Learning Forum

[kariml229]

Dear All,

For more than a month I have read many discussions in that forum and searched on the Web. However, could not succeed.

I am analyzing a benchmark from the 1960s and trying to get the same failure and similar results.

I have modeled a plate girder with bearing and intermediate stiffeners as shown in the image.

1. Boundary conditions: It is a simply supported girder. The left end (with 152,4 mm offset to the inside ) is a pin and the right end (with 152,4 mm offset to the in) is a roller. I have provided Rigid body motion at the left pinned support in Z direction.
2. Meshing: I have used 50x50 mm mesh and in the geometry section, and parts are bonded using shared topology
3. Loading: Experimentally beam was tested under Pure bending by applying two point loads respectively in equal distances from center. Applied point load but in a spread option.Have not used plates not for complicating the model.I do not think it can be a problem,just excessive stresses in contact areas,even that is not happening since model fails to converge

In experiments 40KN of load is applied in each 5 minutes until it reaches 570kN and plastically fails. Web buckles with flange inducing

So,I tried to simulate everything as possible as it is,however, can not get any similar results.

I do have some doubts, I would be more than happy if any of you can clarify them

1.I do have convergency problems especially not at the beginning but, towards the end elements become highly distorted and it fails to convergence. I tried dividing the load into many small increments towards the end of the test, but it did not help. Tried to play with the values and increments, did not help at all. Any suggestions?

2. Since I have modeled using shell elements they do have orientations. I tried to create an element orientation under the geometry section and modify them, however, could not succeed,too. Since it is a girder plate just 90-degree oriented itslef,flange and stiffener plates, may be they are correct at default? Z directions are perpendicular to the surface,as far as I know. X and Z might be not aligned correctly. How to correctly orient them? Tried adpl code,did not work too

I am suspected of these two cases .I would highly appreciate and hint comment and advice. I am struggling with it for more than a month, searching the web, checked many comment and discussions from here, too but could not succeeded

[peteroznewman]

The physical test of the plate girder failed when the web and flange buckled. That was probably induced by the parts having some small variation from a perfect shape. Your simulated parts have a perfect shape so don't initiate a bucking failure without some help. There are a few methods to create model geometry with some small variation. One method is to run a buckling analysis, then add a small fraction of the buckled shape to the perfect geometry. When you do that, the failure can be induced closer to the experimental result. You can put in a larger fraction of the buckled shape to induce the failure at lower loads.
Since you have an isotropic material, you don't need to worry about shell element orientation, that is only a concern when using orthotropic materials.

[kariml229]

Dear Peter Thanks for your immediate answer. Thanks for your clarification about shell elements!
Well, I have used the real dimensions which I obtained from the laboratory test data, but the variation can , occur as you mentioned. The result of the flange-induced web buckling, in reality, is the depth to thickness ratio of the web which is 1270(mm)/3.27(mm). So, I expect that failure when modeling, too. In that case, I considered the web thickness to height ratio to be my "help" for getting the buckling failure, since that is the main reason. Do you think that is not enough, still?

[peteroznewman]

Dear Kari
No, it's not enough. Here is an old discussion on Buckling: https://forum.ansys.com/discussion/12847/buckling-in-static-structural
You have to use some method to induce the buckling when your load is centered with no eccentricity and when the geometry is perfect. You also must turn on Large Deflection under Analysis Settings.
https://www.youtube.com/watch?v=Wc3Eukyl4KQ&ab_channel=AnsysLearning
https://courses.ansys.com/index.php/courses/structural-instabilities/
Here is a post on adding a fraction of displacement from the Eigenvalue Buckling analysis to a Static Structural analysis: https://forum.ansys.com/discussion/24250/initial-imperfection-and-scale-factor

[kariml229]

Many thanks for your help, Peter!
I will try these advices and see what will happen!