(CalculiX Solver)

The simulation type Frequency enables the computation of the eigenfrequencies and eigenmodes of a structure. Those depend on the applied boundary conditions (Displacement constraints and preload boundary conditions).

As a result the numerical values of the eigenfrequencies as well as the displacement representation of the eigenmodes can be analysed. The eigenfrequencies can help you understand at which frequencies there might occur resonances for example when passing a frequency band during the start-up of an engine. If you are interested in a special periodic loading you should also consider running a Harmonic analysis

frequency analysis of a truss bridge

Frequency analysis of a truss bridge

Apart from the eigenfrequencies and the eigenmodes the normalized effective modal mass for each mode and each rigid body motion is also available as a result. For the calculation one first defines the generalized mass \(m_{\pmb{\Phi}^i}\) of the mode \(\pmb{\Phi}^i\) as:

\[\begin{equation} m_{\pmb{\Phi}^i} = \pmb{\Phi}^{iT}\pmb{M}\pmb{\Phi}^i \end{equation}\]

where \(\pmb{M}\) is the mass matrix and \(i\) the number of the mode. For the six rigid body motions one gets the effective modal mass for each eigenmode with following equation:

\[\begin{equation} m_{\pmb{\Phi}^i,d} = \frac{(\pmb{\Phi}^{iT}\pmb{M}\pmb{U}_d)^2}{\pmb{\Phi}^{iT}\pmb{M}\pmb{\Phi}^i} \end{equation}\]

where \(\pmb{U}_d\) is a unit displacement vector or a unit rotation vector in the x-, y- or z-direction (marked by the index \(d\)). The effective modal mass quantifies the size of the rigid motion and therefore the importance of the eigenmode. This value is then normalized with help of the total effective mass \(m_{total,d}\), which is also given as a table in the Post-Processor.

\[\begin{equation} \tilde{m}_{\pmb{\Phi}^i,d} = \frac{m_{\pmb{\Phi}^i,d}}{m_{total,d}} \end{equation}\]

This is done, because the sum of the modal effective mass of a rigid body motion over all eigenmodes is equal to the total effective mass corresponding to the rigid body motion. If one would calculate an infinite number of modes, the sum over the normalized effective modal mass would therefore be 1. To ensure a good representation of all the available modes in the conducted simulation, the following relation should be satisfied:

\[\begin{equation} \sum_{i=1}^{n} \tilde{m}_{\pmb{\Phi}^i,d} \geq 0.9 \end{equation}\]

where \(n\) is the number of the calculated modes. For more information regarding the modal mass see Paramètres modaux et norme des vecteurs propres in the Code_Aster documentation. On the platform the normalized effective modal mass is accumulated over all modes, so one can see the importance of the mode and the completeness of the simulation in the same plot.

Plot for the accumulated normalized effective modal mass

Plot for the accumulated normalized effective modal mass

In the following the different simulation settings you have to define are described in detail as well as the various options you can add.


In order to perform an analysis a given geometrical domain you have to discretize your model by creating a mesh out of it. Details of CAD handling and Meshing are described in the Pre-processing section.

After you assigned a mesh to the simulation you can add some optional domain-related settings and have a look on the mesh details. Please note that if you have an assembly of multiple bodies that are not fused together, you have to add Contacts if you want to build connections between those independent parts.


In the model section everything that defines the physics of the simulation is specified e.g. material properties, boundary conditions etc. On the top level you can adapt some generic settings. For a Frequency analysis you can add a gravitational load for the whole domain. As with all load boundary conditions in a Frequency analysis the load is applied in a preceding static step.


In order to define the material properties of the whole domain, you have to assign exactly one material to every part. You can choose the material behavior describing the constitutive law that is used for the stress-strain relation and the density of the material. Please note that the density is used for volumetric loads e.g. gravitation. Inertia effects are only considered in dynamic simulations (Dynamic). Please see the Materials section for more details.

Boundary Conditions

In a Frequency analysis you can define Constraints (Displacement boundary conditions) and Preload boundary conditions (Forces). You might be interested in the eigenfrequencies of the structure when allowed to move freely (without displacement constraints) as well as the eigenfrequencies when fixed with bearings. All loads (including gravitation) are applied prior to the frequency analysis in a static preload step. Thus it is possible to introduce a initial stress that influences the stiffness of the system and thus the eigenfrequencies and eigenmodes.

Constraint types (Displacement boundary conditions)

Preload types (Force boundary conditions)


Under numerics you can set the equation solver of your simulation. For a Frequency analysis the Arpack solver is the only choice. Please note that using multi-core machines in the Simulation Control section does not influence the solver performance as multithreading is not supported but increases the available memory for the calculation, see Number of computing cores. For the static preload step the Spooles solver is used.

Simulation Control

The Simulation Control settings define the overall process of the simulation. In a Frequency analysis you can define the number of computing cores (only influences the available memory, see Numerics) as well as the the maximum time you want your simulation to run before it is automatically cancelled. Furthermore you can define the frequency settings that determine how many frequencies will be calculated at maximum and in which frequency range you are interested. If there are more eigenfrequencies within this range as defined above, the lowest frequencies are chosen.


The described Frequency analysis is solved on the SimScale platform using the finite element code CalculiX Crunchix (CCX). See our Third-party software section for further information.