Vibration Analysis of a Deep Beam

PDF

Vibration Analysis of a Deep Beam

This example studies free and forced vibrations of a deep beam. With the increase of the ratio of section area per beam length, shear deformations and rotational inertia effects can no longer be neglected as it is done in the Euler-Bernoulli theory.

The solution for Eigenfrequency, frequency response and transient analysis are computed using a Timoshenko beam and compared with analytical results.

Model Definition

The model studied in this example consists of a simply supported beam with a square cross section. One end is pinned and has a constrained rotation along the beam axis. At the other end, the displacements in the plane of beam cross section are constrained.

For the forced vibration cases, a load in the y direction is applied all along the beam.

•

Beam length, L = 10 m

•

Beam cross section dimension l = 2 m

•

Young’s modulus, E = 200 GPa

•

Poisson’s ratio, ν = 0.3

•

Mass density, ρ = 8000 kg/m3

•

Rayleigh damping coefficient: α = 5.36 s-1, β = 7.46e-5 m/s

At x = 0, u = v = w =0; thx =0

At x = 10, v = w = 0

The load with a magnitude F0 = 106N/m is applied and oriented in the local positive y direction. The following forced vibration cases are studied:

•

Harmonic response at a frequency of 20 Hz

•

Periodic response with the following force distribution:

with f = 20 Hz.

•

Transient response using a suddenly applied step load.

To satisfy the benchmark specifications, 5 edge elements are used to mesh the geometry.

Results and Discussion

In Table 1 the computed results are compared with the analytical results for the free vibration case. The agreement is good. The accuracy decreases with increasing complexity of the mode shape, because the possibility for the relatively coarse mesh to describe such a shape is limited.

Table 1: Comparison between analytical and computed natural frequencies.
Mode number	Analytical frequency (Hz)	COMSOL result (Hz)	Error (%)	Type
1, 2	42.65	42.67	4.7e-2	Flexural
3	71.2	71.51	0.4	Torsional
4	125	125.5	0.4	Extensional
5, 6	148.15	150.4	1.5	Flexural
7	213.61	221.6	3.7	Torsional
8, 9	283.47	300.1	5.9	Flexural

Harmonic Forced Vibration

In Table 2 the computed results are compared with the analytical results for the harmonic forced vibration case. The agreement is good.

Table 2: Comparison between analytical and computed Harmonic responses.
	Reference	COMSOL	Error (%)
Peak displacement (mm)	13.45	13.42	0.2
Peak stress (MPa)	241.9	238.6	1.4
Frequency (Hz)	42.65	42.65	0

In Figure 1 the displacement at the middle of the beam is shown versus the frequency.

Figure 1: Displacement versus frequency, harmonic response.

In Figure 1 the bending stress at the middle of the beam is shown versus the frequency.

Figure 2: Bending stress versus frequency, harmonic response.

Periodic Forced Vibration

In Table 3 the computed results are compared with the analytical results. The agreement is good. The accuracy decreases with increasing complexity of the mode shape, because the possibility for the relatively coarse mesh to describe such a shape is limited.

Table 3: Comparison between analytical and computed periodic responses.
	Reference	COMSOL	Error (%)
Peak displacement (mm)	0.951	0.948	0.3
Peak stress (MPa)	17.1	16.95	0.8

In Figure 3 the displacement at the middle of the beam is shown versus the time.

Figure 3: Displacement versus time, periodic response.

In Figure 4 the bending stress at the middle of the beam is shown versus the time.

Figure 4: Bending stress versus time, periodic response.

Transient Forced Response

In Table 4 the computed results are compared with the analytical results. The agreement is good. The accuracy decreases with increasing complexity of the mode shape, because the possibility for the relatively coarse mesh to describe such a shape is limited.

Table 4: Comparison between analytical and computed transient responses.
	Reference	COMSOL	Error (%)
Peak displacement (mm)	1.043	1.037	0.6
Peak stress (MPa)	18.76	18.14	3.3
Peak time (s)	0.0117	0.0117	0
Static displacement	0.538	0.534	0.7

In Figure 5 the displacement at the middle of the beam is shown versus the time.

