Calculation models for evaluating the behavior of Emmedue floors

European Centre for Training and Research in
Earthquake Engineering - EUCENTRE
Calculation models for evaluating the
behavior of Emmedue floors
1
Index
1.
Purpose of the research and work setup ............................................................................... ...3
2.
Description of the EMMEDUE floor system ............................................................................. .3
2.1
3.
Definition and design of the case studies ........................................................................ .4
Evaluation of the deformability: Finished elements model ... .......................................................5
3.1
Results of the analyses and comparison with the experimental data ... .......................... .10
3.2
Extrapolation of the data and new cases ... .................................................................. ..17
4.
Simplified model for calculating the maximum height ... ........................................................ ..22
5.
Tensional approach and simplified method for calculating the resistant capacity ............... ...27
2
1. Purpose of the research and work setup
The objective of this research is to determine a simplified calculation method for the design or
evaluation of the behavior of EMMEDUE floors, given the generic load condition and based on
characteristics of the floors themselves.
This simplified method shall be based on the same mathematical instruments used with the linear
approach; nonlinear behavior shall be evaluated through the use of corrective coefficients for the
rigidity or for the concrete-polystyrene adhesion, which will be properly calibrated using the results of
the experimental testing, described in a previous report.
Two different approaches were considered in order to respectively assess the maximum height and
the resistant capacity. More specifically, the following approaches were used:
1. an approach based on the displacements with which, by means of an extremely detailed
modeling with finished elements, the deformation behavior of the system ceiling was
determined. The results from the experimental tests performed on the floors were also used for
the purpose of comparing the numerical results and, consequently, for calibrating the
magnitudes employed in the numeric model. In practice a predictor-corrector method was used,
the principal goal of which was to identify the numerical parameters for the experimental data
and thus to arrive at a solution that could be further employed for generating new cases, in
addition to the experimental ones (which by definition are limited).
2. a tensional approach based on the efforts by which, through an analysis of the section, the
actual resistant capacity was deduced, taking into account the cooperation of the polystyrene
layer. The simplified model thus defined was justified by a preliminary analysis of the floor by
means of a finished element modeling, which was aimed at assessing the actual distribution of
stresses along the width of the section.
2. Description of the EMMEDUE floor system
EMMEDUE panels consist of two steel wire nets in welded galvanized steel, placed adjacent to the
faces of a central wave-shaped polystyrene foam slab.
The density of the polystyrene slabs of the floors examined in this report varied between either 15 or 25
kg/m3, while its relative thickness was of 80 or 160 mm.
The nets consist of wire mesh grids with a pitch of 70 mm, made respectively with 3.5 mm and 2.5 mm
diameter wire, in the longitudinal and transversal directions of the floor.
The two nets are united with double metallic connectors (•3 mm) which overlap the bonds at
distribution of approximately 72 per m2.
The panels have a width which is based upon 112.5 cm modules and a length that is varies based on
the technical and design requirements.
The steel used for these nets is drawn with hot-dip galvanizing. The resistance to tensile stress yield
characteristic is greater than 600 MPa, while the rupture characteristic is greater than 680 MPa
(EMMEDUE data sheets). Figure 1 (a) shows a diagram of a standard module for the floor in question
(www.mdue.it).
The basic components of the EMMEDUE panel which will be modeled during the schematization
phase with finished elements are specifically the following (Figure 1 (b)):
1. Polystyrene foam slab;
2. welded steel wire drawn and galvanized mesh positioned both sides of the polystyrene slab and
connected to it with steel connectors with the same characteristics of the mesh itself;
3
3. panel finished with shot concrete (lower surface), or screed coating (upper surface).
(a) Standard floor module diagram
(b) cross-section detail
Figure 1 Geometrical characteristics of the floor (Emmedue data sheet)
Definition and design of the case studies
Table 1 Characteristics of the laboratory-tested floors
Test
No.
1
2
3
4
1
2
3
4
5
6
7
8
Floor
Dimensions
(m.)
2.25 x 4.0
2.25 x 4.0
2.25 x 4.0
2.25 x 4.0
2.25 x 5.0
2.25 x 5.0
2.25 x 5.0
2.25 x 5.0
Polystyrene
thickness
(cm.)
8
8
8
8
16
16
16
16
Upper
floor
Lower
floor
Polystyrene
density
(cm.)
5.5
5.5
5.5
5.5
5.5
5.5
5.5
5.5
(cm.)
3.5
3.5
3.5
3.5
3.5
3.5
3.5
3.5
(kg/m3)
15
15
25
25
15
15
25
25
4
Various configurations previously tested in the laboratory were studied: All of the manufactured
models listed below refer to a 2250 mm wide reinforced concrete floor, with a total thickness of 170 mm
or 250 mm and a length of 4000 mm or 5000 mm. Table 1 shows the cases experimentally analyzed in
the laboratory which were subsequently modeled with finished elements in order to reproduce the
behavior and to calibrate the parameters of the floor system.
