Finite Element Analysis – Crane Foundation Analysis and related structure
Crane foundation and adjacent structure
The focus of this study is to evaluate the structural response of a crane foundation and adjacent structure. The crane is a knuckle boom type crane, with 50-ton capacity, and it’s incorporated in a Multipurpose Support Vessel (MSV).
The purpose of the Finite Element Analysis (FEA) reported in this report is to assess the response of the crane foundation and related structure.
2.1. Job Specification
The job specification calls for a static, linear elastic, FEA of the crane-related structure.
The finite element model is based on the drawings provided by Bureau D’Etudes Mauric (Ref.2 and Ref.3).
The acceptance criteria for the analysis are as follow
2.2. The logic for using the Finite Element Method
The structure under study is too complex to be analyzed by hand calculation particularly in regions of high-stress concentrations.
2.3. FEA Software
ANSYS finite element software (Version 17.0) developed and supported by ANSYS Inc. Houston, PA, was used for the finite element work performed and presented here. ANSYS is a well established FEA package has a proven track record in analyzing structures of the type under consideration.
3.1. Analysis Type and Assumptions
Since the stresses are limited to the yield stress the material behaviour is assumed to be linear. Similarly, because large deflections are not expected geometric behaviour is assumed to be linear as well.
The load is assumed to be static and the interest of this study is centred on the strength of the crane foundation and adjacent structure. Hence, the dynamic behaviour of the structure is not within the scope of this analysis.
The overall strength of the structure is the primary focus of this analysis, and therefore the analysis is not optimized to examine stress concentration at structural discontinuities such as those that will exist around openings for example.
3.2. Global Geometry
The crane foundation is considered above the vessel Main Deck (5.5mm above baseline) between bulkheads #8 and #14, from the starboard side (outboard) to the longitudinal at 4.2 m from the centerline. The crane pedestal is 8 meters long, from the main deck to the top, with 2620 mm in diameter. There is also a deckhouse wrap around the pedestal (deckhouse top at 4.5m above the main deck).
The crane foundation and the surrounding structure are shown in Figure 3.1. A section of the structure is shown in Figure 3.2, as an example.
The crane pedestal is considered but the focus of this study is the supporting structure, not the pedestal per se.
3.3. The extent of Model
The structure adjacent to the crane foundation, between the transverse bulkheads (#8 and #14), is a series of ring frames divided by a longitudinal bulkhead located at 4.2 meters from the centerline. These frames are connected by all longitudinally oriented structure (framing members and plating). There is also a staircase aligned with the starboard longitudinal bulkhead (4200 FCL) between frames #11 and #14.
In this study, the structure was the only model between the outboard (starboard side) and centerline and from the tank top to the top of the crane pedestal. This is considered sufficient if the correct boundary conditions are applied as discussed in Section 3.6.
A section of the structure is shown in Figure 3.2, as an example.
3.4. Material Properties
There are two types of steel in this structure; Table 3.1 lists the relevant material properties.
| Type | Type | |
|---|---|---|
| Material Properties | S230 | S355 |
| Yield Strength [MPa] | 230 | 355 |
| Young’s Modulus [MPa] | 210 | 210 |
The steel with the higher yield strength (355 MPa) is only considered for the crane pedestal.
The Young’s Modulus was taken as 210 MPa for both types of steel. Parameters such as initial imperfections and residual strains were not included in the analysis, and no allowance is made for corrosion.
3.5. Loads
The design load consists of a set of forces and a set of moments.
Forces:
Moments:
The design loads applied are illustrated in Figure 3.3.
