Bead optimization adds stiffening beads to a shell structure to increase the moment of inertia, which leads to a greater stiffness or higher eigenfrequencies. The resulting beads are easy to reproduce in a sheet metal stamping process and add no mass and little cost to the finished product.

Figure 1: Seven cases (in order) analyzed for their response to blast loading

VIDEOS 1 & 2: Bead optimization (left) and response to blast loading for case 6

Bead optimization supports two algorithms—the general algorithm, which is more flexible and can be applied to most problems but does not generate a distinct bead pattern, and the condition-based algorithm, which is more efficient at creating beads but has limited capabilities. Unlike the regular circular beads generated by the condition-based algorithm, the seemingly random bead structure generated by the general algorithm can be hard to manufacture. The condition-based algorithm supports only strain energy (a measure of stiffness) or eigenfrequency as the objective function and the bead height as an equality constraint. It always uses three design cycles and the bead width value can either be specified or a default value can be used.

In this example, condition-based bead optimization has been performed using Tosca for Abaqus and Isight to maximize the blast resistance of a plate structure without adding mass. The 2 m square plate is firmly clamped on all four sides and is constructed of 25 mm thick steel (elastic-plastic material model). Since the plate thickness is significantly smaller than any other global dimensions, shell elements can be used to model the plate. The response of this plate subjected to a blast loading in Abaqus/Explicit is analyzed for seven different cases shown in figure 1. Three equally spaced stiffeners are welded to the plate for case 2. The stiffeners are made from 12.5 mm thick plate and have a depth of 100 mm. 

Figure 2: Isight optimization to obtain an equivalent pressure load

Since the condition-based algorithm for bead optimization only supports a linear static procedure, downhill simplex optimization technique in Isight (figure 2) is used to obtain a value of pressure load that would generate the same maximum deformation of the central node in a linear static analysis as the maximum deformation of that node due to blast loading in a dynamic explicit analysis. This equivalent linear static model is used for bead optimization in cases 3-7. The optimized geometries from each of these cases are analyzed with a dynamic explicit procedure to assess their response to blast loading.

Figure 3: Isight optimization of bead height and width to obtain minimum deformation of the central node

User specified bead dimensions are used for bead optimization in cases 3-6. In order to maximize the plate stiffness, Isight is used to optimize the bead width and height in case 7 (figure 3) to produce a bead optimized plate that results in the least deformation of the central node.

Table 1: Comparison of maximum response of the central node to blast loading for the seven cases

Figure 4: Comparison of response of the central node to blast loading for the seven cases

Figure 5: Comparison of plate stresses prior to the optimization (left - case 1) and after the introduction of the stiffening beads (right - case 7) at 0.008 seconds

The comparison of response of the central node to blast loading for the seven cases has been shown in table 1 and figure 4. Note that the addition of stiffeners to the plate causes a reduction of 9.2% (case 2) in the maximum deformation of the central node when subjected to blast loading, whereas bead optimization with bead width and depth optimized by Isight causes a reduction of 92.6% (case 7)! Figure 5 shows a comparison of plate stresses prior to the optimization (case 1) and after the introduction of the stiffening beads (case 7) at 0.008 seconds.

This is an example model for the purpose of demonstration only. Refer to the Abaqus documentation more information on this topic.

All model files are attached (you will need to configure the file locations for the Isight models).

Other posts you might find useful:

1. Modeling Grains of Complex Shapes and Particle Fragmentation using Discrete Element Method (DEM) in Abaqus

2.Particle Methods in Abaqus: DEM vs. SPH [Webinar]

3. Mesh-to-Mesh Solution Mapping in Abaqus to Simulate Sharp Indentation Using Python Scripting and User Element Subroutine

4. New to Abaqus? Try this tutorial video with step-by-step instructions to simulate bending of a cantilever beam!

5. Getting Started with Discrete Element Method in Abaqus (with and without Particle Generator)

6. Low-Cycle Fatigue Analysis of 316LN Stainless Steel Rebars using Abaqus, Isight and fe-safe

7. Thermo-Mechanical Abaqus Simulation of Friction Drilling Process based on Isight Optimization and Data Matching

8. Introduction to Finite Element Analysis with Abaqus - eSeminar Playback