Engineering

Finite element analysis of beambracketProblem Statement:

A static structural and linear buckling analysis of a “Beam Bracket” was carried out for assessing its safety factors. The bracket is made of structural steel with given material properties.

 

 

Young’s Modulus 200 GPa
Poisson’s Ratio 0.3
Yield Strength 250 MPa

 

The “Beam Bracket” consists of a seat plate (flange) and a web plate. The bracket is design to withstand a load of 27 kN, which is assumed to be uniformly distributed over the seat plate.

This analysis is carried out to check:

  • Would the maximum stress excess the allowable stress?
  • Would the web plate buckle under the load?

Problem Statement

 

 

1. Static Structural Analysis of a solid model:

The static structural analysis of the solid model was performed with the following mesh parameters and boundary conditions.

Step 1: In first step the analysis is carried out by the default mesh settings, a 27 kN force is applied on seat plate in downward direction and the fixed support is provided to the back part of the web plate. The problem was solved for Total deformation, Equivalent Stress, Structural Error and Safety Factor.

Total Deformation:

Total deformation beam

 

Equivalent Stress:

Equivalent Stress

 

Safety Factor:

Safety Factor

 

Structural Error:

Structural Factor 

 

The structural error can be used as an indicator of global mesh adequacy as well as local mesh adequacy, in general the structural error should be as small as possible, and at the same time, its distribution should be as uniform as possible.

So for decreasing the structural error, mesh quality should be improved, we refine the mesh and applied the “multi zone method” for mesh control. The meshed model and its parameters are shown below in fig 6:

Meshed Model

 

After refining the mesh, we obtained the results as shown below:

Total Deformation:

 Total deformation after refining the mesh

 

Equivalent Stress:

Equivalent stress after refining the mesh

 

Safety Factor:

Safety factor after refining the mesh

 

Structural Error:

Structural error after refining the mesh

                 

Conclusion:

Solution accuracy depends on the mesh quality,in this case the solutions obtained after refining the mesh were more accurate than the previous solutions. Here, we applied a “multi zone” meshing method for achieving a high quality meshing and accurate solution, and we obtained the more accurate value for total deformation, equivalent stress, safety factor and the structural error reduces 1/4th of the previous one. This shows that higher the mesh quality, more accurate the results.


2. Static Structural Analysis of a Surface Model:

Since the seat plate (flange) and the web plate are relatively thin and have uniform thicknesses, we again model the beam bracket as a surface body, solve it by applying same boundary conditions and default mesh settings and then compare its solutions from the solid model.


Total Deformation:


Total Deformation by Static Structural Analysis

Equivalent Stress:

Equivalent Stress by static structural analysis

 

Safety Factor:

Safety Factor by Static Structural Analysis


Structural Error:

Structural Error by Static Structural Analysis 

 

 

Surface Model vs Solid Model:

The results we obtained for the solid model are quite comparable to the results we obtained for the surface model. The surface model in this case consist of about 1000 nodes while the solid model consist of 15000 nodes.

Hence before approaching to the solid modelling, we should first consider the surface/line modelling.

The maximum stress obtained is 83.267 MPa in solid model and 77.559 MPa in surface model which is less than the yield strength value i.e. 250 MPa, hence the structure is safe under the design load.

 

 

Linear Buckling Analysis of Beam Bracket:

In this analysis process, we analyze the structure under compressive load to make sure that, under the design load, the web does not buckle. The mesh parameters and the boundary conditions for the problem would be same as of above. The analysis was performed to find the total deformation under two modes.

 

Total Deformation Mode 1:

Total Deformation mode 1

Total Deformation Mode 2:

 

Total deformation mode 2

                   

Final Deduction:

The load multiplier can be viewed as a safety factor. It predicts that 203 times of design load will initiate the buckling. Hence the structure is safe.