PDF
Bracket — Eigenfrequency Analysis
Introduction
In this example you learn how to perform an eigenfrequency analysis for both an unloaded structure and a prestressed structure.
When the structure is subjected to a constant external load, the stiffness generated by the stress may affect the natural frequencies of the structure. Tensile stresses tend to increase the natural frequencies, while compressive stresses tend to decrease them.
It is recommended you review the Introduction to the Structural Mechanics Module, which includes background information and discusses the bracket_basic.mph model relevant to this example.
Model Definition
This tutorial is an extension of the example described in the section “The Fundamentals: A Static Linear Analysis” in the Introduction to the Structural Mechanics Module.
The model geometry is represented in Figure 1.
Figure 1: Geometry of the bracket.
In the first case, the natural frequency of the unloaded bracket is studied, while in the second case it is considered how the natural frequencies are affected by a static external load applied at the bracket holes. The left arm is under a pure tensile load while the right arm is under a pure compressive load.
Results and Discussion
Figure 2 and Figure 3 show the first six eigenmodes for both the unloaded and the prestressed case, respectively. The difference in the two first mode shapes between the two load cases is significant.
The two first mode shapes correspond to the bending mode in the x direction in the bracket arms. For the unloaded case these are expected to be approximately equal because of the symmetry. For the prestressed case, however, there will be a difference because of stress stiffening (left arm) and stress softening (right arm).
Figure 2: Six first eigenmode shapes for the unloaded case.
Figure 3: Six first eigenmode shapes for the prestressed case.
When comparing eigenmodes, it should be noted that the modes may be computed with reversed signs. This can even happen when the same study is run twice.
In Figure 4, the stress state from the static preload is shown.
Figure 4: Equivalent stress from the preload. Note the nonlinear color scale.
In Figure 5 below, the frequency shift in the two first eigenmodes is clearly visible.
Figure 5: Six first eigenfrequencies for the unloaded case (stars) and the prestressed case (circles).
For the unloaded case, the two first eigenfrequencies are 115 Hz and correspond to the bending mode in the x direction for the two bracket arms. For the prestressed load case, the eigenfrequencies for the bending modes are 107 Hz for one of the arms and 128 Hz for the other. Such a frequency shift is expected since a tensile load causes stress stiffening, while a compressive load causes stress softening. The other mode shapes are not significantly affected by the prestress.
Notes About the COMSOL Implementation
For a structural mechanics physics interface in COMSOL Multiphysics, there are two predefined study types available for eigenfrequency analysis: Eigenfrequency and Prestressed Analysis, Eigenfrequency.
The plain eigenfrequency analysis computes the natural frequencies of the unloaded structure. The contribution of any load boundary condition is disregarded and the Prescribed displacement constraints are considered as having the value zero.
In the prestressed eigenfrequency analysis, a stationary analysis is first performed to take into account the different loads and nonzero displacement constraints. The resulting stress is then automatically taken into account in the stiffness used in the eigenfrequency calculation.
Application Library path: Structural_Mechanics_Module/Tutorials/bracket_eigenfrequency
Modeling Instructions
Application Libraries
1
From the File menu, choose Application Libraries.
2
In the Application Libraries window, select Structural Mechanics Module>Tutorials>bracket_basic in the tree.
3
Click  Open.
Add Study
1
In the Home toolbar, click  Add Study to open the Add Study window.
2
Go to the Add Study window.
3
Find the Studies subsection. In the Select Study tree, select General Studies>Eigenfrequency.
4
Click Add Study in the window toolbar.
5
In the Home toolbar, click  Add Study to close the Add Study window.
Study 1
Step 1: Eigenfrequency
In the Eigenfrequency study node you have the possibility to select the number of eigenfrequencies to compute, and the frequency around which you would like to search for these frequencies. By default, the eigenvalue solver finds the six lowest frequencies.
1
In the Settings window for Eigenfrequency, locate the Study Settings section.
2
Select the Desired number of eigenfrequencies check box.
