Prediction of Punching Strength of Reinforced Concrete Footings by Finite Element Method

Tables index

Veiw figure View Table

View next table

Hegger et. al. (2006) ^[6] tested five 900×900 mm reinforced concrete footings (DF1 to DF5) with realistic boundary conditions and designed to fail in punching. Full details of the tested footings are given in Table 2. The square column stubs were cast monolithically at the center of the slabs. The footings DF4 and DF5 were designed to investigate the effect of small shear slenderness (a/d) on the punching behavior. Although specimen DF3 had shear reinforcement, but this is out of the scope of this work and it will be discarded.

Table 2. Experimental data of previous column-footing experiments

Download as

Tables index

Veiw figure View Table

View previous table

View next table

The specimens were tested in a sandbox and their dimensions were chosen to fit into it. They developed a design model for the punching strength of footings taking into consideration the soil-structure interaction. The work results showed that the failure angle is steeper than observed in punching tests on flat slabs, and the shear slenderness considerably affects the punching shear capacity. Furthermore, the sand density does not affect the distribution of stresses below the footing, i.e. considering a uniform stress distribution gives sufficient safety against punching. The derived model was based on BS8110-1:1997 ^[2] provisions.

Few years later and in order to supplement their previous work, Hegger et. al. (2009) ^[7] completed their works ^[4] and tested additional 17 reinforced concrete footings (DF6 to DF22) to study the punching shear behavior. Several (a/d) and concrete compressive strength were taken. The tests were divided into two series, (DF6 to DF10) were realistically supported on sand. The second one (DF11 to DF22) were inverted upside down so that it supported on the column stub and a load applied on footing via 16 Polytetrafluoroethylene (PTFE) bearings connected to steel beams to simulate the case of uniformly distribution.

The experimental investigations proved the previous conclusion that the angle of the shear crack was steeper in specimens on compact footings than observed in tests on more slender slabs. Furthermore, the (a/d) significantly affects the punching shear capacity since more loads will be distributed out of the punching failure cone. Based on the test results, the ACI and Eurocode-2 provisions were reviewed and improvements were proposed. The experimental program and its implementation are described in Table 2.

The schematic of the experimental setup of Folić et. al. (2013) ^[4] consisting of a test frame, six test specimens, hydraulic jack, and prepared sub-grade. The frame is placed at the bottom of the footing pit measuring 4×5 m in plan with 3m depth. Gravel layers are compacted by vibrator at the bottom of testing steel frame. The gravel layers and the sub-soil compacted so that the modulus of compressibility was chosen to be about 40 to 70 MPa, which represent the normal compaction of the subsoil.

The adopted footing dimensions were 850×850 mm in plan, and they correspond to experiments made by Hegger et al. (2006) ^[6] for the sake of result comparison possibilities, and also to be within the capacity of the available test equipment (approximately 1000 kN). Foundations TIII and TVIII did not fail since their punching capacity was higher than the capacity of the testing machine. The dimensions and characteristics of the footing are given in Table 2.

They concluded that the punching strength is mostly related to the floor structures, and less to the footings under columns. The results obtained were compared with the predicted results based on various codes/regulations and showed that the punching shear capacity values based on these codes are significantly underestimated.

3. The Finite Element Model

All material models used for simulate the material properties of the specimens to the computer program are given in this section. ANSYS 15 finite element program is used for analysis, and the material properties of concrete, reinforcement, soil, and pads are defined to feed the software to complete footing modeling.

3.1. Concrete

The eight nodded solid element, SOLID65, is used for the 3D modeling of solids with and without reinforcing bars since it has rebar capability for modeling reinforcement and its behavior. The element is able to crack in tension and crush in compression in three orthogonal directions, and capable of plastic deformation. The geometry and other specifications for this element are specified in the software technical specification. Three types of cracking in SOLID65 are possible which are labeled ‘first’, ‘second’ and ‘third’ according to their occurrence order and can be visualized based on these labels. The element features are not including calculating the crack width, so cracks existence does not mean that these cracks are visible. In this study, crack profiles with ‘second’ cracks are more consistent with the experimental cracks than the ‘first’ and ‘third’.

