Understanding the strengths in shells

== Introduction ==

The ''finite element'' method permits to solve the governing equation of a structural model by using numerical methods over one model discretization. When the structure is thin (have one dimension much smaller than the other two), it is possible to consider the problem as a ''shell finite element'' problem. The results of this analysis are the displacements and rotations in every node of the mesh and the ''strengths'' in some interior element positions.

In order to get valuable information of the analysis, it is necessary a good understanding and interpretation of the ''strengths''. This document will explain what the ''strengths'' in shells are and how can they be used for dimensioning or evaluating one structural model.

We are going to define mathematically the strengths in shells as they are used in the standard shell ''Reissner-Mindlin'' theory. Basically, the strengths are a set of values obtained as integration of the stress tensor through the shell thickness. This set of values describes fully the stress tensor for every point in the shell mid plane.
{| class='floating_imageSCP' style='text-align: center; border: 1px solid #BBB; margin: 1em auto; width: 100%;max-width: 100%;'
|-
|[[Image:Draft_Ribo Rodriguez_725859212-shell_desc.svg]]
|- style='text-align: center; font-size: 75%;'
| colspan='1' | '''Image 1'''. Shell is represented by its mid plane
|}

== Definitions ==

One structure can be considered a ''Shell'' if it is thin (have one dimension much smaller than the other two).

Some definitions:

; Shell
: is a plane or curved surface in the 3D space that geometrically is positioned in the mid plane of the structure (based on the thickness direction). This Shell and the thickness in every point over the ''shell'' represents completely the geometry of the structure
; Thickness
: for every point in the structure, the thickness is the width of the model through the small dimension
; Local axes
: for every point in the structure it is necessary to define an attached local axes system X’, Y’ and Z’ where axe Z’ will always be orthogonal to the Shell. X’, Y’ can be any axes but must be defined for every point in the Shell prior to the calculation. All strengths will be expressed on these axes
; Section
: is the part of the structure which is the intersection between the structure and a plane orthogonal to the Shell mid plane

and then, the ''Reissner-Mindlin'' hypotheses are defined as follows:

* One planar section, after deformation will continue to be planar. The deformed section does not generally remain orthogonal to the mid-surface
* The normal stress through the thickness is ignored (<math display="inline">\sigma_{z'}=0</math>)
* There is a linear variation of displacement across the plate thickness and the plate thickness does not change during deformation

== Definition of the strengths in the shell ==

In any internal point of the structure the ''stress tensor'' represents the stresses in that point. As we have simplified the shell structure by the mid plane, it is necessary to define some values that are calculated as the integrals of the stress tensor through the shell thickness so as they represent completely, under the accepted hypotheses, the stresses in the mid plane.
{| class='wikitable' style='text-align: center; border: 1px solid #BBB; margin: 1em auto; width: 100%;max-width: 100%;'
|-
|[[Image:Draft_Ribo Rodriguez_725859212-shell_strengths.svg]]
|- style='text-align: center; font-size: 75%;'
| colspan='1' | '''Image 2'''. Strengths in the shell
|}

The strengths are three axial forces in the plane, three bending/twisting moments and two shears

<div id="table:1" class="mytable">

{|
|+ Table 1. Definition of strengths
!width="27%"| Axial force in X’
!align="center" width="26%"| Axial force in Y’
!align="center" width="45%"| Axial force in XY’
|-
| <math display="inline">N_x=\int_{-t/2}^{t/2}{\sigma_x dz}</math>
|align="center"| <math display="inline">N_y=\int_{-t/2}^{t/2}{\sigma_y dz}</math>
|align="center"| <math display="inline">N_{xy}=\int_{-t/2}^{t/2}{\tau_{xy} dz}</math>
|-
| '''Bending moment X’'''
|align="center"| '''Bending moment Y’'''
|align="center"| '''Twisting moment XY’'''
|-
| <math display="inline">M_x=\int_{-t/2}^{t/2}{\sigma_x z dz}</math>
|align="center"| <math display="inline">M_y=\int_{-t/2}^{t/2}{\sigma_y z dz}</math>
|align="center"| <math display="inline">M_{xy}=\int_{-t/2}^{t/2}{\tau_{xy} z dz}</math>
|-
| '''Shear force in X’'''
|align="center"| '''Shear force in Y’'''
|align="center"|
|-
| <math display="inline">Q_x=\int_{-t/2}^{t/2}{\tau_{xz} dz}</math>
|align="center"| <math display="inline">Q_y=\int_{-t/2}^{t/2}{\tau_{yz} dz}</math>
|align="center"|
|}


