15.8. Linear Perturbation Analysis

The following linear perturbation analysis topics are available:

15.8.1. Assumptions and Restrictions

The following assumptions and restrictions apply to the linear perturbation method:

  • Valid for structural degrees of freedom (DOFs) only.

  • Supports only certain structural element types. See Elements Under Linear Perturbation in the Element Reference for a complete list.

  • Performed by first running a linear or nonlinear static or full (TRNOPT,FULL) transient analysis, then restarting the analysis with the appropriate linear perturbation analysis type.

  • For a linear perturbation modal analysis, the mass density and damping information should be supplied in the analysis phase of the static or full transient procedure (if they are needed later for the linear perturbation analysis).

15.8.2. Description of Analysis

In many engineering applications, the linear behavior of a structure based on a prior linear or nonlinear preloaded status is of interest. The linear perturbation analysis procedure is designed to solve a linear problem from this preloaded case. Typically, the Newton-Raphson procedure is used in the nonlinear analysis (see Figure 14.9: Newton-Raphson Solution - One Iteration). Without loss of generality, the nonlinear static problem is discussed here. A similar process can apply to linear static and linear or nonlinear full transient analyses.

In the case of a nonlinear static analysis, the mode frequency of the structure based on load level is needed. The tangent matrix can be used in the linear perturbation analysis in order to obtain the effect of preload, as the linear stiffness matrix without preloading does not give the correct solution.

Equation 14–153 at iteration i is recast here for convenience of discussion:

(15–239)

Here, is the global tangent matrix which can be symbolically segregated into other matrices as follows:

(15–240)

where:

= the part of the tangent stiffness contributed from the material property
= the stress stiffening matrix introduced by non-zero stresses from the structure; superscript N indicates nonlinear (that is, the stress stiffening matrix is obtained from a nonlinear analysis – not to be confused with the linear stress stiffening matrix obtained from the first phase of a linear perturbation buckling analysis)
= the load stiffening matrix introduced by external pressure loads or by follower force effect (element FOLLW201)
= the total stiffness matrix contributed from contact elements of the model
= the spin-softening matrix introduced by rotational velocities

In the preload (or base) analysis, could be generally nonlinear. In the subsequent linear perturbation analysis, the material behavior must be linear. Depending on the material option specified on the PERTURB command and the material properties used, the program handles materials in the linear perturbation analysis differently. The program uses the consistent material Jacobian of hyperelastic materials at iteration i as the material behavior in the linear perturbation analysis. For other nonlinear materials, the program uses the linear portion of the material in the linear perturbation analysis by default. For any linear materials, the same behaviors are assumed in both the base and the linear perturbation analyses. For nonlinear materials, an option is available to use the consistent material tangent Jacobian (see the PERTURB command for more information).

In the case of contact analysis from the static or full transient runs, is by default the consistent tangent (total) stiffness matrix from the contact elements based on their status at iteration i. However, you are optionally allowed to change contact behavior and, hence, contact stiffness for all contact pairs by using the PERTURB command in the linear perturbation analysis or the CNKMOD command for individual contact pairs. All contact behavior can be changed into the following form (similar to KEYOPT(12) in the contact element descriptions; for example, CONTA174) from whatever behavior it was in the previous static or full transient analysis to:

1 -- Rough
2 -- No separation (sliding permitted)
3 -- Bonded
4 -- No separation (always)

15.8.3. Static Analysis Based on Linear Perturbation

A static analysis can be performed by using the linear perturbation analysis procedure. The effect of the structure from the previous static or full transient analysis is included.

The theoretical steps can be summarized as follows:

  1. Perform a static or full transient base analysis; use the RESCONTROL command to create the restart files for the load points of interest (i.e., at various substeps of a load step).

  2. Restart the analysis at the load point of interest and issue the commands PERTURB,STATIC and SOLVE,ELFORM. The program regenerates the total tangent stiffness matrix from the restart point.

  3. For the static analysis, the perturbation load is required and must be defined or modified at this step (see Application of Perturbation Loads and also the PERTURB command description).

  4. Upon the onset of the second SOLVE command, the nodal coordinates are updated automatically if the base analysis includes large-deflection effects (NLGEOM,ON). The program then calculates the static solution using the following the equation (similar to Equation 15–1):

    (15–241)

  5. Along with the static solution phase, a stress calculation is carried out based on the material definition specified via the PERTURB command. (See Interpretation of Structural Element Results After a Linear Perturbation Analysis in the Element Reference for details.)