3. Evaluation of the deformability: Finished elements model
The evaluation of the behavior of the floor system, which, as described previously, is made up of three
different elements, consists in determining the interaction between various layers (slabs of cement or
concrete, steel mesh and polystyrene). To achieve this purpose, it was decided to create a detailed
three-dimensional model: the finished element program Ansys (ANSYS Engineering Analysis
System, 2002) was selected for this purpose.
Thanks to the use of Ansys, which renders available a wide range of elements together with a highly
developed graphical user interface, several models were able to be created before reaching the final
solution.
1. in the first model (Figure 2) it was decided to divide the short side (2.25 m as shown in Table 1)
into 8 elements and the long side into 14 elements (4 m as shown in Table 1), while the
thickness, made up of the two slabs as well as the polystyrene, was subdivided into several
layers. In particular, it was decided to model the layer of polystyrene using a three-element
configuration along the thickness. The analyses showed an extremely rigid behavior in this
model compared to the results obtained from the laboratory tests. This may be caused by the
presence of finished elements, as shown in Figure 2, where the Jacobian of the transformation
employed in the rigidity matrix is negatively influenced numerically; in practice, the elements
are very far from an ideal cubic geometric configuration and are quite "stretched" in the
horizontal plane, resulting a situation which, in a geometric non-linear field, can often lead to
analytical problems (since the additions are made Gaussian points of the thickness which are
therefore even more closely spaced than the element’s bonds);
Figure 2 Floor with a span of 4m: before modeling performed with Ansys
2. the next step, starting with the same geometry for the 4m floor described in the previous
paragraph, was to build a model with a much denser mesh in the plane and much more
widespread in thickness. In detail (as shown in Figure 3), 22 elements were employed along the
sort side (2.25
5
m) and 40 elements were employed in the long side of the floor (4m); a single layer for modeling
the polystyrene thickness (0.08 m) was also introduced. In practice, following the usual
recommendations for the creation of an efficient mesh for use in non-linear approaches, solid
"brick" elements were realized, which were as similar as possible to a cubic geometric
configuration. Since, at the end of the analyses, and following the comparisons with the results
of the experiments, this model was deemed to be that which best interpreted the experimental
results, this model was selected as the most reliable in order to extrapolate a greater number of
cases to be studied.
Once the calibration of the geometric mesh was performed, we proceeded to describe in detail the
characteristics of finished elements employed within the Ansys code. For the modeling of the
polystyrene, only a single layer of three-dimensional solid "brick" elements with 8 bonds for the 4 m
floors was utilized; while, still keeping with the "optimal design" philosophy in order to obtain
geometrically uniform elements, three layers were utilized for 5 m floors (in order to always obtain
elements of equal dimensions as shown in Figure 4). In addition, for the 5 m floors (Figure 4), 22
elements were always utilized along the short side (2.25 m), while 50 elements were used in the long
side of the floor (5 m).
Figure 3 Floor with a span of 4m: according to modeling performed with Ansys
Figure 4 Floor with a span of 5 m: according to modeling performed with Ansys
The layers of concrete, below and above the polystyrene, were divided into two elements along the
thickness, one representing the reinforcement of the layer (the part closest to the polystyrene to ensure
adherence) and one representing the non-reinforced part of the layer (the outer surface). For both layers,
solid three-dimensional "brick" elements called SOLID65 were utilized (Figure 5).
6
These are 8 bond elements, defined and developed specifically for modeling the nonlinear behavior of
reinforced concrete, into which a reinforcement may be inserted, distributed along the three main
directions as shown in Figure 5. In the developed model, within the concrete elements, the
reinforcement has been arranged in both the longitudinal and transverse directions, as shown in the
actual design of the floor elements (Figure 1 (a)). In the numerical model, this allowed for the exact
determination of the effect of inserting the actual arrangement and the actual amount of reinforcement.
In the wall configuration studied, the layers adjacent to the polystyrene were reinforced respectively
with • 3.5 / 70 mm and • 2.5 / 70 mm reinforcement rods, in the longitudinal and transverse directions.
Figure 5 Typical SOLID65 element employed in the finished element model (Ansys manual)
With regards to the constitutive equations of the materials (concrete and steel) used within the finished
element model, the following parameters, derived from characterization tests performed in the
laboratory, were defined and utilized.
-
Shot concrete as shown in Figure 6 (lower floor)
Coefficient of elasticity:
E = 28380 MPa
Poisson’s coefficient:
• = 0.2
Compression resistance:
•c = 23 MPa
Tensile stress resistance:
•t = 1.5 MPa
Deformation corresponding to the maximum compression stress:
•c0 = 0.2 %
Ultimate deformation:
•u = 0.6 %
-
Cast cement (upper floor):
Coefficient of elasticity:
E = 32000 MPa
Poisson’s coefficient:
• = 0.2
Compression resistance:
•c = 33 MPa
Tensile stress resistance:
•t = 1.5 MPa
Deformation corresponding to the maximum compression stress:
•c0 = 0.2 %
Ultimate deformation:
•u = 0.6 %
7
35
30
25
20
15
10
5
0
0
0.001
0.002
0.003
0.004
0.005
0.006
deformation
Figure 6 Stress-deflection relationship utilized in the model to simulate the concrete.
