COMSOL 6.4 - Eigenmodes of a Viscoelastic Structural Damper

Eigenmodes of a Viscoelastic Structural Damper

The example studies the natural frequencies and corresponding eigenmodes of a typical viscoelastic damper. Damping elements involving layers of viscoelastic materials are often used for the reduction of seismic and wind induced vibrations in buildings and other tall structures. The common feature for such structures is that the frequency of their possible forced vibrations is low. Thus, it is important to use dampers with natural frequencies that are high enough to avoid any failures due to resonances.

Solving for eigenfrequencies in a structure where the deformation to a large extent is controlled by a viscoelastic material (or any other material which has frequency dependent material properties) requires special techniques. A standard eigenfrequency problem without damping can be formulated as

(1)

where K is the stiffness matrix, M is the mass matrix, u is the eigenmode displacement vector, and f is the frequency. In most cases, K is independent of frequency, but for a viscoelastic material the eigenvalue equation actually is

(2)

In this example, it is shown how you can handle this type of problem.

Model Definition

The geometry of the viscoelastic damper is shown in Figure 1 (from Ref. 1). The damper consists of two layers of viscoelastic material confined between mounting elements made of steel.

Figure 1: Viscoelastic damping element.

One of the mounting elements is modeled as fixed, and two other elements are partially constrained to represent a typical operating regime of the damper.

The viscoelastic layers are modeled using complex valued material data. For frequency domain and eigenfrequency analyses, the frequency decomposition for the deviatoric stress and strain tensors is in general performed as:

where f is the frequency.

The deviatoric stress is related then to the strain as

(3)

where the complex valued shear modulus is written as

where the G' and G'' are the storage and loss moduli, respectively.

In this example, the moduli are specified by their reference values given at two reference frequencies fr1 = 200 Hz and fr2 =1000 Hz:

Table 1: Storage and loss moduli.
f	fr1	fr2
G’	3.0848E7 Pa	7.8348E7 Pa
G”	3.6551E7 Pa	8.4935E7 Pa

The frequency dependency is approximated by straight lines in the log-log space using the above data. Thus, the following expressions are used for the moduli:

where

and

where

Substituting the deviatoric stress given by Equation 3 into the equation of motion gives

which, together with the boundary conditions, will result in a nonlinear eigenvalue problem for f. The eigenvalue problem will determine the natural frequencies of the system.

COMSOL Multiphysics solves such nonlinear problems by expanding all expressions containing the frequency down to quadratic polynomials using a frequency linearization point fLwhich you can specify in the node (100 Hz is used by default).

The eigenvalue problem, which is solved, is then

Thus, the results become dependent on the choice of the frequency linearization point.

Starting from COMSOL 6.3, there are two options to handle the nonlinearity.

You can use a new eigenvalue solver, ARPACK nonlinear. This solver approximates the nonlinear functions with polynomials using Taylor expansion, and then it will build and solve a number of equivalent linear eigenvalue problems. The use of this approach can be computationally expensive for larger models.

As an alternative, you can compute an approximation of the complex valued shear modulus using the partial fraction fit. The approximation corresponds to an equivalent Generalized viscoelasticity model, and it can be used in both Eigenfrequency and Time Dependent study steps. For the eigenfrequency computations, the eigenvalues problem will be linear. The approximation computation needs to be performed as a preprocessing step, but it is very fast and independent of the model size.

This example demonstrates the use of both approaches.

You model in 3D using the Solid Mechanics interface with a and add a subnode to the domains representing the viscoelastic layers. The approximation computation becomes available directly on the subnode when the viscoelasticity model is selected.

Results and Discussion

Six eigenfrequencies are initially computed using the default linear eigenvalue solver using 100 Hz as the default frequency linearization point. The first computed eigenmode is shown in Figure 2.

Figure 2: First eigenmode computed using linear solver with default frequency linearization point.

The computed eigenfrequencies can only be expected to be correct by the order of magnitude. This allows you to identify the frequency range 200 − 1000 Hz for further investigations.

The approximation computed for the storage and loss moduli contributions from the Viscoelasticity subnode is shown in Figure 3.

Figure 3: Storage and loss moduli contribution. Solid line is the approximation, the line markers correspond to the user defined expressions.

Figure 4 shows the eigenfrequencies computed using different approaches.

Figure 4: The eigenfrequency distribution in the complex plane.

Thus, the results of using the approximation and nonlinear eigenvalue solver are in good agreement with each other. The first eigenmode computed using the approximation is shown in Figure 5.

Figure 5: First eigenmode computed a linear eigenvalue solver together with the approximation of viscoelastic data via the partial fraction fit.

References

1. S.W. Park “Analytical Modeling of Viscoelastic Dampers for Structural and Vibration Control,” Int. J. Solids and Structures, vol. 38, pp. 694–701, 2001.

2. K.L. Shen and T.T. Soong, “Modeling of Viscoelastic Dampers for Structural Applications,” J. Eng. Mech., vol. 121, pp. 694–701, 1995.

Structural_Mechanics_Module/Dynamics_and_Vibration/viscoelastic_damper_eigenmodes

Modeling Instructions

From the menu, choose .

New

In the window, click

Model Wizard

In the window, click

In the tree, select > .

Click .

Click

In the tree, select > .

Click

Global Definitions

Parameters 1

Import the viscoelastic material data from a file.

In the window, under click .

In the window for , locate the section.

Click

Browse to the model’s Application Libraries folder and double-click the file viscoelastic_damper_eigenmodes_parameters.txt.

The data contains the reference values of the storage and loss moduli given at two reference frequencies. You approximate the data by straight lines in the log-log space. This can be done by using analytic functions as follows.

Analytic 1 (an1)

In the toolbar, click

and choose > .

In the window for , type gstor in the text field.

Locate the section. In the text field, type gsr1*(f/fr1)^ns.

In the text field, type f.

Locate the section. In the text field, type Pa.

In the table, enter the following settings:


Argument	Unit
f	Hz

Click to expand the section. Select the checkbox.

Locate the section. In the table, enter the following settings:


Plot	Argument	Lower limit	Upper limit	Fixed value	Unit
√	f	fr1	fr2	0	Hz

Analytic 2 (gstor2)

Right-click and choose .

In the window for , type gloss in the text field.

Locate the section. In the text field, type glr1*(f/fr1)^nl.

Geometry 1

Import the predefined geometry from a file.

In the toolbar, click and choose .

Browse to the model’s Application Libraries folder and double-click the file viscoelastic_damper_geom_sequence.mph.

Click the

button in the toolbar.

Click the

button in the toolbar.

The imported geometry should look similar to that shown in Figure 1.

Solid Mechanics (solid)

Linear Elastic Material 2

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Select Domains 2 and 5 only.

Viscoelasticity 1

In the toolbar, click

and choose .

Use the analytic functions to enter the viscoelastic moduli as functions of frequency.

In the window for , locate the section.

From the list, choose .

In the G′ text field, type gstor(solid.freq).

In the G′′ text field, type gloss(solid.freq).

Add Material

In the toolbar, click

to open the window.

Go to the window.

In the tree, select > .

Click the button in the window toolbar.

In the toolbar, click

to close the window.

Materials

Viscoelastic

In the window, under right-click and choose .

In the window for , type Viscoelastic in the text field.

Select Domains 2 and 5 only.

Locate the section. In the table, enter the following settings:


Property	Variable	Value	Unit	Property group
Bulk modulus	K	4e8	N/m²	Bulk modulus and shear modulus
Shear modulus	G	5.86e4	N/m²	Bulk modulus and shear modulus
Density	rho	1060	kg/m³	Basic