PDF
Static and Eigenfrequency Analyses of an Elbow Bracket
Introduction
The component shown in Figure 1 is part of a support mechanism and is subjected to different types of loads. This tutorial model takes you through the steps to carry out a detailed analysis of the part using the Structural Mechanics Module.
Figure 1: Geometry of the elbow bracket.
In the various parts of the example you are introduced to using the some basic analysis types, together with numerous postprocessing possibilities. These analysis types are:
•
Static analysis
•
Eigenfrequency analysis
•
Damped eigenfrequency analysis
In an extended version of this model, also the following study types are covered:
•
Transient analysis
•
Modal based transient analysis
•
Frequency response analysis
•
Modal based frequency response analysis
•
Parametric analysis
•
Linear buckling analysis
This tutorial model comes in two versions:
•
A short version, elbow_bracket_brief, treating the three first analysis types in the above list.
•
A complete version, elbow_bracket, treating all nine analysis types.
Each of the listed analysis types corresponds to a study type; the available studies are described in the section Study Types in the Structural Mechanics Module User’s Guide. The chapter Structural Mechanics Modeling in the same manual provides further assistance.
Model Definition
The geometry for this part, see Figure 1, has been created with a CAD software, and it is available for you to import into COMSOL Multiphysics.
Material
The material is structural steel, as taken from the material library, with Young’s modulus 200 GPa and Poisson’s ratio of 0.33.
Damping
The Structural Mechanics Module supports several types damping for dynamic analysis. You can also use no damping, which is the default option.
In some of the studies Rayleigh damping is used. It is defined by two scalar damping parameters that are multipliers to the mass matrix (αdM) and stiffness matrix (βdK) in the following way:
where C is the damping matrix, M is the mass matrix, and K is the stiffness matrix. The damping is specified locally in each domain; this means that you can specify different damping parameters in different parts of the model. This is an extension of the common definition of Rayleigh damping.
To find values for the Rayleigh damping parameters, you can use the relations between the critical damping ratio and the Rayleigh damping parameters. It is often easier to interpret the critical damping ratios, which are given by
where ξi is the critical damping ratio at a specific angular frequency ωi. Knowing two pairs of corresponding ξi and ωi results in a system of equations from which the damping parameters can be determined. This method of determining the Rayleigh damping parameters is built-in.
Assume that the structure has a constant damping ratio of 0.1. Select two frequencies near the excitation frequency, 400 Hz and 600 Hz. This will result in αdM = 302 s-1 and βdK = 3.18·10−5 s.
For more information see the section Mechanical Damping and Losses in the Structural Mechanics Module User’s Guide.
If modal-based dynamic response studies are performed, it is usually easier to give the critical damping ratios directly. This also gives more detailed control over the damping properties over a large frequency range.
Loads and Constraints
The displacement are fixed in all directions on the face shown in Figure 2. The load is described under each study, but in all cases it is distributed over the face as shown in this figure.
Figure 2: Constraint and loading of the bracket.
The Application Libraries note immediately below appears in the discussion of every model. The path indicates the location of the example file in the Application Libraries root directory. The most convenient way to open it is from the Application Libraries window in the COMSOL Desktop, which you can open from the File menu.
Application Library path: Structural_Mechanics_Module/Tutorials/elbow_bracket_brief
Modeling Instructions
From the File menu, choose New.
New
In the New window, click  Model Wizard.
Model Wizard
1
In the Model Wizard window, click  3D.
2
In the Select Physics tree, select Structural Mechanics>Solid Mechanics (solid).
3
Click Add.
4
Click  Study.
5
In the Select Study tree, select General Studies>Stationary.
6
Click  Done.
Geometry 1
Import 1 (imp1)
1
In the Home toolbar, click  Import.
2
In the Settings window for Import, locate the Import section.
3
From the Source list, choose COMSOL Multiphysics file.
4
Click  Browse.