-
Steel (as shown in Figure 7):
•c = 750 MPa
•t = 850 MPa
•y = 0.2 %
•u = 12 %
Tensile stress yield resistance:
Tensile stress ultimate resistance:
Yield deformation:
Ultimate deformation:
900
800
700
600
500
400
300
200
100
0
0
0.02
0.04
0.06
0.08
0.1
0.12
0.14
deformation
Figure 7 Stress-deflection relationship utilized in the model to simulate the steel.
Regarding the definition of the polystyrene characteristics, however, reference was made to the
experimental indications given in AIPE volume ( "Isolate the foundations with EPS”, 2004), as shown in
the following Table 2.
It must be noted, however, that the above indications served as an initial approach for the assessment
of the deformation capacity of the floors. The definitive values of the polystyrene‘s mechanical
characteristics, shown below, are derived from an iterative procedure with which the analytical experimental equality was set up in terms of force-displacement law.
8
Table 2 Mechanical characteristics of the sintered polystyrene foam (from AICAP, 2004)
-
High density polystyrene (HD in Figure 8):
E = 5 MPa
• = 0.4
•c = 0.20 MPa
•t = 0.32 MPa
Coefficient of elasticity:
Poisson’s coefficient:
Compression resistance:
Tensile stress resistance:
Deformation corresponding to the
maximum compression stress:
•c0 = 15 %
- Low density polystyrene (LD in Figure 8):
Coefficient of elasticity:
Poisson’s coefficient:
Compression resistance:
Tensile stress resistance:
Deformation corresponding to the
maximum compression stress:
E = 2 MPa
• = 0.4
•c = 0.12 MPa
•t = 0.15 MPa
•c0 = 15 %
deformation
Figure 8 stress – deformation relationship utilized to simulate
the compression behavior of the polystyrene.
9
Results of the analyses and comparison with the experimental data
The finished element model previously described was subjected to static, non-linear analyses
("pushover" type) for displacement control, which were capable of reproducing the test system
employed in the experimental research.
Hereafter, in the figures below, are shown the force-displacement curves obtained with the finished
element model created with Ansys (green-colored curves). These curves are compared with the results
obtained from the experimental testing which was performed upon the floors: In particular, the
experimental curves corresponding to the potentiometers positioned at the center are displayed. The
force values correspond to the total vertical reaction at the base of the floor and the displacement
represents the maximum height.
The descriptions of the diagrams shown follow:
- Figure 9 and Figure 10 represent the numerical - experimental overlap of the
force-displacement curves for the 4 m floor by with low density polystyrene;
- Figure 11 and Figure 12 represent the numerical - experimental overlap of the
force-displacement curves for the 4 m floor by with high density polystyrene;
- Figure 13 and Figure 14 represent the numerical - experimental overlap of the
force-displacement curves for the 5 m floor by with low density polystyrene;
- Figure 15 and Figure 16 represent the numerical - experimental overlap of the
force-displacement curves for the 5 m floor by with high density polystyrene;
The excellent correlation between the data obtained from the experiments and the numerical
predictions, both in terms of displacement development over the “fake” time test, as well as in terms of
maximum force reached, allows for the reliable definition of the non-linear finished element model (both
in terms of geometry and in terms of materials) constructed with Ansys. This model is capable imitating,
with an optimal approximation, the development of the highly nonlinear behavior of the floor, even
considering the large discontinuity in the thickness of the material’s parameters that exists in transition
from reinforced concrete to polystyrene.
With this model, it is therefore possible to extrapolate new data in order to increase the database of
available tests, since experimental testing, as such, is always limited to a reduced number of samples
to be tested.
