Modal analysis

Tekla Structural Designer
2024
Tekla Structural Designer

Modal analysis

What is modal analysis?

Tekla Structural Designer's modal analysis is an analysis of undamped and simple-harmonic vibrations.

To formulate a solution we begin by considering the discrete dynamic equation used in finite element analysis:

[M]{ü} + [C]{u̇} + [K]{u} = {F}

Where [M] is the mass matrix, [C] is the damping matrix and [K] the stiffness matrix. All three matrices are constant in linear dynamics. {ü}, {u̇} and {u} are respectively the acceleration vector, velocity vector and the displacement vector. All three vectors vary as a function of time, as does {F} which is the load-vector (sometimes referred to as the forcing function).

Thinking about this equation in physical terms; [M]{ü} is the inertial force (from Newton's 2nd law), [C]{u̇} the damping force and [K]{u} the internal elastic force (i.e. strain energy).

By making some simplifications - such as that damping is zero - this can be reduced to:

[M]{ü} + [K]{u} = 0

A physical explanation of this equation is that, for a valid vibration mode at any instant of time, the inertial forces ([M]{ü}) and internal elastic forces ([K]{u}) are equal and opposite, while no external force is applied to the system. This is known as free vibration. Free vibration isn't related to static loading (other than where this defines mass) and will identify frequencies at which the structure can naturally resonate, based on its mass distribution and stiffness alone.

Solutions for the above equation have the following form:

{u}(t) = {U}eiωt and {ü}(t) = -ω2{U}eiωt

Substituting and dividing by eiωt (which represents the time-response and is simply a sine wave since the behaviour is simple harmonic) we obtain the eigenvalue equation:

([K] - ω2[M]){U} = {0}

In which ω2 is the eigenvalue and {U} the eigenvector.

Dividing by {U} and rearranging gives the following equation, which you may recognize as being of the same form as the fundamental equation for frequency (valid only for a single degree of freedom (SDOF) system) f ∝ √ (k/m) :

ω = √ ( [K]/[M] )

Note the eigenvalue equation contains no terms for force or acceleration.

Tekla Structural Designer’s modal analysis is a solution of this eigenvalue equation for the specific model. The method of solution is highly complex - if you are interested, details can be found in any good reference on vibration theory (we can recommend Vibration: Fundamentals and Practice Clarence W. de Silva, Boca Raton: CRC Press LLC, 2000). There are many (numerical) methods of solution, no fewer than three of which are implemented in TSD; Jacobi, Subspace and FEAST (the selection of the method used being automated).

The solution to the eigenvalue equation is the vector {U} - which is the mode shape - with a corresponding frequency which is the square root of the eigenvalue; ω = √ ω2. The mode shape is just that; a shape. It can have any amplitude - modal analysis does not give this, just the shape. So it does not produce ‘real’ deflections or forces.

Note that ω is the angular (or ‘circular’) frequency in terms of radians and so must be converted (by dividing by 2π ) to be in Hz.

There is not a single solution to the eigenvalue equation (other than for a single degree of freedom (SDOF) system) - a structure which has many DOFs will have multiple mode shapes*. Each mode shape occurs at a very specific frequency called the natural frequency of the mode in question.

*In reality the number of modes of even a simple structure is potentially infinite, however in the finite element method solution it is finite and is governed by the discretization of the numerical model i.e. how many elements and nodes it contains.
  • We can easily calculate the number of mode shapes for any numerical model - it is the number of free nodes (i.e. those not at a support) multiplied by the number of DOF’s (i.e. mass directions) at each node. In 3D space and using the consistent mass matrix (the default), there are 6 DOFs (3 translational and 3 rotational). Hence a model with 100 nodes will have 100*6 = 600 modes.

  • From this you will appreciate that even a relatively small model will have a large number of modes, while a large model will have 1000’s. However we are generally only interested in the lower modes - i.e. those with lower frequencies - which a) will involve the majority of the structure and b) are most likely to be excited (by whatever forcing function is in play - e.g. an earthquake or human movement) and thus problematic.