3.2. Reinforcement

The rebars used in this work are smeared within the SOLID65 elements, and then the reinforcement defined using the real constants of SOLID65 element. This method needs more efforts in modeling than discrete it with the LINK8 element. The required steel properties to feel the software include density, modulus of elasticity, and Poisson’s ratio and they are shown in Table 2 and Table 3.

Table 3. Material properties for ANSYS model

Download as

Tables index

Veiw figure View Table

View previous table

View next table

3.3. Modeling of Bearings Pad

SOLID65 is also used to represent the PTFE bearing pads. They were modeled as a linear isotropic material with properties as shown in Table 3.

3.4. Modeling of Soil

The soil was modeled as an isotropic material with the basis of the Drucker–Prager’s elastic-perfectly plastic material criteria. The models were developed using 3D SOLID65 Element. In order to use this material model, it is necessary to define the cohesion (C), and angle of internal friction (φ) which are given in the original references, with modulus of elasticity and Poisson’s ratio. For sand or gravel soils (i.e. cohesion C = 0), implies that the material does not have any uniaxial compressive or tensile strength. The material, therefore, has to be iterated into a stable position. This leads to convergence difficulties, so it is advised to use an adequately small value instead of zero for the cohesion while using the Mohr-Coulomb (LAW = 1) yield conditions [ANSYS, 2015].

3.5. Modeling Interaction Contact

In ANSYS, several possible ways to represent the interaction contacts are possible. In this research Node-to-Surface model is used to represent the contact between footing and pads/soil elements. CONTA175 element is used here, which has a great ability to simulate large sliding and deformation. Contact occurs when the element surface penetrates one of the target segment elements (TARGE170) on a specified target surface. The nonlinear contact elements CONTA175 were added to the surface of the footing, while TARGE170 elements were added to the bearing pad and soil surfaces. [ANSYS, 2015].

3.6. Boundary Conditions

Although the model was symmetric, the whole models were simulated. The nodes of the bearing pads in the lowest plane were constrained in all degrees of freedom (DOF); the left and right planes were left free without any constraints, so that it could move in all directions. For the case of soil, all nodes located on all lateral faces of soil block were released in vertical direction while in other direction were constrained. Nodes located on bottom face of soil block were constrained in all directions. See Figure 1.

Download as

Veiw figureFigures index

NEW
View larger figure in new window

Figure 1. ANSYS Loads and boundary conditions

3.7. Loads and Load Stepping

In this work, the total applied load was divided into a series of load steps (increments). The ANSYS software controls the size of these steps whether maximum or minimum load step size is required according to the previous solution history and the convergence behavior whether it is smooth or abrupt. The total numerical applied load was that from the experiment increased by 10%.

4. Discussions of Results

The aims of this study were to show:

(1) To check the applicability of ANSYS software for analyzing and predicting the crack patterns and failure loads of RC footings;

(2) To show the entire phases of the FE model behavior from initial cracking until failure.

4.1. Load Deflection Curves

A number of experimental deflection curves carried out by Hegger et. al. (2009) ^[7] with the corresponding ANSYS load-deflection curves obtained for the footings are illustrated in Figure 2. The curves, in general, showed a good agreement in FE analysis with the test results. It’s been noticed that deflection by the ANSYS is slightly stiffer than the actual footings because full bond between concrete and reinforcement is assumed (no slip) in the finite element analyses, but for the actual footings slip occurs anyway.

Download as

Veiw figureFigures index

Figure 2. Load-deflection curves obtained for the footings; (a) Original test, (b) Deflection by FE (ANSYS)

4.2. Failure Load

Results showed that the failure load obtained from the FE analysis is slightly smaller (conservative) than the experimental load. The final loads for the finite element models are the last applied load step before the solution diverges due to numerous cracks and large deflections, see Figure 3, (i.e. as example, by comparing Figure 3 with Figure 2(b) above, the deflection is increased dramatically in one load step!).

Download as

Veiw figureFigures index

Figure 3. Large deflection when reaching the ultimate load

Table 4 shows comparison between the ultimate loads of the experimental footings and the final loads from the FE models.

Table 4. Comparison of ultimate normal force in column

Download as

Tables index

Veiw figure View Table

View previous table

4.3. Cracks Pattern

The ANSYS program save the cracks pattern for each load step, displaying circles at cracks locations or crushing in the concrete elements. Cracking is displayed as a small circle in the crack plane, while crushing is shown as an octahedron outline. The ‘first’ crack at integration point is shown with a red circle outline, the ‘second’ crack with a green outline, and the ‘third’ crack with a blue outline [ANSYS, Inc 2015].