15.8.4. Modal Analysis Based on Linear Perturbation

A modal analysis can be performed by using the linear perturbation analysis procedure. The effect of the structure from the previous static or full transient analysis is included. The theoretical steps can be summarized as follows:

  1. Perform a static or full transient base analysis; use the RESCONTROL command to create the restart files for the load points of interest (i.e., at various substeps of a load step).

  2. Restart the analysis at the load point of interest and issue the commands PERTURB,MODAL and SOLVE,ELFORM. The program regenerates the total tangent stiffness matrix from the restart point.

  3. If a downstream analysis is desired using the load vector from the modal analysis, the perturbation load can be defined or modified here (see Application of Perturbation Loads and also the PERTURB command description) for the downstream analyses.

  4. Upon the onset of the second SOLVE command, the nodal coordinates are updated automatically if large-deflection was included in the base analysis (NLGEOM,ON). The program then calculates the eigensolution using the following equation (similar to Equation 14–198):

    (15–242)

    where:

    = total tangent matrix from the load point of interest
    = eigenvector
    = structural mass matrix

    The structural material behavior in a linear perturbation analysis is discussed above and can be controlled by the PERTURB command. The UNSYM and DAMP eigensolvers can be used as well. In the case of the DAMP eigensolution, the following equation (similar to Equation 14–210) is solved:

    (15–243)

    where:

    = structural damping matrix

  5. Along with the modal solution phase, a stress expansion pass is carried out. (See Interpretation of Structural Element Results After a Linear Perturbation Analysis in the Element Reference for details.) To use the appropriate material property and to obtain the total sum of elastic strain/stress due to the linear perturbation analysis and the base analysis, a stress expansion pass must be done along with the modal analysis. A separate expansion pass (EXPASS command) is not allowed after the linear perturbation analysis.

15.8.5. Eigenvalue Buckling Analysis Based on Linear Perturbation

An eigenvalue buckling analysis can be performed by using the linear perturbation analysis procedure. Unlike the preceding modal analysis description, this procedure is more complicated since the perturbation load is a prerequisite for calculating the linearly perturbed stresses; then the perturbed stresses are used to calculate the linearly perturbed stress stiffening matrix before the buckling analysis can be started. Physically, the total perturbation load multiplied by the buckling load factor plus the total loads available from the restart load point is used to determine the ultimate buckling loads from the analysis.

If the base analysis is linear, however, the total perturbation load multiplied by the buckling load factor represents the ultimate buckling load. This procedure is similar to the linear eigenvalue buckling analysis outlined in Buckling Analysis. It can be viewed as restarting the analysis with the tangent matrix equal to the linear stiffness matrix, and load vector . The prediction of the buckling load can be written:

(15–244)

The theoretical steps for a linear perturbation buckling analysis with a nonlinear base analysis can be summarized as follows:

  1. Perform a static or full transient base analysis; use the RESCONTROL command to create the restart files for the load points of interest (i.e., at various substeps of a load step).

  2. Restart the analysis at the load point of interest and issue the commands PERTURB,BUCKLE and SOLVE,ELFORM. The program regenerates the total tangent stiffness matrix from the restart point.

  3. The perturbation load is required and must be defined or modified at this step (see Application of Perturbation Loads and also the PERTURB command description) for the calculation of the linearly perturbed displacements and stresses.

  4. Upon the onset of the second SOLVE command, is used to calculate the linearly perturbed displacement following the equation:

    (15–245)

    Then, internally, is used to calculate the linearly perturbed stresses , and the linearly perturbed stress stiffening matrix is calculated:

    (15–246)

    following a formula similar to Equation 3–61.

    Next, the nodal coordinates are updated automatically if large-deflection was included in the base analysis (NLGEOM,ON). The program then calculates the eigensolution using the following equation (similar to Equation 15–107):

    (15–247)

    where is the total tangent matrix from the load point of interest. is the linearly perturbed stress stiffening matrix generated by Equation 15–245 and Equation 15–246.

  5. Along with the eigenvalue buckling solution phase, a stress expansion pass is carried out. (See Interpretation of Structural Element Results After a Linear Perturbation Analysis in the Element Reference for details.) To use the appropriate material property and to obtain the total sum of elastic strain/stress due to the linear perturbation analysis and the base analysis, a stress expansion pass must be done along with the buckling analysis. A separate expansion pass (EXPASS command) is not allowed after the linear perturbation analysis.

