Deep Excavation

There are two ways to model an excavation in COMSOL Multiphysics, both of which include a parametric sweep. One option involves removing the soil one step at a time by means of a sweep of the geometry. As the soil is removed, the support it supplies is removed as well, subjecting the retaining wall to soil stresses from the non excavated side. The other option is to start with the already excavated geometry, and simulate the soil removal by modifying a boundary load. The boundary load applies a force on the excavation side of the retaining wall, equal to (and therefore balancing) the in-situ stresses on the nonexcavated side, for the part of the wall that is below the virtual excavation depth.

This deep excavation example is inspired by a benchmark exercise specified by a working group of the German Society for Geotechnics (Ref. 1 and Ref. 2). In the example, a 26 meter excavation is modeled by means of a parametric sweep. As the excavation deepens, three struts are activated using a ramp function and boolean expressions. As the excavation reaches their depths, the struts are activated as long as the horizontal wall deflection is greater than what it is allowed to be..

Figure 1: Dimensions and boundary conditions for the deep excavation example.

Model Definition

In this example, a Drucker-Prager criterion is used for studying the soil plasticity, and the retaining wall is made of a linear elastic material. The following material parameters are used:

Soil, Upper layer

•

Young’s modulus E = 20 MPa, Poisson’s ratio ν = 0.3, and density ρ = 1900 kg/m3.

•

Cohesion c = 0 Pa, and angle of internal friction

Soil, Lower layer

•

Young’s modulus E = 60 MPa, Poisson’s ratio ν = 0.3, and density ρ = 1900 kg/m3.

•

Cohesion c = 0 Pa, and angle of internal friction

Struts

•

Young’s modulus E = 200 GPa, length l = 30 m and cross sectional area A = 15 cm2.

Retaining Wall

•

Young’s modulus E = 30 GPa, Poisson’s ratio ν = 0.15, and density ρ = 2400 kg/m3.

Constraints and Loads

•

The bottom soil layer is supported by a rigid and perfectly rough base. Therefore, apply a fixed constraint on the lower horizontal boundary.

•

Due to symmetry, model only the right half of the domain. Use the symmetry boundary condition at the left vertical boundary.

•

Add in-situ stresses with the External Stress feature. Note that the stress caused by gravity is compressive, which in the convention used in the Structural Mechanics Module means negative sign.

•

The in-situ stresses account for the local stress prior excavating. You can define a different value in the vertical and horizontal directions. The horizontal in-situ stress, X_stress, is also used on the boundary load applied to the retaining wall.

•

The boundary load on the retaining wall is gradually decreased in order to simulate the excavation steps. At the bottom of the excavation it ensures zero initial displacement. This strategy avoids remeshing the excavated volume and thus saves memory.

•

Add struts that can be activated and deactivated according to the excavation depth by means of boolean expressions.

•

The struts are active after a maximum horizontal deflection is reached. Use a ramp function to restrict the allowed wall deflection U_max to 25 mm, and to supply the axial force that the struts apply to the wall.

•

The boundaries between the retaining wall and the soil are modeled with extrusion operators. These operators constrain the normal displacement between the retaining wall and the soil to stay in contact, while the tangential displacement is unconstrained.

•

The axial stiffness of the struts is estimated from their cross sectional area A, the length l, and the material Young’s modulus E as

Results and Discussion

In order to improve convergence on the soil-wall boundary, apply a mapped mesh on the retaining wall domain, as shown in Figure 2.

Figure 2: A mapped mesh on the retaining wall domain gives a better convergence.

Figure 3 shows the soil deformation and the wall deflection after excavating 26 meters. Figure 4 shows that the different properties of the two soil layers have an impact on the plastic deformation.

Figure 3: Deformation of the soil and the retaining wall after excavating 26 meters of soil.

Figure 4: Plastic deformation after excavating 26 meters of soil.

The struts — placed 4.8 m, 9.3 m, and 14.35 m below the initial surface (Ref. 1) — help to increase the overall stiffness of the retaining wall. In Figure 5, a maximum allowed displacement of 2.5 cm constrains the horizontal displacement of the retaining wall.

Figure 5: Wall deflection as a function of depth for different excavation steps (color lines).

As the excavation progresses, it is possible to observe the settlement of the unexcavated region. As expected, the settlement increases as the excavation progresses, and decreases with the distance to the retaining wall, see Figure 6.

