# Validation of AISI Design of Cold-Formed Steel Beams Using Non-Linear Finite Element Analysis
## 2 Materials and Methods
### Abaqus
#### 2.3.2 Geometry Modeling and Material Properties  
Linear buckling analysis is performed as the first phase of numerical investigations. For this, eight AISI standard sections were modeled in ABAQUS, as per their geometric properties. The following are the key features of the materials and properties used for this study:  
Material grade, Fy = 380 MPa (55 ksi);  
Modulus of elasticity, E = 200 GPa (29,500 ksi);  
Poison ratio = 0.3;  
Unbraced length for torsional buckling = L/3. The length for each investigated section is taken from AISI Chart-II-1. The loads are applied at the L/4 distance from each end. To control the torsional buckling, lateral supports are provided at a spacing of L/3, and to control the general torsional effects, the loads are applied at the shear center. Two shell extruded sections are defined, one for the main channel section and the other for flat plate attached at the back of the channel. Element Type and Mesh Size  
The shell elements are chosen for both the main channel sections and for the plate attached at the back of channel. To initiate the analysis step, eight eigenvalues were requested, with 16 vectors and 300 maximum iterations. In this model, typically, the S4R element was used for meshing because of its effectiveness in capturing the behavior of structures such as plates, shells, and other thin-walled members. The S4R designation indicates a four-node doubly curved thin or thick shell element with reduced integration and hourglass control. To control mesh size sensitivity, initially, a coarser mesh size of 1 mm was provided, and finally, 0.25 mm was chosen for convergence with minimum computing effort. To perform the Riks analysis, a minimum of one eigenvalue is required; however, eight eigenvalues were used in this study because this number was sufficient to capture all buckling modes in relatively less time. Boundary Conditions and Loading Procedure  
For this research work, simply supported boundary conditions were applied at both ends relative to the major axis bending. Laterally, roller supports were provided at both ends and at the L/3 distance intermediately. Two unit point loads were applied at the L/4 distance from the ends. To avoid the twisting moments, loads were applied at the shear center. To achieve this, a flat plate of 5 mm thickness was attached to the back of the main C-section, along the depth of the section. The width of this plate was set equal to the distance from the shear center to the outer edge of the web. Initial Geometric Imperfections Modeling  
After the successful completion of step 1, the first eigenvalue was noted. The same model (Model-1) was copied as Model-2, and the following changes were made to it:  
The material properties were modified for step 2 (non-linear analysis), as shown below. For the plastic material properties, the parameters include:  
Yield stress = 380 MPa (55 ksi); plastic strain = 0;  
Yield stress = 517 MPa (75 ksi); plastic strain = 0.2. Then, the first eigenvalue noted in Model-1 was applied as a point load in Model-2. The boundary conditions were kept the same for the non-linear analysis; however, this step required the use of the modified Static-Riks method, thus mandating that the boundary conditions be assigned again. The Static-Riks step in ABAQUS is specialized type of analysis step used for solving non-linear problems, particularly those involving instability phenomena such as buckling or snap-through behavior; it is also used for the post-buckling behavior of structures. This approach is also known as the arc-length method. The Static-Riks step is primarily used for buckling analysis to capture the post-buckling behavior of structures. In the next step, the Model-2 input file keywords were modified with some additional text to capture the first mode behavior of Model-1. The following texts were added by using Model-2's Edit Keywords command at a specified location. *IMPERFACTION, FILE = JOB-1, STEP = 1  
Then, the new job was created and submitted for analysis.