SOLVERS Home: Initial Conditions (Natural Frequency)

Description

Initial Conditions File

Selects a previously generated results file (the initial conditions file) from which a result case, or <None>, can be selected.

There are three main reasons for selecting an initial file and result case to define initial conditions in a natural frequency analysis:

To consider the effects of pre-load on the natural frequencies of a structure. For example, the lateral frequency of a string increases as the string is tensioned. By including a static analysis that models the pre-load, the tensioning effect can be taken into account in the natural frequency analysis.
To consider the contact condition between two or more bodies or compression-only supports, due to an applied load. The tangent stiffness, and therefore frequencies, of a structure may be affected by the amount of contact area (the contact patch) between parts and/or supports. For example, an inactive compression-only support attribute in the result case of the initial file will also be inactive in the natural frequency analysis.
To consider a change in tangent stiffness due to nonlinear material behaviour at a specified load level. For example, a Cutoff Bar that is inactive in the result case of the initial file will also be inactive in the natural frequency analysis.

The pre-load effect is always included when the initial file includes geometric nonlinearity (initial files that can include geometric nonlinearity are generated by the Nonlinear Static and Quasi-static solvers) and when the initial file is generated by the Linear Static solver (there is no other reason to include initial conditions from a Linear Static result file). The pre-load effect may also be optionally considered with initial files that do not include geometric nonlinearity (i.e., initial files generated by the Nonlinear Static and Quasi-static solvers when the GNL option is not set).

The contact condition is always included if the initial file is generated by the Nonlinear Static or Quasi-static solvers, but never included if the initial file is generated by the Linear Static solver. This also applies to compression-only support attributes.

If the initial file considers material nonlinearity, the element tangent stiffness matrix used in the natural frequency analysis takes this into account.

In addition to the above, if the initial file uses staging, the natural frequency analysis will consider only the active elements in the stage used in the result case of the initial file.

Irrespective of the initial conditions used, the natural frequency solution will always be a linear, small-displacement solution based on a constant tangent stiffness defined by the initial conditions; contact elements, for example, do not change their active state as the structure vibrates in the natural frequency analysis; they remain in the state in which they were in the initial conditions result.

If the natural frequency results file is subsequently used by any of the mode superposition solvers, namely the Harmonic Response, Spectral Response or Linear Transient Dynamic (Mode Superposition) solvers, all of the conditions that affect the global stiffness matrix in the natural frequency analysis are carried forward to these solvers. In other words, modal superposition results will use the same stiffness matrix as used in the natural frequency analysis.

Include Stress Stiffness [KG]

The effect of pre-load is considered in a natural frequency analysis by the addition of the geometric stress stiffness matrix, [KG], to the structural stiffness matrix. This geometric stress stiffness matrix is based on stress calculated from the result case in the initial file.

If the initial file considers geometric nonlinearity, or the initial file is from a Linear Static analysis, the geometric stress stiffness matrix, [KG], is always added to the structural stiffness matrix for the natural frequency analysis. If the initial file does not consider geometric nonlinearity, the geometric stress stiffness matrix will be added only when this option is set.

Include Follower Load [KG] (local distributed lateral loads only)

If set, the geometric stress stiffness matrix will be augmented by an additional load stiffness matrix that depends on the change in tangent stiffness that occurs when an applied load changes direction as the structure deforms. Only some load types will change direction as the structure deforms. These are the so-called follower loads. Note that a change in load magnitude is not the same as a change in load direction.

In Straus7, the option applies to the following element attributes:

Beam Distributed Force applied in the principal lateral directions of Beam, Truss, Cutoff-Bar and Spring elements;
Plate Edge Normal Pressure applied to Plate/Shell, 3D-Membrane, Plane Stress, Plane Strain and Axisymmetric elements;
Plate Face Normal Pressure applied to Plate/Shell and 3D-Membrane elements;
Brick Face Normal Pressure (all brick elements).

If the model does not contain any of these attributes, the option is not relevant.

Note

The eigenvalue solver in Straus7 considers only symmetric matrices. The load stiffness matrix is usually non-symmetric and only a symmetric component is added when performing eigenvalue analysis with initial conditions. The natural frequencies might therefore be inaccurate, depending on the model - more details are available in the theoretical manual. A nonlinear transient dynamic analysis should be undertaken to fully account for the load stiffness.