Figure 4 shows crack patterns progressing developed for some models at the last loading step. It is clear that, in general, the generated cracks have almost the same crack shape and angle corresponding to the experimental specimens at failure stage.

Download as

Veiw figureFigures index

Figure 4. Crack patterns for some models with the corresponding real test

4.3.1. Deflection and Stress Comparison at First Cracking

The cracking patterns in the footings can be obtained using the Crack/Crushing plot option in ANSYS. Vector Mode plots must be turned on to view the cracking in the model. The initial cracking of the footing DF12 (as example) in the FE model corresponds to a load of 800 kN (which is represent about 34% of the ultimate punching capacity of footing) and induces stress beyond the modulus of rupture of concrete (3.14 MPa) as shown in Table 2.

The stress increases up to 3.24 MPa at the centerline when the first crack occurs. The first crack can be seen in Figure 5, which is a flexural crack with maximum deflection of 0.356 mm.

Download as

Veiw figureFigures index

Figure 5. First concrete crack at 800 kN for DF12

4.3.2. Behavior after First Crack

In the non-linear region of the response, subsequent cracking occurs as more loads are applied. Cracking increases in the region, and the footing starts cracking out at a load of 1,150 kN. Significant flexural cracking occurs in the footing at 1,500 kN. Also, diagonal tension cracks are starting to appear in the model. This cracking can be seen in Figure 6 and Figure 7.

Download as

Veiw figureFigures index

Figure 6. Cracking at 1,150 kN for DF12

Download as

Veiw figureFigures index

Figure 7. Increased cracking after yielding of reinforcement at 1,500 kN for DF12

4.3.3. Reinforcement Yielding and Beyond It

Yielding of steel reinforcement occurs when a force of 1,500 kN is applied, see Figure 7. At this point in the response, the displacements of the footing begin to increase at a higher rate as more loads are applied. The cracked moment of inertia, yielding steel and nonlinear concrete material, now defines the flexural rigidity of the member. Larger deflections occur at the center and the ability of the footing to distribute load throughout the cross section decreased greatly.

Figure 8 shows successive cracking of the concrete footing after yielding of the steel occurs. At 2,200 kN, the footing has increasing flexural cracks, and diagonal tension (shear) cracks. Cracking reached the top face, failure is soon to follow.

Download as

Veiw figureFigures index

Figure 8. Failure of the concrete footing at 2,200 kN for DF12

At load of about 2,300 kN, the footing can no longer support additional load. Severe cracking throughout the bottom face region occurs.

5. Use of Codes of Practice in Predicting the Failure Loads

Generally, codes do not differentiate between punching shear strength of flat plates and footings, but it allows subtracting a part of the soil reaction from the punching load. However, this amount differs from one code to another according to the critical path location. In this study, no reaction is subtracted since this area, in some codes, are bigger than the footing itself.

According to the design code, the ultimate shear is:

where:

: Shear stress at punching of the control section,

: Perimeter of the control section according to adopted regulations, see Figure 9.

d: Effective depth of footing.

Describing the detailed procedure and recommendations of these codes are not within the scope of this paper.

The ultimate axial force shown in Table 4 was calculated for the purpose of comparison, and it was assumed that the safety reduction factors equal to one.

5.1. ACI 318-14 Code

The ACI code ^[7] takes the critical section at (0.5 d) from the column face and its shape similar to the column shape. The concrete punching shear capacity in the control section is calculated according to the equations (a), (b) and (c) listed in Table 22.6.5.2 of the ACI code.

5.2. BS 8110-1:1997 Code

This code takes the critical section at a distance of (1.5 d) from the column face and its shape also similar to the column shape. In this work, the partial safety factor taken is γm = 1.25.

5.3. Eurocode 2 [3] Code

The punching shear capacity around the column is checked on two places, along the column perimeter and in the basic control section at the distance of (2.0 d) from the face of the column. The material resistance factor for concrete taken is γ_c = 1.5, σ_cp= 1.5, and β=1.15.

Download as

Veiw figureFigures index