PDF
Mechanical Modeling of Bentonite Clay
Introduction
The Barcelona Basic Model (BBM) is one of the most widely used constitutive models for representing hydromechanical behavior in partially saturated soils. In COMSOL Multiphysics, a modified version of the original model is implemented, the so-called Extended Barcelona Basic Model (BBMx) as described in Ref. 1. By including the suction as a state variable in the constitutive relationship, the BBM and BBMx models can describe partially saturated soils. As opposed to fully saturated soils, partially saturated soils can be loaded either hydraulically or mechanically, or by combination of both mechanisms.
This example validates the BBMx model implemented in COMSOL Multiphysics (Ref. 1) by qualitatively matching the results of mechanical modeling to results of the oedometer, triaxial and suction tests presented in Ref. 2 for bentonite clays. However, the experiments in Ref. 2 are set up to determine suitable material parameters to characterize the BBM model, and while the fundamental principles are the same, there are some differences between the BBM and BBMx models. In addition to the tests described in Ref. 2, an additional test of constrained swelling is carried out to compare the results with analytical formulas.
The Cam-Clay family of soil models, like the BBMx model, do not define any stiffness at zero stress, hence numerical simulations that use these soil models always prescribe an initial mean stress equal to the reference pressure at zero strain.
Model Definition
A cylindrical soil specimen of 3.91 cm in diameter and 8 cm in height is used for all tests. The specimen is represented by a 2D axisymmetric geometry due to the intrinsic symmetry of the problem.
For the oedometer test, initial stresses in the radial, circumferential and axial directions are applied. In the first stage, the bottom and side boundaries are constrained in the normal direction. In the second stage, an axial load is applied on the top boundary.
For the uniaxial swelling test, initial stresses in the radial, circumferential and axial directions are applied together with a constant load on the top boundary. The sample is then subjected to changes in suction.
For the triaxial test (Figure 1), an initial stress is applied to create a state of isotropic compression, the soil sample is then compressed further in the axial direction.
In the constrained swelling test, all boundaries are mechanically constrained, and the sample is then subjected to changes in suction.
Figure 1: Dimensions, boundary conditions, and boundary loads for the triaxial test.
Soil Properties
•
Soil properties from Ref. 2 that are used for the BBMx model are presented in Table 1.
Table 1: Material properties for The soil model.
Property
Variable
Oedometer test
Uniaxial swelling test/constrained swelling test
Triaxial test
Poisson’s ratio
 ν
0.224
0.2
0.3
Density
 ρ
2400 kg/m3
2400 kg/m3
2400 kg/m3
Swelling index
 κ
0.057
0.06
0.1
Swelling index for changes in suction
 κs
0
0.3/0.03
0
Compression index at saturation
 λ
0.101
0.9
0.135
Compression index for changes in suction
 λs
0.01
0.8
0.1
Angle of internal friction
 
25.37°
25.37°
13.34°
Weight parameter
 w
1
0.75
1
Soil stiffness parameter
 m
1 MPa
33.33 MPa
1 MPa
Plastic potential smoothing parameter
 bs
100
100
100
Tension to suction ratio
 ks
0.1
0.1
0.1
Initial yield value for suction
 sy
50 MPa
150 MPa
1 MPa
Initial void ratio
 e0
0.772
0.579
1.212
Initial suction
 s0
28 MPa
101.5 MPa
0 MPa
Reference pressure
 pref
0.1 MPa
0.2 MPa
0.1 MPa
Initial consolidation pressure
 pc0
7.7 MPa
3.5 MPa
1.5 MPa
•
The compression index for changes in current suction, the plastic potential smoothing parameter, and the initial yield value for suction are not specified in Ref. 2.
•
The angle of internal friction is computed from the slope of the critical state line, M, using the formula
•
In COMSOL Multiphysics, either the void ratio at reference pressure together with the saturation eref0, or the initial void ratio e0 are needed as a material property. For this example, an initial void ratio is provided as an input material property.
•
For the oedometer and triaxial tests, the compression index at current suction is independent of the suction, since suction values are held constant in Ref. 2. To achieve this, the weight parameter is set to zero. In COMSOL Multiphysics, the formula for the compression index at current suction is implemented in a different way, therefore, the weight parameter is set to one in order to achieve the same effect as shown in Ref. 2. In these cases the choice of the soil stiffness parameter does not matter.
•
The yield function and the plastic potential used in COMSOL Multiphysics is different than the expressions given in Ref. 2. The nonassociative parameter for the plastic potential is always set to one in COMSOL Multiphysics as compared to Ref. 2.
Constraints and Loads
•
It is sufficient to model the right half of the domain due to axial symmetry.
•
For the oedometer test, an initial stress of −2.97 MPa is applied in the radial and circumferential directions, while −0.18 MPa is applied in the axial direction.
•
Note that the reference pressure pref acts as an initial stress, therefore the values of the diagonal components of the in situ stress tensor defined in the External Stress node are −2.87 MPa, −2.87 MPa, and −0.08 MPa.
•
During the loading stage of the oedometer test, the axial compressive stress is increased from 0.18 MPa to 19.77 MPa, and then decreased from 19.77 MPa to 1.00 MPa. Roller boundary conditions are applied on the bottom and side boundaries. The suction value is kept constant throughout the analysis.
•
For the uniaxial swelling test, an initial stress of −2.54 MPa is applied in the radial and circumferential directions, while −8.90 MPa is applied in the axial direction. The reference pressure pref acts as an initial stress, so the values of the diagonal components of the in situ stress tensor in the External Stress node are -2.34 MPa, −2.34 MPa, and −8.70 MPa.
•
In the loading step of the uniaxial swelling test, the axial compressive stress is maintained constant at −8.90 MPa, while the suction is reduced from 101.5 MPa to 12.6 MPa. Roller boundary conditions are applied on the bottom and side boundaries.
