PDF
Viscoelastic Structural Damper — Transient Analysis
Introduction
The model studies the forced response of a typical viscoelastic damper. Damping elements involving layers of viscoelastic materials are often used for reduction of seismic and wind induced vibrations in buildings and other tall structures. The common feature is that the frequency of the forced vibrations is low.
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.
The viscoelastic layers are modeled with the generalized Maxwell model available in COMSOL Multiphysics. The generalized Maxwell model represents the viscoelastic material as a series of branches, each with a spring-dashpot pair.
Eighteen viscoelastic branches guarantee the accurate representation of the material behavior for different excitation frequencies, when the damper is subjected to forced vibration. The values of the shear moduli and relaxation times for each branch are available in Ref. 1. They are summarized in the following table:
Table 1: Model Data for the Viscoelastic Damper Model.
Property
Value
Description
 K
40 GPa
Bulk modulus
 G
58.6 kPa
Long time shear modulus
 ρ
1.06 g/cm3
Density
 G1
13.3 MPa
Shear modulus, branch 1
 τ1
10-7 s
Relaxation time, branch 1
 G2
286 MPa
Shear modulus, branch 2
 τ2
10-6 s
Relaxation time, branch 2
 G3
291 MPa
Shear modulus, branch 3
 τ3
3.16·10-6 s
Relaxation time, branch 3
 G4
212 MPa
Shear modulus, branch 4
 τ4
10-5 s
Relaxation time, branch 4
 G5
112 MPa
Shear modulus, branch 5
 τ5
3.16·10-5 s
Relaxation time, branch 5
 G6
61.6 MPa
Shear modulus, branch 6
 τ6
10-4 s
Relaxation time, branch 6
 G7
29.8 MPa
Shear modulus, branch 7
 τ7
3.16·10-4 s
Relaxation time, branch 7
 G8
16.1 MPa
Shear modulus, branch 8
 τ8
10-3 s
Relaxation time, branch 8
 G9
7.83 MPa
Shear modulus, branch 9
 τ9
3.16·10-3 s
Relaxation time, branch 9
 G10
4.15 MPa
Shear modulus, branch 10
 τ10
10-2 s
Relaxation time, branch 10
 G11
2.03 MPa
Shear modulus, branch 11
 τ11
3.16·10-2 s
Relaxation time, branch 11
 G12
1.11 MPa
Shear modulus, branch 12
 τ12
0.1 s
Relaxation time, branch 12
 G13
0.491 MPa
Shear modulus, branch 13
 τ13
0.316 s
Relaxation time, branch 13
 G14
0.326 MPa
Shear modulus, branch 14
 τ14
1 s
Relaxation time, branch 14
 G15
8.25·10-2 MPa
Shear modulus, branch 15
 τ15
3.16 s
Relaxation time, branch 15
 G16
0.126 MPa
Shear modulus, branch 16
 τ16
10 s
Relaxation time, branch 16
 G17
3.73·10-2 MPa
Shear modulus, branch 17
 τ17
100 s
Relaxation time, branch 17
 G18
1.18·10-2 MPa
Shear modulus, branch 18
 τ18
1000 s
Relaxation time, branch 18
One of the mounting elements is fixed; the other two are loaded with periodic forces with a frequency of 3 Hz.
Some viscoelastic branches may relax much faster or much slower than the time scale of the excitation period. In such cases the corresponding dashpots may be considered to be either fully relaxed or rigid. These branches may then be removed and instead grouped into equivalent branches. This reduction of the number of individual branches, or “pruning”, is beneficial because each branch adds auxiliary strain variables that need to be solved for in a time-dependent study. Therefore, including a large number of branches may increase the computational cost unnecessarily as some of the branches may have no significant effect on the results. Excluding branches which do not contribute in a relevant way given a range of the excitation frequency is described in more detail in the theory chapter of the Structural Mechanics Module User’s Guide under Structural Mechanics Theory > Material Models > Linear Viscoelasticity.
