Bracket — Random Vibration Analysis

The various examples based on a bracket geometry form a suite of tutorials that summarizes the fundamentals of modeling structural mechanics problems in COMSOL Multiphysics and the Structural Mechanics Module.

This example shows how to perform a random vibration analysis for a structure using power spectral density (PSD). The computations are based on the modal reduced-order model (ROM).

Model Definition

The model geometry is represented in Figure 1.

Figure 1: Bracket geometry. Rigid connector and its center of rotation are shown using special physics symbols.

The bracket is made of structural steel. Four smaller holes in the bracket are fully constrained to represent a bolted connection.

A pin connects two larger holes in the bracket arms. The pin is assumed to be perfectly rigid and is modeled with a rigid connector. Thus, the pin is not represented in the model geometry.

The rigid connector has the translational and rotational degrees of freedom of a rigid body. Options for this feature include applying an external load to such rigid body. In this tutorial, you use two components of such load as random excitations applied to the structure. The input PSD for the load components are shown in Figure 2.

Figure 2: Input PSD for random load components. Log-log scale is used.

The two applied load components are assumed to be uncorrelated. Physically, this means that it is two different sources of excitation which causes the load in the two directions.

You will compute the displacement response at a point with coordinates: X = 0, Y = 0, Z =-0.45, which is a representative location in the lower plate of the bracket.

Results and Discussion

Figure 3 shows the PSD for two displacement components, calculated for the frequency range that contains the first three natural frequencies of the structure. Note that there are three peaks on the resulting PSD. The left and right ones correspond to two natural frequencies of the structure, while the middle peak corresponds to the maximum of the input excitation.

The cross-correlation between the two displacement components is shown in Figure 4.

Figure 3: PSD for the horizontal (U) and vertical (W) displacement response at the selected location.

Figure 4: Cross-correlation between the horizontal and vertical displacement response at the selected location.

Figure 5 and Figure 6 show the PSD for the horizontal and vertical displacement, respectively, computed at a particular frequency.

Figure 5: PSD of u-displacement component (m2/Hz).

Figure 6: PSD of w-displacement component (m2/Hz).

Figure 7, Figure 8 and Figure 9 show the RMS for the horizontal and vertical displacements, as well as for the displacement magnitude, computed using integration of their corresponding PSD over the frequency range from 150 to 800 Hz.

Figure 7: RMS of u-displacement component (m).

Figure 8: RMS of w-displacement component (m).

Figure 9: RMS of displacement magnitude (m).

Since the horizontal displacement is dominant, Figure 7 and Figure 9 are almost identical.

In Figure 10, the RMS of the total acceleration is shown. It can be noted that the distribution over the structure differs fundamentally from that of the displacement (Figure 9). The reason is that the vertical motion of the central section of the bracket is related to a higher eigenfrequency than the horizontal motion of the two arms. This is why accelerations are more pronounced than displacements, in this part of the bracket.

In Figure 9, the RMS of the von Mises equivalent stress is shown.

Figure 10: RMS of acceleration magnitude (m/s2).

Figure 11: RMS of von Mises stress (Pa)

The interpretation of results from a random vibration analysis requires special attention. Usually, the RMS is the result. The RMS is defined as

(1)

for some long time T. In many cases, you are more interested in the maximum value than in the RMS. For many statistical distributions, for example the normal distribution, the tail of the distribution extends to infinity. Mathematically the response can then reach an arbitrarily high value with a probability that increases with time.

In practice, it is customary to assume that the maximum value does not exceed a certain factor times the RMS value. This factor is often taken as 3 or 4. Thus, the maximum stress can be estimated to 50 to 65 MPa.

For vibrating structures, fatigue is often a more important aspect than the maximum stress. In the Fatigue Module, you can find an example where this model is extended by a fatigue analysis.

Notes About the COMSOL Implementation

The simplest way to set up a random vibration analysis in COMSOL Multiphysics is to add a predefined study called . This will automatically add two study nodes configured to act as a sequence.

The first added study is an eigenfrequency analysis that serves as a basis for the modal reduced-order model (ROM) required for the system response analysis. Note that any nodes should be manually disabled under this study node for all structural interfaces in the model. This is needed because the eigenmode extraction should be always done for undamped system.

It is enough to compute the last of the two studies. This will automatically compute the requested number of eigenfrequencies and then create a ROM based on the computed eigenmodes.

When you add a study, A node with subnodes will be also added automatically under . These nodes are used for specifying the model control parameters (inputs) and to enter expressions for the input PSD to be used in the random vibration computations. Such computations are performed as postprocessing steps. However, if the PSD expressions are changed under , a solution update might be needed.

The evaluations are done using special operators that become available as part of the random vibration analysis.

The input PSD as functions of the frequency are often specified using linear interpolation in the log-log representation of the data. The model shows how to set up such functions.

Structural_Mechanics_Module/Tutorials/bracket_random_vibration

Modeling Instructions

Root

This file serves as starting point for various examples based on a bracket geometry. It sets up the model geometry, material, and mesh. It also adds a Solid Mechanics interface with a fixed constraint applied to the bolt holes.

Application Libraries

From the menu, choose .

In the window, select in the tree.

Click

Add Study

In the toolbar, click

to open the window.

Go to the window.

Find the subsection. In the tree, select .

Right-click and choose .

In the toolbar, click

to close the window.

Solid Mechanics (solid)

Linear Elastic Material 1

In the window, expand the node, then click .

Damping 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

In the f1 text field, type 400.

