** Direct Strength Analysis**

**7.2 Structural Analyses – Modeling & Procedure .1 Purpose**

3D FE structural analyses as specified in this section are to be carried out to verify that the following are within the acceptance criteria when subjected to the specified static and dynamic loads:

a) Stress level in the longitudinal hull girder members, primary supporting members and the transverse bulkheads.

b) Buckling capability of plates and stiffened panels and other primary supporting members subjected to compressive stresses.

c) Deflection of primary supporting members.

**7.2.2 ** **Extent of model **

7.2.2.1 The minimum extent of the hull structure model is to be such as to cover all compartments
that lie within the region of 0.6Lamidships. Where, there is a significant change in the structural
arrangement or special features, the extent may have to be suitably increased.** **

The overall analyses may comprise of structural analyses carried out in parts. The extent of the structure included in each “part model ” is to cover at least three compartments. The transverse

bulkheads at the ends are to be included, together with their associated structures. Both ends of the model are to form vertical planes. The FE model is to include both sides of ship structures allowing application of the unsymmetrical loads.

7.2.2.2 Where the global/part model analysis reveals local areas of high stress or stress
concentration, a further investigation using local fine mesh model would be required. Appropriate
boundary conditions determined from the larger scale model are to be imposed in the local models
to ensure structural continuity and load transfer between the two levels of models. * *

**7.2.3 Finite element modeling **

**7.2.3.1 **All main structural members (plates, stiffeners, girders and pillars) detailed are to be
represented in FE model, e.g.:

− inner and outer shell,

− inner bottom and decks

− transverse and longitudinal bulkheads

− floors / girders systems / pillars and secondary stiffeners associated with the above mentioned plating

**7.2.3.2 **Mesh boundaries of finite elements are to simulate the stiffening systems on the actual
structures as far as practical and are to represent the correct geometry of the panels between
stiffeners. Similarly, sufficient compatibility between the hydrodynamic and structural models is to be
ensured so that the application of fluid pressures onto the finite element mesh of the structural
model can be done appropriately.

**7.2.3.3 **Stiffness of each structural member is to be represented by using element type appropriately
as given below :

(1) Stiffeners are to be modeled by beam elements having axial, torsional, bi-directional shear and bending stiffness. However, stiffeners on girder webs and face plates of primary supporting members may be modeled by bar elements having only axial stiffness and a constant cross-sectional area along its length.

(2) Plates are to be modeled by shell element having out-of-plane bending stiffness in addition to bi-axial and in-plane stiffness. However, membrane element having only bi-axial and in- plane stiffness can be used for plates that are not subject to lateral pressures.

For membrane and shell elements, only linear quad or triangle elements, as shown in Fig 7.2.3.3, are to be adopted. Triangle elements are to be avoided as far as possible, especially in highly stressed areas and in areas around openings and at bracket connections where significant stress gradient should be predicted.

**Fig. 7.2.3.3 : Linear Membrane and Shell Quad & Triangle Elements **

**7.2.3.4 **When orthotropic elements are not used in FE model:

− mesh size is to be equal to or less than the representative spacing of secondary stiffeners on the relevant load bearing plating e.g. deck, shell, bulkhead plating

− stiffeners are to be modeled by using beam or bar elements, as per 7.2.3.3 (1) above

− In spaces such as a double bottom, webs of primary supporting members e.g. double bottom girders and plate floors, are to be divided in at least four rows of elements, height-wise

− In general, girders and transverses and deep stiffeners, large end brackets etc. are to be modeled by using shell elements for web and shell or beam or bar elements for face plate.

− aspect ratio of all shell elements is not to exceed 1:4.

**7.2.4 Boundary conditions **
**7.2.4.1 General requirements **

The model of the hull girder structure should be close to equilibrium state when all the loads (static and dynamic) are applied.

Any unbalanced forces in the model’s global axis system for each load case need to be determined and resolved appropriately. The magnitude of the unbalanced forces, and the procedure used to balance the structural model in equilibrium is to be fully documented.

The boundary conditions applied to the model are to be such as to closely represent the physical structural behaviour, a standard method for this purpose is given in 7.2.4.2.

**7.2.4.2 Standard method **

At both end sections of a part model, the point of intersection of neutral axis with the ships’

centerline, located within the transverse bulkhead, is to be considered as a “Master Node”. These

“Master Nodes” are to have support conditions as given in Table 7.2.4.1. Other nodes on the longitudinal members at each end section are to be linked to the respective “Master Node” as shown in Table 7.2.4.2, so that the transverse sections remain plane after bending.