Results and Discussion
Figure 2 shows the results of the transient computations after three seconds of forced vibrations.
Figure 2: Displacement field.
The typical viscoelastic hysteresis loops for a point within one of the mounting elements are shown in Figure 3. The hysteresis loops are plotted for the cases when including all 18 viscoelastic branches and when pruning some of the branches. In the latter case effectively only six branches are solved for. The case with pruning shows only a small difference when compared to the solution including all branches; however, the pruned case has a significantly lower computation time. In both time-dependent cases the solutions converge to the response obtained by a frequency-domain analysis.
Figure 3: Displacement versus applied force.
Notes About the COMSOL Implementation
The damper is excited with a harmonic load at 3 Hz. Not all branches listed inTable 1 contribute in a significant way and may therefore be “pruned” with a corresponding setting in the model’s Viscoelasticity node. The pruning is done automatically and only requires you to enter cutoff frequencies; that is, frequencies deemed not relevant given the load frequency. To show the difference in results as well as in computation cost, two studies will be set up: one including all viscoelastic branches and the other with pruning enabled. The latter study has a lower computational cost as fewer auxiliary variables need to be solved for.
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.
Application Library path: Structural_Mechanics_Module/Dynamics_and_Vibration/viscoelastic_damper_transient
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 > Time Dependent.
6
Click  Done.
Geometry 1
Import the predefined geometry from a file.
1
In the Geometry toolbar, click Insert Sequence and choose Insert Sequence.
2
Browse to the model’s Application Libraries folder and double-click the file viscoelastic_damper_geom_sequence.mph.
The imported geometry should look similar to that shown in Figure 1.
Solid Mechanics (solid)
Linear Elastic Material 2
1
In the Physics toolbar, click  Domains and choose Linear Elastic Material.
2
In the Settings window for Linear Elastic Material, locate the Linear Elastic Material section.
3
From the Specify list, choose Bulk modulus and shear modulus.
4
From the Use mixed formulation list, choose Pressure formulation.
The local computations at Gauss points during assembly are expensive for the viscoelasticity model. Using a reduced integration scheme will reduce the overall simulation time.
5
Locate the Quadrature Settings section. Select the Reduced integration checkbox.
6
Select Domains 2 and 5 only.
Viscoelasticity (No Pruning)
1
In the Physics toolbar, click  Attributes and choose Viscoelasticity.
2
In the Settings window for Viscoelasticity, type Viscoelasticity (No Pruning) in the Label text field.
Since there are 18 branches in this material model, the data has been collected in a text file which you can load.
3
Locate the Viscoelasticity Model section. Click to select the first row in the table.
4
Click  Delete.
5
Click  Load from File.
6
Browse to the model’s Application Libraries folder and double-click the file viscoelastic_damper_viscoelastic_data.txt.
Viscoelasticity (With Pruning)
1
Right-click Viscoelasticity (No Pruning) and choose Duplicate.
2
In the Settings window for Viscoelasticity, type Viscoelasticity (With Pruning) in the Label text field.
3
Locate the Viscoelasticity Model section. Select the Prune viscoelastic branches checkbox.
4
In the flower text field, type 0.3.
5
In the fupper text field, type 30.
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 > Steel AISI 4340.
4
Click the Add to Component button in the window toolbar.
Materials
Viscoelastic
1
In the Model Builder window, under Component 1 (comp1) right-click Materials and choose Blank Material.
2
In the Settings window for Material, type Viscoelastic in the Label text field.
3
Select Domains 2 and 5 only.
4
Locate the Material Contents 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
5
In the Materials toolbar, click  Add Material to close the Add Material window.
6
In the Settings window for Materials, in the Graphics window toolbar, clicknext to  Colors, then choose Show Material Color and Texture.
Definitions
Ramp 1 (rm1)
1
In the Definitions toolbar, click  More Functions and choose Ramp.
