This study investigated the vibration response of a stiffened plate using beam, shell, and solid finite element modeling techniques in Abaqus, . Abaqus was chosen due to its widespread commercial use and robust finite element solver. Finite element results from each model were compared using wavenumber analysis. A spatial Fourier transform of the displacement along several points on the plate was used to evaluate the wavenumber results in Matlab, . The following sections provide the details and assumptions that went into the model creation and analysis.
In general, a stiffened plate can be modeled with 2D shell elements for the plating and 1D beam elements for the stiffeners, or entirely with shell elements using plate theory . At low frequencies when the wavelengths are long, the bending behavior is dominant, and plate theory is appropriate to capture the effects adequately of the plate. Modeling the stiffeners as simple beam elements accurately captures the bending behavior since beam elements are based on exact bending solutions . As the frequency increases, plate modes of vibration can be excited within stiffeners, with the first fundamental mode occurring at the frequency when a half wavelength forms along the depth of the stiffener. This effect cannot be captured using beam elements based on beam bending equations only, so stiffeners must be modeled as shell elements. At even higher frequencies, full wavelengths can form within small structural features, such as compression or shear waves through the thickness of a plate, or a bending wave along the depth of a beam flange. 3D Solid elements based on three-dimensional elasticity theory are needed to model the vibrations in this case. Although solid elements can capture the through thickness effects at higher frequencies, solid element models will have many more degrees of freedom and be more computationally intensive to solve than plate and beam models. This study observes the divergence of the predicted response due to different element types using wavenumber analysis. The specific element types used for each model case are described in Section 2.2.
Abaqus was used to create a total of five models with the initial mesh being created in HyperMesh, . The first model was a simple unstiffened plate as a baseline case to compare results to expected analytical responses. This served to validate the boundary conditions used and the plate modes.
The other models included stiffeners on the plate. Each case was modeled using different element types. The cases are listed below:
The plate was modeled with shell elements and the stiffeners were modeled with beam elements.
The plate was modeled with shell elements and the stiffeners were modeled with shell elements.
The plate was modeled with solid elements and the stiffeners were modeled with solid elements. This case was broken into two subcases as follows:
The solid elements were first-order reduced integration solid elements.
The solid elements were first-order full integration solid elements with incompatible modes.
Details about the plate geometry, materials, and common assumptions are provided in Section 2.2.1. Descriptions of each model can be found in Sections 2.2.2 to 2.2.5.
The following sections outline the modeling assumptions and methods used to create the finite element models.
A longitudinally-stiffened steel plate was assumed as the geometry for the analysis. The plate and stiffener dimensions are listed in Table . Five rectangular stiffeners running across the length of the plate were evenly spaced 20in. apart from each other. The two end stiffeners were 10in. from the edge of the plate. These dimensions were chosen for the geometry as being large enough to see plate modes at low frequencies.
Table Geometry Assumptions
The plate and the stiffeners were assumed to be HY-80 steel, commonly used for large structures. The properties are listed in Table .
Table Material Properties for Steel
Elastic Modulus, E
Poisson’s Ratio, ν
Mass Density, ρ
The stiffened plate was assumed to be simply supported on all sides. To represent this condition, the nodal displacements in the y-direction were fixed (forced to equal zero) for each edge as well as the rotations for the perpendicular direction to the edge . Figure uses the baseline model to illustrate how the boundary conditions were applied.
Figure Boundary Conditions on Baseline Model
The baseline model and the first two stiffened plate models used shell elements to represent the plate. Applying the boundary conditions to the edges is equivalent to applying them to the edges at the mid-plane location of the plate, since the 2D shell elements are located at the mid-plane of the plate’s thickness. To fix the edges of the solid element models, the boundary conditions were applied to the nodes located at the mid-plane of the three-dimensional plate thickness, as seen in Figure . This ensures that the boundary conditions are consistent between the models.
The finite element models needed to have a sufficient level of mesh refinement to capture the dynamic response of the plate throughout the frequency range. If there are not enough elements per wavelength, the waves of vibration will appear blocky, since the model cannot accurately represent the shape of the wave. This limitation is observed at higher frequencies, because the small wavelengths present at high frequencies cannot be resolved. Setting a maximum element size that ensures a minimum of twelve elements per wavelength throughout the frequency range is recommended by the Abaqus user guide, 
.To ensure sufficient mesh refinement, the element size was based on the bending wavelength in the plate at 1000 Hz. This was calculated using the equations for an infinite unstiffened plate . This was a conservative calculation since the stiffening added to the plate will increase the wavelengths, thus permitting larger elements than the model actually uses.