•
For the triaxial test in isotropic compression, an initial hydrostatic stress of 1.1 MPa is applied. As the reference pressure pref acts as an initial stress, the values of the diagonal components of the in situ stress tensor defined in the External Stress node are −1 MPa.
•
During the axial compression stage of the triaxial test, the soil sample is compressed by a prescribed displacement on the top boundary. The top-right corner is allowed to expand freely in the radial direction, and a roller boundary condition is applied at the bottom boundary.
•
For the constrained swelling test, all boundaries are constrained in the normal direction and the suction is reduced from 101.5 MPa to 12.6 MPa.
Results and Discussion
Note that for consistency with the geomechanics sign convention, compressive stress and strain is plotted along the positive axis in all figures, while tensile stress and strain is plotted along the negative axis.
The evolution of both the void ratio and the radial stress versus axial stress during the loading and unloading phases in the oedometer test are shown in Figure 2, and the evolution of both the deviatoric stress and the mean stress in Figure 3. The results of both phases of the test resembles the results shown in Ref. 2, but there are some differences mainly in the unloading phase. These differences may be attributed to the implementation of different yield functions and plastic potentials.
Figure 2: Evolution of void ratio and radial stress versus axial stress for the oedometer test.
Figure 3: Stress path in the p-q plane for the oedometer test.
The evolution of both the void ratio and the radial stress versus suction in the uniaxial swelling test are shown in Figure 4. Both curves match the numerical results given in Ref. 2. The evolution of the mean stress is shown in Figure 5. The void ratio, the radial stress, and the mean stress all level out at a suction around 80 MPa, which is also reported in Ref. 2. This behavior is due to the accumulation of plastic strains. Moreover, at the end of the suction cycle, the void ratio shows an increasing trend, and this behavior is also reported in Ref. 2.
The evolution of the volumetric strain and the deviatoric stress versus axial strain are shown in Figure 6 and Figure 7, respectively. These results show good qualitative agreement with the results presented in Ref. 2. The slight mismatch is anticipated due to the different implementation of the material models, given by the different definitions for the yield function and the plastic potential.
The stress path in the p-q plane for the triaxial test is shown in Figure 8. The deviatoric stress equals 0.3 MPa when the mean stress is 1.2 MPa. this stress state coincides with the initial yield surface. These are the same value as reported in Ref. 2.
For the constrained swelling stress, evolution of the mean stress versus suction is shown in Figure 9. This result matches exactly the analytical expression given by Equation 1 in the pure elastic range.
For the BBMx model, the evolution of the volumetric strain is given by
 with and
For constrained swelling there is no change in volumetric strain, hence
Integrating this equation, and finding the integration constant based on the initial values, gives
(1) with
For the constrained swelling test, both the volumetric strain and the void ratio remain constant as suction changes; this is portrayed in Figure 10.
Figure 4: Evolution of void ratio and radial stress versus suction in the uniaxial swelling test.
Figure 5: Evolution of mean stress versus suction in the uniaxial swelling test.
Figure 6: Evolution of volumetric strain versus axial strain in the triaxial test.
Figure 7: Evolution of deviatoric stress versus axial strain in the triaxial test.
Figure 8: Stress path in the p-q plane for the triaxial test.
Figure 9: Evolution of mean stress versus suction in the constrained swelling test.
Figure 10: Evolution of void ratio and volumetric strain versus suction in the constrained swelling test.
Notes About the COMSOL Implementation
The in situ stresses are the stresses in the soil sample in a strain-free configuration. There are two methods to account for in situ stresses in COMSOL Multiphysics. One way is to create two stationary study steps or studies, with a combination of the Initial Stress and Strain and External Stress nodes. The second method is to use the In situ stress option in the External Stress node with single study. This option gives initial stresses in the soil sample without imposing any strains. In this example, the second method is used to model the in situ stresses in the soil sample.
References
1. D. Pedroso and M. Farias, “Extended Barcelona Basic Model for unsaturated soil under cyclic loadings,” Computers and Geotechnics, vol. 38, no. 5, pp. 731–740, 2011.
2. O. Kristensson and M. Åkesson, “Mechanical modeling of MX-80 - Quick tools for BBM parameter analysis,” Physics and Chemistry of the Earth, vol. 33, pp. 5508–5515, 2008.
Application Library path: Geomechanics_Module/Verification_Examples/mechanical_modeling_of_bentonite_clay
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 Axisymmetric.
2
In the Select Physics tree, select Structural Mechanics > Solid Mechanics (solid).
3
Right-click and choose Add Physics.
4
Repeat the two previous instructions three times to add four Solid Mechanics interfaces in total.
5
Click  Study.
6
In the Select Study tree, select General Studies > Stationary.
7
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
para
0
0
Parameter
disp3
0[cm]
0 m
Axial displacement
BBMx Material Parameters
1
In the Home toolbar, click  Parameters and choose Add > Parameters.
First set up a physics interface for each soil test.
2
In the Settings window for Parameters, type BBMx Material Parameters in the Label text field.
3
Locate the Parameters section. Click  Load from File.
4
Browse to the model’s Application Libraries folder and double-click the file mechanical_modeling_of_bentonite_clay_oedometer_parameters.txt.
5
In the Home toolbar, click  Parameter Case.
6
In the Settings window for Case, type Oedometer Test Parameters in the Label text field.
7
In the Home toolbar, click  Parameter Case.
8
In the Settings window for Case, type Uniaxial Swelling Test Parameters in the Label text field.
9
Locate the Parameters section. Click  Load from File.
10
Browse to the model’s Application Libraries folder and double-click the file mechanical_modeling_of_bentonite_clay_uniaxial_swelling_parameters.txt.
11
In the Home toolbar, click  Parameter Case.
