7.5 The Basic Procedure of Vibration Analysis

Back

In this section, a typical procedure in using commercial software packages to conduct vibration analysis

is outlined.

7-16 Vibration and Shock Handbook

© 2005 by Taylor & Francis Group, LLC

7.5.1 Planning

This is a very important part of the entire analysis process, as it helps to ensure the success of the

modeling. The quality of the results is strongly dependent on how accurately the model represents the

actual problem being investigated. In order to generate a representative finite element model, all

influencing factors must be scrutinized to determine whether their effects are considerable or negligible

in the final result. The aspects listed below should be given consideration in the planning stage.

* Modeling objectives. Why is the vibration analysis required? What is the major concern of designers?

What are the working conditions? Does the FEA model have to be used for static stress analysis

as well as vibration analysis? These considerations affect how the FEA model is to be built up.

* Modeling considerations. Which type of analysis is required: natural vibration analysis or response

analysis? What types of elements should be used? Where are loads and constraints applied? Can the

model reduction/simplification resulting from symmetrical geometries and loading conditions be

applied? There are no universal guidelines for these, but the aspects below can help you to make

decision:

* If the stress varies linearly through the thickness of thin-walled regions, shell elements can be

used. If it varies parabolically, then at least three solid, second-order elements are required

through the thickness in order to resolve a representative state of stress.

* If a frequency or buckling analysis is being conducted, a full three-dimensional analysis may be

needed to identify non-symmetric mode shapes.

* If the region of interest is local, then a submodel may be appropriate, as it will save considerable

time achieving a solution.

* Large gradients in stress levels will require a high mesh density to capture the behavior

appropriately.

* The effects of simplifications on boundary conditions should be well predicted, for example:

some over-constrained boundary conditions may result in higher natural frequencies of the finite

element model.

The degree of accuracy of a model is very much dependant on the level of planning that has been

carried out. Careful planning is the key to a successful analysis.

7.5.2 Preprocessing

The preprocessor stage in a general FEA package involves the following:

* Defining the element type as planned before the analysis. This may be one-, two-, or threedimensional.

* Creating the geometry. The geometry is drawn in one-, two-, or three-dimensional space according

to what kind of elements are going to be used. The model may be created in the preprocessor, or it

can be imported from other CAD or CAE systems via a neutral file format (IGES, STEP, ACIS,

Parasolid, DXF, etc.). The same units should be applied in all models, otherwise the results will be

difficult to interpret or, in extreme cases, the results will not show up mistakes made during the

loading and restraining of the model.

* Applying a mesh. Mesh generation is the process of dividing the continuum into a number of

discrete parts or finite elements. The finer the mesh, the more accurate the result, but the longer

the processing time. Therefore, a compromise between accuracy and solution speed is usually

made. The mesh may be created manually or generated automatically, or, as in most cases, in a

combined manner.

Manual meshing is a long and tedious process for models with a fair degree of geometric

complication, but with useful tools emerging in preprocessors, the task is becoming easier.

Automatic mesh generators are very useful and popular. The mesh is created automatically by a

mesh engine; the only requirement is to define the mesh density along the model’s edges.

Vibration Modeling and Software Tools 7-17

© 2005 by Taylor & Francis Group, LLC

Automatic meshing has limitations as regards mesh quality and solution accuracy. Automatic

brick element meshers are limited in function, but are steadily improving. Any mesh is usually

applied to the model by simply selecting the mesh command on the preprocessor list of the user

interface.

Usually a complex geometry needs to be decomposed into many smaller components in order

to use the automatic meshing tool.

* Assigning properties. Material properties (Young’s modulus; Poisson’s ratio; the density; and if

applicable, the coefficients of expansion, friction, thermal conductivity, damping effect, specific

heat, etc.) will have to be defined. In addition element properties may need to be set. If twodimensional

elements are being used, the thickness property is required. One-dimensional beam

elements require area, Ixx ; Iyy ; Izz ; J; and the direction of the beam axis in three-dimensional space.

