PDF
Stress Relaxation of a Viscoelastic Tube
Introduction
This example studies the temperature effects on the viscoelastic stress relaxation in a generalized Maxwell material with four branches.
Assume that the viscous part of the deformation is incompressible, so that the volume change is purely elastic. The relaxation shear modulus function is approximated by a Prony series as
(1)
where Gm represents the stiffness of the spring in the mth Maxwell branch, and τm is the relaxation time of the spring-dashpot pair in the same branch.
The instantaneous shear modulus is defined as
The alternative form of Equation 1 is
where the constants μm = Gm/G0 are such that
For many materials the viscoelastic properties have a strong dependence on the temperature. A common assumption is that the material is thermorheologically simple (TRS). In a material of this class, a change in temperature can be directly transformed into a change in the time scale. Thus, the relaxation time for a TRS material is modified to aT(T)τm, where aT(T) is a shift function. One of the most commonly used shift functions is defined by the Williams-Landel-Ferry (WLF) equation:
where a base-10 logarithm is assumed. Usually T0 is the glass transition temperature of the material. Note that aT(T0) = 1. If the temperature drops below T0 − C2, the WLF equation is no longer valid. The constants C1 and C2 are material dependent.
Model Definition
A long thick-walled cylinder has an inner radius of 5 mm and an outer radius of 10 mm. The inner surface is subjected to a prescribed radial displacement of 1 μm. A four-branch generalized Maxwell model represents the viscoelastic material.
In this example, you study the decay of the stresses during a period of two hours under the influence of the temperature field. You model a quarter of the cylinder and use the Solid Mechanics interface in 2D to compute the displacements in the cylinder cross section. The geometry is shown in Figure 1.
Figure 1: Geometry and mesh.
Study the following two cases:
•
Apply a stationary temperature field, causing the problem to lose its axisymmetry.
•
Make the temperature field transient.
Material Parameters
•
Elastic data: The instantaneous shear modulus is G0 = 27.46 GPa, the long-term shear modulus is G = μ0G0, and the bulk modulus K = 39.88 GPa.
•
Viscoelastic data: Four-branch Generalized Maxwell material with the shear modulus per branch defined from Gm = μmG0 where
-
 μ1 = 0.04, τ1 = 30 s
-
 μ2 = 0.08, τ2 = 300 s
-
 μ3 = 0.09, τ3 = 3000 s
-
 μ4 = 0.25, τ4 = 12000 s
•
Thermal properties: A WLF shift function is used with C1 = 17.44 and C2 = 51.6. These values are reasonable approximations for many polymers.
•
The reference temperature is 500 K.
•
Heat transfer properties: ρ = 7850 kg/m3, Cp = 2100 J/(kg·K), k = 6·10−2 W/(m·K).
Constraints
•
The circumferential displacements are constrained on the radial edges.
•
The inner edge of the hole is constrained to a radial displacement of 1 μm.
Heat Transfer Boundary Conditions
•
Stationary analysis: The inner and outer circular edges both have a temperature distribution varying linearly with the y-coordinate from 500 K at the y = 0 symmetry plane to 506 K at the x = 0 symmetry plane.
•
Transient analysis: The temperature distribution obtained from the stationary analysis is used as initial condition, while all edges are insulated.
Results and Discussion
In the first case, the temperature field is stationary and is shown in Figure 2.
Figure 2: Stationary temperature distribution.
The stress relaxation is faster where the temperature is higher. In Figure 3, the plots of radial stresses at radius 7.5 mm display this effect. The solid line is taken at y = 0 (cold) and the dashed line at x = 0 (warm).
Figure 3: Stress relaxation under a stationary temperature distribution.
In the second case, the temperature initially has the same distribution as shown in Figure 2, but it is allowed to settle in time to a final homogeneous value. Again, compare the radial stresses at radius 7.5 mm. The initial behavior is similar to the previous case, but as the difference in material properties decreases, the curves approach each other (Figure 4). The strain rate in the initially warm point decreases, while it increases in the initially colder point.