12
In the Settings window for Case, type Triaxial Test Parameters in the Label text field.
13
Locate the Parameters section. Click  Load from File.
14
Browse to the model’s Application Libraries folder and double-click the file mechanical_modeling_of_bentonite_clay_triaxial_parameters.txt.
15
In the Home toolbar, click  Parameter Case.
16
In the Settings window for Case, type Constrained Swelling Test Parameters in the Label text field.
17
Locate the Parameters section. Click  Load from File.
18
Browse to the model’s Application Libraries folder and double-click the file mechanical_modeling_of_bentonite_clay_constrained_swelling_parameters.txt.
Geometry 1
Rectangle 1 (r1)
1
In the Geometry toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type 1.955[cm].
4
In the Height text field, type 8[cm].
5
Click  Build Selected.
Solid Mechanics [Oedometer Test]
1
In the Model Builder window, under Component 1 (comp1) click Solid Mechanics (solid).
2
In the Settings window for Solid Mechanics, type Solid Mechanics [Oedometer Test] in the Label text field.
Elastoplastic Soil Material 1
1
In the Physics toolbar, click  Domains and choose Elastoplastic Soil Material.
The provided material data does not include the void ratio at reference pressure and saturation but instead gives the initial void ratio. Hence, change the default option of the initial void ratio property to From material instead of deriving it from void ratio at reference pressure and saturation.
2
Select Domain 1 only.
3
In the Settings window for Elastoplastic Soil Material, locate the Elastoplastic Soil Material section.
4
From the Material model list, choose Extended Barcelona basic.
5
From the Γ(θ) list, choose Matsuoka–Nakai.
6
Find the Parameters subsection. In the s0 text field, type s0.
7
In the s text field, type s0.
8
In the pref text field, type pref.
9
In the pc0 text field, type pc0.
External Stress 1
1
In the Physics toolbar, click  Attributes and choose External Stress.
The oedometer test is carried out in two steps. The first step is needed to get the initial stress state of the sample, and the second step is a compressive loading. The initial stress state can be modeled using the In situ stress option of the External Stress node.
2
In the Settings window for External Stress, locate the External Stress section.
3
From the Stress input list, choose In situ stress.
4
From the list, choose Symmetric.
5
Specify the σins matrix as
-2.87[MPa]
0
0
0
-2.87[MPa]
0
0
0
-0.08[MPa]
Roller 1
1
In the Physics toolbar, click  Boundaries and choose Roller.
2
Select Boundaries 2 and 4 only.
Instead of adding a boundary load on the top boundary, prescribe the displacement as a function of the axial stress.
Elastoplastic Soil Material 1
In the Model Builder window, collapse the Component 1 (comp1) > Solid Mechanics [Oedometer Test] (solid) > Elastoplastic Soil Material 1 node.
Definitions
Interpolation 1 (int1)
1
In the Definitions toolbar, click  Interpolation.
2
In the Settings window for Interpolation, locate the Definition section.
3
In the Function name text field, type sigmaZ.
4
In the table, enter the following settings:
t
f(t)
0
-0.18
1
-19.77
2
-1
5
Locate the Units section. In the Argument table, enter the following settings:
Argument
Unit
t
1
6
In the Function table, enter the following settings:
Function
Unit
sigmaZ
MPa
Average 1 (aveop1)
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Average.
2
Select Domain 1 only.
3
In the Settings window for Average, locate the Advanced section.
4
From the Frame list, choose Material  (R, PHI, Z).
5
Clear the Compute integral in revolved geometry checkbox.
Solid Mechanics [Oedometer Test] (solid)
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 Prescribed Displacement section.
4
From the Displacement in z direction list, choose Prescribed.
5
In the u 0 z text field, type disp1.
Add a global equation to compute the axial displacement, so that the axial stress equals the reaction force for such a prescribed displacement. Show the equation-based contributions to add a global equation.
6
Click the  Show More Options button in the Model Builder toolbar.
7
In the Show More Options dialog, in the tree, select the checkbox for the node Physics > Equation Contributions.
8
Click OK.
Global Equations 1 (ODE1)
1
In the Physics toolbar, click  Global and choose Global Equations.
Multiply the global equation by a suitable penalty factor in order to strictly satisfy this equation. For the current model, 1e5 is an appropriate penalty factor.
2
In the Settings window for Global Equations, locate the Global Equations section.
3
In the table, enter the following settings:
Name
f(u,ut,utt,t) (1)
Initial value (u_0) (1)
Initial value (ut_0) (1/s)
Description
disp1
(aveop1(solid.SZZ)-sigmaZ(para))*1e5
0
0
 
4
Locate the Units section. Click  Select Dependent Variable Quantity.
5
In the Physical Quantity dialog, type disp in the text field.
6
In the tree, select General > Displacement (m).
7
Click OK.
8
In the Settings window for Global Equations, locate the Units section.
9
Click  Select Source Term Quantity.
10
In the Physical Quantity dialog, type pressure in the text field.
11
In the tree, select General > Pressure (Pa).
12
Click OK.
Definitions
Interpolation 2 (int2)
1
In the Definitions toolbar, click  Interpolation.
2
In the Settings window for Interpolation, locate the Definition section.
3
In the Function name text field, type suction.
4
In the table, enter the following settings:
t
f(t)
0
101.5
1
12.6
5
Locate the Units section. In the Argument table, enter the following settings:
Argument
Unit
t
1
6
In the Function table, enter the following settings:
Function
Unit
suction
MPa
Solid Mechanics [Uniaxial Swelling Test]
1
In the Model Builder window, under Component 1 (comp1) click Solid Mechanics 2 (solid2).
2
In the Settings window for Solid Mechanics, type Solid Mechanics [Uniaxial Swelling Test] in the Label text field.
Elastoplastic Soil Material 1
1
In the Physics toolbar, click  Domains and choose Elastoplastic Soil Material.