Figure 5: Displacement versus time, transient response.

1. J. Maguire, D.J. Dawswell, L. Gould, “Selected Benchmarks for Forced Vibration,” NAFEMS R0016, 1989.

Structural_Mechanics_Module/Verification_Examples/vibrating_deep_beam

Modeling Instructions

From the menu, choose .

In the window, click

.

1

In the window, click

.

2

In the tree, select .

3

4

5

In the tree, select .

6

Global Definitions

1

In the window, under click .

2

In the window for , locate the section.

3

In the table, enter the following settings:


Name	Expression	Value
L	10[m]	10 m
F0	1e6[N/m]	1E6 N/m

Polygon 1 (pol1)

1

In the toolbar, click

and choose .

2

In the window for , locate the section.

3

In the table, enter the following settings:


x (m)	y (m)	z (m)
0	0	0
L	0	0

Form Union (fin)

1

In the window, click .

2

In the window for , click

.

Material 1 (mat1)

1

In the window, under right-click and choose .

2

In the window for , locate the section.

3

In the table, enter the following settings:


Property	Variable	Value	Unit	Property group
Young’s modulus	E	2e11	Pa	Basic
Poisson’s ratio	nu	0.3	1	Basic
Density	rho	8000	kg/m³	Basic

1

In the window, under click .

2

In the window for , locate the section.

3

From the list, choose .

Cross-Section Data 1

1

In the window, under click .

2

In the window for , locate the section.

3

From the list, choose .

4

In the hy text field, type 2.

5

In the hz text field, type 2.

Section Orientation 1

1

In the window, expand the node, then click .

2

In the window for , locate the section.

3

From the list, choose .

4

Specify the V vector as


0	X
0	Y
1	Z

Prescribed Displacement/Rotation 1

1

In the toolbar, click

and choose .

2

Select Point 1 only.

3

In the window for , locate the section.

4

From the list, choose .

5

From the list, choose .

6

From the list, choose .

7

Locate the section. From the list, choose .

8

Select the check box.

9

Select the check box.

Prescribed Displacement/Rotation 2

1

In the toolbar, click

and choose .

2

Select Point 2 only.

3

In the window for , locate the section.

4

From the list, choose .

5

From the list, choose .

1

In the toolbar, click

and choose .

2

In the window for , locate the section.

3

From the list, choose .

1

Right-click and choose .

2

Right-click and choose .

1

In the window, click .

2

In the window for , type Free Vibration in the text field.

Step 1: Eigenfrequency

1

In the window, under click .

2

In the window for , locate the section.

3

Select the check box.

4

In the associated text field, type 10.

5

In the text field, type 40.

To get all eigenfrequencies, including the duplicates at higher frequency, set a tighter tolerance in the solver sequence by following the steps below.

Solution 1 (sol1)

1

In the toolbar, click

.

2

In the window, expand the node, then click .

3

In the window for , locate the section.

4

In the text field, type 1.0E-10.

5

.

Change the to 0.1 for better visualization.

1

In the window, expand the node, then click .

2

In the window for , locate the section.

3

In the text field, type 0.1.

1

In the toolbar, click

and choose .

2

In the window for , locate the section.

3

From the list, choose .

4

Locate the section. Specify the FL vector as


0	X
0	Y
F0	Z

5

Right-click and choose .

Linear Elastic Material 1

In the window, click .

1

In the toolbar, click

and choose .

2

In the window for , locate the section.

3

In the αdM text field, type 5.36.

4

In the βdK text field, type 7.46e-5.

1

In the toolbar, click

to open the window.

2

Go to the window.

3

Find the subsection. In the tree, select .

4

Click in the window toolbar.

5

In the toolbar, click

to close the window.

Harmonic Forced Vibration

1

In the window, click .

2

In the window for , type Harmonic Forced Vibration in the text field.

3

Locate the section. Clear the check box.

Step 2: Frequency Domain, Modal

1

In the window, under click .

2

In the window for , locate the section.

3

In the text field, type range(0,2,38) range(40,5e-2,45) range(46,2,60).