Figure 6: Surface settlement as a function of the distance from the wall. The different color lines show the settlement for different excavation stages (0 to 26 m).

References

1. H.F. Schweiger, Benchmarking in Geotechnics 1. Technical Report CGG IR006 2002, Institute for Soil Mechanics and Foundation Engineering, Graz University of Technology, Austria.

2. D. Potts and L. Zdravkovic, Finite Element Analysis in Geotechnical Engineering, Thomas Telford Publishing, 2001.

Geomechanics_Module/Soil/deep_excavation

Modeling Instructions

From the menu, choose .

New

In the window, click

Model Wizard

In the window, click

In the tree, select .

Click .

Click

In the tree, select .

Click

Global Definitions

Parameters 1

In the window, under click .

In the window for , locate the section.

In the table, enter the following settings:


Name	Expression	Value	Description
X_stress	-24e3[Pa]	-24000 Pa	In-situ stress, xx component
Y_stress	-35e3[Pa]	-35000 Pa	In-situ stress, yy component
Z_stress	-24e3[Pa]	-24000 Pa	In-situ stress, zz component
E_struts	2e5[MPa]	2E11 Pa	Young's modulus of the struts
A_struts	15[cm^2]	0.0015 m²	Cross section area of the struts
l_struts	30[m]	30 m	Length of struts
S_struts	E_struts*A_struts/l_struts	1E7 N/m	Stiffness of the struts
U_max	-25[mm]	-0.025 m	Allowed wall deflection
Stage_1	-4.8[m]	-4.8 m	First excavation step, first strut
Stage_2	-9.3[m]	-9.3 m	Second excavation step, second strut
Stage_3	-14.35[m]	-14.35 m	Third excavation step, third strut
Depth	0[m]	0 m	Excavation depth (parameter)

In-situ stresses are set with negative sign to fit the structural mechanics convention. That convention assumes negative stresses in compression and positive in tension.

Ramp 1 (rm1)

In the toolbar, click

and choose .

In the window for , locate the section.

In the text field, type -U_max.

In the text field, type S_struts/U_max.

Click to expand the section. Select the check box.

In the associated text field, type 0.0001.

Geometry 1

Create the geometry.

To simplify this step, you can insert a prepared geometry sequence. In the toolbar, click . Browse to the model’s Application Libraries folder and double-click the file deep_excavation.mph. Click In the toolbar. Then, continue with the instruction after the geometry plot below.

Otherwise, proceed with the following instructions to create the geometry from scratch:

Rectangle 1 (r1)

In the toolbar, click

In the window, expand the node, then click .

In the window for , locate the section.

In the text field, type 90.

In the text field, type 60.

Locate the section. In the text field, type -60.

Click

Rectangle 2 (r2)

In the toolbar, click

In the window for , locate the section.

In the text field, type 90.

In the text field, type 20.

Locate the section. In the text field, type -20.

Click

Union 1 (uni1)

In the toolbar, click

and choose .

Click in the window and then press Ctrl+A to select both objects.

In the window for , click

Rectangle 3 (r3)

In the toolbar, click

In the window for , locate the section.

In the text field, type 30.

Locate the section. In the text field, type -30.

Click

Rectangle 4 (r4)

In the toolbar, click

In the window for , locate the section.

In the text field, type 0.8.

In the text field, type 30.

Locate the section. In the text field, type 30.

In the text field, type -30.

Click

Difference 1 (dif1)

In the toolbar, click

and choose .

Select the object only.

In the window for , locate the section.

Find the subsection. Select the

toggle button.

Select the objects and only.

Select the check box.

Click

Delete Entities 1 (del1)

In the window, right-click and choose .

In the window for , locate the section.

From the list, choose .

Click

Select the objects and only.

Click

Line Segment 1 (ls1)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

Locate the section. In the text field, type 30.

Locate the section. In the text field, type Stage_1+1.

Locate the section. In the text field, type Stage_1.

Click

Line Segment 2 (ls2)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

Locate the section. In the text field, type 30.

Locate the section. In the text field, type Stage_2+1.

Locate the section. In the text field, type Stage_2.

Click

Line Segment 3 (ls3)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

Locate the section. In the text field, type 30.