10
FLOOR NO.1
FORCE _DISPLACEMENT
4
3.5
3
2.5
CH5
CH5-2
Ansys
2
1.5
1
0.5
0
0
10
20
30
40
50
60
mm
Figure 9 Force-displacement curve for the low-density 4m floor (test sample no.1)
FLOOR NO.2
FORCE _DISPLACEMENT
4
3.5
3
2.5
CH4
CH4-2
Ansys
2
1.5
1
0.5
0
0
10
20
30
40
50
60
mm
Figure 10 Force-displacement curve for the low-density 4m floor (test sample no.2)
11
FLOOR NO.3
FORCE _DISPLACEMENT
7
6
5
4
CH4
CH4-2
Ansys
3
2
1
0
0
10
20
30
40
50
60
70
80
mm
Figure 11 Force-displacement curve for the high-density 4m floor (test sample no.3)
FLOOR NO.4
FORCE _DISPLACEMENT
7
6
5
4
CH5
CH5-2
Ansys
3
2
1
0
0
10
20
30
40
mm
50
60
70
80
Figure 12 Force-displacement curve for the high-density 4m floor (test sample no.4)
12
FLOOR NO.5
FORCE _DISPLACEMENT
7
6
5
4
CH4
CH4-2
CH4-3
3
Ansys
2
1
0
0
10
20
30
40
50
60
70
80
90
mm
Figure 13 Force-displacement curve for the low-density 5 m floor (test sample no.5)
FLOOR NO.6
FORCE _DISPLACEMENT
7
6
5
4
CH5
CH5-2
Ansys
3
2
1
0
0
10
20
30
40
50
60
70
80
90
mm
Figure 14 Force-displacement curve for the low-density 5 m floor (test sample no.6)
13
FLOOR NO.7
FORCE _DISPLACEMENT
7
6
5
4
CH4
CH4-2
Ansys
3
2
1
0
0
10
20
30
40
50
60
70
80
90
100
mm
Figure 15 Force-displacement curve for the high-density 5 m floor (test sample no.7)
FLOOR NO.8
FORCE _DISPLACEMENT
7
6
5
4
CH5
CH5-2
Ansys
3
2
1
0
0
10
20
30
40
50
mm
60
70
80
90
100
Figure 16 Force-displacement curve for the high-density 5 m floor (test sample no.8)
Given the force-displacement curves obtained from experimental tests described above, there are
fixed points of reference to be used for the extrapolation of the results required for comparison
14
with the numerical analyses performed with Ansys. Table 3 shows two points: The first refers to the
point of maximum force extrapolated from the experimental graphs (the blue point in the previous
figures 9 through 16), shown in Table 4; the second point (red) represents the maximum displacement
recorded during the test, once the maximum was surpassed.
It must be noted that, while the first point (point of maximum force) is uniquely defined, the second point
(maximum displacement) depends on the test procedure and does not constitute an effective
comparison value. For this reason, the numerical – experimental comparison is based on the values
given by the first point.
Another important consideration has to do with the fact that in the case of the floors of 5 m in length, the
results obtained have a low sensitivity to the density characteristics assigned to the polystyrene.
Table 3 Characteristics in terms of the behavior of the laboratory-tested floors
2
3
4
Experimental results
Maximum point
Ultimate conditions
Floor
Dimensions
Max.
Displ.
Max.
Force
Max.
Moment
Max.
Displ.
Max.
Force
Max.
Moment
(m.)
(mm.)
(ton.)
(kNm)
(mm.)
(ton.)
(kNm)
1
2.25 x 4.0
40.17
3.45
19.80
44.6
3.38
19.40
2
2.25 x 4.0
40.3
3.3
18.94
58.4
3.5
20.09
3
2.25 x 4.0
51.5
5.5
31.56
51.5
5.5
31.56
4
2.25 x 4.0
75.8
5.7
32.71
75.8
5.7
32.71
5
2.25 x 5.0
50.4
5
28.69
81.1
4.7
26.97
6
2.25 x 5.0
74.2
5.6
32.14
74.2
5.6
32.14
7
2.25 x 5.0
91.7
6
34.43
91.7
6
34.43
8
2.25 x 5.0
80.6
6
34.43
80.6
6
34.43
Test
No.
1
Experimental results
Therefore, based on that which is shown above, once the maximum values of displacement, force and
moment have been determined from the numerical force-displacement curves obtained by Ansys, and
shown in Table 4 together with the experimental values corresponding to the maximum point, the
percentage difference between the force and displacement value was estimated (Table 4).
15
Table 4 Comparison of the numerical results (Ansys model) with the experimental ones.
Experimental data
Analytical results
Max.
Displ.
Max.
Force
Max.
Moment
Max.
Displ.
Max.
Force
Max.
Moment
(mm.)
(ton.)
(kNm)
(mm.)
(ton.)
(kNm)
1
40.17
3.45
19.80
2
40.3
3.3
18.94
42.68
3.30
18.93
3
51.5
5.5
31.56
4
75.8
5.7
32.71
5
50.4
5
28.69
6
74.2
5.6
32.14
7
91.7
6
34.43
8
80.6
6
34.43
Test
No.
65.91
77.80
77.80
5.43
5.95
5.95
31.14
43.77
43.77
% displ.
difference
% force
difference
-6.25%
4.35%
-5.91%
0.00%
-27.98%
1.27%
13.05%
4.74%
-54.37%
-19.00%
-4.85%
-6.25%
15.16%
0.83%
3.47%
0.83%
The results of Table 4 have been plotted in the graph in Figure 17. With the exception of test sample 5,
which is a special case, one can observe how the force percentage difference is always less than 5%,
and therefore very low. The displacement percentage difference is greater, as expected, due to the
complexity of the numerical model described above and the uncertainties inherent to any numerical
method.