2
Select Domain 1 only.
3
In the Settings window for Elastoplastic Soil Material, locate the Elastoplastic Soil Material section.
4
From the Material model list, choose Extended Barcelona basic.
5
From the Γ(θ) list, choose Matsuoka–Nakai.
6
Find the Parameters subsection. In the s0 text field, type s0.
7
In the s text field, type suction(para).
8
In the pref text field, type pref.
9
In the pc0 text field, type pc0.
External Stress 1
1
In the Physics toolbar, click  Attributes and choose External Stress.
The uniaxial swelling test is carried out in two steps. The first step is needed to get the initial stress state of the sample, and the second step is a reduction in the suction while keeping a constant axial stress. The initial stress state can be modeled using the In situ stress option of the External Stress node.
2
In the Settings window for External Stress, locate the External Stress section.
3
From the Stress input list, choose In situ stress.
4
From the list, choose Symmetric.
5
Specify the σins matrix as
-2.34[MPa]
0
0
0
-2.34[MPa]
0
0
0
-8.70[MPa]
Roller 1
1
In the Physics toolbar, click  Boundaries and choose Roller.
2
Select Boundaries 2 and 4 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 Prescribed Displacement section.
4
From the Displacement in z direction list, choose Prescribed.
5
In the u 0 z text field, type disp2.
Global Equations 1 (ODE2)
1
In the Physics toolbar, click  Global and choose Global Equations.
2
In the Settings window for Global Equations, locate the Global Equations section.
3
In the table, enter the following settings:
Name
f(u,ut,utt,t) (1)
Initial value (u_0) (1)
Initial value (ut_0) (1/s)
Description
disp2
(aveop1(solid2.SZZ)+8.90[MPa])
0
0
 
4
Locate the Units section. Click  Select Dependent Variable Quantity.
5
In the Physical Quantity dialog, type disp in the text field.
6
In the tree, select General > Displacement (m).
7
Click OK.
8
In the Settings window for Global Equations, locate the Units section.
9
Click  Select Source Term Quantity.
10
In the Physical Quantity dialog, type pressure in the text field.
11
In the tree, select General > Pressure (Pa).
12
Click OK.
Solid Mechanics [Triaxial Test]
1
In the Model Builder window, under Component 1 (comp1) click Solid Mechanics 3 (solid3).
2
In the Settings window for Solid Mechanics, type Solid Mechanics [Triaxial Test] in the Label text field.
Elastoplastic Soil Material 1
1
In the Physics toolbar, click  Domains and choose Elastoplastic Soil Material.
2
Select Domain 1 only.
3
In the Settings window for Elastoplastic Soil Material, locate the Elastoplastic Soil Material section.
4
From the Material model list, choose Extended Barcelona basic.
5
From the Γ(θ) list, choose Matsuoka–Nakai.
6
Find the Parameters subsection. In the s0 text field, type s0.
7
In the s text field, type s0.
8
In the pref text field, type pref.
9
In the pc0 text field, type pc0.
Decrease the relative tolerance in the feature’s Advanced section. To see this section, activate advanced physics settings as follows.
10
Click the  Show More Options button in the Model Builder toolbar.
11
In the Show More Options dialog, in the tree, select the checkbox for the node Physics > Advanced Physics Options.
12
Click OK.
13
In the Settings window for Elastoplastic Soil Material, click to expand the Advanced section.
14
From the Local method list, choose Backward Euler.
15
In the Relative tolerance text field, type 1e-8.
External Stress 1
1
In the Physics toolbar, click  Attributes and choose External Stress.
The triaxial test is carried out in two steps. The first step is needed to get the initial stress state of the sample, and the second step is an axial compressive loading. The initial stress state can be modeled using the In situ stress option of the External Stress node.
2
In the Settings window for External Stress, locate the External Stress section.
3
From the Stress input list, choose In situ stress.
4
In the σins text field, type -1[MPa].
Roller 1
1
In the Physics toolbar, click  Boundaries and choose Roller.
2
Select Boundary 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 Prescribed Displacement section.
4
From the Displacement in z direction list, choose Prescribed.
5
In the u 0 z text field, type -disp3.
Solid Mechanics [Constrained Swelling Test]
1
In the Model Builder window, under Component 1 (comp1) click Solid Mechanics 4 (solid4).
2
In the Settings window for Solid Mechanics, type Solid Mechanics [Constrained Swelling Test] in the Label text field.
Elastoplastic Soil Material 1
1
In the Physics toolbar, click  Domains and choose Elastoplastic Soil Material.
2
Select Domain 1 only.
3
In the Settings window for Elastoplastic Soil Material, locate the Elastoplastic Soil Material section.
4
From the Material model list, choose Extended Barcelona basic.
5
From the Γ(θ) list, choose Matsuoka–Nakai.
6
Find the Parameters subsection. In the s0 text field, type s0.
7
In the s text field, type suction(para).
8
In the pref text field, type pref.
9
In the pc0 text field, type pc0.
Roller 1
1
In the Physics toolbar, click  Boundaries and choose Roller.
2
Select Boundaries 2–4 only.
Definitions
Variables 1
1
In the Model Builder window, under Component 1 (comp1) right-click Definitions and choose Variables.
2
In the Settings window for Variables, locate the Variables section.
3
In the table, enter the following settings:
Name
Expression
Unit
Description
P_analytical
solid4.epm1.pref*exp(-solid4.epm1.kappaSwellings/solid4.epm1.kappaSwelling0*log((solid4.epm1.ss+solid4.epm1.patm)/(solid4.epm1.ss0+solid4.epm1.patm)))
N/m²
Analytical formula for pressure
Materials
MX-80 Bentonite Clay
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 MX-80 Bentonite Clay in the Label text field.
3
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Poisson’s ratio
nu
Nu
1
Critical state model
Friction angle
internalphi
Phi
rad
Critical state model
Density
rho
Rho
kg/m³
Basic
Swelling index at saturation
kappaSwelling0
kappa
1
Barcelona Basic
Swelling index for changes in suction
kappaSwellingsu
kappa_s
1
Barcelona Basic
Compression index at saturation
lambdaComp0
lambda
1
Barcelona Basic
Compression index for changes in suction
lambdaCompssu
lambda_s
1
Barcelona Basic
Weight parameter
wb
ws
1
Barcelona Basic
Soil stiffness parameter
mb
m
Pa
Barcelona Basic
Plastic potential smoothing parameter
bb
bs
1
Barcelona Basic
Tension to suction ratio
kb
ks
1
Barcelona Basic
Initial yield value for suction
sy0
sy
Pa
Barcelona Basic
Initial void ratio
evoid0b
e0
1
Barcelona Basic
Mesh 1
Mapped 1
In the Mesh toolbar, click  Mapped.
Only using a few mesh elements is sufficient for this analysis.
Distribution 1
1
Right-click Mapped 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Boundary Selection section.
3
From the Selection list, choose All boundaries.
4
Locate the Distribution section. In the Number of elements text field, type 1.
5
Click  Build Selected.
Set up the studies for all tests.
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
Right-click and choose Add Study.
5
In the Select Study tree, select General Studies > Stationary.
6
Right-click and choose Add Study.
7
In the Select Study tree, select General Studies > Stationary.
8
Right-click and choose Add Study.
9
In the Home toolbar, click  Add Study to close the Add Study window.
Study [Oedometer Test]
1
In the Settings window for Study, type Study [Oedometer Test] in the Label text field.
2
Locate the Study Settings section. Clear the Generate default plots checkbox.
Parametric Sweep
1
In the Study toolbar, click  Parametric Sweep.
2
In the Settings window for Parametric Sweep, locate the Study Settings section.
3
Click  Add.
4
From the Sweep type list, choose Parameter switch.
5
Click  Add.
6
In the table, enter the following settings:
Switch
Cases
Case numbers
BBMx Material Parameters
User defined
1
Step 1: Stationary
1
In the Model Builder window, click Step 1: Stationary.
2
In the Settings window for Stationary, locate the Physics and Variables Selection section.
3
In the Solve for column of the table, under Component 1 (comp1), clear the checkboxes for Solid Mechanics [Uniaxial Swelling Test] (solid2), Solid Mechanics [Triaxial Test] (solid3), and Solid Mechanics [Constrained Swelling Test] (solid4).
4
Click to expand the Study Extensions section. Select the Auxiliary sweep checkbox.
5
Click  Add.
6
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
para (Parameter)
range(0,0.005,2)
 
Use appropriate scaling and the Constant (Newton) nonlinear method to improve convergence.
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 [Oedometer Test] > Solver Configurations > Solution 1 (sol1) > Dependent Variables 1 node, then click Global Equations 1 (comp1.ODE1).
4
In the Settings window for State, locate the Scaling section.
5
From the Method list, choose Manual.
6
In the Scale text field, type 1e-3.
7
In the Model Builder window, expand the Study [Oedometer Test] > Solver Configurations > Solution 1 (sol1) > Stationary Solver 1 node, then click Fully Coupled 1.
8
In the Settings window for Fully Coupled, click to expand the Method and Termination section.
9
From the Nonlinear method list, choose Constant (Newton).
10
From the Stabilization and acceleration list, choose Anderson acceleration.
11
In the Study toolbar, click  Compute.
Study [Uniaxial Swelling Test]
1
In the Model Builder window, click Study 2.
2
In the Settings window for Study, type Study [Uniaxial Swelling Test] in the Label text field.
3
Locate the Study Settings section. Clear the Generate default plots checkbox.
Parametric Sweep
1
In the Study toolbar, click  Parametric Sweep.
2
In the Settings window for Parametric Sweep, locate the Study Settings section.
3
From the Sweep type list, choose Parameter switch.
4
Click  Add.
5
In the table, enter the following settings:
Switch
Cases
Case numbers
BBMx Material Parameters
User defined
2
Step 1: Stationary
1
In the Model Builder window, click Step 1: Stationary.
2
In the Settings window for Stationary, locate the Physics and Variables Selection section.
3
In the Solve for column of the table, under Component 1 (comp1), clear the checkboxes for Solid Mechanics [Oedometer Test] (solid), Solid Mechanics [Triaxial Test] (solid3), and Solid Mechanics [Constrained Swelling Test] (solid4).
4
Locate the Study Extensions section. Select the Auxiliary sweep checkbox.
5
Click  Add.
6
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
para (Parameter)
range(0,0.005,1)
 
Use appropriate scaling and the Constant (Newton) nonlinear method to improve convergence.
Solution 4 (sol4)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 4 (sol4) node.
3
In the Model Builder window, expand the Study [Uniaxial Swelling Test] > Solver Configurations > Solution 4 (sol4) > Dependent Variables 1 node, then click Global Equations 1 (comp1.ODE2).
4
In the Settings window for State, locate the Scaling section.
5
From the Method list, choose Manual.
6
In the Scale text field, type 1e-3.
7
In the Model Builder window, expand the Study [Uniaxial Swelling Test] > Solver Configurations > Solution 4 (sol4) > Stationary Solver 1 node, then click Fully Coupled 1.
8
In the Settings window for Fully Coupled, locate the Method and Termination section.
9
From the Nonlinear method list, choose Constant (Newton).
10
From the Stabilization and acceleration list, choose Anderson acceleration.
11
In the Study toolbar, click  Compute.
Study [Triaxial Test]
1
In the Model Builder window, click Study 3.
