[GTS NX] 2D Excavation with Retaining System

0. Contents 

1. Overview

1-1 Learning Purpose

This tutorial aims to identify ground-structure interaction by analyzing the construction stage of 2D excavation works with a retaining system, including retaining walls and struts. The objective is to review the stability of retaining walls using the finite element method to calculate displacements and stresses based on the elastic-plastic characteristics of the ground and the interaction between the retaining wall and structural members. By employing this method, users can verify not only the forces and deflection of the retaining wall but also their impact on the surrounding ground and adjacent structures simultaneously.

The retaining wall is located on both sides, with two layers of struts for three excavation stages. The retaining wall is modeled using beam elements to verify bending moments and shear forces, while struts are modeled using truss elements to verify axial forces. Additionally, an interface is added between the ground and retaining wall to simulate ground-structure interaction more realistically.

Analysis Model Overview

In this tutorial, the following concepts will be explained :

1. Applying the Mohr-Coulomb model

2. Modeling diaphragm walls with beam elements, struts with truss elements, and interfaces

3. Considering surcharge and water conditions

4. Verifying ground settlement, structural deflection, and forces

1-2 Modeling and Analysis Summary

The model presents a 5m depth and 8m width excavation, supported by a temporary support system comprising a diaphragm wall and two layers of struts. The excavation process consists of three stages (at depths of 1.7m, 3.7m, and 5m), with total supports installed at two layers (at depths of 1m and 3m). The ground consists of four layers, with variations in depth between the left and right sides based on the excavation area.

Cross Section

To minimize the influence of boundary conditions, the total ground area width is set to 68m, which is 8.5 times wider than the excavation width.

2. Analysis Setting

2-1 Starting with Analysis Setting

[  : Analysis → Analysis Case → Setting]

[Open the attached start file (01 2D Excavation_Start)]

Set the model type, gravity direction, and initial parameters. Check the unit system that will apply to the analysis. The unit system can be modified both during the modeling process and after performing the analysis, with input parameters automatically converting to the correct unit system.

This tutorial utilizes a 2D model with the y-gravity direction and employs the SI unit system (kN and m).

Analysis Setting Window

3. Material and Property

3-1 Material Definition for Ground and Structures

For the material model type, apply 'Mohr-Coulomb' for the ground and 'Elastic' for the structure.
The material properties for each ground and structural member are listed in the following table. For the interface material, use the parameters calculated automatically by the wizard.

Ground Material

Structure Material

3-2 Define Properties

Properties represent physical attributes of the meshes and will be assigned to mesh sets during mesh generation. When defining ground and structure properties, first select the material to be used. For structure properties, structure types and cross-section shapes (cross-section stiffness) should be further defined.

Use 'Beam Element' for the diaphragm wall, as they are continuous walls with thickness that need to resist axial, shear, and bending moments. Struts are typically assumed as 'Truss Element,' which only resist axial force.

The ground properties are shown in the following table :

Ground Property

Structure Property

4. Modeling

4-1 Geometry Modeling

Since the purpose of this tutorial is to study 2D geometry, mesh generation, analysis workflow, and results verification, please begin by opening the start file where basic materials and properties have already been predefined.

Import CAD file for Geometry

In this tutorial, we will utilize the import function to import geometry from a DWG file.

① Click on [File] and navigate to the ‘Import’ function

② Select DWG(Wireframe) and click on ‘Select AutoCAD DWG File’

③ Choose the dwg file named ‘01 2D Excavation with Retaining System’ and click on [Open]

④ Click on [OK]

Imported Geometry

⑤ Click on ‘Intersect’ function and select all edges(29 edges)

⑥ Click on [OK] to close the function

[  : Geometry → Point & Curve → Intersect]

4-2 Mesh Generation

In this tutorial, we will define the mesh size using the size control function.

[  : Mesh → Control → Size Control]

① Click on ‘Size Control’ function

② Click on [Select Object] and Select all the edges(25 edges) of the excavated part

③ ‘0.5 m’ for Mesh Size

④ Click on [OK]

Mesh Size Control

[  : Mesh → Generate → 2D]

Generate a 2D mesh using the overall geometry (edges).

① Click on the ‘2D’ function

② Move to the ‘Auto-Area’ tab

③ Select overall edges(64 edges)

④ Enter ‘1.5 m’ for size and Click on [OK]

Mesh Generation for Ground

[  : Mesh → Element → Parameters]

Change the properties of the meshes that have already been generated.

