MOHAMAD

ABOOD

Design Engineer

Product Research, Development, Visualization & Automation

The goal of this project was to investigate buried mass concrete thrust blocks by modelling and analysing them using Finite Element Analysis (FEA) through the employment of the popular computer-aided software package called ABAQUS. This led to an understanding of the behaviour of buried mass concrete thrust blocks in undrained clay and its effectiveness to be used as a means of supporting retaining walls during temporary construction.

 

A gradually increasing inclined load was applied to the centre of the thrust block to measure the induced displacements under variations of parameters such that the relationship between length, depth and the prop angle inclination could be established to help evaluate an effective design by plotting load-displacement curves.

 

The thrust block in this parametric study was analysed in 2-D planar from a set of 15 FEM tests meaning each five tests focused on analysing the results of each single parameter variation while setting the other two as constants. One FEM test was carried out on a trapezoidal cross section in order to assess its efficiency compared to the usual cross section utilized in construction. The maximum forces in all tests have been identified for a limiting displacement of 10 mm with the purpose of observing which parameter had most influence. The results convey that the effectiveness depends on the thrust block’s geometric values and the prop angle inclination of the applied force and thus the validity of the research conducted by Cabrera, Taylor & McNamara (2006) is supported by extensive simulations. It has been observed that all of the load-displacement curves had similar shapes and there exists a different mechanism of load transfer into the soil mass depending on the prop angle of load.

 

LIMITATION OF FINITE ELEMENT ANALYSIS

 

The main limitation of the basic finite element theory is that it is based on the assumption of linear material; however soils do not behave in such a manner since their properties are not completely uniform in the soil skeleton. Regardless, performing FEM analyses enables more accurate solutions for the force-displacement relation since the density is consistent throughout the soil mass. Another limitation is that the accuracy of the acquired solution is generally a function of the mesh resolution and thus finite element methods are approximate methods depending on the number of elements used. A sufficiently refined mesh was developed in order to carefully analyse the overall behaviour of thrust blocks and its interaction with the surrounding soil type.

Three types of designs were considered for the FEM analyses which included the wedge shaped cross section, the rectangular shaped cross section and the trapezoidal shaped cross section.

 

Thrust blocks with a wedge shaped cross section are preferred by some contractors as they are easy to excavate which saves time and costs.

 

Thrust blocks with a rectangular shaped cross section appear to be commonly used in practice and are quite popular in the construction industry for basement works. Research by Taylor, Atkinson, Stallebrass & McNamara (2006) indicates from a series centrifuge model tests and numerical analyses that in general the wedge shaped blocks appeared to be less efficient than rectangular shaped blocks, similar trends in the data were also observed on thrust block stiffness.

 

Data gathered from their research suggests an increase in efficiency in narrower thrust blocks which did not apply to wedge shaped cross sections, where depth seemed to be a more significant factor. This led to a focus on performing finite element method analyses on rectangular shaped cross sections, of which the current design is based on simple earth pressure theory.

 

 

The properties in Table 4.0 were used for the mass concrete thrust block and the clay soil in order to generate results when performing the simulation. The stiffness and flexural rigidity (EI) of the concrete is much higher compared to the soil, thus it was sufficient to consider it as rigid relative to the soil, helping to prevent distortions of the thrust block by the reaction force of the soil.

 

The clay soil and concrete thrust block were both assigned to be uniformly homogenous and isotropic. The tests were restricted to linear elastic two dimensional plane strain conditions meaning that the strain in one direction is zero. An undrained shear strength of 60 kPa has been assumed for the clay with a Young’s Modulus (E) of 100 MPa while setting the Poisson’s ratio (v) to 0.5 for the numerical modelling and analyses.

 

 

A series of finite element method analyses were performed in ABAQUS and only 2-D (plane strain) analyses were carried out, with the focus on reproducing similar data to that gathered from the research of Taylor, Atkinson, Stallebrass and McNamara (2006) to be able to observe similar trends and thus confirm the data presented in literature. The soil used was undrained clay since this type of soil is easier to analyse and thus is sufficient to acquire reliable data conveying the performance of thrust blocks.