The aforementioned loads represent Load case 0. Seven other load cases were created rotating the horizontal force and the overturning moment in steps of 45 degrees. All the load cases are listed in Table 4.1.
| Angle [deg] | Fx [kN] | Fy [kN] | Mx [kN.m] | My [kN.m] |
|---|---|---|---|---|
| 0 | 376.00 | 0.00 | 0.00 | 10417.00 |
| 45 | 265.87 | 265.87 | 7365.93 | 7365.93 |
| 90 | 0.00 | 376.00 | 10417.00 | 0.00 |
| 135 | -265.87 | 265.87 | 7365.93 | -7365.93 |
| 180 | -376.00 | 0.00 | 0.00 | -10417.00 |
| 225 | -265.87 | -265.87 | -7365.93 | -7365.93 |
| 270 | 0.00 | -376.00 | -10417.00 | 0.00 |
| 315 | 265.87 | -265.87 | -7365.93 | 3 7365.93 |
The design loads were provided by Bureau D’Etudes Mauric (Ref.4).
3.6. Boundary Conditions
The model is clamped at the centerline. This boundary condition is applied to all nodes along the centerline (longitudinal) edges of plates.
The bottom part of the model has to types of boundary conditions. The longitudinal, the forward and the aft bulkheads are simply supported, providing translational restrain along the Z-axis. The frames, or half frames, are constrained in the Z and Y-axis. These conditions avoid rigid body motion and mimic the effect that the tank top (and remaining non-model structure) has in the structure in the study.
4.1. General Information
The unit system used is classified by ANSYS as MPA, were the mass, length, time, force, moment, pressure and density are given in, tonne, mm, seconds, N, N.mm, MPa and t.mm-3, respectively.
The global coordinate system for the problem is as follows:
Global X-axis: Longitudinal, trough the length of the ship.
Global Y-axis: Transverse axis (positive to portside)
Global Z-axis: Vertical axis (positive up)
The origin (0,0,0) is considered in the intersection between the centerline, Frame #0 and baseline.
4.2. Element Selection
All the plates are model with (SHELL281) ANSYS elements. This type of elements is suitable for analyzing moderately-thick shell structures. The element has eight nodes with six degrees of freedom at each node: translation in X, Y and Z axis, and rotations about X, Y and Z-axis.
For transfer, the loads described in Section3.5 from the application point to the structure a grid of elements was created. For this (MPC184) rigid link elements were selected. This type of elements comprises a general class of multipoint constrain elements that apply kinetic constraints between nodes. These elements are loosely classified as “constrained elements” (rigid links).
For modelling beam elements, in this case, only one rider bar on the crane pedestal, (BEAM189) elements was selected. The element is a quadratic three-node beam element in 3D.
4.3. Simplifications
Simplifications were made to the FE model in order to avoid too complex meshes in areas where a high degree of refinement is not necessary.
Most of these simplifications are related to the geometry of the real model. Figure 4.1 shows the typical kind of geometrical simplifications that were made, which was transforming all-around corners into line segments.
Cutouts, lugs, brackets and stiffeners along the panels were not modelled. The same for hatch/door openings.
All of these alterations were made taking into account the conservative side, ensuring that the FE model doesn’t exceed the real model in a structural way.
4.4. Mesh Design
The FE model was created with a unitary mesh (h=1), meaning that the model was divided into smaller areas/elements determined by the geometrical features/behaviour of the simplified model. This coarser mesh aims to set a good base mesh that can be refined.
From this coarser mesh, preliminary analyses can be made allowing a global screening of the model structural behaviour and an identification of the most critical areas.
The unitary mesh model can be refined with two finer grades h=2 and h=4. For a grade h=2, each line of every unitary element is divided in two or in four in the case of an h=4 grade. This refinement can be made for the whole model or only in specific areas (high-stress areas, for instance).
The FEM unitary mesh contains a total of 6238 elements and 16262 nodes.