  6. You must perform this step manually. This step determines the total buckling load using the loads from the restart load point and the additional perturbation load . The user should manually calculate the total buckling load from the following equation:

    (15–248)

    where:

    = total loads at the current restart load point (load applications are from the .LDHI file)
    = eigenvalues from Equation 15–247. Normally, the lowest eigenvalue ( when j = 1) of Equation 15–247 is of interest.

    Equation 15–248 is useful in a way that combines linearly or nonlinearly prestressed loads with a linearly perturbed load. For example, if the nonlinear static analysis cannot proceed further due to convergence issues, the buckling loads can still be predicted with this process under the assumption of linear perturbation.

Generally, eigensolutions for equations Equation 15–107 (purely linear eigenvalue buckling) and Equation 15–247 (perturbed eigenvalue buckling) can be performed by using the Block Lanczos eigensolver (BUCOPT,LANB) if stiffness matrix or is non-singular (i.e., no rigid body mechanism is introduced into the model). In the case of purely linear eigenvalue buckling, is positive definite. However, in linear perturbation, can be indefinite (i.e., it contains both positive and negative pivots if it is factorized by a direct sparse equation solver). The following conditions will likely invoke an indefinite matrix from the base analysis:

  1. In the base analysis, the applied load is large enough to trigger nonlinear buckling points in the nonlinear solution process.

  2. In the base analysis, the status of contact elements changes to be open or sliding.

  3. In the base and perturbed eigenvalue buckling analyses, mixed u-P formulation (Lagrange multiplier) elements have been used in the model (see General Element Formulations).

When becomes indefinite (i.e, one of the above conditions occurs), the Block Lanczos eigensolver (BUCOPT,LANB) could fail to produce an eigensolution due to the mathematical limitation of this solver. In such a case, it is recommended that you use the subspace eigensolver (BUCOPT,SUBSP) to achieve a successful solution. The subspace eigensolver can still give a converged solution even when both the and matrices are indefinite. However, if the base nonlinear analysis introduces a singular matrix, then no buckling eigensolutions are possible. This sometimes happens when the stiffness matrix is highly ill-conditioned.

15.8.6. Full Harmonic Analysis Based on Linear Perturbation

A full harmonic analysis can be performed by using the linear perturbation analysis procedure. The effect of the structure from the previous static or full transient analysis is included. The theoretical steps can be summarized as follows:

  1. Perform a static or full transient base analysis; use the RESCONTROL command to create the restart files for the load points of interest (i.e., at various substeps of a load step).

  2. Restart the analysis at the load point of interest and issue the commands PERTURB,HARMONIC and SOLVE,ELFORM. The program regenerates the total tangent stiffness matrix from the restart point.

  3. For the full harmonic analysis, the perturbation load is required and must be defined or modified here (see Application of Perturbation Loads and also the PERTURB command description).

  4. Upon the onset of the second SOLVE command, the nodal coordinates are updated automatically if large-deflection is included in the base analysis (NLGEOM,ON). The program then calculates the harmonic solution using the following equation (similar to Equation 15–52):

    (15–249)

    where:

    = total tangent matrix from the load point of interest
    = structural mass matrix
    = structural damping matrix

    The perturbation load is generally a complex number load vector with frequency dependency. Also, in the second phase of the linear perturbation analysis, the number of harmonic solutions (or substeps) is specified by the NSUBST or DELTIM command.

  5. Along with the harmonic solution phase, a stress calculation is carried out based on the material definition specified via the PERTURB command. (See Interpretation of Structural Element Results After a Linear Perturbation Analysis in the Element Reference for details.)

15.8.7. Substructure or CMS Generation Based on Linear Perturbation

A substructure or CMS (component mode synthesis) generation can be performed by using the linear perturbation analysis procedure. In this section, the term substructure refers to substructuring and CMS analyses. The prestressed effect of the structure from the previous static or full transient analysis is included in the substructure or CMS generation. The theoretical steps can be summarized as follows:

  1. Perform a static or full transient base analysis; use the RESCONTROL command to create the restart files for the load points of interest (i.e., at various substeps of a load step).

  2. Restart the analysis at the load point of interest and issue the commands PERTURB,SUBSTR and SOLVE,ELFORM. The program regenerates the total tangent stiffness matrix from the restart point.