5
Browse to the model’s Application Libraries folder and double-click the file elbow_bracket.mphbin.
6
Click  Import.
7
Click the  Wireframe Rendering button in the Graphics toolbar.
The view in the Graphics window should look like that in the image below.
8
Click the  Wireframe Rendering button in the Graphics toolbar to return to the default surface rendering.
Suppress some edges during meshing, in order to avoid generation of unnecessary small elements.
Ignore Edges 1 (ige1)
1
In the Geometry toolbar, click  Virtual Operations and choose Ignore Edges.
2
On the object fin, select Edges 17, 21, 23, 27, 38, 40, 42, and 44 only.
It might be easier to select the correct edges by using the Selection List window. To open this window, in the Home toolbar click Windows and choose Selection List. (If you are running the cross-platform desktop, you find Windows in the main menu.)
Mesh 1
Free Tetrahedral 1
In the Mesh toolbar, click  Free Tetrahedral.
Size
There are nine predefined combinations of mesh parameter settings. They range from Extremely fine to Extremely coarse, with Normal as the default setting. Unless any other mesh parameters are set, this is the setting that is used if you use Build All or Build Selected to generate the mesh.
As a stress concentration can be expected in the corner of the bracket, put a finer mesh there.
Size 1
1
In the Model Builder window, right-click Free Tetrahedral 1 and choose Size.
2
In the Settings window for Size, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Boundary.
4
Locate the Element Size section. From the Predefined list, choose Extra fine.
5
Select Boundaries 13 and 14 only.
6
In the Model Builder window, right-click Mesh 1 and choose Build All.
Materials
Next, specify the material properties. You can do this either by explicitly typing them in or by selecting a library material in the Material Browser. For this model, use a library material.
Add Material
1
In the Home toolbar, click  Add Material to open the Add Material window.
2
Go to the Add Material window.
3
In the tree, select Built-in>Structural steel.
4
Click Add to Component in the window toolbar.
In the Home toolbar, click  Add Material to close the Add Material window.
Static Analysis
A static analysis has no explicit or implicit time dependencies. This situation corresponds to the steady state with constant (in time) boundary conditions and material properties.
The purpose of such analysis can be to find the maximum stress level and compare it with the material’s yield strength, as well as to check that the deformation of the component is within the limits of the design criteria.
Results and Discussion
The analysis shows that the von Mises equivalent stress has a maximum value of about 190 MPa, which, compared with the material’s yield strength of 350 MPa, results in a utilization factor of 54%.
The analysis also gives the maximum static displacements as 1.14 mm.
Three different representations of the stress state are shown in Figure 3 through Figure 5.
Figure 3: Equivalent stresses on the boundary of the domain.
Figure 4: Isosurface plot of the equivalent stress.
Figure 5: Arrow plot of the principal stresses.
Modeling Instructions
Solid Mechanics (solid)
Fixed Constraint 1
1
In the Model Builder window, under Component 1 (comp1) right-click Solid Mechanics (solid) and choose Fixed Constraint.
2
Select Boundary 1 only.
Boundary Load 1
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
Select Boundary 21 only.
3
In the Settings window for Boundary Load, locate the Force section.
4
Specify the FA vector as
3[MPa]
x
0
y
3[MPa]
z
Study 1 (Static)
In this model, where there are many different studies, it is a good idea to assign manual names to some nodes in the model tree.
1
In the Model Builder window, click Study 1.
2
In the Settings window for Study, type Study 1 (Static) in the Label text field.
The default settings in the generated solver are OK for this model, so it can be run directly.
3
In the Home toolbar, click  Compute.
Before moving on to analyzing the solution, rename the solver.
Solution, Static
1
In the Model Builder window, expand the Study 1 (Static)>Solver Configurations node, then click Solution 1 (sol1).
2
In the Settings window for Solution, type Solution, Static in the Label text field.
Results
Similarly, rename the solution dataset.
