Skip to main content

Modal dynamic analysis : Modal analysis

A modal dynamic analysis is set up using the Analysis wizard from the Analysis > New analysis task command. The next page allow the user to specify the task name (a name to associate with this modal analysis) and number.

The following page allows the user to specify the modal calculation strategy and mass option.

There are three options available for modal calculation strategy. This is because the number of modes needed and the criteria for determining the important modes are dependant on the structure and the intended application for the modal results.

Specify number of modes is the simplest option and is recommended if you want to look at the first set of modes in a structure. The number of modes required is dependent on the structure and intended application for the modal results. For a simple structure or where all that is required is the frequency of the fundamental mode, only a few modes are required. A large, complex structure may require 100 modes or more.

Specify frequency range allows the user to focus only on the modes within a frequency range. This option is recommended if you want to perform a footfall analysis using the modal results.

Specify target mass participation ratio allows the user to specify a target mass participation ratio and limit the results to only the modes that contribute to the specified target. This is particularly useful if you want to perform a response spectrum analysis using the modal results. When looking at seismic code there is typically a requirement on the effective mass captured - often around 90% when carrying out response spectrum analysis.

Modelling implications​

In most cases a dynamic analysis follows on from a linear static analysis, so a model set up for static analysis is the normal starting point. The dynamic response should normally be considered in three dimensions so generally global restraints should be avoided.

In a modal analysis there is a structure mass matrix in addition to structure stiffness matrix. This is assembled from the element mass matrices in a similar way to the stiffness matrix. This requires some additional specification information, which is set when setting up a modal analysis. The user must decide how the mass is to be distributed around the structure and can derive additional mass from loading.

The three mass options allow for the mass of the structure to be accounted for in different ways.

  • Mass lumped at nodes – the mass of the elements (including mass properties) is lumped at the nodes (inertias are ignored). For a beam element half of the mass is assigned to each node.
  • Masses calculated from the element shape function – the mass and inertia of the element are accounted for.
  • Mass of mass properties only – the mass of the structural elements is ignored and the user has to specify mass properties on nodes to distribute mass around the structure.

In general the first option will be the most useful. If the mass calculated from the element shape function is used it may lead to modes which involve vibration of individual elements rather than the structure as a whole.

The element mass is derived from the element properties and geometry. For beam and bar elements the mass is not the catalogue mass per unit length but is derived from the unmodified section area, element length and material density.

In most cases not all the mass of the structure is accounted for by the mass of the structural elements, but some is represented in the model as loading on the structure. The option to derive mass from loads allows for some loading to be converted to mass for the modal analysis. Loads are vectors, whereas mass is a scalar so the direction allows the appropriate component of the loading to be selected. The converted loads (load component divided by g) are then considered like lumped masses at the nodes.

Results​

The results for a modal analysis are similar to those for a static analysis, but the interpretation of the results is different.

The displacements represent the mode shape, rather than an actual deflected form, and are arbitrarily scaled or normalised. The default normalisation gives a maximum displacement of 1m. The basis of normalisation can be changed in the GSS advanced settings > Eigensolution dialog, both in terms of units and whether based on mode shape or modal mass.

In addition to the modal displacements, forces and reactions there are the dynamic details results with information such as frequency, modal mass and stiffness, participation factors and effective masses. All of these quantities will depend on the displacement units in that they depend on the modal displacements.

Details of results available and how they can be viewed are in the Results display options section.