4.5. Finite Element Attributes
The attributes of the elements used in the model are listed in Table 4.2.
| Item No | Description | Type of Element | Section No | Thickness Or Area [mm/mm2] | Iyy [mm4] | Izz x 106 [mm4] |
|---|---|---|---|---|---|---|
| 1 | Plate / Rider Bar | SHELL 281 | 2 | 20 | - | - |
| 2 | Plate / Rider Bar | SHELL 281 | 3 | 15 | - | - |
| 3 | Plate / Rider Bar | SHELL 281 | 4 | 10 | - | - |
| 4 | Plate | SHELL 281 | 5 | 8 | - | - |
| 5 | Plate | SHELL 281 | 6 | 7 | - | - |
| 6 | Plate / Rider Bar | SHELL 281 | 7 | 12 | - | - |
| 7 | Rider Bar | BEAM 189 | 8 | 2250 | 42188 | 4.218 |
| 8 | Rigid Link | MPC 184 | - | - | - | - |
4.6. FE Model Loads and Boundary Conditions
The general information on the applied load is provided in Section 3.5. The load is applied in a master node, located at the centre of the pedestal, which is connected to the model by rigid links (see Section 4.2). Figure 4.2 shows the rigid link structure.
The finite element boundary conditions are explained in Section 3.6. Referring to the global coordinate system described in Section 4.1. All nodes along the coordinate Y=0 (centerline) are clamped. All nodes along the coordinate Y=-4200 between Z= 1600 and Z=2240 are restrained in Z direction, as well as the nodes at X=9600 along the coordinate Z= 2240 (aft bulkhead) and at X= 16800 along the coordinate Z= 1600 (forward bulkhead). All the frames between the aft and forward bulkhead are constrained in the Z and the Y direction. The intersection of these frames with the coordinate Y=-8015 (bilge) are restrained in the X and the Z direction.
Table 4.2 lists all of the boundary conditions. See also Figure 4.3.
| Location | Description | Degrees of Freedom (DOF)* | |||||
| Ux | Uy | Uz | ROTx | ROTy | ROTz | ||
| Centerline | Plate edges | ||||||
| Aft Bulkhead | Bottom (connection w/tank top) | ||||||
| Fwd Bulkhead | Bottom (connection w/tank top) | ||||||
| Lng. Bulkhead | Bottom (connection w/tank top) | ||||||
| Longitudinal | At Y=-5850 (connection w/tank top) | ||||||
| Frames | At Y=-4200 (connection w/tank top) | ||||||
| Frames | Starboard side (bilge) | ||||||
4.7. FE Model Check
Before the FE model was run, the following checks were made:
The following checks were conducted using ANSYS graphical interface. ANSYS provides a listing of the requested information for specifically select entities. Also, symbols can be turned on/off to view various aspects, such as boundary conditions, loads, etc, of the model.
The following checks are built into ANSYS and are performed during the data checking process. Warning or error messages issued when the model fails to pass the check. The outputs from such data check run were reviewed.
5.1. General Solution Checks
The following post-run checks were performed:
5.2. Post Processing Method
The ANSYS graphical post-processor was extensively used to review stress and displacement results. In all stress contours, plot element solution un-averaged was used. The displacements and rotation are calculated at each node but stress and strain are evaluated at the element integration points, then these results are extrapolated to the nodes. Each node can be common to different elements so the nodes can have multiple values of stress from each element. Thus, the average of those values is considered as a nodal solution and they are continuous across the elements. On the other hand, the element solution has un-averaged stress values.
5.3. Structural Response
5.3.1.Displacement and VonMises Stress
The finite element analysis was run for the load cases listed in Section 3.5. Table 5.1 lists the maximum values of stress and displacement obtained.