Test sample no. 5 is a special case, because, despite the difference of about 20% in the maximum
numerical and experimental force and the corresponding difference in displacement of about 50%, the
numerical curve, in fact, still passes through the experimental maximum point.
In any case, even taking into consideration the results of test sample no. 5, the average differences in
force and displacement are respectively lower than 2% and 9%. These values are reduced to 1% and
2% if test sample no. 5 is not taken into account.
20%
Average error
[%] in force
10%
0%
-10%
-20%
Average error
[%] in
-30%
displacement
-40%
% displacement difference
-50%
% force difference
-60%
Floor 1
Floor 2
Floor 3 Floor 4
Floor 5
Floor 6
Floor 7
Floor 8
Figure 17 Percentage difference between the numerical and experimental results
16
3.2 Extrapolation of the data and new cases
The comparisons with the 8 experimental tests (Table 1) were initially necessary to calibrate and
subsequently to validate the numerical finished element model created with Ansys. In order to expand
the number of case studies, since experimental testing is, by its nature, limited to a small number of
cases, it was decided to study ulterior load combinations in addition to the standard combination utilized
in the tests. In these additional load cases, it was decided to maintain the geometry of the floor
unchanged (both in plane as well as in thickness) in order to achieve an ample congruence with that
which, up until this point, has been elaborated in the preceding paragraphs (validation of a numerical
model relative to 8 experimental tests on the same number of floors).
The case studies analyzed and utilized in the extrapolation are shown below:
-
Floor of 4 m in length:
[1] initial scheme employed in the experimental tests (a = 1170 mm)
[2] load positioned at the center of the slab (a = b = 1750 mm):
[3] load positioned at the distance of (¼ of the length of the long side) measured starting
from the edge of the short side:
[4] evenly distributed load:
17
-
Floor of 5 m in length:
[1] initial scheme employed in the experimental tests:
[2] load positioned at the center of the slab:
[3] load positioned at the distance of (¼ of the length of the long side) measured starting
from the edge of the short side:
[4] evenly distributed load:
Once the new load cases had been defined, the next step was to conduct further analysis with Ansys,
in order to increase the output number of cases studied and, consequently, the number of
force-displacement curves. Below are shown, for each type of floor and for each static diagram, the
numerical force-displacement curves calculated for each of the load schemes described above.
18
6
5
4
3
Floor 1
2
1
0
0
10
20
30
40
50
mm
Figure 18 Floor of 4 m in length, low density polystyrene, case [2] central load.
6
5
4
3
Floor 1
2
1
0
0
5
10
15
20
25
mm
Figure 19 Floor of 4 m in length, low density polystyrene, case [3] load at ¼.
6
5
4
Floor 1
3
2
1
0
0
10
20
30
40
50
60
mm
Figure 20 Floor of 4 m in length, low density polystyrene, case [4]
evenly distributed load.
19
8
7
6
5
4
Floor 2
3
2
1
0
0
10
20
30
40
50
60
70
mm
Figure 21 Floor of 4 m in length, high density polystyrene, case [2] central load.
8
7
6
5
4
Floor 2
3
2
1
0
0
10
20
30
40
50
60
70
mm
Figure 22 Floor of 4 m in length, high density polystyrene, case [3] load at ¼.
8
7
6
5
4
3
2
1
0
floor 2
0
10
20
30
40
50
60
70
80
mm
Figure 23 Floor of 4 m in length, high density polystyrene, case [4]
evenly distributed load.
20
7
6
5
4
Floor 4
3
2
1
0
0
20
40
60
80
mm
Figure 24 Floor of 5 m in length, high and low density polystyrene, case [2] central load.
7
6
5
4
Floor 4
3
2
1
0
0
20
40
60
80
mm
Figure 25 Floor of 5 m in length, high and low density polystyrene, case [3] load at ¼.
8
7
6
5
Floor 4
4
3
2
1
0
0
20
40
60
80
mm
Figure 26 Floor of 5 m in length, high and low density polystyrene, case [4]
evenly distributed load.
21
4. Simplified model for calculating the maximum height
Using the data obtained so far, both experimentally and numerically, the objective was to derive a
simplified formula for the calculation of the height of the floors through the traditional formulas used for
the inflexible beams.
A reductive coefficient of the term EJ is appropriately included in these formulas (related to the
stiffness of an inflexible beam and calibrated according to the results obtained from the finished
element model). This coefficient takes into account the status of the section (integral or cracked) and
the presence of the layer of polystyrene, with pre-established characteristics, along the thickness.
Given the results of the analyses using the finished element program, Ansys, the maximum
displacement values obtained (s in mm) are listed in Table 5. The theoretical height (f) was
subsequently calculated for each floor and for each static scheme so as to determine the reductive
coefficient (c) of the section’s rigidity, such that s = f / c.