4

In the toolbar, click

.

1

In the toolbar, click

.

2

In the window for , locate the section.

3

From the list, choose .

4

Locate the section. In the text field, type L/2.

5

In the text field, type 0.

6

In the text field, type 0.

Harmonic Peak Displacement

1

In the toolbar, click

.

2

In the window for , type Harmonic Peak Displacement in the text field.

3

Locate the section. From the list, choose .

1

Right-click and choose .

2

In the window for , locate the section.

3

In the text field, type beam.uAmpZ.

4

From the list, choose .

5

In the toolbar, click

.

Harmonic Peak Stress

1

In the window, right-click and choose .

2

In the window for , type Harmonic Peak Stress in the text field.

1

In the window, expand the node, then click .

2

In the window for , locate the section.

3

In the text field, type abs(beam.sb1).

4

From the list, choose .

5

In the toolbar, click

.

Harmonic Peak Displacement

1

In the toolbar, click

and choose .

2

In the window for , type Harmonic Peak Displacement in the text field.

3

Locate the section. From the list, choose .

4

From the list, choose .

5

In the list, select .

6

Select Edge 1 only.

7

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


Expression	Unit	Description
beam.uAmpZ	mm	Displacement amplitude, Z component

8

Harmonic Peak Stress

1

Right-click and choose .

2

In the window for , type Harmonic Peak Stress in the text field.

3

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


Expression	Unit
abs(beam.sb1)	MPa

4

, then choose .

Interpolation 1 (int1)

1

In the toolbar, click

and choose .

2

In the window for , locate the section.

3

In the text field, type phase.

4

In the table, enter the following settings:


t	f(t)
20	-pi/2
60	pi/2

5

Locate the section. From the list, choose .

6

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

7

In the text field, type rad.

1

In the toolbar, click

and choose .

2

Select Edge 1 only.

3

In the window for , locate the section.

4

Specify the FL vector as


0	X
0	Y
F0	Z

1

In the toolbar, click

and choose .

2

In the window for , locate the section.

3

Specify the φ vector as


0	x
0	y
phase(freq)	z

1

In the toolbar, click

to open the window.

2

Go to the window.

3

Find the subsection. In the tree, select .

4

.

5

In the toolbar, click

to close the window.

Step 1: Frequency Domain

1

In the window for , locate the section.

2

In the text field, type 20 60.

3

Locate the section. Select the check box.

4

In the tree, select .

5

Frequency to Time FFT

1

In the toolbar, click

and choose .

2

In the window for , locate the section.

3

In the text field, type range(0.0,1/(200*20),1/20).

4

From the list, choose .

5

Locate the section. Select the check box.

6

In the tree, select .

Solution 4 (sol4)

1

In the toolbar, click

.

2

In the window, expand the node, then click .

3

In the window for , locate the section.

4

From the list, choose .

5

In the window, click .

6

In the window for , type Periodic Forced Vibration in the text field.

7

Locate the section. Clear the check box.

8

In the toolbar, click

.

1

In the toolbar, click

.

2

In the window for , locate the section.

3

From the list, choose .

4

Locate the section. In the text field, type L/2.

5

In the text field, type 0.

6

In the text field, type 0.

Periodic Peak Displacement

1

In the toolbar, click

.

2

In the window for , type Periodic Peak Displacement in the text field.

3

Locate the section. From the list, choose .

1

Right-click and choose .

2

In the window for , locate the section.

3

In the text field, type w.

4

From the list, choose .

5

In the toolbar, click

.

Periodic Peak Stress

1

In the window, right-click and choose .

2

In the window for , type Periodic Peak Stress in the text field.

1

In the window, expand the node, then click .

2

In the window for , locate the section.

3

In the text field, type beam.sb1.

4

From the list, choose .

5

In the toolbar, click

.

Periodic Peak Displacement

1

In the toolbar, click

and choose .

2

In the window for , type Periodic Peak Displacement in the text field.

3

Locate the section. From the list, choose .

4

Select Edge 1 only.

5

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


Expression	Unit
abs(w)	mm

6

Locate the section. From the list, choose .