**Table 7.2.4.1: Support condition of Master Node **
**Location **

**Translational ** **Rotational **

**Dx ** **Dy ** **Dz ** **Rx ** **Ry ** **Rz **

**Master Node **on aft end of the model - Fixed Fixed - - -
**Master Node **on fore end of the model Fixed Fixed Fixed Fixed - -
Dx, Dy and Dz mean restrains on displacements along X, Y and Z axis, respectively.

Rx, Ry and Rz mean restrains on rotations about X, Y and Z axis, respectively.

X, Y and Z axes are in the longitudinal, transverse and vertical directions respectively.

**Table 7.2.4.2: Rigid Plane links at both end sections **
**Nodes on longitudinal members at **

**both ends of the model **

**Translational ** **Rotational **

**Dx ** **Dy ** **Dz ** **Rx ** **Ry ** **Rz **

RL RL RL - - -

RL means linked to the applicable “Master Node” to allow the necessary degrees of freedom

(displacements) in relation to the “Master Node”, so that the transverse sections at ends remain plane after bending.

**7.2.5 Loading conditions **

3D FE analyses are to be carried out considering the ship loading conditions and load cases specified in Section 7.3.

**7.2.6 Consideration of hull girder loads **

7.2.6.1 The hull girder loads to be considered for each loading condition are to consist of the still
water loads and appropriate values of wave-induced loads based on the Load Combination Factors
(LCFs) given in Section 7.3. These are to be applied at the Master Nodes at the end sections of the
part model. Thus, the vertical bending moment, **M ****V** and the horizontal bending moment, **M ****H** to be
applied at each master node are given by :

M V = MSW + LCF. MWV M H = LCF. MWH

Where,

MSW: Design vertical Still water bending moment, See Chapter 3

MWV: Vertical wave bending moment, in hogging or sagging condition, See Chapter 3 MWH: Horizontal wave bending moment, See Chapter 3

LCF: The Load Combination Factor applicable for the load component corresponding to the load case being considered. LCF is to be determined by hydrodynamic analysis using the Equivalent Design Wave method given in 7.3.

In addition to the above, incremental corrections

### M

V_T _INCR and### M

H_T_INCR to the vertical bending moment and the horizontal bending moment to account for the moments caused by the application of local loads within the FE model, are to be applied at each web frame between the aft and forward end sections. See 7.2.6.3. These correction moments may be equally distributed on the nodes on longitudinal members at that section.### M

V_T _INCR =### M

V_T### (

at the web frame under consideration) –### M

V_T (at the web frame immediately aft of that under consideration)### M

H_T_INCR =### M

H_T### (

at the web frame under consideration) –### M

H_T (at the web frame immediately aft of that under consideration)_{ }

### M

V_T and### M

H_T at any web frame between the aft and forward end sections are to be obtained as per 7.2.6.2.7.2.6.2 Alternatively, the superimposition method can be used to consider the effect of hull girder loads in the overall strength assessment. In this method, instead of applying the hull girder vertical and horizontal bending moments on the model, the resulting stresses are superimposed on to the stresses obtained from the structural analysis based on the local lateral loads. The hull girder stress,

### σ

*SIM*, in each element participating in the longitudinal strength is given by :

### (

^{_}N

### )

^{_}

### / z /

*V T* *H T*

*SIM*

*Y* *Z*

*M* *M*

*I* *z* *I* *y*

### σ = −

### −

Where,

*I*

*Y*: Vertical inertia of the section under consideration about the horizontal neutral axis

*I*

*Z*: Horizontal inertia of the section under consideration about the vertical neutral axis ( Z axis ) zN : Distance of the horizontal neutral axis above base line

y: *Y *co-ordinate of the element
z*:* *Z *co-ordinate of the element

MV_T, MH_T: Target (equivalent) vertical and horizontal bending moments at the section under consideration, respectively, after taking into account the required corrections due to local loads, M V_T = MV – M V_FEM

M H_T = MH – M H_FEM

M V_FEM: Local vertical bending moment correction due to local loads as per 7.2.6.3
M H_FEM**: **Local horizontal bending moment correction due to local loads as per 7.2.6.3

7.2.6.3 The vertical and horizontal bending moment corrections M V_FEM and M H_FEM respectively, are the moments caused by the application of local loads within the FE model, which at each web frame between the aft and forward end sections, may be obtained from a 2D beam model, simply supported at the forward & aft end and subjected to summation of all loads in Z and Y directions, respectively.

The vertical and horizontal bending moments, M V_FEM and M H_FEM respectively, are the required corrections to account for the moments caused by the application of local loads within the FE model.

The values of moment corrections M V_FEM and M H_FEM at each web frame between the aft and forward end sections, may be obtained from an independent 2D beam model simply supported at the forward & aft ends and subjected to summation of all loads in Z and Y directions, respectively.

**7.3 Design Loads for Direct Strength Assessment **