Figure 4: Stress relaxation under temperature settling conditions.
Notes About the COMSOL Implementation
When you solve a problem where a load is applied instantaneously at the beginning of a transient analysis, you can choose between two approaches to compute the initial stresses: The first option is to apply the load over a short period of time at the beginning of the time-dependent study. An alternative approach is to set the viscoelastic material to use an instantaneous static stiffness, and to add a separate stationary step before the time-dependent step. In the present example, you use the latter method.
The results computed during the stationary step are stored and used as the initial value for the consequent transient analysis. COMSOL Multiphysics handles this automatically if you use a single study with one solver sequence. In this example, however, you study two different relaxation histories with different thermal boundary conditions. In the second case, the thermal boundary conditions differ between the computation of the initial state and the transient analysis. For this reason you use two separate studies for the stationary and the time-dependent studies.
Application Library path: Structural_Mechanics_Module/Material_Models/viscoelastic_tube
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  2D.
2
In the Select Physics tree, select Structural Mechanics > Solid Mechanics (solid).
3
Click Add.
4
In the Select Physics tree, select Heat Transfer > Heat Transfer in Solids (ht).
5
Click Add.
6
Click  Done.
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
G_inst
27.46[GPa]
2.746E10 Pa
Instantaneous shear modulus
Geometry 1
1
In the Model Builder window, under Component 1 (comp1) click Geometry 1.
2
In the Settings window for Geometry, locate the Units section.
3
From the Length unit list, choose mm.
Circle 1 (c1)
1
In the Geometry toolbar, click  Circle.
2
In the Settings window for Circle, locate the Size and Shape section.
3
In the Radius text field, type 10.
4
In the Sector angle text field, type 90.
5
Click to expand the Layers section. In the table, enter the following settings:
Layer name
Thickness (mm)
Layer 1
5
Delete Entities 1 (del1)
1
In the Model Builder window, right-click Geometry 1 and choose Delete Entities.
2
In the Settings window for Delete Entities, locate the Entities or Objects to Delete section.
3
From the Geometric entity level list, choose Domain.
4
On the object c1, select Domain 1 only.
5
Click  Build All Objects.
The equations only need to include first-order time derivatives, since the inertia effects can be neglected for this class of problems.
Solid Mechanics (solid)
1
In the Model Builder window, under Component 1 (comp1) click Solid Mechanics (solid).
2
In the Settings window for Solid Mechanics, locate the Structural Transient Behavior section.
3
From the list, choose Quasistatic.
Linear Elastic Material 1
1
In the Model Builder window, under Component 1 (comp1) > Solid Mechanics (solid) click Linear Elastic Material 1.
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.
Viscoelasticity 1
1
In the Physics toolbar, click  Attributes and choose Viscoelasticity.
2
In the Settings window for Viscoelasticity, locate the Viscoelasticity Model section.
3
In the table, enter the following settings:
Branch
Shear modulus (Pa)
Relaxation time (s)
1
0.04*G_inst
30
4
Click  Add.
5
In the table, enter the following settings:
Branch
Shear modulus (Pa)
Relaxation time (s)
2
0.08*G_inst
300
6
Click  Add.
7
In the table, enter the following settings:
Branch
Shear modulus (Pa)
Relaxation time (s)
3
0.09*G_inst
3000
8
Click  Add.
9
In the table, enter the following settings:
Branch
Shear modulus (Pa)
Relaxation time (s)
4
0.25*G_inst
12000
10
Locate the Thermal Effects section. From the Shift function list, choose Williams–Landel–Ferry.
11
In the Tref text field, type 500[K].
12
Locate the Viscoelasticity Model section. From the Stiffness used in stationary studies list, choose Instantaneous.
Symmetry 1
1
In the Physics toolbar, click  Boundaries and choose Symmetry.