Shell elements, which are two-dimensional elements in three-dimensional space, require

orientation and neutral surface offset parameters to be defined. Special elements such as mass,

contact, spring, gap, coupling, damper, and so on require properties (specific to the element type)

to be defined for their use.

* Applying loads. In the case of transient response analysis, some type of load is usually applied to

the analysis model. The loading may be in the form of a point force, a pressure or a displacement,

or a temperature or heat flux in a thermal analysis. The loads may be applied to a point, an edge, a

surface, or even a complete body. The loads should be in the same unit system as the model

geometry and material properties specified. In the case of modal analyses, a load does not have to

be specified for the analysis to run.

* Applying boundary conditions. Structural boundary conditions are usually in the form of zero

displacements; thermal boundary conditions are usually specified temperatures. A boundary

condition may be specified to act in all directions ðx; y; zÞ; or in certain directions only. Boundary

conditions can be placed on nodes, key points, lines, or areas. The boundary conditions applied on

lines or areas can be of a symmetric or antisymmetric type, one allowing inplane rotations and out

of plane translations, the other allowing in plane translations and out of plane rotations for a given

line or area. The application of correct boundary conditions is critical to the accurate solution of

the design problem.

7.5.3 Solution

The FEA solver can be logically divided into three main parts: the presolver, the mathematical-engine,

and the postsolver. The presolver reads in the model created by the preprocessor and formulates the

mathematical representation of the model. All the parameters defined during the preprocessing stage are

used to do this, so if something has been omitted the presolver is very likely to stop the call to the

mathematical-engine. If the model is correct, the solver proceeds to form the element stiffness matrix and

the element mass matrix for the problem and calls the mathematical-engine, which calculates the result.

The results are returned to the solver and the postsolver is used to calculate strains, stresses, velocities,

response, and so on for each node within the component or continuum. All these results are sent to a

result file that may be read by the postprocessor.

7.5.4 Postprocessing

Here the results of the analysis are read and interpreted. They can be presented in the form of a table, a

contour plot, a deformed shape of the component, or the mode shapes and natural frequencies if

frequency analysis is involved. Most postprocessors provide animation tools.

Contour plots are usually the most effective way of viewing results for structural type problems. Slices

can be made through three-dimensional models to facilitate the viewing of internal stress and

deformation patterns.

7-18 Vibration and Shock Handbook

© 2005 by Taylor & Francis Group, LLC

All postprocessors now include the calculation of stresses and strains in any of the x; y; or z directions;

or indeed in a direction at an angle to the coordinate axes. The principal stresses and strains may also be

plotted, or if required, the yield stresses and strains according to the main theories of failure (Von Mises,

St Venant, Tresca, etc.).

7.5.5 Engineering Judgment

For many reasons, the vibration analysis results may not represent the actual vibration problem very well.

Software packages will not reveal anything about this, and so it is the responsibility of modelers to make

judgments.

Sound judgment comes from a thorough understanding of the actual vibration problem; indepth

knowledge of vibration theory, FEA, and the software package used; and also rich experience in

modeling. When you are not confident of your vibration analysis results you should check the following:

1. What units have been used, SI units or Imperial units? Are the units used consistent and

compatible with the software package you are using?

2. What are the material’s properties?

3. Is the boundary free or partially constrained, or flexibly connected to other parts?

4. How are the interconnections between different parts modeled (e.g., the interconnection between

a two-dimensional plate and a three-dimensional block)?

Sometimes, a judgment is made by comparing your model’s results and the results of different models

that are similar in some sense to the one of concern, but which have been validated. A judgment can also

be made by vibration measurements or testing under laboratory conditions or in real-life situations (see

Chapter 17 and Chapter 18). By properly exploiting the combined test and analysis data, modelers can

effectively and reliably identify otherwise only approximately known structural properties (e.g., joint

stiffness), material properties, and loading; validate and refine the FEA model (simplification validation,

model updating, etc.) by using test results as reference data; identify unknown or badly known physical

properties; and better assess uncertainties in the FEA model.

Навигация