It can be observed that all the maximum values occurred in the top of the crane pedestal, namely in the boundary with the rigid links. These maximum values can be seen as singularities 7 due to the proximity with the imposed load. Moreover, remember that the crane pedestal is out of the scope of this study, the assessment is to be made for the supporting structure, not for the pedestal (Section 3.2).
| Load Case | Stress [MPa]* | Description | Displacement [mm] | Description |
|---|---|---|---|---|
| 0 deg | 394.59 | Pedestal top | 8.93 | Pedestal top |
| 45 deg | 406.96 | Pedestal top | 7.93 | Pedestal top |
| 90 deg | 378.26 | Pedestal top | 6.70 | Pedestal top |
| 135 deg | 401.86 | Pedestal top | 8.03 | Pedestal top |
| 180 deg | 402.94 | Pedestal top | 8.92 | Pedestal top |
| 225 deg | 399.63 | Pedestal top | 7.51 | Pedestal top |
| 270 deg | 382.86 | Pedestal top | 6.00 | Pedestal top |
| 315 deg | 391.58 | Pedestal top | 7.61 | Pedestal top |
*VonMises Stress
The deflected shape of the structure is shown in Figure 5.1 and Figure 5.2. The displacement at the deckhouse top is approximately 3 mm.
The VonMises stress plot is shown in Figure 5.3. For this load case, the longitudinal at 7140 mm FCL is under the higher stresses (Figure 5.4). The stress range acting in this area is between 30 and 100 MPa. Except for the two corners near the opening where a local maximum is reached above 150 MPa. On the forward bulkhead, near the boundary conditions, the stress reaches values around 80 MPa.
The deflected shape of the structure is shown in Figure 5.5 and Figure 5.6. The displacement at the deckhouse top is approximately 2.5 mm.
The VonMises stress plot is shown in Figure 5.7. In this case, the load is no longer aligned with the longitudinal 7140 mm FCL, this causes that the longitudinal is not so requested (comparatively to the last case). The higher stresses are now concentrated in the “ring” structure that connects the pedestal to the internal structure (3980 mm above the main deck) reaching values of 130/150 MPa. This can be seen in Figure 5.8.
The deflected shape of the structure is shown in Figure 5.9 and Figure 5.10. The displacement at the deckhouse top is approximately 2.3 mm.
The VonMises stress plot is shown in Figure 5.11. The structural response behaviour follows the same nature seen in the previous two cases, i.e., the requested zones are the ones aligned with the load direction (as expected). In this case, the load is aligned with frame #11. The stress range in frame #11 is between 30 and 80 MPa. The connection between this frame, the deckhouse top and the crane pedestal has a maximum near to 150 MPa (Figure 5.12). The connection with this frame and the shell plates has a maximum value of 70 MPa.
The deflected shape of the structure is shown in Figure 5.13 and Figure 5.14.
The VonMises stress plot is shown in Figure 5.15. In this case, like in the load case for 45 degrees, the higher stress zone is concentrated in the “ring” structure that connects the 8 pedestals to the internal structure reaching values of 130/150 MPa.
This can be seen in Figure 5.16. On the aft bulkhead, near the boundary conditions, the stress reaches values around 100 MPa.
The deflected shape of the structure is shown in Figure 5.17 and Figure 5.18.
The VonMises stress plot is shown in Figure 5.19. The internal structure, namely the longitudinal 7140 FCL, reaches values up to 100. Once again near the boundary condition in the aft bulkhead, stress reaches values of 60 MPa (max 100 MPa). The longitudinal bellow main deck (5850mm FCL) is slightly under stress (Figure 5.20).
The deflected shape of the structure is shown in Figure 5.21 and Figure 5.22.
The VonMises stress plot is shown in Figure 5.23. The higher stresses are concentrated in the “ring” structure that connects the pedestal to the internal structure (3980 mm above the main deck) and in the girder at 2000mm above the main deck, reaching values of 130/150 MPa. This can be seen in Figure 5.24.
The deflected shape of the structure is shown in Figure 5.25 and Figure 5.26.
The VonMises stress plot is shown in Figure 5.27. The structural response behaviour follows the same nature seen in the Load case for 90 degrees. The load is aligned with frame #11. The stress range in frame #11 is between 30 and 100 MPa. The higher stresses are concentrated in the “ring” structure that connects the pedestal to the internal structure (3980 mm above the main deck, in the girder at 2000mm above the main deck and in the connection between frame #11 and the deckhouse top, with values up to 100/150 MPa. This can be seen in Figure 5.28.