Create a ramp function to apply the loads smoothly.
2
In the Settings window for Ramp, locate the Parameters section.
3
In the Location text field, type 0.02[s].
4
In the Slope text field, type 10.
5
Click to expand the Smoothing section.
6
Select the Size of transition zone at start checkbox. In the associated text field, type 0.01.
7
Locate the Parameters section. Select the Cutoff checkbox.
8
Locate the Smoothing section.
9
Select the Size of transition zone at cutoff checkbox. In the associated text field, type 0.01.
Solid Mechanics (solid)
Fixed Constraint 1
1
In the Physics toolbar, click  Boundaries and choose Fixed Constraint.
2
In the Settings window for Fixed Constraint, locate the Boundary Selection section.
3
From the Selection list, choose Bottom Holes.
Prescribed Displacement 1
1
In the Physics toolbar, click  Boundaries and choose Prescribed Displacement.
2
In the Settings window for Prescribed Displacement, locate the Boundary Selection section.
3
From the Selection list, choose Right Hole.
4
Locate the Prescribed Displacement section. From the Displacement in x direction list, choose Prescribed.
5
From the Displacement in y direction list, choose Prescribed.
Boundary Load 1
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
In the Settings window for Boundary Load, locate the Boundary Selection section.
3
From the Selection list, choose Right Hole.
4
Locate the Force section. Specify the fA vector as
0
x
0
y
8.5[MPa]*sin(pi/2+2*pi*t*3[Hz])*rm1(t)
z
Prescribed Displacement 2
1
In the Physics toolbar, click  Boundaries and choose Prescribed Displacement.
2
In the Settings window for Prescribed Displacement, locate the Boundary Selection section.
3
From the Selection list, choose Left Hole.
4
Locate the Prescribed Displacement section. From the Displacement in y direction list, choose Prescribed.
Boundary Load 2
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
In the Settings window for Boundary Load, locate the Boundary Selection section.
3
From the Selection list, choose Left Hole.
4
Locate the Force section. Specify the fA vector as
0.5[MPa]*sin(2*pi*t*3[Hz])*rm1(t)
x
0
y
8.5[MPa]*sin(2*pi*t*3[Hz])*rm1(t)
z
Definitions
Set up a nonlocal integration coupling to compute the total force applied to one of the mounting holes. You configure the integration to be performed in the material frame, because this is the frame used within the Solid Mechanics interface.
Integration 1 (intop1)
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Integration.
2
In the Settings window for Integration, locate the Advanced section.
3
From the Frame list, choose Material  (X, Y, Z).
4
Locate the Source Selection section. From the Geometric entity level list, choose Boundary.
5
From the Selection list, choose Left Hole.
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
Fz1
intop1(solid.FperAreaz)
N
Total force, Z component
Mesh 1
Free Quad 1
1
In the Mesh toolbar, click  More Generators and choose Free Quad.
2
Select Boundary 30 only.
Size 1
1
Right-click Free Quad 1 and choose Size.
2
In the Settings window for Size, locate the Element Size section.
3
From the Predefined list, choose Finer.
Distribution 1
1
In the Model Builder window, right-click Free Quad 1 and choose Distribution.
2
Select Edge 65 only.
Swept 1
1
In the Mesh toolbar, click  Swept.
2
In the Settings window for Swept, locate the Domain Selection section.
3
From the Geometric entity level list, choose Domain.
4
Select Domain 7 only.
Distribution 1
1
Right-click Swept 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Distribution section.
3
In the Number of elements text field, type 2.
Free Quad 2
1
In the Mesh toolbar, click  More Generators and choose Free Quad.
2
Select Boundaries 2 and 61 only.
Size 1
1
Right-click Free Quad 2 and choose Size.
2
In the Settings window for Size, locate the Element Size section.
3
From the Predefined list, choose Fine.
Swept 2
1
In the Mesh toolbar, click  Swept.
