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 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.
Results and Discussion
Figure 2 shows the results of the transient computations after two seconds of forced vibrations.
The typical viscoelastic hysteresis loops for a point within one of the mounting elements are shown in Figure 3.
Figure 2: Displacement field.
Figure 3: Displacement vs. applied force.
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.
Import 1 (imp1)
1
In the Home toolbar, click  Import.
2
In the Settings window for Import, locate the Import section.
3
Click Browse.
4
Browse to the model’s Application Libraries folder and double-click the file viscoelastic_damper.mphbin.
5
Click Import.
The imported geometry should look similar to that shown in Figure 1.
Solid Mechanics (solid)
Linear Elastic Material 2
1
In the Model Builder window, under Component 1 (comp1) right-click Solid Mechanics (solid) and choose Material Models>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.
5
Select Domains 2 and 4 only.
Viscoelasticity 1
1
In the Physics toolbar, click  Attributes and choose Viscoelasticity.
Since there are 18 branches in this material model, the data has been collected in a text file which you can load.
2
In the Settings window for Viscoelasticity, locate the Viscoelasticity Model section.
3
Click to select row number 1 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.
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 Add to Component in the window toolbar.
Materials
Steel AISI 4340 (mat1)
Select Domains 1, 3, and 5 only.
Viscoelastic
1
In the Model Builder window, 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 4 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 Home toolbar, click  Add Material to close the Add Material window.
6
Click the Show Material Color and Texture button in the Graphics toolbar.
Definitions
Ramp 1 (rm1)
1
In the Home toolbar, click  Functions and choose Local>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 2e-2.
4
In the Slope text field, type 10.
5
Click to expand the Smoothing section. Select the Size of transition zone at start check box.
6
In the associated text field, type 0.01.
7
Locate the Parameters section. In the Location text field, type 0.02.
8
Select the Cutoff check box.
9
Locate the Smoothing section. Select the Size of transition zone at cutoff check box.
10
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
Select Boundaries 24–27 only.
Prescribed Displacement 1
1
In the Physics toolbar, click  Boundaries and choose Prescribed Displacement.
2
Select Boundaries 40 and 41 only.
3
In the Settings window for Prescribed Displacement, locate the Prescribed Displacement section.
4
Select the Prescribed in x direction check box.
5
Select the Prescribed in y direction check box.
Boundary Load 1
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
Select Boundaries 40 and 41 only.
3
In the Settings window for Boundary Load, locate the Force section.
4
Specify the FA vector as
0
x
0
y
8.5[MPa]*sin(pi/2+2*pi*t*3[Hz])*rm1(t[1/s])
z
Prescribed Displacement 2
1
In the Physics toolbar, click  Boundaries and choose Prescribed Displacement.
2
Select Boundaries 32 and 33 only.
3
In the Settings window for Prescribed Displacement, locate the Prescribed Displacement section.
4
Select the Prescribed in y direction check box.
Boundary Load 2
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
Select Boundaries 32 and 33 only.
3
In the Settings window for Boundary Load, locate the Force section.
4
Specify the FA vector as
0.5[MPa]*sin(2*pi*t*3[Hz])*rm1(t[1/s])
x
0
y
8.5[MPa]*sin(2*pi*t*3[Hz])*rm1(t[1/s])
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
Select Boundaries 32 and 33 only.
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
Mesh the side surfaces of the viscoelastic layers and then sweep the resulting mesh into the layers.
Mapped 1
1
In the Mesh toolbar, click  Boundary and choose Mapped.
2
Select Boundaries 6 and 20 only.
3
In the Settings window for Mapped, click  Build Selected.
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 Domains 2 and 4 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 3.
Swept 1
1
In the Model Builder window, right-click Swept 1 and choose Build Selected.
Mesh the rest of the geometry using a free tetrahedral mesh.
Free Tetrahedral 1
1
In the Mesh toolbar, click  Free Tetrahedral.
2
In the Settings window for Free Tetrahedral, click  Build Selected.
The complete mesh should look similar to that shown in the figure below.
Study 1
Step 1: Time Dependent
1
In the Model Builder window, under Study 1 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(0,0.01,4).
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>Solver Configurations>Solution 1 (sol1)>Dependent Variables 1 node, then click Auxiliary pressure (comp1.solid.pw).
4
In the Settings window for Field, locate the Scaling section.
5
In the Scale text field, type 1e6.
Excluding algebraic error estimates allows the solver to take larger time steps.
6
In the Model Builder window, click Time-Dependent Solver 1.
7
In the Settings window for Time-Dependent Solver, click to expand the Time Stepping section.
8
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.
3D Plot Group 1
In the Home toolbar, click  Add Plot Group and choose 3D Plot Group.
Surface 1
1
Right-click 3D Plot Group 1 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 Expression section. From the Unit list, choose mm.
4
Locate the Coloring and Style section. From the Color table list, choose RainbowLight.
Deformation 1
Right-click Surface 1 and choose Deformation.
Study 1
Step 1: Time Dependent
1
In the Settings window for Time Dependent, click to expand the Results While Solving section.
2
Select the Plot check box.
Solution 1 (sol1)
In the Model Builder window, under Study 1>Solver Configurations right-click Solution 1 (sol1) and choose Compute.
Results
The computed solution should closely resemble that shown in Figure 2.
To plot the displacement vs. 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.
1D Plot Group 2
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, click to expand the Title section.
3
From the Title type list, choose Manual.
4
In the Title text area, type Hysteresis loops .
Point Graph 1
1
Right-click 1D Plot Group 2 and choose Point Graph.
2
Select Point 23 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 x-Axis Data section. From the Unit list, choose mm.
7
Locate the y-Axis Data section. In the Expression text field, type Fz1.
8
From the Unit list, choose kN.
Table Graph 1
1
In the Model Builder window, right-click 1D Plot Group 2 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
Set the Width value to 3.
5
Click to expand the Legends section. Select the Show legends check box.
6
From the Legends list, choose Manual.
7
In the table, enter the following settings:
Legends
Frequency domain solution
1D Plot Group 2
1
In the Model Builder window, click 1D Plot Group 2.
2
In the Settings window for 1D Plot Group, locate the Legend section.
3
From the Position list, choose Upper left.
4
In the 1D Plot Group 2 toolbar, click  Plot.