 

This means that in this condition the pore water is unable to drain out of the soil and thus the rate of loading is much quicker than the rate at which the pore water is able to drain out of the soil skeleton. As a result, most of the external loading is taken by the pore water, resulting in an increase in the pore water pressure. The tendency of soil to change volume is suppressed during undrained loading which makes the modelling of the soil in ABAQUS simpler and straightforward.

 

The final models as shown in Figure 5.0 and 5.1 for the rectangular cross section and trapezoidal cross section respectively consisted of a thrust block surrounded by the clay soil with a force applied at the centre of the thrust block to measure the displacements induced and thus find out the maximum forces needed to generate a limiting displacement of 10 mm.

 

The element type has been chosen to be “family – plane stain” and “geometric order – quadratic” was selected. The default element used is CPE8R, an 8-node biquadratic plane strain quadrilateral reduced integration. An 8 noded quadrilateral element is widely used in geotechnical finite element software. The main requirement during the analyses performed is that the element types should be useful for all the geometric situations which may arise, including cases where structures have curved boundaries or curved material interfaces, therefore both triangular and quadrilateral types of elements could equally have been employed to mesh the soil and thrust block. However the quadrilateral family has been used since the finite element equations are slightly easier to formulate. It was ensured the elements are not distorted which could have led to different forms of inaccuracy.

 

After seeding the parts with an approximate global size of 0.4, the mesh in Figure 5.2 was produced. The mesh was created as very dense in order to obtain accurate displacements and forces developing throughout the model.

An in-situ stress check was performed with the boundary conditions and gravitational load which was done by creating a geostatic gravitational load in the Load Module before creating any further Steps, and inputting a value of -10 in Component 2 (y-direction), this is done in order to guarantee the in-situ stresses are in equilibrium.

 

The base of the model was restricted to move in U2

(y-direction) whereas the two sides of the mesh were fixed in U1

(x-direction), this allowed the mesh to compress as one would observe in a real life soil behaviour.

 

The thrust block interaction with the soil skeleton can be observed in Figure 6.0, 6.1 and 6.2 in which the arrows represent the direction of displacement induced by the same amount of maximum load for 20, 40 and 50 degrees. The displacements in the soil at a degree of 20 seem to be acting parallel to the top surface as shown in Figure 6.0 whereas in Figure 6.1 the displacements seem to start to follow a curved path which at the back is perpendicular to the surface which means the height of the soil mesh at the back of the thrust block has increased as shown in Figure 6.2. While increasing the degrees, the displacements acting on the thrust blocks take a circular path thereby suggesting that the thrust block is rotating to counteract the forces and achieve equilibrium.

 

The stresses induced throughout the thrust block are shown in Figure 6.3. The highest stresses coloured in red seem to have developed at the back face of the thrust block due to the rotation of the structure. A similar trend was observed in all tests.

 

The passive and active pressures generated by the soil are also shown in Figure 6.4, where the passive pressures appear to be higher since the load has been applied in that direction causing the thrust block to move.

 

The most important aspect of the foundation design is the necessary check for the stability of the foundation under various imposed loads. The foundation should remain stable under all the different combinations of loading, to which it is likely subjected under the most severe conditions.

 

All the load-displacement curves depicted a non-linear response that was similar to the bearing pressure and settlement graphs for shallow foundations with vertical loads.

 

The performed FEM analyses show that there exists a different mechanism of load transfer into the soil mass which is dependent on the angle the load acting on the centre of the thrust block and the relationship between its geometric values such as the depth and length, while the width has been assumed constant since 2-D planar analyses were carried out.

 

It has also been found that the length of the thrust block bears more influence than its depth on the maximum forces generated and thus should be considered first when designing a thrust block. This is due to the rotational movement the thrust block was experiencing and therefore could explain why a larger base area would potentially counter greater forces.

 

2016 © Mohamad Abood, all rights reserved.

LinkedIn     GrabCAD     Contact