To find the deflection of a steel I-section using shell elements in ANSYS APDL, first define keypoints to model the I-section geometry (flanges and web). Use areas to build the cross-section and extrude it along the beam length. Assign material properties (e.g., EX, PR) and real constants for shell elements like SHELL181. Apply meshing with adequate refinement. Define boundary conditions to simulate simple supports (e.g., UX=UY=UZ=0 at one end, UX=UZ=0 at the other). Apply the UDL as surface pressure on the top flange. Solve the model, then use PLNSOL,U,Y to plot or extract deflection at midspan.

Carlos Francisco Lucena Gonzalez Sir few of more doubts regarding your mentioned answer.

1. How should I join flanges and web together as they are the shell elements made separately, and they gets separate out in deflections.

2. The surface pressure to be applied is on to the lines, elements or areas of the top flange?

How should I join flanges and web together as they are the shell elements made separately, and they get separated out in deflections?

This issue is common when modeling parts of a section (like flanges and web) independently with shell elements. Here's how to ensure proper connectivity:

• Use shared lines/areas when creating the geometry: When building the areas for flanges and web, make sure their edges are coincident. That way, when meshed, they’ll share nodes along the common edges. If you’ve already created them separately and they don’t share nodes, use the command: NUMMRG,NODE This merges coincident nodes (within tolerance), ensuring connectivity between the flange and web.
• Additionally, you can run: EGEN or EASMBL if you're using copying/array operations, to ensure that elements are correctly generated and connected.
• Mesh carefully so that the mesh lines up between parts. If one area is more refined than the other, they may not share nodes unless mesh controls are set.

The surface pressure to be applied is on to the lines, elements, or areas of the top flange?

Since you're using shell elements (like SHELL181), pressure can be applied in a couple of ways, but the most correct and common method is:

• Apply surface pressure on elements (top face of top flange): SFE, ALL, 1, PRES, , value ALL: select the elements of the top flange 1: refers to the face number (for SHELL181, face 1 is the top surface) value: magnitude of the uniformly distributed load (UDL)

Alternatively, you can apply pressure directly on areas before meshing using: SFL, area_id, PRES, value

But in practice, when using shell elements, applying pressure on the element face (SFE) is more precise, especially after meshing.