2
Select Boundaries 1 and 2 only.
Prescribed Displacement 1
1
In the Physics toolbar, click  Boundaries and choose Prescribed Displacement.
2
Select Boundary 3 only.
3
In the Settings window for Prescribed Displacement, locate the Coordinate System Selection section.
4
From the Coordinate system list, choose Boundary System 1 (sys1).
5
Locate the Prescribed Displacement section. From the Displacement in n direction list, choose Prescribed.
6
In the u 0 n text field, type -1[um].
Heat Transfer in Solids (ht)
In the Model Builder window, under Component 1 (comp1) click Heat Transfer in Solids (ht).
Temperature 1
1
In the Physics toolbar, click  Boundaries and choose Temperature.
2
Select Boundaries 3 and 4 only.
3
In the Settings window for Temperature, locate the Temperature section.
4
In the T0 text field, type (500+6*y/sqrt(x^2+y^2))[K].
Materials
Material 1 (mat1)
1
In the Model Builder window, under Component 1 (comp1) right-click Materials and choose Blank Material.
2
Select Domain 1 only.
3
In the Settings window for Material, locate the Material Contents section.
4
In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Bulk modulus
K
39.88[GPa]
N/m²
Bulk modulus and shear modulus
Shear modulus
G
0.54*G_inst
N/m²
Bulk modulus and shear modulus
Density
rho
7850[kg/m^3]
kg/m³
Basic
Thermal conductivity
k_iso ; kii = k_iso, kij = 0
0.06[N/(s*K)]
W/(m·K)
Basic
Heat capacity at constant pressure
Cp
2100[J/(kg*K)]
J/(kg·K)
Basic
Mesh 1
Mapped 1
In the Mesh toolbar, click  Mapped.
Distribution 1
1
Right-click Mapped 1 and choose Distribution.
2
Select Boundary 1 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 12.
Distribution 2
1
In the Model Builder window, right-click Mapped 1 and choose Distribution.
2
Select Boundary 3 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 24.
5
Click  Build All.
Root
Next, add a stationary study to model the instantaneous preloading step.
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 > Stationary.
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: Stationary
1
In the Settings window for Study, type Study: Stationary in the Label text field.
2
In the Study toolbar, click  Compute.
Set default units for result presentation.
Results
Preferred Units 1
1
In the Results toolbar, click  Configurations and choose Preferred Units.
2
In the Settings window for Preferred Units, locate the Units section.
3
Click  Add Physical Quantity.
4
In the Physical Quantity dialog, select Solid Mechanics > Stress tensor (N/m^2) in the tree.
5
Click OK.
6
In the Settings window for Preferred Units, locate the Units section.
7
In the table, enter the following settings:
Quantity
Unit
Preferred unit
Stress tensor
N/m^2
MPa
8
Click  Apply.
Visualize the stationary temperature.
Temperature (ht)
1
In the Model Builder window, under Results click Temperature (ht).
2
In the Temperature (ht) toolbar, click  Plot.
Stress (solid), Temperature (ht)
1
In the Model Builder window, under Results, Ctrl-click to select Stress (solid) and Temperature (ht).
2
Right-click and choose Group.
Stationary Results
In the Settings window for Group, type Stationary Results in the Label text field.
Proceed to add a transient study for analyzing the stress relaxation process.
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: Transient (Constant Temperature)
In the Settings window for Study, type Study: Transient (Constant Temperature) in the Label text field.
Step 1: Time Dependent
1
In the Model Builder window, under Study: Transient (Constant Temperature) 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(0,20,200) range(250,50,1000) range(1100,100,2000) range(2200,200,7200).
Solution 2 (sol2)
1
In the Study toolbar, click  Show Default Solver.
Prescribe the solution of the stationary study as the initial step in the transient analysis.
2
In the Model Builder window, expand the Solution 2 (sol2) node, then click Dependent Variables 1.