So in summary; modal analysis in Tekla Structural Designer is an idealized solution which finds the natural frequencies of a structure that does not consider damping or dynamic loading 'input' to your structure, which may occur in the real world. The results it produces are a list of modes - in order of ascending frequency - together with their: frequency; period; mass participation % and modal mass.

Active mass and mass participation

In a 1st order modal analysis mass is assigned to nodes of the analysis model. In simple terms (neglecting rotation terms for the consistent mass matrix) half of each element mass is assigned to each node it is attached to.

Mass that is assigned to a translational support cannot go anywhere - i.e. it is not "active".

Summed active translational mass

Reported in the Dynamic Masses table, this is the actual total active mass for each direction, but expressed in terms of force units rather than mass.

Summed total translational mass

Reported in the Dynamic Masses table (see above), this is the total system mass for each direction, again expressed in terms of force units rather than mass.

Translation %

Reported in the Summed Mass table, this is the proportion of mass that is active for each direction. For a building this will usually be close to but not quite 100% as some mass always goes to the supports.

Translation % = (Summed Active Mass / Summed Total Translational Mass) x 100

Participation translation %

Reported in the Summed Mass table (see above), this is the sum of Mass Participation % (reported in the Modal Frequencies table, as shown below) for all modes for each direction.

Mass participation is used in seismic analysis - in simple (not literal) terms it is a measure of the momentum of a mode and so a predictor of the base shear it produces.

Design codes stipulate that the sum for all the modes should be ≥ 90% for seismic analysis usually for two orthogonal lateral directions.

Modal mass

After running a 1st order modal analysis, modal masses for each mode are available in the Modal Frequencies table.

In Tekla Structural Designer the modal mass, Mi is given by the following matrix equation:

Mi = { Ψ}iT [M] { Ψ}i

Where {Ψ}i is the unity-scaled mode shape (often termed mode vector) of the ith mode (i.e. any single mode) and [M] is the mass matrix. The meaning of the unity-scaled mode shape is that the (numerically) largest modal displacement is set to unity and all other displacements are scaled accordingly. The term {Ψ}i is used to differentiate this mode shape from the mass-normalized shape {Φ}i which is the mode shape actually reported by Tekla Structural Designer.

This equation comes from modal analysis theory. It may also be termed "generalized mass".

Another way to state this equation, which is found in some design guides, is a summation equation for point masses and their associated modal displacements for a system of discretized mass distribution:

We have from CCIP-016:

CCIP-016_modal_mass_1.png

where i is each on N points on the structure, having mass mi at which the mode shape μj,i is the jth mode is known.

According to this reference - "Conceptually, the modal mass can be thought of as the mass of an equivalent single degree of freedom system... which represents the jth mode."

It can be seen how this is equivalent to the matrix equation given above. Actually Tekla Structural Designer makes use of a shortcut calculation since it already has mode shapes which are normalized to mass.

The mass-normalized mode shape { Φ}i and the unity-normalized mode shape {Ψ}i are related as follows:

CCIP-016_modal_mass_2.png

From this we can state the following, where Φ2 is the largest modal displacement from the mass-normalized mode shape (which we already have from the Tekla Structural Designer modal analysis):

CCIP-016_modal_mass_3.png

Hence:

CCIP-016_modal_mass_4.png

Run a 1st order modal analysis

In order to run a modal analysis on your model, see the following instructions.

Note:

To run a modal analysis, your model must contain an active modal mass combination.

For more information, see Create modal mass combinations.

  1. On the Analyze ribbon, click Settings.

    The Analysis Settings dialog box opens.

  2. In the dialog box, go to the 1st Order Modal page.
  3. If necessary, adjust the analysis options.
  4. On the Analyze tab, click 1st Order Modal.

    Tekla Structural Designer analyzes the model.

    At the end of the analysis process, the Results View opens to allow you to display the mode shapes graphically. Tabular results can also be viewed in a Solver Model Data View.

Was this helpful?
Previous
Next