  3. For the generation pass, the perturbation load is used to generate the first load vector of the substructure. The substructure master degrees of freedom (M) must be specified.

  4. Upon the onset of the second SOLVE command, the nodal coordinates are updated automatically if large-deflection is included in the base analysis (NLGEOM,ON). The program then calculates the reduced substructure matrices based on the following equations (similar to Equation 15–108 to Equation 15–138).

    For a static substructure generation pass:

    (15–250)

    For a dynamic substructure generation pass:

    (15–251)

    where:

    = total tangent matrix from the load point of interest
    = structural mass matrix
    = structural damping matrix

    In the case of a dynamic analysis, CMS generation is recommended.

  5. The generated substructure is assumed to be linear and can be used in a subsequent use pass. The use pass does not require a linear perturbation procedure.

  6. In the expansion pass, all material properties are assumed to be linear, and all contact statuses are frozen as in a linear application. NLGEOM is turned OFF, even if the base analysis for the prestressed substructure generation pass is nonlinear. The expansion pass does not require a linear perturbation procedure.

15.8.8. Application of Perturbation Loads

The total perturbed loads are required for static, eigenvalue buckling, and harmonic analyses and are optional for modal analyses. One of the obvious reasons they would be needed for a modal analysis is because a downstream mode-superposition (MSUP) analysis needs loads.

The total perturbed loads are calculated as follows:

(15–252)

where:

= total loads at the end of the load step of the current restart load point (load applications are read from the .LDHI file, see Figure 15.8: Linear Perturbation Started from Loadstep = 2, Substep = 3). By default, only contains loads contributed by displacement boundary conditions, inertia loads, and thermal loads (see the PERTURB command).
= additional (new) loads prescribed by the user in the second phase of the linear perturbation analysis (after the first SOLVE,ELFORM command is invoked). This additional loading is optional.

Special consideration is required if extra displacement boundary conditions are added or if constraint equations are added or deleted during the linear perturbation analysis because these modifications could introduce discontinuities into the structure.

Figure 15.8: Linear Perturbation Started from Loadstep = 2, Substep = 3 provides a graphic example of the definitions for the different load vectors. Two ramped load steps are shown in the figure. Since a linear perturbation analysis is started at load step = 2, substep = 3, the load vectors by definition are = 40 lb and = 25 lb.

Figure 15.8:  Linear Perturbation Started from Loadstep = 2, Substep = 3

Linear Perturbation Started from Loadstep = 2, Substep = 3

is the total loads at the current restart point. may be useful for some types of linear perturbation analysis; for example, to calculate the ultimate buckling loads in an eigenvalue buckling analysis.

In the first phase of a linear perturbation analysis, the ANTYPE,,RESTART and SOLVE,ELFORM commands resume the Jobname.RDB database and read in the .LDHI file to establish the load.

has a different usage and implication for each perturbed analysis type:

  • For Type = STATIC, is the actual external load for the perturbed static analysis. must be supplied by the user.

  • For Type = MODAL, is calculated and stored in the .FULL and .MODE files for a subsequent mode-superposition, PSD, or other type of modal-based linear dynamic analysis.

  • For Type = BUCKLE, is the actual linear buckling load which is used to generate the linearly perturbed stress stiffening matrix for the eigenvalue buckling analysis. must be supplied by the user.

  • For Type = HARMONIC, is the actual external load for the perturbed full harmonic analysis. , which must be supplied by the user, can be frequency dependent and can use complex input.

  • For Type = SUBSTR, is used to generate the first reduced external load vector of the substructure.

15.8.9. Downstream Analysis Using the Solution of a Linear Perturbation Analysis

Following the linear perturbation analysis, other analysis types can be performed by using the information from the linear perturbation analysis.

If the linear perturbation analysis is a modal analysis, the following analysis types are possible by using the .MODE file generated by the linear perturbation analysis and the database of the model:

  • harmonic or transient analysis of the mode-superposition (MSUP) method

  • response spectrum analysis

  • random vibration analysis

Note that the deformed mesh due to the prior static or full transient analysis is used in the linear perturbation analysis and in the downstream analysis.

In all the above listed analyses, the first load vector used is from Equation 15–252. If more loading cases are required, it is required to regenerate a new load vector by using the MODCONT command. Only linear material properties are supported in these analyses. The program assumes the analyses are purely linear.

Release 18.2 - © ANSYS, Inc. All rights reserved.