3
In the Settings window for Dependent Variables, locate the General section.
4
From the Defined by study step list, choose User defined.
5
Locate the Initial Values of Variables Solved For section. From the Method list, choose Solution.
6
From the Solution list, choose Solution 1 (sol1).
7
Locate the Scaling section. From the Method list, choose Initial-value based.
Force the solver to evaluate results in between the specified time steps.
8
In the Model Builder window, under Study: Transient (Constant Temperature) > Solver Configurations > Solution 2 (sol2) click Time-Dependent Solver 1.
9
In the Settings window for Time-Dependent Solver, click to expand the Time Stepping section.
10
From the Steps taken by solver list, choose Intermediate.
11
In the Study toolbar, click  Compute.
Results
Temperature (ht) 1
Display the stress relaxation.
Cut Point 2D 1
1
In the Results toolbar, click  Cut Point 2D.
2
In the Settings window for Cut Point 2D, locate the Point Data section.
3
In the X text field, type 7.5.
4
In the Y text field, type 0.
5
Locate the Data section. From the Dataset list, choose Study: Transient (Constant Temperature)/Solution 2 (sol2).
Cut Point 2D 2
1
In the Results toolbar, click  Cut Point 2D.
2
In the Settings window for Cut Point 2D, locate the Point Data section.
3
In the X text field, type 0.
4
In the Y text field, type 7.5.
5
Locate the Data section. From the Dataset list, choose Study: Transient (Constant Temperature)/Solution 2 (sol2).
Stress Relaxation (Constant Temperature)
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, locate the Data section.
3
From the Dataset list, choose Study: Transient (Constant Temperature)/Solution 2 (sol2).
4
In the Label text field, type Stress Relaxation (Constant Temperature).
5
Click to expand the Title section. From the Title type list, choose Manual.
6
In the Title text area, type Radial Stress Relaxation.
7
Locate the Plot Settings section.
8
Select the y-axis label checkbox. In the associated text field, type Radial stress (MPa).
Point Graph 1
1
Right-click Stress Relaxation (Constant Temperature) and choose Point Graph.
2
In the Settings window for Point Graph, locate the Data section.
3
From the Dataset list, choose Cut Point 2D 1.
4
Click Replace Expression in the upper-right corner of the y-Axis Data section. From the menu, choose Component 1 (comp1) > Solid Mechanics > Stress > Stress tensor (spatial frame) - N/m² > solid.sGpxx - Stress tensor, xx-component.
5
Click to expand the Coloring and Style section. From the Width list, choose 2.
6
Click to expand the Legends section. Select the Show legends checkbox.
7
From the Legends list, choose Manual.
8
In the table, enter the following settings:
Legends
On x-axis
Point Graph 2
1
In the Model Builder window, right-click Stress Relaxation (Constant Temperature) and choose Point Graph.
2
In the Settings window for Point Graph, locate the Data section.
3
From the Dataset list, choose Cut Point 2D 2.
4
Click Replace Expression in the upper-right corner of the y-Axis Data section. From the menu, choose Component 1 (comp1) > Solid Mechanics > Stress > Stress tensor (spatial frame) - N/m² > solid.sGpyy - Stress tensor, yy-component.
5
Locate the Coloring and Style section. From the Width list, choose 2.
6
Find the Line style subsection. From the Line list, choose Dashed.
7
Locate the Legends section. Select the Show legends checkbox.
8
From the Legends list, choose Manual.
9
In the table, enter the following settings:
Legends
On y-axis
Stress Relaxation (Constant Temperature)
1
In the Model Builder window, click Stress Relaxation (Constant Temperature).
2
In the Settings window for 1D Plot Group, locate the Legend section.
3
From the Position list, choose Lower right.
Stress (solid) 1, Stress Relaxation (Constant Temperature), Temperature (ht) 1
1
In the Model Builder window, under Results, Ctrl-click to select Stress (solid) 1, Temperature (ht) 1, and Stress Relaxation (Constant Temperature).