Table 5 Reduction coefficients (c) of the rigidity for the calibration of the model
Type of
Load
2 symm. forces
1
2
3
4
s
mm
F
ton
M
kNm
Esup
2
N/mm
Jsup
4
mm
Einf
2
N/mm
Jinf
4
mm
EJcls
2
Nmm
Esteel
2
N/mm
Jsup
4
mm
Jsinf
4
mm
EJsteel
2
Nmm
EJtot
2
Nmm
42.7
3.3
18.93
32009 5.64E +0 8
2.84E +04 2.60 E+ 08 2.54E + 13 2.10E +0 5
5.10E +04 5.75 E+ 04 2.28E + 10 2.55E +1 3
centralized forces
38.5
2.61
22.38
32009 5.64E +0 8
2.84E +04 2.60 E+ 08 2.54E + 13 2.10E +0 5
5.10E +04 5.75 E+ 04 2.28E + 10 2.55E +1 3
1 /4 forces
20.7
3.36
21.65
32009 5.64E +0 8
Distributed
54.8
5.69
24.41
32009 5.64E +0 8
2.84E +04 2.60 E+ 08 2.54E + 13 2.10E +0 5
2.84E +04 2.60 E+ 08 2.54E + 13 2.10E +0 5
5.10E +04 5.75 E+ 04 2.28E + 10 2.55E +1 3
5.10E +04 5.75 E+ 04 2.28E + 10 2.55E +1 3
2 symm. forces
65.9
48.3
5.43
3.88
31.14
32.15
32009 5.64E +0 8
32009 5.64E +0 8
2.84E +04 2.60 E+ 08 2.54E + 13 2.10E +0 5
5.10E +04 5.75 E+ 04 2.28E + 10 2.55E +1 3
Centralized forces
1/4 forces
22.4
4.44
36.74
32009 5.64E +0 8
2.84E +04 2.60 E+ 08 2.54E + 13 2.10E +0 5
2.84E +04 2.60 E+ 08 2.54E + 13 2.10E +0 5
5.10E +04 5.75 E+ 04 2.28E + 10 2.55E +1 3
5.10E +04 5.75 E+ 04 2.28E + 10 2.55E +1 3
Distributed
2 symm. forces
70.6
77.8
7.92
5.95
33.98
43.77
32009 5.64E +0 8
32009 1.43E +0 9
2.84E +04 2.60 E+ 08 2.54E + 13 2.10E +0 5
2.84E +04 1.49 E+ 09 8.80E + 13 2.10E +0 5
5.10E +04 5.75 E+ 04 2.28E + 10 2.55E +1 3
9.89E +04 1.12 E+ 05 4.42E + 10 8.81E +1 3
Centralized forces
44.3
3.82
42.11
32009 1.43E +0 9
2.84E +04 1.49 E+ 09 8.80E + 13 2.10E +0 5
9.89E +04 1.12 E+ 05 4.42E + 10 8.81E +1 3
1/4 forces
57.5
64.0
5.38
7.97
44.54
43.98
32009 1.43E +0 9
32009 1.43E +0 9
2.84E +04 1.49 E+ 09 8.80E + 13 2.10E +0 5
2.84E +04 1.49 E+ 09 8.80E + 13 2.10E +0 5
9.89E +04 1.12 E+ 05 4.42E + 10 8.81E +1 3
9.89E +04 1.12 E+ 05 4.42E + 10 8.81E +1 3
Distributed
Type of
Load
1
mm
2 symm. forces
42.7
1.0
0.023
Centralized forces
38.5
0.9
0.023
1/4 Forces
20.7
54.8
0.7
1.2
0.031
0.022
Centralized forces
65.9
48.3
1.6
1.3
0.024
0.028
1/4 Forces
22.4
0.9
0.038
Distributed
70.6
77.8
1.7
1.1
0.024
0.014
1/4 Forces
44.3
57.5
0.8
0.6
0.018
0.011
Distributed
64.0
1.1
0.017
Distributed
2 symm. forces
2
2 symm. forces
3
4
f
s
mm
Centralized forces
c
The individual terms in Table 5 assume the following meanings:
- s is the maximum displacement obtained by the finished element model created with Ansys;
- F is the resultant of the loads applied to the floor for each type of load;
- M is the maximum bending moment which corresponds to the load condition imposed;
- Esup is the elasticity coefficient of the upper layer of cement;
- Jsup is the moment of inertia of the upper layer of cement;
- Einf is the elasticity coefficient of the lower layer of concrete;
- Jinf is the moment of inertia of the lower layer of concrete;
- EJcls is the total value given by the previous contributions (Esup, Jsup, Einf and Jinf) for
the concrete of the floor;
- Esteel is the elasticity coefficient of steel which is the same for the upper and lower layers;
22
-
Jsup is the inertia of the upper layer of steel;
Jinf is the inertia of the lower layer of steel;
EJsteel is the total value given by the previous contributions (Esteel, Jsup, and Jinf) for the steel;
EJtot is the total concrete (EJcls) and steel (Esteel) inertia;
F is the numeric height calculated by means of the formulas below, which are specialized for each
load condition:
Pa(3l 2 • 4a)
24 EJ
Pair of loads:
f =
Centralized and 1/4 load:
f = Pa b
3 EJl
5 pl 4
f=
384 EJ
2
Distributed load:
-
(1)
2
(2)
(3)
c is the reductive coefficient of the rigidity (EJ), such that it is possible to determine the actual height
s = f / c.