3
In the associated text field, type 10.
4
In the Home toolbar, click  Compute.
You can access the different eigenfrequency solutions in the 3D Plot Group Settings.
Note that the displacement values are normalized and have no physical significance. The normalization method can be changed in the Eigenvalue Solver node, located under the Solver Configuration node.
Modify the plot so that the first six eigenmodes are plotted side by side.
Results
Mode Shapes, Original
1
In the Settings window for 3D Plot Group, type Mode Shapes, Original in the Label text field.
2
Click to expand the Title section. From the Title type list, choose None.
3
Click to expand the Plot Array section. Select the Enable check box.
4
From the Array shape list, choose Square.
5
In the Relative row padding text field, type 0.4.
6
In the Relative column padding text field, type 0.4.
Surface 2
1
In the Model Builder window, expand the Mode Shapes, Original node.
2
Right-click Results>Mode Shapes, Original>Surface 1 and choose Duplicate.
3
In the Settings window for Surface, locate the Data section.
4
From the Dataset list, choose Study 1/Solution 1 (sol1).
5
From the Eigenfrequency (Hz) list, choose 115.58.
Surface 3
1
Right-click Surface 2 and choose Duplicate.
2
In the Settings window for Surface, locate the Data section.
3
From the Eigenfrequency (Hz) list, choose 289.84.
Surface 4
1
Right-click Surface 3 and choose Duplicate.
2
In the Settings window for Surface, locate the Data section.
3
From the Eigenfrequency (Hz) list, choose 308.17.
Surface 5
1
Right-click Surface 4 and choose Duplicate.
2
In the Settings window for Surface, locate the Data section.
3
From the Eigenfrequency (Hz) list, choose 365.14.
Surface 6
1
Right-click Surface 5 and choose Duplicate.
2
In the Settings window for Surface, locate the Data section.
3
From the Eigenfrequency (Hz) list, choose 583.22.
4
Click the  Zoom Extents button in the Graphics toolbar.
5
Click the  Show Grid button in the Graphics toolbar.
Parameters
1
In the Results toolbar, click  Parameters.
2
In the Settings window for Parameters, locate the Parameters section.
3
In the table, enter the following settings:
Name
Expression
Value
Description
dx
-0.05
-0.05
Annotation offset, X
dy
-0.3
-0.3
Annotation offset, Y
Annotation 1
1
In the Model Builder window, right-click Mode Shapes, Original and choose Annotation.
2
In the Settings window for Annotation, locate the Annotation section.
3
In the Text text field, type Mode 1.
4
Locate the Position section. In the X text field, type dx.
5
In the Y text field, type dy.
6
Locate the Coloring and Style section. Clear the Show point check box.
7
Click to expand the Plot Array section. Select the Manual indexing check box.
Annotation 2
1
Right-click Annotation 1 and choose Duplicate.
2
In the Settings window for Annotation, locate the Annotation section.
3
In the Text text field, type Mode 2.
4
Locate the Plot Array section. In the Column index text field, type 1.
Annotation 3
1
Right-click Annotation 2 and choose Duplicate.
2
In the Settings window for Annotation, locate the Annotation section.
3
In the Text text field, type Mode 3.
4
Locate the Plot Array section. In the Column index text field, type 2.
Annotation 4
1
Right-click Annotation 3 and choose Duplicate.
2
In the Settings window for Annotation, locate the Annotation section.
3
In the Text text field, type Mode 4.
4
Locate the Plot Array section. In the Row index text field, type 1.
5
In the Column index text field, type 0.
Annotation 5
1
Right-click Annotation 4 and choose Duplicate.
2
In the Settings window for Annotation, locate the Annotation section.
3
In the Text text field, type Mode 5.
4
Locate the Plot Array section. In the Column index text field, type 1.
Annotation 6
1
Right-click Annotation 5 and choose Duplicate.
2
In the Settings window for Annotation, locate the Annotation section.
3
In the Text text field, type Mode 6.
4
Locate the Plot Array section. In the Column index text field, type 2.