① Click on the ‘Parameters’ function

② Move to the ‘2D’ tab and select ‘Change Property’ function

③ Select 1st layer of ground and choose ‘SOIL1’ from property dropdown menu

④ Click on [Apply] and repeat this process for every layer of soil (4 layers)

Change Parameters

In this step, the retaining system (diaphragm wall and struts) will be generated. Use beam elements for the diaphragm wall, which resist axial, shear, and bending moment, and truss elements for the struts, which only resist axial force. Utilize the 'Extract' and ‘Create’ function because both beam and truss elements must share nodes with the ground.

[  : Mesh → Element → Extract]

① Click on the ‘Extract Element’ function

② Choose the ‘Edge’ for type and ‘D-Wall’ for property

③ Select the edges(15 edges) to be used for the retaining wall

④ Change the Mesh set name to ‘RW’

⑤ Click on [OK]

[  : Mesh → Element → Create]

① Click on the ‘Element Create/Delete’ function

② Move to the ‘1D’ tab and choose ‘S1’ for property

③ Select the nodes which are the starting and ending points of the 1st layer of strut

④ Change the Mesh set name to ‘S1’

⑤ Click on [Apply] and repeat this process for 2nd layer of strut

To simulate more realistic behavior between the ground and the structure (retaining wall), use the generated diaphragm wall (beam element) to create interface elements at the side of the excavation area.

The interface function operates as follows: Right after generating the interface element, connected nodes are automatically detached at the spots of the interface. Then, a special element is created between the detached nodes, which has specific rigidity in both normal and tangent directions. In stages where the interface elements are not activated yet, rigid links must be applied to connect the nodes to prevent errors. Conversely, in stages where the interface elements are activated, rigid links should be excluded. In the tutorial, the material properties of the interface elements are automatically set in the wizard by calculating from the surrounding ground parameters.

[  : Mesh → Element → Interface]

① Click on the ‘Create Interface’ function

② Move to the ‘Line’ tab and choose From Truss/Beam’ for Type

③ Select the beam elements (48 elements) that represent the retaining wall

④ Check ‘Merge Nodes’ and select the toes of retaining wall (2 nodes)

⑤ Choose ‘Wizard’ from property parameters and enter ‘0.67’ for strength reduction factor(R)

⑥ Click on [OK]

Mesh Generation for Structures

In this tutorial, there are 3 stages for the excavation. Therefore, the mesh set needs to be defined for each excavation stage using the works-tree for construction stage setting.

① Right-click on the Mesh in the Works Tree window and select 'New Mesh Set'.

② Change the name of the mesh set by selecting it from the works-tree and pressing [F2] on the keyboard.

③ Name the new mesh set 'EX1'.

④ Right-click on the 'EX1' mesh set and select 'Include/Exclude Elements & Nodes'.

⑤ Change the selection method to 'Mesh Set' by pressing [M] on the keyboard.

⑥ Select the mesh sets that represent the 1st excavation area.

⑦ Click on [OK] and repeat this process for the 2nd and 3rd excavation areas.

Define the Mesh for Construction Stage

5. Analysis

5-1 Setting Load Condition

This process sets the surcharge, such as a vehicle load, next to the retaining wall.

[ : Static/Slope Analysis → Load → Press.]

① Click on the 'Pressure' function and navigate to the 'Edge' tab.

② Choose the '2D Element Edge' for the type.

③ Change the selection method to 'edge' by pressing [E] on the keyboard.

④ Select the 5m edges located 1m away from both sides of the retaining wall.

⑤ Enter '10 kN/m' for P or P1 to specify the amount of pressure.

⑥ Enter 'Surcharge' for the load set name and click on [OK].

5-2 Setting Boundary Conditions

This process assigns boundary conditions to the analysis model based on the global coordinate system. In 2D analysis, we constrain the horizontal displacement of the left and right side borders, and constrain both horizontal and vertical displacements of the bottom. GTS NX automatically detects the boundaries of the model and generates boundary conditions.

[ : Static/Slope Analysis → Boundary → Constraint]

① Click on the 'Constraint' function and navigate to the 'Auto' tab.

② Enter the name 'Boundary Condition' for the boundary set and click on [OK].

Surcharge and Boundary Condition

5-3 Setting Water Condition

This process defines the water condition for each excavation stage and considers hydrostatic pressure.

[ : Static/Slope Analysis → Boundary → Water Level]

① Click on the 'Water Level' function and navigate to the 'Edge' tab.

② Select the edges (9 edges) from ground surface to consider the water condition at initial stage.