7

Periodic Peak Stress

1

Right-click and choose .

2

In the window for , type Periodic Peak Stress in the text field.

3

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


Expression	Unit
abs(beam.sb1)	MPa

4

, then choose .

1

In the toolbar, click

and choose .

2

In the window for , locate the section.

3

From the list, choose .

4

Locate the section. Specify the FL vector as


0	X
0	Y
F0	Z

1

In the toolbar, click

to open the window.

2

Go to the window.

3

Find the subsection. In the tree, select .

4

Click in the window toolbar.

5

In the toolbar, click

to close the window.

Step 1: Time Dependent

1

In the window for , locate the section.

2

In the text field, type range(0,1e-4,1.2e-2) range(1.3e-2,1e-3,1.2).

3

From the list, choose .

4

In the text field, type 1e-3.

5

Locate the section. Select the check box.

6

In the tree, select .

7

8

In the tree, select .

9

10

In the window, click .

11

In the window for , type Transient Forced Vibration in the text field.

12

Locate the section. Clear the check box.

Solution 6 (sol6)

1

In the toolbar, click

.

2

In the window, expand the node.

3

In the window, expand the node, then click .

4

In the window for , locate the section.

5

In the text field, type 1e-4.

6

In the window, click .

7

In the window for , click to expand the section.

8

From the list, choose .

9

1

In the toolbar, click

.

2

In the window for , locate the section.

3

From the list, choose .

4

Locate the section. In the text field, type L/2.

5

In the text field, type 0.

6

In the text field, type 0.

Transient Peak Displacement

1

In the toolbar, click

.

2

In the window for , type Transient Peak Displacement in the text field.

3

Locate the section. From the list, choose .

4

Locate the section. Select the check box.

5

In the associated text field, type Time (s).

6

Select the check box.

7

In the associated text field, type Displacement (mm).

8

Locate the section. Select the check box.

9

In the text field, type -1e-2.

10

In the text field, type 0.5.

11

In the text field, type -1e-2.

12

In the text field, type 1.1.

1

Right-click and choose .

2

In the window for , locate the section.

3

In the text field, type w.

4

From the list, choose .

5

In the toolbar, click

.

6

Transient Forced Vibration - Max Displacement

1

In the toolbar, click

and choose .

2

In the window for , type Transient Forced Vibration - Max Displacement in the text field.

3

Locate the section. From the list, choose .

4

From the list, choose .

5

In the list, select .

6

Select Edge 1 only.

7

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


Expression	Unit	Description
w	mm	Displacement field, z component

8

Locate the section. From the list, choose .

9

Transient Forced Vibration - Max Stress

1

Right-click and choose .

2

In the window for , type Transient Forced Vibration - Max Stress in the text field.

3

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


Expression	Unit
abs(beam.sb1)	MPa

4

, then choose .

Transient Forced Vibration - Static Displacement

1

In the window, right-click and choose .

2

In the window for , type Transient Forced Vibration - Static Displacement in the text field.

3

Locate the section. From the list, choose .

4

In the text field, type range(1.1,1e-3,1.2).

5

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


Expression	Unit	Description
w	mm	Displacement field, z component

6

Locate the section. From the list, choose .

7

, then choose .

1

Go to the window.

The vibration analysis is now finished. If you want to save the model and run the study with the configuration set in the previous steps, you need to disable some of the nodes added after you run that particular study. If you do not want to save the model you do not need to follow the steps below.

Step 1: Eigenfrequency

1

In the window, under click .

2

In the window for , locate the section.

3

Select the check box.

4

In the tree, select .

5

Harmonic Forced Vibration

Step 2: Frequency Domain, Modal

1

In the window, under click .

2

In the window for , locate the section.

3

Select the check box.

4

In the tree, select .

5

6

In the tree, select .

7

Periodic Forced Vibration

Step 1: Frequency Domain

1

In the window, under click .

2

In the window for , locate the section.

3

In the tree, select .

4

Step 2: Frequency to Time FFT

1

In the window, click .

2

In the window for , locate the section.

3

In the tree, select .

4