Learning Forum

[Diar]

Dears,

I am using Ansys Workbench 2020 R1 Academic to verify experimental results of a stiffened plate girder subject to nonlinear buckling. 

Everything looks fine, but I am struggling with an issue which is the load-deflection curve of the FEM results do not match with the experimental results.

I have plotted the results as you can see in the attachment. The shapes of the curves look very similar but the values of the FEM modelling is far less than that of the experimental results.

What do you think the reasons might be?

[peteroznewman]

ANSYS staff are not permitted to open attachments. Please use the Insert Image button in future posts (in addition to attaching file) as I have done for you in your post.

Please describe fully the model fully including: column geometry with any initial geometry imperfection, the material model used, the boundary conditions in the model including any eccentricity.

Then describe fully the experimental setup. What were the end conditions of the column in the lab?

The reasons the FEM result could be less than the experimental buckling load is if you have less support than the experiment, for example, you have pinned end conditions in the model while the experiment end condition is closer to fixed.

 

[Diar]

The experimental setup of the stiffened plate girder is an I section as you can see below

Modelled the geometry in DesignModeler and assigned supports as follows:

1. left support is simple support (ux, uy, roty and rotz = 0; uz and rotx = free)

2. right support is hinged support (ux, uy, uz, roty, rotz = 0; rotx = free)

3. used frictionless support at the top flange (to prevent rigid body motion)

For the analysis I have done the following:

1. carried out a static structural analysis and Eigenvalue Buckling analysis

      a. Material properties: nonlinear

      b. Meshing: sweep method with face sizing (to model the whole girder using solidshell 190 element)

      c. Loading: assigned a unit load in order to perform the Eigenvalue Buckling analysis.

2. inserted the results of mode 1 of the Eigenvalue buckling analysis as initial imperfection for the nonlinear buckling analysis

      a. linked (engineering data, geometry and model) from static structural analysis to Eigenvalue buckling analysis

      b. linked solution of the static structural analysis with the setup of the Eigenvalue buckling analysis

3. For the nonlinear buckling analysis I did the following:

      a. linked engineering data from the Eigenvalue analysis to the nonlinear static structural analysis

      b. linked the solution of the Eigenvalue analysis with the model of the nonlinear static structural analysis

      c. did the following for the step controls: step end time 100s; initial substeps:100; min substeps:50; maximum substeps:200; large deflection: on

      d. force: defined by Y component

4. copied direction deformation (y-axis) with the support reaction and plotted experimental and FEM load-deflection curves for comparison.

[Diar]

As you have mentioned, the issue was related to the support type. I have assigned fixed support at the ends and managed to get the following graph:

Although the linear part has a very good match, the nonlinear part is not so well matched.

I have put a tangent modulus of about 10% of the Young's modulus value and have played with it ranging from 10% to 1% but the change is not that significant in the nonlinear buckled part.

If you have a close look at the plateau of the experimental curve, you can see that the slope of the line is almost flat. But the FEM model shows an increase in the slope regardless of changing support type, material properties (in this case E and tangent modulus) and even loading (including increasing number of substeps).

What might be the issue for this? I really appreciate your positive feedback, thanks.

[peteroznewman]

Simulation = 492 kN.  Experiment = 458 kN.   Error = 7%.  Declare victory and go have a drink to celebrate.

[Diar]

Many thanks for your feedback, much appreciated!