Subsequently, the c coefficients for each point obtained from the analyses with Ansys were also
calculated in order to determine the development of the c coefficient itself based on the level of
displacement and the type of load considered.
The tables for these calculations are not given in this report as they would occupy a few pages of
merely numerical data.
The interesting aspect of the results obtained is the following: each numerical force - displacement
curve associated with the different types of loads can be graphed through a tri-linear progression. In
each of the linear tracts, the c coefficients result as being practically independent from the type of load.
This means that in each of these tracts, it is possible to assume an average c coefficient value (Table 6)
to which an essentially null or negligible variation coefficient can be associated.
Table 6 Average c coefficient for the calibration of the model
Average
Up to 10 mm
0.0791
60
Pair of loads
Central load
50
1/4 load
distributed load
from 10 to 20 mm
0.0415
beyond 20 mm
0.0251
40
30
c = 0.0251
20
c = 0.0415
10
c = 0.0791
0
0.0
1.0
2.0
3.0
Load (ton.)
4.0
5.0
6.0
Figure 27 Floor of 4 m in length with low density polystyrene (as shown in Table 5):
c coefficients of rigidity reduction for the different load conditions.
23
Pair of loads
Central load
1/4 load
Distributed load
80
70
60
50
40
c = 0.0251
30
20
c = 0.0415
10
c = 0.0791
0
0.0
1.0
2.0
3.0
4.0
Load (ton.)
5.0
6.0
7.0
8.0
Figure 28 Floor of 4 m in length with high density polystyrene (as shown in Table 5):
c coefficients of rigidity reduction for the different load conditions.
90
Pair of loads
80
Central load
1/4 load
Distributed load
70
60
50
40
c = 0.0251
30
20
c = 0.0415
10
0
c = 0.0791
0.0
1.0
2.0
3.0
4.0
5.0
Load (ton.)
6.0
7.0
8.0
Figure 29 Floor of 5 m in length with low or high density polystyrene (as shown in Table 5):
c coefficients of rigidity reduction for the different load conditions.
In order to render the results obtained (graphed in figures 27 to 29) operational, the following simplified
graphs with a linear tract progression are provided (figures 30 to 32).
It can be seen how each of these diagrams is no other than a force-displacement equation with
inverted axes (this is due to the fact that it was preferred to display the unknown variable on the
ordinate axis).
Each of these diagrams refers to a floor characterized by pre-established span (4 or 5 m), section
typology (cement thickness of 5.5 cm, concrete of 3.5 cm and polystyrene of 8 or 16 cm, of low or high
density) and materials.
24
The value indicated in the abscissa is the resultant of the loads applied for each type of load
associated with each curve, to which an elastic height value, in the ordinate, corresponds for the floor
in question, as well as a reductive coefficient for determining the equivalent rigidity.
In order to better clarify the use of the following diagrams, the following example is made. Suppose
there is a floor with a span of 4 m and a thickness of 17 cm, with 8 cm low density polystyrene, to which
is applied a distributed load whose resultant is equal to 2.5 tons. The graph in figure 30 is therefore
used and the horizontal axis is entered at the value 2.5; the curve associated with the distributed load
(red) is intercepted and the following factors are determined: the actual maximum elastic height s
(equal to about 13 mm) and the coefficient for determining the equivalent rigidity (c = 0.0415).
If the height f were to be analytically calculated through the equation (3), then the value f = 0:54 mm
would be obtained. The actual height would therefore be s = f / c = 0.54 / 0.0415 = 13 mm.
If a finished element model of the floor were to be created, the equivalent beam element should be
characterized by a rigidity EJ reduced by means of the c coefficient in order to be able to properly
determine the actual deformability of the floor itself.
Below are shown the curves for:
- floor 1 (170 mm in length, low density polystyrene) with a span of 4 m (figure 30);.
- floor 2 (170 mm in length, high density polystyrene) with a span of 4 m (figure 31);.
- floors 3 and 4 (250 mm in length, both high and low density polystyrene) with a span of 5m (figure 31);.
60
50
40
30
c = 0.0251
20
c = 0.0415
10
c = 0.0791
0
0.0
1.0
2.0
3.0
Load (ton.)
4.0
5.0
6.0
Figure 30 Tri-linear model for floor 1 with a span of 4 m. as shown in Table 5
for the various load conditions.
25
80
70
60
50
40
30
c = 0.0251
20
c = 0.0415
10
c = 0.0791
0
0.0
1.0
2.0
3.0
4.0
5.0
Load (ton.)
