Simply supported plate girder modelled using shell elements. Consecutive problems getting of results
May 11, 2022 at 6:02 pmkariml229Subscriber
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.
- 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.
- Meshing: I have used 50x50 mm mesh and in the geometry section, and parts are bonded using shared topology
- 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 succeededMay 11, 2022 at 10:16 pmpeteroznewmanSubscriberThe 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.
May 12, 2022 at 10:14 amkariml229SubscriberDear 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?
May 12, 2022 at 10:36 ampeteroznewmanSubscriberDear 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.
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
May 12, 2022 at 10:46 amkariml229SubscriberMany thanks for your help, Peter!
I will try these advices and see what will happen!
Viewing 4 reply threads
Ansys Innovation Space
- The topic ‘Simply supported plate girder modelled using shell elements. Consecutive problems getting of results’ is closed to new replies.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.Trending discussions
- How to do the frequency response of the nonlinear vibration of a flexible PCB?
- Importing Line and Solid Bodies from SpaceClaim to Mechanical
- how to open SendCommand in Ansys
- problems facing during solution
- Still facing the same issue
- Failed to move file from solver directory to scratch directory: file.rst
- Adaptive Sizing
- Stiffness factor
- Import DAT file
- Import pressure data (coordinates and value) to ansys workbench through excel
Top Rated Tags
© 2023 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.