5
In the Mode Shapes, Original toolbar, click  Plot.
Global Evaluation 1
1
In the Results toolbar, click  Global Evaluation.
2
In the Settings window for Global Evaluation, locate the Expressions section.
3
In the table, enter the following settings:
Expression
Unit
Description
freq
Hz
Frequency
4
Click  Evaluate.
Global Definitions
Parameters 1
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, locate the Parameters section.
3
In the table, enter the following settings:
Name
Expression
Value
Description
P0
30[MPa]
3E7 Pa
Peak load intensity
YC
-300[mm]
-0.3 m
Y coordinate of hole center
Definitions
Analytic 1 (an1)
1
In the Home toolbar, click  Functions and choose Local>Analytic.
2
In the Settings window for Analytic, type load in the Function name text field.
3
Locate the Definition section. In the Expression text field, type F*cos(atan2(py,abs(px))).
4
In the Arguments text field, type F, py, px.
5
Locate the Units section. In the table, enter the following settings:
Argument
Unit
F
Pa
py
m
px
m
6
In the Function text field, type Pa.
Boundary System 1 (sys1)
The default boundary coordinate system will have axes that change orientation with the deformation. As an effect, the applied load would be interpreted as a follower load. In this case, the load is intended to have fixed directions.
1
In the Model Builder window, click Boundary System 1 (sys1).
2
In the Settings window for Boundary System, locate the Settings section.
3
From the Frame list, choose Reference configuration.
Solid Mechanics (solid)
Boundary Load 1
1
In the Model Builder window, under Component 1 (comp1) right-click Solid Mechanics (solid) and choose Boundary Load.
Apply a boundary load to the bracket holes.
2
In the Settings window for Boundary Load, locate the Boundary Selection section.
3
From the Selection list, choose Pin Holes.
4
Locate the Coordinate System Selection section. From the Coordinate system list, choose Boundary System 1 (sys1).
5
Locate the Force section. Specify the FA vector as
0
t1
0
t2
load(-P0,Z,Y-YC)*(sign(X)*(Y-YC)<0)
n
Add Study
1
In the Home toolbar, click  Add Study to open the Add Study window.
2
Go to the Add Study window.
The prestressed eigenfrequency analysis is available as a predefined study.
3
Find the Studies subsection. In the Select Study tree, select Preset Studies for Selected Physics Interfaces>Eigenfrequency, Prestressed.
4
Click Add Study in the window toolbar.
5
In the Home toolbar, click  Add Study to close the Add Study window.
Study 2
Step 1: Stationary
Note that the newly generated study combines one stationary analysis and one eigenfrequency analysis.
Step 2: Eigenfrequency
1
In the Model Builder window, click Step 2: Eigenfrequency.
2
In the Settings window for Eigenfrequency, locate the Study Settings section.
3
Select the Desired number of eigenfrequencies check box.
4
In the associated text field, type 10.
5
In the Search for eigenfrequencies around text field, type 100.
6
In the Model Builder window, click Study 2.
7
In the Settings window for Study, locate the Study Settings section.
8
Clear the Generate default plots check box.
9
In the Home toolbar, click  Compute.
Results
Mode Shapes, Prestressed
1
In the Model Builder window, right-click Mode Shapes, Original and choose Duplicate.
2
In the Model Builder window, click Mode Shapes, Original 1.
3
In the Settings window for 3D Plot Group, type Mode Shapes, Prestressed in the Label text field.
4
Locate the Data section. From the Dataset list, choose Study 2/Solution 2 (sol2).
Surface 2
1
In the Model Builder window, click Surface 2.
2
In the Settings window for Surface, locate the Data section.
3
From the Dataset list, choose Study 2/Solution 2 (sol2).
Surface 3
1
In the Model Builder window, click Surface 3.
2
In the Settings window for Surface, locate the Data section.
3
From the Dataset list, choose Study 2/Solution 2 (sol2).
Surface 4
1
In the Model Builder window, click Surface 4.