2
In the Settings window for Swept, locate the Domain Selection section.
3
From the Geometric entity level list, choose Domain.
4
Select Domains 1, 2, and 4 only.
Distribution 1
1
Right-click Swept 2 and choose Distribution.
2
In the Settings window for Distribution, locate the Distribution section.
3
In the Number of elements text field, type 2.
Copy Domain 1
1
In the Model Builder window, right-click Mesh 1 and choose Copying Operations > Copy Domain.
2
Select Domains 1, 2, and 7 only.
3
In the Settings window for Copy Domain, locate the Destination Domains section.
4
Click to select the  Activate Selection toggle button.
5
Select Domains 5, 6, and 8 only.
Free Quad 3
1
In the Mesh toolbar, click  More Generators and choose Free Quad.
2
Select Boundary 10 only.
Swept 3
1
In the Mesh toolbar, click  Swept.
2
In the Settings window for Swept, click  Build All.
The complete mesh should look similar to that shown in the figure below.
Study 1: No Pruning
1
In the Model Builder window, click Study 1.
2
In the Settings window for Study, type Study 1: No Pruning in the Label text field.
Step 1: Time Dependent
1
In the Model Builder window, under Study 1: No Pruning click Step 1: Time Dependent.
2
In the Settings window for Time Dependent, locate the Study Settings section.
3
In the Output times text field, type range(0, 0.01, 3).
4
Locate the Physics and Variables Selection section. Select the Modify model configuration for study step checkbox.
5
In the tree, select Component 1 (comp1) > Solid Mechanics (solid) > Linear Elastic Material 2 > Viscoelasticity (With Pruning).
6
Right-click and choose Disable.
Solution 1 (sol1)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 1 (sol1) node.
3
In the Model Builder window, expand the Study 1: No Pruning > Solver Configurations > Solution 1 (sol1) > Dependent Variables 1 node, then click Auxiliary Pressure (comp1.solid.lemm2.pw).
4
In the Settings window for Field, locate the Scaling section.
5
From the Method list, choose Manual.
6
In the Scale text field, type 1e6.
Excluding algebraic error estimates allows the solver to take larger time steps.
7
In the Model Builder window, under Study 1: No Pruning > Solver Configurations > Solution 1 (sol1) click Time-Dependent Solver 1.
8
In the Settings window for Time-Dependent Solver, click to expand the Time Stepping section.
9
Find the Algebraic variable settings subsection. From the Error estimation list, choose Exclude algebraic.
Results
Before computing the solution, set up a displacement plot that will be displayed and updated after every time step of the transient analysis.
Displacement (No Pruning)
1
In the Results toolbar, click  3D Plot Group.
2
In the Settings window for 3D Plot Group, type Displacement (No Pruning) in the Label text field.
Surface 1
1
Right-click Displacement (No Pruning) and choose Surface.
2
In the Settings window for Surface, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1) > Solid Mechanics > Displacement > Displacement field - m > w - Displacement field, Z-component.
3
Locate the Coloring and Style section. From the Color table list, choose SpectrumLight.
Deformation 1
Right-click Surface 1 and choose Deformation.
Study 1: No Pruning
Step 1: Time Dependent
1
In the Settings window for Time Dependent, click to expand the Results While Solving section.
2
Select the Plot checkbox.
Solution 1 (sol1)
In the Model Builder window, under Study 1: No Pruning > Solver Configurations right-click Solution 1 (sol1) and choose Run.
Results
Displacement (No Pruning)
The computed solution should closely resemble that shown in Figure 2.
To plot the displacement versus applied force, follow these steps:
Table 1
1
In the Results toolbar, click  Table.
Import the frequency domain solution.
2
In the Settings window for Table, locate the Data section.
3
Click  Import.
4
Browse to the model’s Application Libraries folder and double-click the file viscoelastic_damper_frequency_solution.txt.
