Linear Perturbation Options (PERTURB) dialog box (ANSYS)

Properties
Description	Lets you specify an optional description for the modeling object.
PERTURB Parameters
Type to be performed (Type)	Specifies the type of linear perturbation analysis to perform.STATICPerforms a linear perturbation static analysis.MODALPerforms a linear perturbation modal analysis.BUCKLEPerforms a linear perturbation eigenvalue buckling analysis.HARMONICPerforms a linear perturbation full harmonic analysis.SUBSTRPerforms a linear perturbation substructure generation analysis.OFFInstructs the software not to perform a linear perturbation analysis.
Key to use material properties (MatKey)	Controls how the linear perturbation analysis uses material properties.Note: This option applies to all structural elements except contact elements.AUTOANSYS automatically selects the material properties for the linear perturbation analysis.TANGENTANSYS uses the tangent (material Jacobian) on the material's constitutive curve as the material property. The material property remains linear during the linear perturbation analysis. The software obtains the property at the point of the base analysis where the restart occurs.SPOFFANSYS automatically selects the material properties for the linear perturbation analysis. Additionally, the software sets the spin softening matrix to zero and ignores the spin softening effect.
Key to control contact status (ContKey)	Specifies the option that controls contact status for the linear perturbation analysis. This option controls all contact elements globally for all contact pairsCURRENTUses the current contact status from the restart. If the previous analysis is nonlinear, then the software freezes the nonlinear contact status at the point of the restart and uses that status throughout the linear perturbation analysis.STICKINGFor frictional contact pairs (MU>0), uses sticking contact (such as MU*KN for tangential contact stiffness) everywhere the contact state is closed (the contact status is not sticking or sliding). This option applies only to contact pairs that are in contact and have a frictional coefficient (MU) greater than zero. Contact pairs without friction (MU=0) and in a sliding state remain free to slide during the linear perturbation analysis.BONDEDMoves contact pairs that are in the closed (sticking or sliding) state to a bonded state (for example, KN for both normal and tangential contact stiffness). Contact pairs that have a status or far-field or near-field remain open.
Key to control the load vector (LoadControl	Specifies the option that controls how ANSYS calculates the {Fperturbed} load vector. Use this option to control load generation in a linear perturbation analysis. In general, a linear perturbation analysis requires a new set of loads. This option controls all mechanical loads but does not affect non-mechanical (including thermal) loads. ANSYS always keeps non-mechanical loads.ALLKEEPKeeps all the loads and constraints from the end of the load step of the current restart point. This option is helpful when you need to apply additional loads.INERKEEPDeletes all loads and constraints from the restart step, except for displacement constraints and inertia loads.PARKEEPDeletes all loads and constraints from the restart step, except for displacement constraints.DZEROKEEPDeletes all loads and constraints from the restart step, except for displacement constraints, except that ANSYS sets all nonzero displacement constraints to zero when linear perturbation begins.NOKEEPDeletes all the loads and constraints, including all displacement constraints.

How do I

Set up a large deflection, prestressed modal cyclic symmetry analysis

Learn more

ANSYS prestressed modal analyses with linear perturbation

Controlling how ANSYS writes restart files

Modifying the behavior of contact pairs

Specifying linear perturbation options

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Linear Perturbation Options (PERTURB) dialog box (ANSYS), Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });