PDF
Block Verification
Introduction
This example shows how to set up a compression test on a prestressed soil sample. Due to a simple stress state, it is possible to determine the vertical yield stress analytically. The soil sample is modeled with soil plasticity and the Mohr-Coulomb criterion.
Model Definition
In this example, we consider a block of soil of 1 m length on each side. The soil is pressed from the sides by boundary loads in the x and y directions, and from the top by a prescribed displacement.
Figure 1: Dimensions, boundary conditions, and loads for the test.
Elastic Properties
The soil properties are taken from standard clay.
•
Young’s modulus, E = 207 MPa, and Poisson’s ratio ν = 0.3.
Soil Plasticity
•
Cohesion c = 70 kPa, and angle of internal friction .
•
Use the Mohr-Coulomb criterion, with non-associated flow rule, and Drucker-Prager matched at compressive meridian as plastic potential.
Constraints and Loads
•
The test is based on uniaxial compression. Fix the normal displacement at the lower, left, and right boundaries with a roller boundary condition (these are the boundaries at x = 0, y = 0, and z = 0).
•
On the other two vertical walls (x = 1 m and y = 1 m), apply boundary loads of 300 kPa and 200 kPa, as shown on Figure 2.
•
The in-situ stress is prescribed via the External Stress node.
•
The soil sample is subjected to a loading at the top boundary through a prescribed displacement. By means of a parametric sweep, the displacement is gradually increased up to 8 mm.
Figure 2: Boundary loads applied on the block.
Results and Discussion
The cube of soil experiences a homogeneous stress state, as shown by distribution of von Mises stress in Figure 3.
Figure 3: Equivalent stress and deformation in the soil sample after applying 8 mm displacement from the top.
From the Mohr circle, the Mohr-Coulomb criterion can be written in terms of the biggest and smallest principal stress:
Since stress in the y direction is the largest principal stress and the stress in z direction is the smallest principal stress at the onset of yielding, its analytical value can be obtained. Manipulation of the above formula gives
(1)
The stresses history together with the analytical value of the stress in the z direction at the onset of yielding is shown in Figure 4. Plastic yielding is reached after a deflection of about 3.5 mm.
Figure 4: This plot shows how the soil sample behaves elastically until it reaches the yield surface at the compressive meridian.
Application Library path: Geomechanics_Module/Verification_Examples/block_verification
Modeling Instructions
From the File menu, choose New.
New
In the New window, click  Model Wizard.
Model Wizard
1
In the Model Wizard window, click  3D.
2
In the Select Physics tree, select Structural Mechanics>Solid Mechanics (solid).
3
Click Add.
4
Click  Study.
5
In the Select Study tree, select General Studies>Stationary.
6
Click  Done.
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
Disp
0
0
 
X_stress
-3e5[Pa]
-3E5 Pa
In-situ stress, xx component
Y_stress
-2e5[Pa]
-2E5 Pa
In-situ stress, yy component
Z_stress
-1e5[Pa]
-1E5 Pa
In-situ stress, zz component
In-situ stresses are set with negative sign to fit the structural mechanics convention which assumes negative stresses in compression, and positive in tension.
Geometry 1
Block 1 (blk1)
1
In the Model Builder window, expand the Component 1 (comp1)>Geometry 1 node.
2
Right-click Geometry 1 and choose Block.
3
In the Settings window for Block, click  Build All Objects.
The geometry consists of a simple unit block.
Solid Mechanics (solid)
Linear Elastic Material 1
In the Model Builder window, under Component 1 (comp1)>Solid Mechanics (solid) click Linear Elastic Material 1.
Soil Plasticity 1
1
In the Physics toolbar, click  Attributes and choose Soil Plasticity.
2
In the Settings window for Soil Plasticity, locate the Soil Plasticity section.
3
From the Yield criterion list, choose Mohr-Coulomb.
The Mohr-Coulomb criterion is used to define yield surface. Use the non-associated Drucker-Prager plastic potential matched to the Mohr-Coulomb model at the compressive meridian.
Linear Elastic Material 1
In the Model Builder window, click Linear Elastic Material 1.
External Stress 1
1
In the Physics toolbar, click  Attributes and choose External Stress.
2
In the Settings window for External Stress, locate the External Stress section.
3
From the list, choose Diagonal.
4
In the Sext table, enter the following settings:
X_stress
0
0
0
Y_stress
0
0
0
Z_stress
Roller 1
1
In the Physics toolbar, click  Boundaries and choose Roller.
2
Select Boundaries 1–3 only.
Boundary Load 1
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
Select Boundary 6 only.
3
In the Settings window for Boundary Load, locate the Force section.
4
Specify the FA vector as
X_stress
x
0
y
0
z
Boundary Load 2
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
Select Boundary 5 only.
3
In the Settings window for Boundary Load, locate the Force section.
4
Specify the FA vector as
0
x
Y_stress
y
0
z
Prescribed Displacement 1
1
In the Physics toolbar, click  Boundaries and choose Prescribed Displacement.
2
Select Boundary 4 only.
3
In the Settings window for Prescribed Displacement, locate the Prescribed Displacement section.
4
Select the Prescribed in z direction check box.
5
In the u 0 z text field, type -Disp.
Materials
Material 1 (mat1)
1
In the Model Builder window, under Component 1 (comp1) right-click Materials and choose Blank Material.
2
In the Settings window for Material, locate the Material Contents section.
3
In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Young’s modulus
E
207e6
Pa
Basic
Poisson’s ratio
nu
0.3
1
Basic
Density
rho
2000
kg/m³
Basic
Cohesion
cohesion
70e3
Pa
Mohr-Coulomb
Angle of internal friction
internalphi
30[deg]
rad
Mohr-Coulomb
Mesh 1
Mapped 1
1
In the Mesh toolbar, click  Boundary and choose Mapped.
2
Select Boundary 4 only.
Swept 1
In the Mesh toolbar, click  Swept.
Size
1
In the Model Builder window, click Size.
2
In the Settings window for Size, locate the Element Size section.
3
From the Predefined list, choose Extra coarse.
4
Click  Build All.
Study 1
Step 1: Stationary
Set up an auxiliary continuation sweep for the Disp parameter.
1
In the Model Builder window, under Study 1 click Step 1: Stationary.
2
In the Settings window for Stationary, click to expand the Study Extensions section.
3
Select the Auxiliary sweep check box.
4
Click  Add.
5
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
Disp
8[mm]*range(0,0.05,1)
m
6
In the Home toolbar, click  Compute.
Results
Stress (solid)
The default plot shows the von Mises stress for the final step.
1
In the Stress (solid) toolbar, click  Plot.
Add a 1D plot to show the evolution of the stress-tensor components versus the displacement at the top surface.
Stresses vs. Displacement
1
In the Home toolbar, click  Add Plot Group and choose 1D Plot Group.
2
In the Settings window for 1D Plot Group, type Stresses vs. Displacement in the Label text field.
3
Click to expand the Title section. From the Title type list, choose Label.
4
Locate the Plot Settings section. Select the x-axis label check box.
5
In the associated text field, type Vertical displacement (mm).
6
Select the y-axis label check box.
7
In the associated text field, type Stress (kPa).
Point Graph 1
1
Right-click Stresses vs. Displacement and choose Point Graph.
2
Select Point 1 only.
3
In the Settings window for Point Graph, 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.sx - Stress tensor, x component.
4
Locate the y-Axis Data section. From the Unit list, choose kPa.
5
Locate the x-Axis Data section. From the Parameter list, choose Expression.
6
In the Expression text field, type Disp*1000.
7
Click to expand the Coloring and Style section. Click to expand the Legends section. Select the Show legends check box.
8
From the Legends list, choose Manual.
9
In the table, enter the following settings:
Legends
sxx stress
10
In the Stresses vs. Displacement toolbar, click  Plot.
Point Graph 2
1
Right-click Point Graph 1 and choose Duplicate.
2
In the Settings window for Point Graph, 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.sy - Stress tensor, y component.
3
In the Stresses vs. Displacement toolbar, click  Plot.
4
Locate the Legends section. In the table, enter the following settings:
Legends
syy stress
Point Graph 3
1
In the Model Builder window, under Results>Stresses vs. Displacement right-click Point Graph 1 and choose Duplicate.
2
In the Settings window for Point Graph, 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.sz - Stress tensor, z component.
3
In the Stresses vs. Displacement toolbar, click  Plot.
4
Locate the Legends section. In the table, enter the following settings:
Legends
szz stress
Point Graph 4
1
Right-click Point Graph 1 and choose Duplicate.
The analytical yield level is given by Equation 1.
2
In the Settings window for Point Graph, locate the y-Axis Data section.
3
In the Expression text field, type (2*solid.cohesion*cos(solid.internalphi)-Y_stress*(1+sin(solid.internalphi)))/(sin(solid.internalphi)-1).
4
Locate the Coloring and Style section. Find the Line style subsection. From the Line list, choose Dashed.
5
From the Color list, choose Magenta.
6
Locate the Legends section. In the table, enter the following settings:
Legends
Theoretical yield stress
7
In the Stresses vs. Displacement toolbar, click  Plot.