Static Solution
1
In the Model Builder window, expand the Results>Datasets node, then click Study 1 (Static)/Solution, Static (sol1).
2
In the Settings window for Solution, type Static Solution in the Label text field.
In the Results branch, you can create various plot types, evaluate expressions, or animate the results. The result features can visualize any expression containing, for example, the solution variables, their derivatives, and the space coordinates. Many frequently used expressions are predefined as postprocessing variables, and they are directly available in the Expression section menus for the various plot types.
When the solver finishes, a default plot appears. It shows a volume plot of the von Mises stress with the deformed shape of the component. For future reference, you can rename it.
Static Stress Contour
1
In the Model Builder window, under Results click Stress (solid).
2
In the Settings window for 3D Plot Group, type Static Stress Contour in the Label text field.
Volume 1
1
In the Model Builder window, expand the Static Stress Contour node, then click Volume 1.
2
In the Settings window for Volume, locate the Expression section.
3
From the Unit list, choose MPa.
4
In the Static Stress Contour toolbar, click  Plot.
5
Click the  Zoom Extents button in the Graphics toolbar.
The applied loads are also available in a default plot.
Applied Loads, Static Solution
1
In the Model Builder window, under Results click Applied Loads (solid).
2
In the Settings window for Group, type Applied Loads, Static Solution in the Label text field.
Boundary Loads (solid)
In the Model Builder window, expand the Applied Loads, Static Solution node.
In order not to hide any load vectors, a wireframe representation is used for the geometry as a default. The plot group is however prepared for a visualization with hidden surfaces.
Gray Surfaces
In the Model Builder window, expand the Boundary Loads (solid) node.
Transparency 1
1
In the Model Builder window, expand the Gray Surfaces node.
2
Right-click Transparency 1 and choose Disable.
Boundary Loads (solid)
1
In the Model Builder window, under Results>Applied Loads, Static Solution click Boundary Loads (solid).
2
In the Boundary Loads (solid) toolbar, click  Plot.
To evaluate the maximum displacement, use a nonlocal maximum coupling.
Definitions
Maximum 1 (maxop1)
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Maximum.
2
In the Settings window for Maximum, locate the Source Selection section.
3
From the Geometric entity level list, choose Boundary.
4
From the Selection list, choose All boundaries.
Variables 1
1
In the Definitions toolbar, click  Local Variables.
2
In the Settings window for Variables, locate the Variables section.
3
In the table, enter the following settings:
Name
Expression
Unit
Description
U_max
maxop1(solid.disp)
m
Maximum deflection
Study 1 (Static)
Solution, Static (sol1)
1
In the Model Builder window, under Study 1 (Static)>Solver Configurations right-click Solution, Static (sol1) and choose Solution>Update.
This step is necessary in order to access variables that were created after the solution was performed.
Results
Global Evaluation 1
1
In the Results toolbar, click  Global Evaluation.
2
In the Settings window for Global Evaluation, click Replace Expression in the upper-right corner of the Expressions section. From the menu, choose Component 1 (comp1)>Definitions>Variables>U_max - Maximum deflection - m.
3
Locate the Expressions section. In the table, enter the following settings:
Expression
Unit
Description
U_max
mm
Maximum deflection
4
Click  Evaluate.
The result, approximately 1.1 mm appears in the Table window.
Next, add a second plot group and create an isosurface plot. The resulting plot should resemble that in Figure 4.
Static Stress Isosurface
1
In the Results toolbar, click  3D Plot Group.
2
In the Settings window for 3D Plot Group, type Static Stress Isosurface in the Label text field.
Isosurface 1
1
Right-click Static Stress Isosurface and choose Isosurface.
2
In the Settings window for Isosurface, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1)>Solid Mechanics>Stress>solid.mises - von Mises stress - N/m².
3
Locate the Expression section. From the Unit list, choose MPa.
Deformation 1
1
Right-click Isosurface 1 and choose Deformation.