2
In the Settings window for Surface, locate the Data section.
3
From the Dataset list, choose Study 2/Solution 2 (sol2).
Surface 5
1
In the Model Builder window, click Surface 5.
2
In the Settings window for Surface, locate the Data section.
3
From the Dataset list, choose Study 2/Solution 2 (sol2).
Surface 6
1
In the Model Builder window, click Surface 6.
2
In the Settings window for Surface, locate the Data section.
3
From the Dataset list, choose Study 2/Solution 2 (sol2).
4
In the Mode Shapes, Prestressed toolbar, click  Plot.
In the settings for the second plot group you can see the list of the new eigenfrequencies. You can also find them tabulated in the Eigenfrequencies (Study 2) evaluation group
Global Evaluation 1
1
In the Model Builder window, under Results>Derived Values click Global Evaluation 1.
2
In the Settings window for Global Evaluation, locate the Data section.
3
From the Dataset list, choose Study 2/Solution 2 (sol2).
4
Locate the Expressions section. In the table, enter the following settings:
Expression
Unit
Description
freq
Hz
Frequency, Prestress
5
Click  Evaluate.
Stress From Static Load
1
In the Home toolbar, click  Add Plot Group and choose 3D Plot Group.
2
In the Settings window for 3D Plot Group, type Stress From Static Load in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study 2/Solution Store 1 (sol3).
Surface 1
1
Right-click Stress From Static Load and choose Surface.
2
Click the  Zoom Extents button in the Graphics toolbar.
3
In the Settings window for Surface, locate the Expression section.
4
In the Expression text field, type solid.mises.
5
From the Unit list, choose MPa.
6
Locate the Coloring and Style section. From the Color table list, choose Prism.
7
From the Color table transformation list, choose Nonlinear.
8
In the Color calibration parameter text field, type -1.4.
Deformation 1
1
Right-click Surface 1 and choose Deformation.
2
In the Stress From Static Load toolbar, click  Plot.
Arrow Surface 1
1
In the Model Builder window, right-click Stress From Static Load and choose Arrow Surface.
2
In the Settings window for Arrow Surface, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1)>Solid Mechanics>Load>solid.F_Ax,...,solid.F_Az - Load (spatial frame).
3
Locate the Coloring and Style section. From the Arrow base list, choose Head.
4
Locate the Arrow Positioning section. From the Placement list, choose Gauss points.
5
Locate the Coloring and Style section. Select the Scale factor check box.
6
In the associated text field, type 7E-10.
7
Click to expand the Inherit Style section. From the Plot list, choose Surface 1.
8
Clear the Color check box.
9
Clear the Color and data range check box.
Deformation 1
1
Right-click Arrow Surface 1 and choose Deformation.
2
In the Stress From Static Load toolbar, click  Plot.
Eigenfrequency Comparison
1
In the Home toolbar, click  Add Plot Group and choose 1D Plot Group.
2
In the Settings window for 1D Plot Group, type Eigenfrequency Comparison in the Label text field.
3
Locate the Plot Settings section. Select the y-axis label check box.
4
In the associated text field, type Frequency [Hz].
5
Locate the Grid section. Select the Manual spacing check box.
6
Locate the Legend section. From the Position list, choose Upper left.
Table Graph 1
1
Right-click Eigenfrequency Comparison and choose Table Graph.
2
In the Settings window for Table Graph, locate the Data section.
3
From the x-axis data list, choose Row index.
4
From the Plot columns list, choose Manual.
5
In the Columns list, choose Frequency (Hz) and Frequency, Prestress (Hz).
6
Click to expand the Legends section. Select the Show legends check box.
7
Locate the Coloring and Style section. Find the Line style subsection. From the Line list, choose None.
8
Find the Line markers subsection. From the Marker list, choose Cycle.
9
From the Positioning list, choose In data points.
10
In the Eigenfrequency Comparison toolbar, click  Plot.
11
Click the  y-Axis Log Scale button in the Graphics toolbar.