2
In the Settings window for Study, type Study [Triaxial Test] in the Label text field.
3
Locate the Study Settings section. Clear the Generate default plots checkbox.
Parametric Sweep
1
In the Study toolbar, click  Parametric Sweep.
2
In the Settings window for Parametric Sweep, locate the Study Settings section.
3
From the Sweep type list, choose Parameter switch.
4
Click  Add.
5
In the table, enter the following settings:
Switch
Cases
Case numbers
BBMx Material Parameters
User defined
3
Step 1: Stationary
1
In the Model Builder window, click Step 1: Stationary.
2
In the Settings window for Stationary, locate the Physics and Variables Selection section.
3
In the Solve for column of the table, under Component 1 (comp1), clear the checkboxes for Solid Mechanics [Oedometer Test] (solid), Solid Mechanics [Uniaxial Swelling Test] (solid2), and Solid Mechanics [Constrained Swelling Test] (solid4).
4
Locate the Study Extensions section. Select the Auxiliary sweep checkbox.
5
Click  Add.
6
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
disp3 (Axial displacement)
range(0,0.001,0.8)
cm
Use the Constant (Newton) nonlinear method to improve convergence.
Solution 7 (sol7)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 7 (sol7) node.
3
In the Model Builder window, expand the Study [Triaxial Test] > Solver Configurations > Solution 7 (sol7) > Stationary Solver 1 node, then click Fully Coupled 1.
4
In the Settings window for Fully Coupled, locate the Method and Termination section.
5
From the Nonlinear method list, choose Constant (Newton).
6
From the Stabilization and acceleration list, choose Anderson acceleration.
7
In the Study toolbar, click  Compute.
Study [Constrained Swelling Test]
1
In the Model Builder window, click Study 4.
2
In the Settings window for Study, type Study [Constrained Swelling Test] in the Label text field.
3
Locate the Study Settings section. Clear the Generate default plots checkbox.
Parametric Sweep
1
In the Study toolbar, click  Parametric Sweep.
2
In the Settings window for Parametric Sweep, locate the Study Settings section.
3
From the Sweep type list, choose Parameter switch.
4
Click  Add.
5
In the table, enter the following settings:
Switch
Cases
Case numbers
BBMx Material Parameters
User defined
4
Step 1: Stationary
1
In the Model Builder window, click Step 1: Stationary.
2
In the Settings window for Stationary, locate the Physics and Variables Selection section.
3
In the Solve for column of the table, under Component 1 (comp1), clear the checkboxes for Solid Mechanics [Oedometer Test] (solid), Solid Mechanics [Uniaxial Swelling Test] (solid2), and Solid Mechanics [Triaxial Test] (solid3).
4
Locate the Study Extensions section. Select the Auxiliary sweep checkbox.
5
Click  Add.
6
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
para (Parameter)
range(0,0.001,1)
 
Use the Constant (Newton) nonlinear method to improve convergence.
Solution 10 (sol10)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 10 (sol10) node.
3
In the Model Builder window, expand the Study [Constrained Swelling Test] > Solver Configurations > Solution 10 (sol10) > Stationary Solver 1 node, then click Fully Coupled 1.
4
In the Settings window for Fully Coupled, locate the Method and Termination section.
5
From the Nonlinear method list, choose Constant (Newton).
6
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
Select the Apply conversions to expressions with the same dimensions checkbox.
9
Click  Apply.
Void Ratio and Radial Stress
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Void Ratio and Radial Stress 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. Select the Two y-axes checkbox.
5
Select the x-axis label checkbox. In the associated text field, type Axial stress (MPa).
6
Select the Secondary y-axis label checkbox. In the associated text field, type Radial stress (MPa).
7
Locate the Axis section. Select the Manual axis limits checkbox.
8
In the x minimum text field, type 0.1.
9
In the x maximum text field, type 100.
10
In the y minimum text field, type 0.3.
11
In the y maximum text field, type 0.8.
12
In the Secondary y minimum text field, type 0.
13
In the Secondary y maximum text field, type 25.
14
Select the x-axis log scale checkbox.
Point Graph 1
1
Right-click Void Ratio and Radial Stress and choose Point Graph.
2
Select Point 4 only.
3
In the Settings window for Point Graph, locate the y-Axis Data section.
4
In the Expression text field, type solid.evoid.
5
Locate the x-Axis Data section. From the Parameter list, choose Expression.
6
In the Expression text field, type -solid.SZZ.
7
Click to expand the Legends section. Select the Show legends checkbox.
8
From the Legends list, choose Manual.
9
In the table, enter the following settings:
Legends
Void ratio
Point Graph 2
1
Right-click Point Graph 1 and choose Duplicate.
2
In the Settings window for Point Graph, locate the y-Axis Data section.
3
In the Expression text field, type -solid.SRR.
4
Locate the y-Axis section. Select the Plot on secondary y-axis checkbox.
5
Locate the Legends section. In the table, enter the following settings:
Legends
Radial stress
6
In the Void Ratio and Radial Stress toolbar, click  Plot.
Stress Path
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Stress Path in the Label text field.
3
Locate 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 Mean stress (MPa).
6
Select the y-axis label checkbox. In the associated text field, type Deviatoric stress (MPa).
7
Locate the Axis section. Select the Manual axis limits checkbox.
8
In the x minimum text field, type 0.
9
In the x maximum text field, type 15.
10
In the y minimum text field, type 0.
11
In the y maximum text field, type 10.
Point Graph 1
1
Right-click Stress Path and choose Point Graph.
2
Select Point 4 only.
3
In the Settings window for Point Graph, locate the y-Axis Data section.
4
In the Expression text field, type solid.mises.
5
Locate the x-Axis Data section. From the Parameter list, choose Expression.
6
In the Expression text field, type solid.pm.
7
In the Stress Path toolbar, click  Plot.