2
Right-click and choose Group.
Transient Results (Constant Temperature)
In the Settings window for Group, type Transient Results (Constant Temperature) in the Label text field.
Now, simulate the stress relaxation at a constant temperature.
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 3
Step 1: Time Dependent
1
In the Settings window for Time Dependent, locate the Study Settings section.
2
In the Output times text field, type range(0,20,200) range(250,50,1000) range(1100,100,2000) range(2200,200,7200).
3
Locate the Physics and Variables Selection section. Select the Modify model configuration for study step checkbox.
4
In the tree, select Component 1 (comp1) > Heat Transfer in Solids (ht) > Temperature 1.
5
Right-click and choose Disable.
6
In the Model Builder window, click Study 3.
7
In the Settings window for Study, type Study: Transient (Variable Temperature) in the Label text field.
Solution 3 (sol3)
1
In the Study toolbar, click  Show Default Solver.
Prescribe the solution of the stationary study as the initial step in the transient analysis.
2
In the Model Builder window, expand the Solution 3 (sol3) node, then click Dependent Variables 1.
3
In the Settings window for Dependent Variables, locate the General section.
4
From the Defined by study step list, choose User defined.
5
Locate the Initial Values of Variables Solved For section. From the Method list, choose Solution.
6
From the Solution list, choose Solution 1 (sol1).
7
Locate the Scaling section. From the Method list, choose Initial-value based.
Force solver to evaluate results in between the specified time steps.
8
In the Model Builder window, under Study: Transient (Variable Temperature) > Solver Configurations > Solution 3 (sol3) click Time-Dependent Solver 1.
9
In the Settings window for Time-Dependent Solver, locate the Time Stepping section.
10
From the Steps taken by solver list, choose Intermediate.
11
In the Study toolbar, click  Compute.
Results
Stress (solid) 2
Plot the results of the stress relaxation.
Cut Point 2D 3
1
In the Model Builder window, under Results > Datasets right-click Cut Point 2D 1 and choose Duplicate.
2
In the Settings window for Cut Point 2D, locate the Data section.
3
From the Dataset list, choose Study: Transient (Variable Temperature)/Solution 3 (sol3).
Cut Point 2D 4
1
In the Model Builder window, under Results > Datasets right-click Cut Point 2D 2 and choose Duplicate.
2
In the Settings window for Cut Point 2D, locate the Data section.
3
From the Dataset list, choose Study: Transient (Variable Temperature)/Solution 3 (sol3).
Stress Relaxation (Variable Temperature)
1
In the Model Builder window, right-click Stress Relaxation (Constant Temperature) and choose Duplicate.
2
Right-click Stress Relaxation (Constant Temperature) 1 and choose Move Out.
3
In the Model Builder window, click Stress Relaxation (Constant Temperature) 1.
4
In the Settings window for 1D Plot Group, type Stress Relaxation (Variable Temperature) in the Label text field.
Point Graph 1
1
In the Model Builder window, expand the Stress Relaxation (Variable Temperature) node, then click Point Graph 1.
2
In the Settings window for Point Graph, locate the Data section.
3
From the Dataset list, choose Cut Point 2D 3.
Point Graph 2
1
In the Model Builder window, click Point Graph 2.
2
In the Settings window for Point Graph, locate the Data section.
3
From the Dataset list, choose Cut Point 2D 4.
4
In the Stress Relaxation (Variable Temperature) toolbar, click  Plot.
Stress (solid) 2, Stress Relaxation (Variable Temperature), Temperature (ht) 2
1
In the Model Builder window, under Results, Ctrl-click to select Stress Relaxation (Variable Temperature), Stress (solid) 2, and Temperature (ht) 2.
2
Right-click and choose Group.
Transient Results (Variable Temperature)
In the Settings window for Group, type Transient Results (Variable Temperature) in the Label text field.