Element length for bending in the plate was calculated for both shell and solid elements using Equations 1, 2, and 3, .
Equation 1 calculates the bending stiffness, D, based on the material properties of the plate and the plate thickness. Equation 2 uses Equation 1 and the maximum frequency in the analysis range, f, to calculate the flexural wavenumber, kf. Equation 3 finds the flexural wavelength, λ. The full calculation is provided in Appendix A. The element length was calculated to be 1.633in at a frequency of 1000 Hz. This was rounded to 1.5in when creating the finite element models.
The compressional wavelength was also calculated for the solid elements. This calculation used Equations 4, 5, and 6, .
Equation 4 gives the compressional wave velocity, cp, based on the material properties of the plate. Equation 5 uses the compressional wave velocity to calculate the compressional wavenumber. Finally, Equation 6 calculates the compressional wavelength. The full calculation is provided in Appendix A. The element length was calculated to be 17.642in at a frequency of 1000 Hz. Since the element length required for bending was much smaller than the required element length for compression, all models were meshed to the bending wavelength.
For the model meshed with solid elements, four elements through the thickness of the plate and the stiffeners were modeled. This was to reduce hourglass effects caused by solid elements . It also helped to ensure that cross-sectional deformation effects were captured.
The baseline model was a simple plate, unstiffened, that was meshed to the same refinement as the rest of the models and simply supported on all edges. The standard shell element type in Abaqus, S4R, was used. Figure shows the meshed baseline model with the boundary conditions as displayed along the edges in Abaqus.
Figure Baseline Model
An eigen analysis was performed on the baseline model and compared to an analytical solution for an unstiffened simply-supported plate for validation. The results are discussed in Section 3.1.
The case 1 model was a stiffened plate modeled with the plate modeled using S4R shell elements and the stiffeners modeled using standard Abaqus B31 beam elements. Figure shows the meshed model with the boundary conditions. The red lines running along the plate are the beam elements representing the stiffeners.
Figure Shell Element Plate with Beam Stiffeners
Figure shows the model with the beam elements with their cross-sections visualized so the beam placement can be seen.
Figure Shell Element Plate with Beam Stiffeners (Beam Element Profile Displayed)
Beam elements are connected in the middle of the beam profile. To ensure the beam profile was correct, the beam elements were offset by half the thickness of the plate plus half the thickness of the beam. Figure demonstrates this offset.
Figure Beam Element Offset
In Figure (a), the offset from the midpoint of the beam profile to the plate is shown. Figure (b) shows how this offset causes the beam profile to match up with the plate edge when the plate thickness is visualized.
2.2.4Case Two Model
The case 2 model was the stiffened plate with both the plate and the stiffeners modeled using the standard Abaqus S4R shell elements. Figure shows this model with the boundary conditions displayed along the edges in Abaqus.
Figure Shell Element Plate with Shell Element Stiffeners
The case 3 model was the stiffened plate with the plate and the stiffeners modeled using solid elements. Figure shows this model with the boundary conditions displayed along the edges in Abaqus. The application of the boundary conditions to the solid model is described in Section 184.108.40.206.
Sub-case a) was modeled with C3D8R elements. These are first-order reduced integration elements. The reduced integration mitigates shear locking in the solid elements . Shear locking is the tendency of fully-integrated solid elements to be too stiff in bending. However, the reduced integration solid elements suffer from hourglassing, which causes them to be too soft . Abaqus inserts a small “hourglass stiffness” into the C3D8R element formulation to counteract this. Abaqus also recommends that solid models consisting of C3D8R elements be modeled with four elements through the thickness. Sub-case b) was modeled with C3D8I elements which are first-order full integration elements with incompatible modes. The incompatible modes formulation mitigates the shear locking that is common to fully integrated elements while maintaining high solution accuracy. Abaqus states that the C3D8I elements produce results that very closely match analytical solutions for high quality meshes (meshes with minimal distortion), . Both solid element cases share the same mesh, which is of high mesh quality and contains four elements through the thickness. This maintains compatibility with both the C3D8R and C3D8I element types effects and insure an accurate solution.
Figure Brick Element Plate with Brick Element Stiffeners
The mesh refinement across the plate is similar to the previous models except around the connections between the stiffeners and the plate. Figure shows the refinement in one of these regions. Figure also shows the four layers of elements modeled through the thickness of the plate and the stiffeners.