2
Click the  Go to Default View button in the Graphics toolbar.
With the following steps you can reproduce the principal stress arrow plot shown in Figure 5:
Static Principal Stress Arrow Plot
1
In the Results toolbar, click  3D Plot Group.
2
In the Settings window for 3D Plot Group, type Static Principal Stress Arrow Plot in the Label text field.
Principal Stress Volume 1
1
In the Static Principal Stress Arrow Plot toolbar, click  More Plots and choose Principal Stress Volume.
2
In the Settings window for Principal Stress Volume, locate the Positioning section.
3
Find the X grid points subsection. In the Points text field, type 10.
4
Find the Y grid points subsection. In the Points text field, type 15.
5
Find the Z grid points subsection. In the Points text field, type 10.
In the Static Principal Stress Arrow Plot toolbar, click  Plot.
Eigenfrequency Analysis
An eigenfrequency analysis finds the eigenfrequencies and modes of deformation of a component. The eigenfrequencies f in the structural mechanics field are related to the eigenvalues λ returned by the solvers through
In COMSOL Multiphysics you can choose between working with eigenfrequencies and working with eigenvalues according to your preferences. Eigenfrequencies is the default option for all physics interfaces in the Structural Mechanics Module.
If no damping is included in the material, the undamped natural frequencies are computed.
The purpose of the following eigenfrequency analysis is to find the six lowest eigenfrequencies and corresponding mode shapes.
Results and Discussion
The first six eigenfrequencies are:
Eigenfrequency
Frequency
 f1
416 Hz
 f2
573 Hz
 f3
1924 Hz
 f4
2459 Hz
 f5
3112 Hz
 f6
3956 Hz
The mode shapes corresponding to the two lowest eigenfrequencies are shown in Figure 6. The deformed plot indicates an oscillation in the xy-plane for the lowest eigenfrequency, while the second lowest eigenmode shows an oscillation in the yz-plane.
Figure 6: Eigenmodes of the two lowest eigenfrequencies.
Notes About the COMSOL Implementation
Any loads present on the model, such as the load from the static load case above, are ignored in the default eigenfrequency analysis. It is also possible to include effects from prestress. You can find an example of such an analysis in the example Vibrating String.
Modeling Instructions
Add a new study to your model.
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 2 (Eigenfrequency)
1
In the Model Builder window, click Study 2.
2
In the Settings window for Study, type Study 2 (Eigenfrequency) in the Label text field.
3
In the Home toolbar, click  Compute.
Solution, Eigenfrequency
1
In the Model Builder window, expand the Study 2 (Eigenfrequency)>Solver Configurations node, then click Solution 2 (sol2).
2
In the Settings window for Solution, type Solution, Eigenfrequency in the Label text field.
Results
Eigenfrequency Solution
1
In the Model Builder window, under Results>Datasets click Study 2 (Eigenfrequency)/Solution, Eigenfrequency (sol2).
2
In the Settings window for Solution, type Eigenfrequency Solution in the Label text field.
Undamped Mode Shapes
As a default, the first eigenmode is shown. Follow these steps to reproduce the plot in the left panel of Figure 6.
Take a look at the second mode as well.
1
In the Model Builder window, under Results click Mode Shape (solid).
2
In the Settings window for 3D Plot Group, locate the Data section.
3
From the Eigenfrequency (Hz) list, choose 573.44.
4
In the Mode Shape (solid) toolbar, click  Plot.
Compare the resulting plot to that to the right in Figure 6.
You can give the plot a more descriptive name:
5
In the Label text field, type Undamped Mode Shapes.
Animation 1
In the Undamped Mode Shapes toolbar, click  Animation and choose Player.
Mode Shape Animation
This creates an animation showing how the elbow bracket would deform if subjected to a harmonic load with a frequency near the selected eigenfrequency, in this case 571 Hz. To play the movie again, click the Play button in the Graphics toolbar.