Stress Path, Void Ratio and Radial Stress
1
In the Model Builder window, under Results, Ctrl-click to select Void Ratio and Radial Stress and Stress Path.
2
Right-click and choose Group.
Oedometer Test
In the Settings window for Group, type Oedometer Test in the Label text field.
Void Ratio and Radial Stress 1
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Void Ratio and Radial Stress 1 in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study [Uniaxial Swelling Test]/Solution 4 (sol4).
4
Locate the Title section. From the Title type list, choose None.
5
Locate the Plot Settings section. Select the Two y-axes checkbox.
6
Select the x-axis label checkbox. In the associated text field, type Suction (MPa).
7
Select the Secondary y-axis label checkbox. In the associated text field, type Radial stress (MPa).
8
Locate the Axis section. Select the Manual axis limits checkbox.
9
In the x minimum text field, type 0.
10
In the x maximum text field, type 120.
11
In the y minimum text field, type 0.5.
12
In the y maximum text field, type 0.7.
13
In the Secondary y minimum text field, type 0.
14
In the Secondary y maximum text field, type 20.
Point Graph 1
1
Right-click Void Ratio and Radial Stress 1 and choose Point Graph.
2
Select Point 4 only.
3
In the Settings window for Point Graph, locate the y-Axis Data section.
4
In the Expression text field, type solid2.evoid.
5
Locate the x-Axis Data section. From the Parameter list, choose Expression.
6
In the Expression text field, type solid2.epm1.ss.
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
Void ratio
Point Graph 2
1
Right-click Point Graph 1 and choose Duplicate.
2
In the Settings window for Point Graph, locate the y-Axis Data section.
3
In the Expression text field, type -solid2.SRR.
4
Locate the y-Axis section. Select the Plot on secondary y-axis checkbox.
5
Locate the Legends section. In the table, enter the following settings:
Legends
Radial stress
6
In the Void Ratio and Radial Stress 1 toolbar, click  Plot.
Mean Stress
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Mean Stress in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study [Uniaxial Swelling Test]/Solution 4 (sol4).
4
Locate the Title section. From the Title type list, choose None.
5
Locate the Plot Settings section.
6
Select the x-axis label checkbox. In the associated text field, type Suction (MPa).
7
Select the y-axis label checkbox. In the associated text field, type Mean stress (MPa).
8
Locate the Axis section. Select the Manual axis limits checkbox.
9
In the x minimum text field, type 0.
10
In the x maximum text field, type 120.
11
In the y minimum text field, type 0.
12
In the y maximum text field, type 20.
Point Graph 1
1
Right-click Mean Stress and choose Point Graph.
2
Select Point 4 only.
3
In the Settings window for Point Graph, locate the y-Axis Data section.
4
In the Expression text field, type solid2.pm.
5
Locate the x-Axis Data section. From the Parameter list, choose Expression.
6
In the Expression text field, type solid2.epm1.ss.
7
In the Mean Stress toolbar, click  Plot.
Stress Path 1
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Stress Path 1 in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study [Uniaxial Swelling Test]/Solution 4 (sol4).
4
Locate the Title section. From the Title type list, choose None.
5
Locate the Plot Settings section.
6
Select the x-axis label checkbox. In the associated text field, type Mean stress (MPa).
7
Select the y-axis label checkbox. In the associated text field, type Deviatoric stress (MPa).
8
Locate the Axis section. Select the Manual axis limits checkbox.
9
In the x minimum text field, type 0.
10
In the x maximum text field, type 10.
11
In the y minimum text field, type 0.
12
In the y maximum text field, type 8.
Point Graph 1
1
Right-click Stress Path 1 and choose Point Graph.
2
Select Point 4 only.
3
In the Settings window for Point Graph, locate the y-Axis Data section.
4
In the Expression text field, type solid2.mises.
5
Locate the x-Axis Data section. From the Parameter list, choose Expression.
6
In the Expression text field, type solid2.pm.
7
In the Stress Path 1 toolbar, click  Plot.
Mean Stress, Stress Path 1, Void Ratio and Radial Stress 1
1
In the Model Builder window, under Results, Ctrl-click to select Void Ratio and Radial Stress 1, Mean Stress, and Stress Path 1.
2
Right-click and choose Group.
Uniaxial Swelling Test
In the Settings window for Group, type Uniaxial Swelling Test in the Label text field.
Volumetric Strain
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Volumetric Strain in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study [Triaxial Test]/Solution 7 (sol7).
4
Locate the Title section. From the Title type list, choose None.
5
Locate the Plot Settings section.
6
Select the x-axis label checkbox. In the associated text field, type Axial strain (%).
7
Select the y-axis label checkbox. In the associated text field, type Volumetric strain (%).
8
Locate the Axis section. Select the Manual axis limits checkbox.
9
In the x minimum text field, type 0.
10
In the x maximum text field, type 12.
11
In the y minimum text field, type 0.
12
In the y maximum text field, type 2.
Point Graph 1
1
Right-click Volumetric Strain and choose Point Graph.
2
Select Point 4 only.
3
In the Settings window for Point Graph, locate the y-Axis Data section.
4
In the Expression text field, type -solid3.evol.
5
From the Unit list, choose %.
6
Locate the x-Axis Data section. From the Parameter list, choose Expression.
7
In the Expression text field, type -solid3.eZZ.
8
From the Unit list, choose %.
9
In the Volumetric Strain toolbar, click  Plot.
Deviatoric Stress
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Deviatoric Stress in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study [Triaxial Test]/Solution 7 (sol7).
4
Locate the Title section. From the Title type list, choose None.
5
Locate the Plot Settings section.
6
Select the x-axis label checkbox. In the associated text field, type Axial strain (%).
7
Select the y-axis label checkbox. In the associated text field, type Deviatoric stress (MPa).