</div>
All the integrals are in Z’ axe from <math display="inline">-t/2</math> to <math display="inline">t/2</math>, being <math display="inline">t</math> the thickness of the shell in that point. Z’ is the local axis defined as parallel to the normal to the surface at the point.

We need to consider that the real <math display="inline">Q_x</math> and <math display="inline">Q_y</math> have a parabolic shape through the shell thickness with null values in the top and bottom layers. However, we accept the simplification of considering the shear as constant through all the thickness.
{| class='floating_imageSCP' style='text-align: center; border: 1px solid #BBB; margin: 1em auto; width: 100%;max-width: 100%;'
|-
|[[Image:Draft_Ribo Rodriguez_725859212-shear_strengths.svg]]
|- style='text-align: center; font-size: 75%;'
| colspan='1' | '''Image 3'''. Real parabolic shear stress is simplified as constant through the thickness
|}

== Finite element analysis ==

The ''Finite element'' analysis is a method to solve ''numerically'' the ''differential equation'' that governs the structural behavior of the model. To do so, it is necessary to discretize the model into a '''mesh''', which is a collection of '''elements''' connected between them by '''nodes'''. The variables to solve in the problem are the displacements and rotations of every node of the mesh. From these values, it is possible to interpolate the value of displacements for every point over the structure and it is also possible to calculate the strengths as a derived result of the displacements.
{| class='floating_imageSCP' style='text-align: center; border: 1px solid #BBB; margin: 1em auto; width: 100%;max-width: 100%;'
|-
|[[Image:Draft_Ribo Rodriguez_725859212-shell_mesh.svg]]
|- style='text-align: center; font-size: 75%;'
| colspan='1' | '''Image 4'''. The discretization is the shell mesh
|}

Once discretized, the finite element problem becomes:

<div id="f:fe1" class="myformula">

{| class='formulaSCP' style='width: 100%; text-align: left;'
|-
| 
{| style='text-align: left; margin:auto;width: 100%;' 
|- 
| style='text-align: center;' |  <math display="inline">Ka=f</math>
| style='width: 5px;text-align: right;white-space: nowrap;' |  (1)
|}
|}



</div>
where <math display="inline">K</math> is the stiffness matrix, <math display="inline">f</math> is the external forces vector and <math display="inline">a</math> is the displacements vector. As every node has 6 degrees of freedom (<math display="inline">d_x,d_y,d_z,\theta_x,\theta_y,\theta_z</math>), the dimension of <math display="inline">a</math> is 6 x number of nodes.

If the problem is linear, <math display="inline">K</math> and <math display="inline">f</math> do not depend on <math display="inline">a</math> and the problem can be solved by simply solving the linear system once.

If the problem is non linear, <math display="inline">K</math> or <math display="inline">F</math> depend on <math display="inline">a</math> and then it is necessary to solve the problem by iterating through a non-linear solver.

If the problem is dynamic, the equation to solve becomes:

<div id="f:fe2" class="myformula">

{| class='formulaSCP' style='width: 100%; text-align: left;'
|-
| 
{| style='text-align: left; margin:auto;width: 100%;' 
|- 
| style='text-align: center;' |  <math display="inline">M\ddot{a}+C\dot{a}+Ka=f</math>
| style='width: 5px;text-align: right;white-space: nowrap;' |  (2)
|}
|}



</div>
see [[#r:1|[1]]] for more details.

