Reply To: Solution seems to be different from the experimental results

[peteroznewman]

Ryo, thank you for a detailed reply.

Changing Young’s modulus to make your model match the experimental Force-Deflection curve is not the correct approach, you should use the true values for the material. I think the discrepancy between your initial model and experiment is due to using a coarse mesh and overly idealizing the geometry and boundary conditions.

The baseplate of the column is likely bolted to the floor. If so, you should fix the bolt holes in the baseplate, not the entire basebplate surface, and use a compression only support to the bottom of the baseplate to allow the baseplate to deform.

You should find out the bolt torque used to tension the bolts in the gusset plate and use a bolt pretension. You should model the actual bolt hole diameter and bolt shank diameter. On the experimental curve, where the slope flattens out around 15 kN, that is probably the gusset plate slipping and the clearance between the holes and the bolts being taken up .When that is finished, the slope goes back to a steeper slope as the bolt shank carries the shear force by contact with the sides of the holes.

How many elements are meshed through the wall thickness of the gusset plate and the beam walls?  You need at least 4 linear elements through the thickness and 8 would be better in order for the plastic deformation to be properly represented. The bolt holes need more elements around the circumference, at least 12, and a small element size in the radial direction of each hole surface. You can use a mesh method of Inflation to cause that to happen. Or you can split the body using a cylindrical surface to create an annular ring of material around each hole so that a uniform mesh can be created around each bolt hole. If you split the body, use the Share button on the Workbench tab in SpaceClaim to create Shared Topology on each individual part (beam, gusset plate, column) to connect the mesh without using bonded contact.  Don’t use Share on the Assembly otherwise the mesh will connect between the parts and you don’t want that. Using the Inflation mesh method may be safer…

What is the actual conditions at the top of the vertical column?  You selected a face and set a displacement, which means that face cannot rotate, but if the true condition is simple contact against a rigid support, then that face should be allowed to rotate. You can do that with a Remote Displacement scoped to that face and then just set X to 0 and leave all others Free.  Is it valid to assume the top support is rigid?  What is the stiffness of that support?  Maybe you should use a spring to ground and enter the spring constant for that support. In that case, you don’t need a Remote Displacement.

What does the column, beam and gusset plate look like at the end of the experiment?  Did the parts buckle?  Please show a photograph if you can.  You can perform an Eigenvalue Buckling analysis on the column to predict the buckled shape, and add a tiny amount of that deformed shape to your Static Structural model to seed the structure with imperfect geometry, which is more realistic than the perfect geometry you have from CAD, before the loads are applied. That will also help the simulation more closely match the experimental result.