8
Locate the Axis section. Select the Manual axis limits checkbox.
9
In the x minimum text field, type 0.
10
In the x maximum text field, type 12.
11
In the y minimum text field, type 0.
12
In the y maximum text field, type 0.8.
Point Graph 1
1
Right-click Deviatoric Stress and choose Point Graph.
2
Select Point 4 only.
3
In the Settings window for Point Graph, locate the y-Axis Data section.
4
In the Expression text field, type solid3.mises.
5
Locate the x-Axis Data section. From the Parameter list, choose Expression.
6
In the Expression text field, type -solid3.eZZ.
7
From the Unit list, choose %.
8
In the Deviatoric Stress toolbar, click  Plot.
Stress Path 2
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Stress Path 2 in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study [Triaxial Test]/Solution 7 (sol7).
4
Locate the Title section. From the Title type list, choose None.
5
Locate the Plot Settings section.
6
Select the x-axis label checkbox. In the associated text field, type Mean stress (MPa).
7
Select the y-axis label checkbox. In the associated text field, type Deviatoric stress (MPa).
8
Locate the Axis section. Select the Manual axis limits checkbox.
9
In the x minimum text field, type 0.
10
In the x maximum text field, type 2.
11
In the y minimum text field, type 0.
12
In the y maximum text field, type 0.8.
Point Graph 1
1
Right-click Stress Path 2 and choose Point Graph.
2
Select Point 4 only.
3
In the Settings window for Point Graph, locate the y-Axis Data section.
4
In the Expression text field, type solid3.mises.
5
Locate the x-Axis Data section. From the Parameter list, choose Expression.
6
In the Expression text field, type solid3.pm.
7
In the Stress Path 2 toolbar, click  Plot.
Deviatoric Stress, Stress Path 2, Volumetric Strain
1
In the Model Builder window, under Results, Ctrl-click to select Volumetric Strain, Deviatoric Stress, and Stress Path 2.
2
Right-click and choose Group.
Triaxial Test
In the Settings window for Group, type Triaxial Test in the Label text field.
Mean Stress 1
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Mean Stress 1 in the Label text field.
3
Locate the Title section. From the Title type list, choose None.
4
Locate the Data section. From the Dataset list, choose Study [Constrained Swelling Test]/Solution 10 (sol10).
5
Locate the Plot Settings section.
6
Select the x-axis label checkbox. In the associated text field, type Suction (MPa).
7
Select the y-axis label checkbox. In the associated text field, type Mean stress (MPa).
Point Graph 1
1
Right-click Mean Stress 1 and choose Point Graph.
2
Select Point 4 only.
3
In the Settings window for Point Graph, locate the y-Axis Data section.
4
In the Expression text field, type solid4.pm.
5
Locate the x-Axis Data section. From the Parameter list, choose Expression.
6
In the Expression text field, type solid4.epm1.ss.
7
Click to expand the Coloring and Style section. 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
Mean stress
Point Graph 2
1
Right-click Point Graph 1 and choose Duplicate.
2
In the Settings window for Point Graph, locate the y-Axis Data section.
3
In the Expression text field, type P_analytical.
4
Locate the Legends section. In the table, enter the following settings:
Legends
Mean stress, analytical
5
Locate the Coloring and Style section. From the Color list, choose From theme.
6
Find the Line style subsection. From the Line list, choose None.
7
Find the Line markers subsection. From the Marker list, choose Circle.
8
From the Positioning list, choose Interpolated.
9
In the Number text field, type 20.
10
In the Mean Stress 1 toolbar, click  Plot.
Void Ratio and Volumetric Strain
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Void Ratio and Volumetric Strain in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study [Constrained Swelling Test]/Solution 10 (sol10).
4
Locate the Title section. From the Title type list, choose None.
5
Locate the Plot Settings section. Select the Two y-axes checkbox.
6
Select the x-axis label checkbox. In the associated text field, type Suction (MPa).
7
Select the y-axis label checkbox. In the associated text field, type Void ratio (1).
8
Select the Secondary y-axis label checkbox. In the associated text field, type Volumetric strain (%).
9
Locate the Axis section. Select the Manual axis limits checkbox.
10
In the x minimum text field, type 10.
11
In the x maximum text field, type 105.
12
In the y minimum text field, type 0.4.
13
In the y maximum text field, type 0.8.
14
In the Secondary y minimum text field, type -10.
15
In the Secondary y maximum text field, type 10.
Point Graph 1
1
Right-click Void Ratio and Volumetric Strain and choose Point Graph.
2
Select Point 4 only.
3
In the Settings window for Point Graph, locate the y-Axis Data section.
4
In the Expression text field, type solid4.evoid.
5
Locate the x-Axis Data section. From the Parameter list, choose Expression.
6
In the Expression text field, type solid4.epm1.ss.
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
Void ratio
Point Graph 2
1
Right-click Point Graph 1 and choose Duplicate.
2
In the Settings window for Point Graph, locate the y-Axis Data section.
3
In the Expression text field, type solid.evol.
4
From the Unit list, choose %.
5
Locate the y-Axis section. Select the Plot on secondary y-axis checkbox.
6
Locate the Legends section. In the table, enter the following settings:
Legends
Volumetric strain
Void Ratio and Volumetric Strain
1
In the Model Builder window, collapse the Results > Void Ratio and Volumetric Strain node.
2
In the Model Builder window, click Void Ratio and Volumetric Strain.
3
In the Void Ratio and Volumetric Strain toolbar, click  Plot.
Mean Stress 1, Void Ratio and Volumetric Strain
1
In the Model Builder window, under Results, Ctrl-click to select Mean Stress 1 and Void Ratio and Volumetric Strain.
2
Right-click and choose Group.
Constrained Swelling Test
In the Settings window for Group, type Constrained Swelling Test in the Label text field.