== Results of the finite element analysis ==

The finite element analysis gets reduced to the resolution of a system of equations where the variables are the displacements and rotations defined in every node of the mesh. As these variables are defined in the nodes that are shared between neighboring elements, the displacements and rotations fields are continuum through the elements by the natural definition of the problem.

As described before, the strengths are the integration of the stress tensor through the thickness of the shell and the stresses are the derivatives of the displacements. Both the stresses and the strength are calculated inside every element. Specifically, they are calculated in the integration points used to calculate the numerical integration inside the element during the analysis. These points are called ''Gauss points'' and are used due to the fact that the result is more precise on that points.

As the strengths are calculated inside every element, this leads to two effects that are important to consider:

<ol style="list-style-type: decimal;">
<li><p>The strengths fields are discontinuous between elements</p></li>
<li><p>When displaying the strengths in a postprocessing program, the software extrapolates the values calculated internally to new values in every node of the element boundary. For relatively small increments of the strength for every ''Gauss point'', it is possible that the calculated value for the nodes has a too great or too small magnitude. This leads in some cases to values than can</p>
<p>be considered as invalid (for example a variable that is known to be positive can have negative extrapolated values).</p></li></ol>

== Smoothing ==

As the strengths fields are discontinuous between elements, in some cases it might be convenient to calculate another field, similar to the original one, that is continuous in the node. This is only possible between elements that share equal local axes definition. The smoothed field is calculated by comparing the values in every node from each of the neighboring elements. Some kind of mean value is obtained and used as the value for the node.

This correction is generally good, as it provides a value that is closer in most cases to the real value. However, in extreme cases and specially near the shell boundary or in points over external elements or beams, it can lead to incorrect values. This effect can be maximized by adding up the smoothing correction to the extrapolation to nodes in boundary elements.

It is important to visualize and compare the non-smoothed results and the smoothed ones in order to understand better the strengths field.

<div id="table:sm1" class="table100 mytable">

{|
|+ Table 2. Moments in coarse mesh. Gauss points results
| [[Image:Draft_Ribo Rodriguez_725859212-rectangular_plate_mx_02-3.png|rp-02-gp]]
| [[Image:Draft_Ribo Rodriguez_725859212-rectangular_plate_mx_02-4.png|rp-02-gp1]]
| [[Image:Draft_Ribo Rodriguez_725859212-rectangular_plate_mx_02-5.png|rp-02-gp2]]
|}


</div>
<div id="table:sm2" class="table100 mytable">

{|
|+ Table 3. Moments in coarse mesh. Smoothed results
| [[Image:Draft_Ribo Rodriguez_725859212-rectangular_plate_mx_02-0.png|rp-02-sm]]
| [[Image:Draft_Ribo Rodriguez_725859212-rectangular_plate_mx_02-1.png|rp-02-sm1]]
| [[Image:Draft_Ribo Rodriguez_725859212-rectangular_plate_mx_02-2.png|rp-02-sm2]]
|}


</div>
<div id="table:sm3" class="table100 mytable">

{|
|+ Table 4. Moments in fine mesh. Gauss points results
| [[Image:Draft_Ribo Rodriguez_725859212-rectangular_plate_mx_005-6.png|rp-005-gp]]
| [[Image:Draft_Ribo Rodriguez_725859212-rectangular_plate_mx_005-7.png|rp-005-gp1]]
| [[Image:Draft_Ribo Rodriguez_725859212-rectangular_plate_mx_005-8.png|rp-005-gp2]]
|}


</div>
<div id="table:sm4" class="table100 mytable">

{|
|+ Table 5. Moments in fine mesh. Smoothed results
| [[Image:Draft_Ribo Rodriguez_725859212-rectangular_plate_mx_005-9.png|rp-005-sm]]
| [[Image:Draft_Ribo Rodriguez_725859212-rectangular_plate_mx_005-10.png|rp-005-sm1]]
| [[Image:Draft_Ribo Rodriguez_725859212-rectangular_plate_mx_005-11.png|rp-005-sm2]]
|}


</div>
We can summarize some of the results in table 6. We can see that the error, specially for the coarse mesh, is quite high.