In the ζ1 text field, type 0.05.

In the f2 text field, type 700.

In the ζ2 text field, type 0.03.

Study 1

Step 1: Eigenfrequency

You need to disable the damping for this study because the eigenmode computation should be performed for the undamped system. The damping will however be used in the following modal reduced-order model and random response analysis.

In the window, under click .

In the window for , locate the section.

Select the check box.

In the tree, select .

Right-click and choose .

Global Definitions

Set up two control parameters to be used as loads.

Global Reduced Model Inputs 1

In the window, expand the node, then click .

In the window for , locate the section.

In the table, enter the following settings:


Control name	Expression
Fx	100[N]
Fz	100[N]

Solid Mechanics (solid)

Now add a rigid connector to the holes in the bracket arms to simulate the presence of a connecting pin.

Rigid Connector 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

By default the location of the center of rotation is computed automatically. You can also manually specify its location.

To visualize its position you need to enable the physics symbols.

In the window, click .

In the window for , locate the section.

Select the check box.

The displacement of the rigid connector in the y direction and all rotations are constrained.

In the window, click .

In the window for , locate the section.

Select the check box.

Locate the section. From the list, choose .

Select the check box.

Applied Force 1

In the toolbar, click

and choose .

Apply a load at the center of rotation of the rigid body.

In the window for , locate the section.

Specify the F vector as


Fx	x
0	y
Fz	z

Definitions

Variables 1

In the window, under right-click and choose .

Set up variables to evaluate the displacement components at a selected point.

In the window for , locate the section.

In the table, enter the following settings:


Name	Expression	Unit	Description
U	at3(0, 0, -0.045, u)	m	Displacement, X component
W	at3(0, 0, -0.045, w)	m	Displacement, Z component

Study 2

Frequency Domain 1

In the window, expand the node, then click .

In the window for , locate the section.

In the text field, type 500.

Study 1

In the toolbar, click

Study 2

The computation of the solution for Study 2 will find the requested number of eigenfrequencies and create a reduced-order model based on the computed eigenmodes.

Click

Global Definitions

Next, set up the input PSD for the random loads.

Interpolation 1 (int1)

In the toolbar, click

and choose .

In the window for , locate the section.

Click

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

Piecewise 1 (pw1)

In the toolbar, click

and choose .

In the window for , locate the section.

In the text field, type f.

Find the subsection. In the table, enter the following settings:


Start	End	Function
150	800	exp(int1(log(f+250)))

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

In the text field, type N^2/Hz.

Piecewise 2 (pw2)

Right-click and choose .

In the window for , locate the section.

Find the subsection. In the table, enter the following settings:


Start	End	Function
150	800	exp(int1(log(f)))

Random Vibration 1 (rvib1)

Assume that the two random loads are uncorrelated, and have different power spectral densities.

In the window, under click .

In the window for , locate the section.

From the list, choose .

In the table, enter the following settings:


Control name	Power spectral density
Fx	pw1(freq)
Fz	pw2(freq)

Locate the section. In the text field, type 150.

In the text field, type 800.

Update the study to make the input change available for the solution.

Study 2

In the toolbar, click

Results

Global Evaluation Sweep 1

In the toolbar, click

and choose .

Plot the input PSD for the load components in a range of frequencies containing first three natural frequencies of the structure.

In the window for , locate the section.

In the table, enter the following settings:


Parameter name	Parameter value list
freq	range(150,5,800)[Hz]

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


Expression	Unit	Description
pw1(freq)	kg^2*m^2/s^3	PSD of load, X component
pw2(freq)	N^2/Hz	PSD of load, W component

Locate the section. From the list, choose .

Click

Table

Go to the window.

Click in the window toolbar.

Results

Table Graph 1

In the window, under click .

In the window for , locate the section.

Find the subsection. From the list, choose .

Click to expand the section. Select the check box.

Click the

button in the toolbar.

Click the

button in the toolbar.

PSD of Loads

In the window, under click .

In the window for , type PSD of Loads in the text field.

Locate the section. From the list, choose .

The random response computations can be performed as postprocessing steps using the updated solution. First, evaluate and plot the PSD for the displacement response at the chosen point.

Global Evaluation Sweep 2

In the toolbar, click

and choose .

In the window for , locate the section.

In the table, enter the following settings:


Parameter name	Parameter value list
freq	range(150,5,800)[Hz]

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


Expression	Unit	Description
rvib1.psd(U)		PSD of U displacement (m^2/Hz)
rvib1.psd(W)		PSD of W displacement (m^2/Hz)

Locate the section. From the list, choose .

Click

Table

Go to the window.

Click in the window toolbar.

Results

Table Graph 1

In the window, under click .

In the window for , locate the section.

Find the subsection. From the list, choose .

Locate the section. Select the check box.

PSD of Displacements

In the window, under click .

In the window for , type PSD of Displacements in the text field.

Locate the section. From the list, choose .

Global Evaluation Sweep 3

In the toolbar, click

and choose .

Also evaluate and plot the cross-correlation for two different components of displacement responses at the chosen point. For verification, you also plot the non-random frequency response result.

In the window for , locate the section.

In the table, enter the following settings:


Parameter name	Parameter value list
freq	range(150,5,800)[Hz]

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


Expression	Unit	Description
real(rvib1.cross(U,W))		Cross-correlation of U and W, real part
imag(rvib1.cross(U,W))		Cross-correlation of U and W, imaginary part
abs(rvib1.cross(U,W))		Cross-correlation of U and W, absolute value