Error Message Database

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).

1. 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.
2. 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.

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.

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.

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.

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.

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

1. 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.
2. Check the model and rerun the problem.

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.

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

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.

1. 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.
2. Try to update the operating system, if running on Windows.
3. Disable real time protection, and add an exception, for files with the extension .rs~ and OptiStruct related files (.fem, and so on).

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).

1. 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).
2. 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.

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.

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

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.

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.

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

1. Run Normal Modes Analysis and look for Rigid Body Modes. If any exist, there are massless mechanisms in the model.
2. 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).
3. 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.

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

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

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.

1. 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.
2. Running Normal Modes Analysis or Linear Static Analysis by adding MECHCHECK helps detect the massless mechanisms.

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.

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

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

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

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.

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.

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.

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.

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.

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.

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

1. Try to force in-core solution using -corein.
2. Disable dynamic memory allocation and set the total allowable static RAM using -fixlen.

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.

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.

1. Find all RBE3 elements in the model and look for improperly constrained independent grid points.
2. 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.

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.

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

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.

This is an error inside the optimizer.

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

Generic

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

1. Contact OptiStruct support

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.

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

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

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

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

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

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.

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.

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.

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.

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.

1. For Free-Size Buckling Optimization, the base thickness value should be set in the T0 field on the DSIZE Bulk Data Entry.
2. 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.
3. Composites should have non -zero ply thickness defined for DOTTPRM, TMINPLY card.

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.

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.

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.

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.

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

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.

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

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

AMSES and AMLS are not supported for buckling analysis.

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

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.

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.

1. 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.
2. 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.

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.

1. 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.
2. If you want to use total strain data instead, then use a minimum of three data-pairs on the TABLES1 entry.

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.

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