<div id="table:sm5" class="mytable">

{|
|+ Table 6. Some results for the different meshes
! Mesh
!align="center"| Gauss points/Smooth
!align="right"| <math display="inline">M_{x,border}</math>
!align="right"| <math display="inline">M_{x,max}</math>
!align="right"| <math display="inline">M_{x,min}</math>
|-
| coarse
|align="center"| GP
|align="right"| -2.30
|align="right"| 20.0
|align="right"| -77
|-
| coarse
|align="center"| SM
|align="right"| -2.30
|align="right"| 13.0
|align="right"| -75
|-
| fine
|align="center"| GP
|align="right"| -0.17
|align="right"| 5.8
|align="right"| -74
|-
| fine
|align="center"| SM
|align="right"| -0.17
|align="right"| 4.6
|align="right"| -73
|}


</div>
== Main strengths and main stresses ==

For any tensor defined in a local axes system, there exists another local axes system in that point that maximizes and minimizes the diagonal values and converts to zero the non-diagonal values.

This system is calculated finding the '''eigenvalues''' and '''eigenvectors''' of the matrix.

The local axes systems for main moments, main axial strengths and main stresses need not to be equivalent and typically will be different between them.

Note that the following matrices are symmetrical and <math display="inline">N_{xy}=N_{yx}</math>, <math display="inline">M_{xy} = M_{yx}</math>, <math display="inline">\tau_{xy} = \tau_{yx}</math>, etc.

{|
!align="center" width="57%"| Strengths in local axes <math display="inline">L_0</math>
!align="center" width="32%"| Main strengths
!align="center" width="10%"|
|-
|align="center"| '''Axial strengths as membrane components'''
|align="center"|
|align="center"|
|-
|align="center"| <math display="inline">\begin{bmatrix} N_x & N_{xy} \\ N_{yx} & N_y \end{bmatrix}</math>
|align="center"| <math display="inline">\begin{bmatrix} N_{11} & 0 \\ 0 & N_{22} \end{bmatrix}</math>
|align="center"| <math display="inline">LA_N</math>
|-
|align="center"| '''Bending and twisting moments'''
|align="center"|
|align="center"|
|-
|align="center"| <math display="inline">\begin{bmatrix} M_x & M_{xy} \\ M_{yx} & M_y \end{bmatrix}</math>
|align="center"| <math display="inline">\begin{bmatrix} M_{11} & 0 \\ 0 & M_{22} \end{bmatrix}</math>
|align="center"| <math display="inline">LA_M</math>
|-
|align="center"| '''Stress tensor'''
|align="center"|
|align="center"|
|-
|align="center"| <math display="inline">\begin{bmatrix} \sigma_x & \tau_{xy} & \tau_{xz} \\ \tau_{yx} & \sigma_y & \tau_{yz} \\ \tau_{zx} & \tau_{zy} & \sigma_z \end{bmatrix}</math>
|align="center"| <math display="inline">\begin{bmatrix}\sigma_{11} & 0 & 0 \\ 0 & \sigma_{22} & 0 \\ 0 & 0 & \sigma_{33}\end{bmatrix}</math>
|align="center"| <math display="inline">LA_S</math>
|}

Where <math display="inline">LA_0, LA_N, LA_M</math> and <math display="inline">LA_S</math> will represent typically different local axes systems with a common Z’ axe.
{| class='floating_imageSCP' style='text-align: center; border: 1px solid #BBB; margin: 1em auto; width: 100%;max-width: 100%;'
|-
|[[Image:Draft_Ribo Rodriguez_725859212-shell_main_axes.svg]]
|- style='text-align: center; font-size: 75%;'
| colspan='1' | '''Image 5'''. Main strengths in <math display="inline">LA_M</math> and <math display="inline">LA_M</math>
|}

== Stresses in top and bottom layers ==

In the shell model, we assume that stresses vary linearly through the thickness of the Shell. As a consequence, both the maximum and the minimum of any stress component will be located in either the top or the bottom layer for any shell point.