6.0
7.0
8.0
Figure 31 Tri-linear model for floor 2 with a span of 4 m. as shown in Table 5
for the various load conditions.
90
80
70
60
50
40
30
20
c = 0.0251
10
c = 0.0415
c = 0.0791
0
0.0
1.0
2.0
3.0
4.0
Load (ton.)
5.0
6.0
7.0
8.0
Figure 32 Tri-linear model for floors 3 and 4 with spans of 5 m. as shown in Table 5
for the various load conditions.
It should be noted that the height calculated in the field of elasticity in the examples above is the instant
one, or rather, that viscous effects were not counted.
26
5. Tensional approach and simplified method for calculating the
resistant capacity
The resistance of the floor is also determined by means of a simplified formulation in which the
section’s capacity, intended as fully cooperative amongst its individual components, is reduced by
means of an experimentally determined coefficient.
Firstly, in accordance with the scheme of the experimental test, the floor was treated as a beam of
unitary width, whose transverse cross section was made up of an upper layer of cement reinforced
with a •3.5 / 70 x 70 mm wire net, by an intermediate layer of polystyrene and by a lower layer of
concrete, also reinforced by a •3.5 / 70 x 70 mm wire net (Figure 33).
An analysis of the floor was initially performed by modeling “rolled” elements with the Straus7
calculation code. The objective of these analyses was to assess the progression of the normal stress
along the thickness of the floor itself.
As shown in the figure below by the typical "butterfly" trend, the floors are characterized by a level of
collaboration which is not negligible.
Figure 33 Progression of the normal stress along the thickness of the inflexible floor evaluated in various
centered ordinates at the center
Based on this information, the section of the floor was subsequently modeled in such a way so that the
two reinforced floors collaborated perfectly (this hypothesis was satisfied by the analysis of a double
"T" section in which the core, or connecting element, had an infinitesimal thickness and the
polystyrene was considered as a void).
27
Figure 34 Generic cross section of the floor
Figure 35 Modeling of the cross section (lower and upper floor perfectly collaborating by
means of a rigid connecting element)
The moment-curvature scheme is determined from this cross section by means of a classic
procedure, listed below:
- The section is sub-divided into horizontal strips (problem of right-angle compression and
bending stress);
- A curvature value is established;
- the position of the neutral axis is determined through successive iterations in which the transfer
balances of the applied forces are imposed;
- una volta raggiunta la convergenza, si calcola il momento resistente;
- the collapse condition is determined by the reaching of the maximum compression deformation of
the cement (0.45%) or else the maximum tensile stress of the steel (12%).
The Mander - Priestley - Park constitutive equation, specialized for the non-confined case,
was used for the cement, while the behavior of the steel was represented by the Dodd Restrepo Posada equation.
The average values of resistance and deformation were used, in accordance with the
characteristics of the materials described in the initial part of the previous report.
In order to assess the actual collaboration between the two floors and the effective flow shear
stress transmitted by the layer of polystyrene, the following simplified method is employed.
The moment - curvature diagram of each section analyzed is calculated for various conditions
of materials efficiency. Specifically, each curve shown in the figure below refers to the
condition f • = • fc and f• = • fs , where f• and f• are the degraded cement and steel
resistances by means of the coefficient • ( 1 • • < 0 ).
The graphs which follow, therefore, also show the experimental resistant moment values in
such a way so as to directly evaluate the value of the reference coefficient •.
In essence, the actual collaboration of the two floors guaranteed by a given type of
polystyrene is considered, in the scope of this simplified equivalent method, by means of
degraded material resistance values (cement and steel).
In the case of the 170 mm thick section of low density polystyrene (in accordance with Table 5),
a material resistance reduction coefficient of • = 0 4 appears to adequately represent the
resistance capacity of the section.
In the case of the same section, but with high density polystyrene (Table 5), this degradation is
less consistent. The coefficient • = 0 7 can be used.
Both these cases have been evaluated experimentally on the floor with a span of 4 m.
In the case of the 250 mm thick section the density of the polystyrene has a less pronounced
influence, as can be seen from the ultimate resistant moment shown in Figure 37.
28
Again in this case, for the low density polystyrene • = 0.4 is appropriate, while
for high-density polystyrene, this coefficient may be slightly higher: • = 0.45
4 m floor section
50
1
45
0.9
40
0.8
35
HD
0.7
Polystyrene
30
0.6
25
0.5
LD
20
Polystyrene
0.4
15
10
5
0
0.00
0.10
0.20
0.30
0.40
0.50
0.60
0.70
Curvature [1/m]
Figure 36 4 m floor, as shown in Table 5.
5 m floor section
70
1
60
0.9
0.8
50
0.7
40
0.6
HD
Polystyrene
0.5
30
0.4
LD
Polystyrene
20
10
0
0.00
0.10
0.20
0.30
0.40
0.50
0.60
0.70
Curvature [1/m]
Figure 37 5 m floor, as shown in Table 5.
29