entries is 3.`

This error can occur in a run wherein the
TABLES1 entry, containing less than 3 data pairs, is
referenced by a MATS1 Bulk Data Entry on the
`TID` field, and if the `TYPSTRN` field on
the MATS1 entry is set to
0.

- The
`TYPSTRN`=0 setting indicates that the`TID`curve on TABLES1 entry defines the stress-strain curve in terms of the total strain. However, the TABLES1 entry defines only two pairs of data, which corresponds to plastic strain. Therefore, you can set the`TYPSTRN`field equal to 1, which utilizes the plastic strain based data for MATS1. - If you want to use total strain data instead, then use a minimum of three data-pairs on the TABLES1 entry.

### Error 4754

`STATSUB(BUCKLING) of subcase ‘x’ points to a nonlinear subcase with large
displacement, which is not supported`

The STATSUB command can be used in the Subcase Information section to select a static solution subcase. STATSUB(BUCKLING) is used to reference static subcase is used in forming the geometric stiffness needed for the linear buckling solution.

- Check and make sure that the STATSUB case does not points to the nonlinear subcase with large displacement.
- To a nonlinear subcase with large displacement, only small displacement option with STATSUB (BUCKLING) is supported.