'''Note''': shear stresses in y’ and z’ have a real parabolic shape through the Shell thickness, with a maximum in the middle plane of the shell. However, in our simplified model, we assume a constant value for the shear stresses in the thickness. So, maximum and minimum are also in the external layers.

Top and bottom stresses are calculated in the following way:

<div id="f:topbottom1" class="myformula">

{| class='formulaSCP' style='width: 100%; text-align: left;'
|-
| 
{| style='text-align: left; margin:auto;width: 100%;' 
|- 
| style='text-align: center;' |  <math display="inline">W_b=\frac{I_z}{z_{max}}=\frac{b h^2}{6}</math>
| style='width: 5px;text-align: right;white-space: nowrap;' |  (3)
|}
|}



</div>
<div id="f:topbottom2" class="myformula">

{| class='formulaSCP' style='width: 100%; text-align: left;'
|-
| 
{| style='text-align: left; margin:auto;width: 100%;' 
|- 
| style='text-align: center;' |  <math display="inline">A_b=b h</math>
| style='width: 5px;text-align: right;white-space: nowrap;' |  (4)
|}
|}



</div>
where <math display="inline">b=1.0</math> and <math display="inline">h=t</math>

then:

{|
|width="28%"| <math display="inline">\sigma_x=\frac{N_x}{A_b}\pm\frac{M_x}{W_b}</math>
|align="center" width="35%"| <math display="inline">\sigma_y=\frac{N_y}{A_b}\pm\frac{M_y}{W_b}</math>
|align="center" width="35%"| <math display="inline">\sigma_z=0</math>
|-
| <math display="inline">\tau_{xy}=\frac{N_{xy}}{A_b}\pm\frac{M_{xy}}{W_b}</math>
|align="center"| <math display="inline">\tau_{xz}=\frac{Q_x}{A_b}</math>
|align="center"| <math display="inline">\tau_{yz}=\frac{Q_y}{A_b}</math>
|}

== Dimensioning metallic materials ==

Based on the stresses tensor calculated before, it is possible to calculate the '''Von Mises stress''' for the top and bottom layers following the formula:

<div id="f:von_mises" class="myformula">

{| class='formulaSCP' style='width: 100%; text-align: left;'
|-
| 
{| style='text-align: left; margin:auto;width: 100%;' 
|- 
| style='text-align: center;' |  <math display="block">\sigma_{vm}=\sqrt{\frac{(\sigma_I-\sigma_{II})^2+(\sigma_{II}-\sigma_{III})^2+(\sigma_{III}-\sigma_I)^2}{2}}</math>
| style='width: 5px;text-align: right;white-space: nowrap;' |  (5)
|}
|}



</div>
where <math display="inline">\sigma_I, \sigma_{II}, \sigma_{III}</math> are the main stresses associated to the stress tensor <math display="inline">\sigma_x, \sigma_y, \sigma_z, \tau_{xy}, \tau_{xz}, \tau_{yz}</math>.

The '''Von Mises stress''' as defined in (5) can be used as a yield criteria for the material. This is commonly used as yield criteria for metallic materials.

== Dimensioning structural concrete ==

Structural concrete is a composite material made of concrete and steel bars. Several normatives, like ''Eurocode'' and ''ACI'' and other national regulations, offer guidelines to dimension and check the concrete cross section and the amount of steel.