Locate the section. In the text field, type Stage_3+1.

Locate the section. In the text field, type Stage_3.

Click

Union 2 (uni2)

In the toolbar, click

and choose .

Select the objects , , , and only.

In the window for , click

Form Union (fin)

In the window, under click .

In the window for , locate the section.

From the list, choose .

Clear the check box.

Click

Definitions

Wall diaphragm

In the toolbar, click

In the window for , type Wall diaphragm in the text field.

Locate the section. From the list, choose .

Select Boundary 20 only.

Wall soil

In the toolbar, click

In the window for , type Wall soil in the text field.

Locate the section. From the list, choose .

Select Boundaries 5 and 6 only.

General Extrusion 1 (genext1)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Click

In the dialog box, type 12 in the text field.

Click .

In the window for , locate the section.

From the list, choose .

Locate the section. In the text field, type X.

In the text field, type Y.

General Extrusion 2 (genext2)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

Locate the section. In the text field, type X.

In the text field, type Y.

Solid Mechanics (solid)

Linear Elastic Material 1

In the window, under click .

Soil Plasticity 1

In the toolbar, click

and choose .

In the window for , locate the section.

Select the check box.

Select Domains 1 and 2 only.

Linear Elastic Material 1

In the window, click .

External Stress 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

In the Sext table, enter the following settings:


X_stress	0	0
0	Y_stress	0
0	0	Z_stress

Symmetry 1

In the toolbar, click

and choose .

Select Boundary 1 only.

Fixed Constraint 1

In the toolbar, click

and choose .

Select Boundary 2 only.

Roller 1

In the toolbar, click

and choose .

Select Boundaries 9 and 10 only.

Prescribed Displacement 1

In the toolbar, click

and choose .

Select Boundary 4 only.

In the window for , locate the section.

Select the check box.

In the u 0 y text field, type genext1(v).

Prescribed Displacement 2

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. Select the check box.

In the u 0 x text field, type genext2(u).

Boundary Load 1

In the toolbar, click

and choose .

Select Boundaries 3, 8, and 19 only.

In the window for , locate the section.

Specify the FA vector as


0	x
Y_stress	y

Boundary Load 2

In the toolbar, click

and choose .

Select Boundaries 11 and 13–18 only.

In the window for , locate the section.

Specify the FA vector as


-X_stress*(y<Depth)	x
0	y

Strut_1

In the toolbar, click

and choose .

In the window for , type Strut_1 in the text field.

Select Boundary 17 only.

Locate the section. From the list, choose .

Specify the Ftot vector as


-rm1(-u[1/m])*(Depth<Stage_1)	x
0	y

Strut_2

In the toolbar, click

and choose .

In the window for , type Strut_2 in the text field.

Select Boundary 15 only.

Locate the section. From the list, choose .

Specify the Ftot vector as


-rm1(-u[1/m])*(Depth<Stage_2)	x
0	y

Strut_3

In the toolbar, click

and choose .

In the window for , type Strut_3 in the text field.

Select Boundary 13 only.

Locate the section. From the list, choose .

Specify the Ftot vector as


-rm1(-u[1/m])*(Depth<Stage_3)	x
0	y

Materials

Soil, upper layer

In the window, under right-click and choose .

In the window for , type Soil, upper layer in the text field.

Locate the section. From the list, choose .

Click

Select Domain 2 only.

Locate the section. In the table, enter the following settings:


Property	Variable	Value	Unit	Property group
Young’s modulus	E	20e6	Pa	Basic
Poisson’s ratio	nu	0.3	1	Basic
Density	rho	1900	kg/m³	Basic
Cohesion	cohesion	0	Pa	Mohr-Coulomb
Angle of internal friction	internalphi	35[deg]	rad	Mohr-Coulomb

Soil, lower layer

Right-click and choose .

In the window for , type Soil, lower layer in the text field.

Select Domain 1 only.

Locate the section. In the table, enter the following settings:


Property	Variable	Value	Unit	Property group
Young’s modulus	E	60e6	Pa	Basic
Poisson’s ratio	nu	0.3	1	Basic
Density	rho	1900	kg/m³	Basic
Cohesion	cohesion	0	Pa	Mohr-Coulomb
Angle of internal friction	internalphi	35[deg]	rad	Mohr-Coulomb