The deflected shape of the structure is shown in Figure 5.29 and Figure 5.30.
The VonMises stress plot is shown in Figure 5.31. Like in the previous case the “ring” structure that connects the pedestal to the internal structure is under higher stresses (Figure 5.32).
5.3.2.Buckling Check
The buckling check was made based on DNV-RP-201 (Ref.5). For this check, two types of panels were selected: girder panel (plate and girder) and simple panel (plate only).
Based on the analysis made on the previous subsection the 180deg load case was selected for this code check. From all the considered load cases this is the one who causes more stress in the internal structure.
Two girder panels and one simple panel were selected for this check, which is located at the longitudinal 7140 FCL. Figure 5.33 shows the three panels. The plate associated with the girder panel has the following dimensions: 2588x1850mm for Girder Panel 1 and 2035x1850mm for Girder Panel 2. The simple panel is a 2615x2033mm plate. All thicknesses are according to Ref.3.
The three panels were checked with the Ref.5 to see the maximum stresses (Sigxx and Sigyy) that would cause buckling (see Annex A). Table 5.2 lists the stresses obtained.
| Panel | Sigxx [MPa] | Sigyy [MPa] |
|---|---|---|
| Panel Girder 1 | 100 | 80 |
| Panel Girder 2 | 90 | 90 |
| Simple Panel | 50 | 45 |
Figures 5.34, 5.35, 5.36, 5.37, 5.38 and 5.39 show the stresses for the same three panels obtained by the finite element model. The stresses magnitudes are well below the stresses listed in Table 5.2, meaning that these panels will not suffer buckling effects.
The crane foundation and surrounding structure as designed and analyzed meet the acceptance criteria. A total of eight load cases were applied and for all of them the structure remains predominantly elastic except in very localized regions, namely: around openings, in the connections between the horizontal girder (at 2000 mm above Main Deck) and the crane pedestal and between the “ring” structure (3890 mm above Main Deck) and the crane pedestal.
The localized high stresses around openings can be justified by the geometrical simplifications made in the model.
Regarding the horizontal girder and the ring structure (located at 2000 mm and 3890 mm above the main deck, respectively) it’s recommended that the detail design is revised for a more smooth transition in the connection with the crane pedestal.
![Figure 5.34 - SigXX [MPa] for Girder Panel 1](https://portfolio.veranavis.com/wp-content/uploads/2020/09/crane-foundation-figure-5.34-1030x686.png "Figure 5.34 – SigXX [MPa] for Girder Panel 1")
![Figure 5.35 - SigYY [MPa] for Girder Panel 1](https://portfolio.veranavis.com/wp-content/uploads/2020/09/crane-foundation-figure-5.35-1030x686.png "Figure 5.35 – SigYY [MPa] for Girder Panel 1")
![Figure 5.36 - SigXX [MPa] for Girder Panel 2](https://portfolio.veranavis.com/wp-content/uploads/2020/09/crane-foundation-figure-5.36-1030x686.png "Figure 5.36 – SigXX [MPa] for Girder Panel 2")
![Figure 5.37 - SigYY [MPa] for Girder Panel 2](https://portfolio.veranavis.com/wp-content/uploads/2020/09/crane-foundation-figure-5.37-1030x686.png "Figure 5.37 – SigYY [MPa] for Girder Panel 2")
![Figure 5.38 - SigXX [MPa] for Simple Panel](https://portfolio.veranavis.com/wp-content/uploads/2020/09/crane-foundation-figure-5.38-1030x686.png "Figure 5.38 – SigXX [MPa] for Simple Panel")
![Figure 5.39 - SigYY [MPa] for Simple Panel](https://portfolio.veranavis.com/wp-content/uploads/2020/09/crane-foundation-figure-5.39-1030x686.png "Figure 5.39 – SigYY [MPa] for Simple Panel")