For a model where the main axial forces axes <math display="inline">LA_N</math> and the main momentum axes <math display="inline">LA_M</math> are coincident with the element local axes <math display="inline">L_0</math>, the strengths in the section will be <math display="inline">N_{x'}</math>, <math display="inline">M_{x'}</math> and <math display="inline">Q_{x'}</math> in the <math display="inline">x'</math> direction and <math display="inline">N_{y'}</math>, <math display="inline">M_{y'}</math> and <math display="inline">Q_{y'}</math> in the <math display="inline">y'</math> direction. With these strengths, it is possible to dimension by using the standard regulations.

In the general case, there is an additional twisting moment <math display="inline">M_{xy}</math> that is different to zero. It is not in the security side to dimension the section without considering this twisting moment in the verification of the main steel bars in both directions.

It is necessary to use some method, that satisfies the equilibrium and geometric compatibility in the section and that has some bearing strengths greater that the external actions.

One commonly used method is the ''Wood and Armer''. In this method, the bearing <math display="inline">m_{ux}</math> and <math display="inline">m_{uy}</math> are increased based on the value of <math display="inline">m_{xy}</math>. These values are used for dimensioning.

The ''CEB-FIP Model Code'' proposes and alternative method where the thickness is divided into three layers and the strengths are converted into pairs of forces and shear forces for dimensioning.

=== Wood and Armer method ===

The Wood and Armer method is based on the normal moment yield criterion (Johansen’s yield criterion) and proposes that the dimensioning of the maximum bear moments for some given directions <math display="inline">x</math> and <math display="inline">y</math> can be calculated as follows:

<div id="f:wood_amer1" class="myformula">

{| class='formulaSCP' style='width: 100%; text-align: left;'
|-
| 
{| style='text-align: left; margin:auto;width: 100%;' 
|- 
| style='text-align: center;' |  <math display="inline">m_{ux}=m_x \pm \left| m_{xy} \right|</math>
| style='width: 5px;text-align: right;white-space: nowrap;' |  (6)
|}
|}



</div>
<div id="f:wood_amer2" class="myformula">

{| class='formulaSCP' style='width: 100%; text-align: left;'
|-
| 
{| style='text-align: left; margin:auto;width: 100%;' 
|- 
| style='text-align: center;' |  <math display="inline">m_{uy}=m_y \pm \left| m_{xy} \right|</math>
| style='width: 5px;text-align: right;white-space: nowrap;' |  (7)
|}
|}



</div>
if <math display="inline">m_{x}</math> and <math display="inline">m_{y}</math> have different sign, and <math display="inline">m_{x}</math> is bigger then:

<div id="f:wood_amer3" class="myformula">

{| class='formulaSCP' style='width: 100%; text-align: left;'
|-
| 
{| style='text-align: left; margin:auto;width: 100%;' 
|- 
| style='text-align: center;' |  <math display="inline">m_{ux}=m_x \pm \left| \frac{m_{xy}^2}{m_y} \right|</math>
| style='width: 5px;text-align: right;white-space: nowrap;' |  (8)
|}
|}



</div>
<div id="f:wood_amer4" class="myformula">

{| class='formulaSCP' style='width: 100%; text-align: left;'
|-
| 
{| style='text-align: left; margin:auto;width: 100%;' 
|- 
| style='text-align: center;' |  <math display="inline">m_{uy}=0</math>
| style='width: 5px;text-align: right;white-space: nowrap;' |  (9)
|}
|}



</div>
Theoretical justification of the Wood and Armer method:

Given external moments <math display="inline">m_x, m_y</math> and <math display="inline">m_{xy}</math>, the moments in direction <math display="inline">n</math> where the angle between <math display="inline">x</math> and <math display="inline">n</math> is <math display="inline">\theta</math> are the following:

<div id="f:wood_amer5" class="myformula">

{| class='formulaSCP' style='width: 100%; text-align: left;'
|-
| 
{| style='text-align: left; margin:auto;width: 100%;' 
|- 
| style='text-align: center;' |  <math display="inline">m_n=m_x \cos^2 \theta+m_y \sin^2 \theta+2m_{xy}\cos \theta \sin \theta</math>
| style='width: 5px;text-align: right;white-space: nowrap;' |  (10)
|}
|}



</div>
<div id="f:wood_amer6" class="myformula">

{| class='formulaSCP' style='width: 100%; text-align: left;'
|-
| 
{| style='text-align: left; margin:auto;width: 100%;' 
|- 
| style='text-align: center;' |  <math display="inline">m_{nt}=(m_y-m_x)\cos \theta \sin \theta + m_{xy}(\cos^2\theta-sin^2\theta)</math>
| style='width: 5px;text-align: right;white-space: nowrap;' |  (11)
|}
|}



</div>
On the other side, if <math display="inline">m_{ux}</math> and <math display="inline">m_{uy}</math> are the moment capacities in axes x,y then, the bearing capacity of the section in direction <math display="inline">n</math> where the angle between <math display="inline">x</math> and <math display="inline">n</math> is <math display="inline">\theta</math> is the following:

<div id="f:wood_amer7" class="myformula">

{| class='formulaSCP' style='width: 100%; text-align: left;'
|-
| 
{| style='text-align: left; margin:auto;width: 100%;' 
|- 
| style='text-align: center;' |  <math display="inline">m_{un}=m_{ux} \cos^2\theta+m_{uy}\sin^2\theta</math>
| style='width: 5px;text-align: right;white-space: nowrap;' |  (12)
|}
|}



</div>
Imposing that <math display="inline">m_{un}</math> in (12) must be bigger that <math display="inline">m_n</math> in (10) for any direction, it is possible to justify that the ''Wood and Armer'' proposal is an upper bound of the capacity for any direction.

The justifications and details of the method are described in [[#r:2|[2]]] and [[#r:3|[3]]].

=== CEB-FIP Model Code ===

The slab model is decomposed into three layers, each with <math display="inline">1/3</math> of the slab thickness. Bending moments are decomposed into pairs of forces and applied to the layers as normal forces. Twisting moments are equally decomposed into pairs of force that are applied as shear forces in the two external layers. Finally, the shear forces are applied to the central layer for verification.

== Dimensioning composite laminate material ==

A composite laminate material or fiber reinforced plastic (FRP) is built by adding several layers of fiber that get glued together by the use of a resin. In order to dimension or check its bearing capacity, it is typically necessary to evaluate a failure criterion for every one of its constitutive layers or plies.

Every single layer can be defined by its components of fiber and resin and are normally orthotropic, having different resistance values for every one of the orthogonal directions. This anisotropic composite materials will also have different resistance capacities in tension and compression.

It is common to use the ''Tsai–Wu failure criterion'' in order to check the capacity of each single layer.
{| class='floating_imageSCP' style='text-align: center; border: 1px solid #BBB; margin: 1em auto; width: 100%;max-width: 100%;'
|-
|[[Image:Draft_Ribo Rodriguez_725859212-shell_laminate.svg]]
|- style='text-align: center; font-size: 75%;'
| colspan='1' | '''Image 6'''. Analysis of a laminate ply
|}

=== Tsai–Wu failure criterion ===

The criterion is defined as follows:

<div id="f:tsai_wu1" class="myformula">

{| class='formulaSCP' style='width: 100%; text-align: left;'
|-
| 
{| style='text-align: left; margin:auto;width: 100%;' 
|- 
| style='text-align: center;' |  <math display="inline">\sum_{i=1}^{6} F_i \sigma_i + \sum_{i=1}^{6}\sum_{j=1}^{6} F_{ij} \sigma_i \sigma_j \leq 1</math>
| style='width: 5px;text-align: right;white-space: nowrap;' |  (13)
|}
|}



</div>
where <math display="inline">\sigma_i</math> is one of <math display="inline">(\sigma_{xx},\sigma_{yy},\sigma_{zz},\sigma_{yz},\sigma_{xz},\sigma_{xy})</math> and <math display="inline">F_i</math> and <math display="inline">F_{ij}</math> are some coefficients calculated from laboratory results.