Hysteresis Loops
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Hysteresis Loops in the Label text field.
3
Click to expand the Title section. From the Title type list, choose None.
4
Locate the Plot Settings section.
5
Select the x-axis label checkbox. In the associated text field, type Fz1 [kN].
6
Select the y-axis label checkbox. In the associated text field, type w [mm].
Table Graph 1
1
Right-click Hysteresis Loops and choose Table Graph.
2
In the Settings window for Table Graph, locate the Coloring and Style section.
3
Find the Line style subsection. From the Line list, choose Dashed.
4
From the Width list, choose 2.
5
Click to expand the Legends section. Select the Show legends checkbox.
6
From the Legends list, choose Manual.
7
In the table, enter the following settings:
Legends
Frequency-domain solution
Point Graph 1
1
In the Model Builder window, right-click Hysteresis Loops and choose Point Graph.
2
Select Point 25 only.
3
In the Settings window for Point Graph, locate the x-Axis Data section.
4
From the Parameter list, choose Expression.
5
Click Replace Expression in the upper-right corner of the x-Axis Data section. From the menu, choose Component 1 (comp1) > Solid Mechanics > Displacement > Displacement field - m > w - Displacement field, Z-component.
6
Locate the y-Axis Data section. In the Expression text field, type Fz1.
7
From the Unit list, choose kN.
8
Click to expand the Legends section. Select the Show legends checkbox.
9
From the Legends list, choose Manual.
10
In the table, enter the following settings:
Legends
Time-domain solution (no pruning)
Hysteresis Loops
1
In the Model Builder window, click Hysteresis Loops.
2
In the Settings window for 1D Plot Group, locate the Legend section.
3
From the Position list, choose Upper left.
4
In the Hysteresis Loops toolbar, click  Plot.
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 > Time Dependent.
4
Click the Add Study button in the window toolbar.
5
In the Home toolbar, click  Add Study to close the Add Study window.
Study 2: With Pruning
1
In the Settings window for Study, type Study 2: With Pruning in the Label text field.
2
Locate the Study Settings section. Clear the Generate default plots checkbox.
Step 1: Time Dependent
1
In the Model Builder window, under Study 2: With Pruning click Step 1: Time Dependent.
2
In the Settings window for Time Dependent, locate the Study Settings section.
3
In the Output times text field, type range(0, 0.01, 3).
4
Locate the Physics and Variables Selection section. Select the Modify model configuration for study step checkbox.
5
In the tree, select Component 1 (comp1) > Solid Mechanics (solid) > Linear Elastic Material 2 > Viscoelasticity (No Pruning).
6
Right-click and choose Disable.
Solution 2 (sol2)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 2 (sol2) node.
3
In the Model Builder window, expand the Study 2: With Pruning > Solver Configurations > Solution 2 (sol2) > Dependent Variables 1 node, then click Auxiliary Pressure (comp1.solid.lemm2.pw).
4
In the Settings window for Field, locate the Scaling section.
5
From the Method list, choose Manual.
6
In the Scale text field, type 1e6.
7
In the Model Builder window, under Study 2: With Pruning > Solver Configurations > Solution 2 (sol2) click Time-Dependent Solver 1.
8
In the Settings window for Time-Dependent Solver, locate the Time Stepping section.
9
Find the Algebraic variable settings subsection. From the Error estimation list, choose Exclude algebraic.
10
In the Model Builder window, right-click Solution 2 (sol2) and choose Run.
Results
Point Graph 2
1
In the Model Builder window, under Results > Hysteresis Loops right-click Point Graph 1 and choose Duplicate.
2
In the Settings window for Point Graph, locate the Data section.
3
From the Dataset list, choose Study 2: With Pruning/Solution 2 (sol2).
4
Locate the Legends section. In the table, enter the following settings:
Legends
Time-domain solution (with pruning)
5
In the Hysteresis Loops toolbar, click  Plot.