The default animation sequence type when you add a player this way is Dynamic data extension. If you set the Sequence type to Stored solutions and then click the Generate Frame button, you get an animation where each frame corresponds to an eigenmode in the Eigenfrequency list. By using the Frame number slider in the Frames section you can then easily browse the eigenmodes.
Rename the player:
1
In the Model Builder window, expand the Results>Undamped Mode Shapes node, then click Results>Export>Animation 1.
2
In the Settings window for Animation, type Mode Shape Animation in the Label text field.
Damped Eigenfrequency Analysis
If the material has damping, the eigenvalue solver automatically switches to computation of the damped eigenfrequencies. The damped eigenfrequencies and eigenmodes are complex. The real part of the eigenfrequency corresponds to the frequency and the imaginary part represents the damping.
Results and Discussion
The first six eigenfrequencies (rounded to three digits) are given below, and can be compared with the results from the undamped model.:
Eigenfrequency
Frequency
undamped Frequency
 f1
414+41.3i Hz
416 Hz
 f2
571+56.9i Hz
573 Hz
 f3
1884+394i Hz
1924 Hz
 f4
2377+628i Hz
2459 Hz
 f5
2950+992i Hz
3112 Hz
 f6
3623+1589i Hz
3956 Hz
The damping ratio of a certain mode is the ratio between the imaginary and the real part. It can be seen that the damping ratio increases rapidly as the natural frequency increases. This is an effect of the Rayleigh damping model.
You can find a table of the eigenfrequencies and corresponding damping in the evaluation group Eigenfrequencies (Study 3 (Damped Eigenfrequency)).
Modeling Instructions
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.
Solid Mechanics (solid)
Add damping.
Linear Elastic Material 1
In the Model Builder window, under Component 1 (comp1)>Solid Mechanics (solid) click Linear Elastic Material 1.
Damping 1
1
In the Physics toolbar, click  Attributes and choose Damping.
2
In the Settings window for Damping, locate the Damping Settings section.
3
From the Input parameters list, choose Damping ratios.
4
In the f1 text field, type 400.
5
In the ζ1 text field, type 0.1.
6
In the f2 text field, type 600.
7
In the ζ2 text field, type 0.1.
Study 3 (Damped Eigenfrequency)
1
In the Model Builder window, click Study 3.
2
In the Settings window for Study, type Study 3 (Damped Eigenfrequency) in the Label text field.
3
In the Home toolbar, click  Compute.
Solution, Damped Eigenfrequency
1
In the Model Builder window, expand the Study 3 (Damped Eigenfrequency)>Solver Configurations node, then click Solution 3 (sol3).
2
In the Settings window for Solution, type Solution, Damped Eigenfrequency in the Label text field.
Results
Damped Eigenfrequency Solution
1
In the Model Builder window, under Results>Datasets click Study 3 (Damped Eigenfrequency)/Solution, Damped Eigenfrequency (sol3).
2
In the Settings window for Solution, type Damped Eigenfrequency Solution in the Label text field.
Damped Mode Shapes
1
In the Model Builder window, under Results click Mode Shape (solid).
2
In the Settings window for 3D Plot Group, type Damped Mode Shapes in the Label text field.
The mode shape identical to the one obtained when solving the undamped problem. Only the frequency has changed.
Surface 1
The second study should still produce undamped eigenfrequencies when it is run next time, so you must make sure that the newly added Damping node is ignored.
Study 2 (Eigenfrequency)
Step 1: Eigenfrequency
1
In the Model Builder window, expand the Damped Mode Shapes node, then click Study 2 (Eigenfrequency)>Step 1: Eigenfrequency.
2
In the Settings window for Eigenfrequency, locate the Physics and Variables Selection section.
3
Select the Modify model configuration for study step check box.
4
In the tree, select Component 1 (Comp1)>Solid Mechanics (Solid)>Linear Elastic Material 1>Damping 1.
5
Click  Disable.