For '''plane stress''', where <math display="inline">\sigma_z=\sigma_{yz}=\sigma_{xz}=0</math>, the criteria is reduced to:

<div id="f:tsai_wu2" class="myformula">

{| class='formulaSCP' style='width: 100%; text-align: left;'
|-
| 
{| style='text-align: left; margin:auto;width: 100%;' 
|- 
| style='text-align: center;' |  <math display="inline">F_1\sigma_{xx}+F_2\sigma_{yy}+F_{11}\sigma_{xx}^2+</math> <math display="inline">F_{22}\sigma_{yy}^2+F_{66}\tau_{xy}^2+2F_{12}\sigma_{xx}\sigma_{yy} \leq 1</math>
| style='width: 5px;text-align: right;white-space: nowrap;' |  (14)
|}
|}



</div>
where:

{|
|width="57%"| <math display="inline">F_1=\frac{1}{\sigma_{1t}}-\frac{1}{\sigma_{1c}}</math>
|width="42%"| <math display="inline">F_2=\frac{1}{\sigma_{2t}}-\frac{1}{\sigma_{2c}}</math>
|-
| <math display="inline">F_{11}=\frac{1}{\sigma_{1c}\sigma_{1t}}</math>
| <math display="inline">F_{22}=\frac{1}{\sigma_{2c}\sigma_{2t}}</math>
|-
| <math display="inline">F_{66}=\frac{1}{\tau_{12}^2}</math>
|
|}

As it is difficult to obtain the value of <math display="inline">F_{12}</math> from a laboratory test, some references suggest to use the value <math display="inline">F_{12}=0</math>. Tsai recommends to obtain its value based on the following relationship:

<div id="f:tsai_wu3" class="myformula">

{| class='formulaSCP' style='width: 100%; text-align: left;'
|-
| 
{| style='text-align: left; margin:auto;width: 100%;' 
|- 
| style='text-align: center;' |  <math display="inline">F_{12}=-0.5(F_{11}F_{22})^{0.5}</math>
| style='width: 5px;text-align: right;white-space: nowrap;' |  (15)
|}
|}



</div>
Where <math display="inline">\sigma_{1t}</math> and <math display="inline">\sigma_{1c}</math> are the tensile and compressive allowable stress in the longitudinal direction and <math display="inline">\sigma_{2t}</math> and <math display="inline">\sigma_{2c}</math> are the tensile and compressive allowable stress in the transverse direction. <math display="inline">\tau{12}</math> is the allowable shear stress.

see [[#r:4|[4]]] and see [[#r:5|[5]]] for a detailed description.

== References ==

<div id="r:1" class="myreference">

[1] Oñate E. (1991) Cálculo de estructuras por el método de los elementos finitos. ISBN 8487867006


</div>
<div id="r:2" class="myreference">

[2] Shin M., Bommer A., Deaton, J.B. and Alemdar, B.N. (2009) Twisting Moments in Two-Way Slabs. Concrete international. Available: https://www.academia.edu/15396812


</div>
<div id="r:3" class="myreference">

[3] OBrien E., O’Dwyer D. (2015). A review of the Wood and Armer equations for torsion in bridge slabs. 93. 40-43


</div>
<div id="r:4" class="myreference">

[4] Tsai S.W. and Wu E.M. (1971) A general theory of strength for anisotropic materials. J Compos Mater, 5. pp. 58-80


</div>
<div id="r:5" class="myreference">

[5] Hopkins P. (2005) Benchmarks for Membrane and Bending Analysis of Laminated Shells. ISBN 1874376085


</div>