③ Enter the name ‘[W] Initial’ and click on [Apply]

④ Select the edges (10 edges) from both ground surface behind the retaining wall and bottom of 1st excavation

⑤ Enter the name ‘[W] EX1’ and click on [Apply]

⑥ Repeat this process for [W] EX2 and [W] EX3, to consider the water condition for 2nd and 3rd excavation

5-4 Define Construction Stages

In this process, we define construction stages to check analysis results from each step. To define construction stages, mesh sets should be pre-divided. Then, load and boundary conditions are assigned to relevant mesh sets in each step. Starting from the original ground stress condition, each construction stage, such as excavation and installation of the support system, can be defined using this function.

[ : Static/Slope Analysis → Construction Stage → Stage Set]

① Click on ‘Stage Set’ function

② Enter the name ‘Excavation’ and select ‘Stress’ for the stage type

③ Click on [Add] and double-click on created stage set, ‘Excavation’

④ The activated and deactivated data are defined for each stage (8 stages), referring to the following figures

Stage 1. Initial

Stage 2. Surcharge

Stage 3. Install Retaining Wall

Stage 4. 1st Excavation

Stage 5. Install 1st Strut

Stage 6. 2nd Excavation

Stage 7. Install 2nd Strut

Stage 8. 3rd Excavation

5-5 Define Analysis Case

This process sets the analysis method and model data for the analysis. The analysis and output types can be defined using the advanced options.

[ : Analysis → Analysis Case → General]

① Click on ‘General’ function

② Enter the name ‘Excavation’ for title and select ‘Construction Stage’ for solution type

③ Select the ‘Excavation’ for construction stage set

④ Click on ‘Analysis Control’ and check on ‘Initial Stage for Stress Analysis’ and ‘Apply K0 Condition’

Analysis Case & Option

5-6 Perform Analysis

Perform the analysis. Once the analysis is complete, it will automatically switch to 'Post-Mode (Confirmation of the Results)'. To make further modifications to the model and options, you need to switch back to the 'Pre-Mode'.

[ : Analysis → Analysis → Perform]

① Click on ‘Perform’ function

② Click on [OK]

6. Results

6-1 Results Verification

After the analysis, we can check the results such as displacements, stresses, and member forces of each construction stage in the Result tab under the Work-Tree. All the results can be displayed in the form of contour, table, and graph. The main result items that need to be checked in this tutorial are listed below.

Ground : Displacement in the X and Y directions

Diaphragm Wall : Horizontal deflection and forces (Axial force, Shear force and Bending moment)

Strut : Axial force

6-2 Results Checking for Ground

Verify the 'Displacements' in the Results tab from the Work-Tree after performing the analysis. Tx, Ty, and Tz represent displacements based on the x, y, and z directions, respectively. Tx denotes horizontal displacement, Ty indicates vertical displacement, which is settlement in the geotechnical industry for 2D analysis. Tz is not considered in the 2D analysis. Additionally, '(V)' stands for 'vector', indicating a result that can represent both contour and vector simultaneously. In GTS NX, it is possible to display contour and vector at the same time for displacements and principal stresses.

Double-click on 'Displacements' to check the displacement at the last stage. Then, double-click on 'Ty Translation(V)' to check the settlement of the ground.

Ground Settlement

By moving the stage bar at the bottom of the Work-Window, you can navigate to other stages.

Stage Bar

[ : Result → Advanced → Cutting Diag.]

Click on the 'On-Curve Diagram' function and select the starting node and ending node where we need to verify ground settlement. Choose '(+)Y Dir.' to define the direction and click on OK.

Cutting Diagram

6-3 Results Checking for Retaining System

This process will demonstrate how to check not only the forces from the retaining wall and strut but also the deflection of the retaining wall.

Select the last stage in the Result-Tree, choose 'Beam Element Forces', and double-click on 'Axial Force', 'Shear Force Z', and 'Bending Moment Y' to verify the forces from the diaphragm wall.

Retaining Wall Shear Force

Retaining Wall Bending Moment

[ : Result → Advanced → Cutting Diag.]

Click on the 'On-Curve Diagram' function and select the nodes from the top and bottom of the left side of the retaining wall. Choose '(+)X Dir.' for the direction and click on OK. Repeat the process for the right-hand side of the retaining wall.
In the Result-Tree, double-click on 'Displacement' at the last stage and select 'Tx Translation (V)' to check the deflection of the retaining wall.

Retaining Wall Deflection

Click on the Model tab under the Work-Tree and specify only the strut mesh sets 'S1' and 'S2' under the Mesh-Tree. Then, go to the Results tab and double-click on 'Truss Element Forces'. Click on 'Axial Force' to check the axial force from the struts.

Strut Axial Force