Abaqus - Variation of fundamental period with number of elements 1

[s_saranya]

I have created a 2D wire RC frame in ABAQUS of 3 bays in X direction. No of storey is 5. Column and beam are of rectangular sections. If the number of elements are increased while meshing, the fundamental period is increased. Can anyone tell the reason? Since the stiffness is increased by increasing the number of elements, the fundamental period should decrease right?

 

[FEA way]

Mesh must be sufficiently refined mainly to correctly capture higher modes of vibration but the first natural frequency may also vary slightly with mesh refinement. Too few elements tend to overstiffen the results which may lead to a higher frequency and lower period.

 

[s_saranya]

Can you please explain how few elements will overstiffen the structure in ABAQUS? In SAP it is exactly opposite. If the elements are many, stiffness will increase in SAP. I could not correlate both

 

[FEA way]

At least that's the case in stress analyses. It's a general property of the finite element solution but of course, modern FEA software may mitigate it in different ways. Here's a quote from "Finite Element Procedures" by Bathe:

(...) we observe that in the finite element solution the displacements are (on the "whole") underestimated and hence the stiffness of the mathematical model is (on the "whole") overestimated. (...) As the finite element discretization is refined (...) convergence to the exact solution (and stiffness) of the mathematical model is obtained.

 

[IceBreakerSours]

I am going by my recollection here but I was looking at convergence results using a few three-dimensional continuum elements in a particular commercial solid mechanics code and the convergence behavior differed in the elements. I haven't done the comparative analysis myself but the work was detailed enough to leave an impression on me.

*********************************************************
Are you new to this forum? If so, please read these FAQs:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[FEA way]

This is also discussed and shown in "Computational Structural Engineering. Automatic calculation of mechanical structures" by C. Gianini. This book uses examples from Abaqus. One of the tests clearly shows the difference caused by mesh refinement:

(...) lower mesh density in a finite element model tends to overestimate the stiffness of the structure. (...) we can see how the model with coarse mesh tends to have, generally, higher frequency values than the corresponding model with fine mesh, a clear indication that, mass being equal, the calculated stiffness is higher in the first case.

Also in "Building Better Products with Finite Element Analysis" by V. Adams it's advised to pay attention to mesh density when performing modal analyses:

(...) as with a displacement analysis, an overly coarse mesh will result in an overly stiff structure and fictitiously high modes. A modal analysis must be converged as any other structural study.

 

[s_saranya]

Thank for suggesting this book "Building Better Products with Finite Element Analysis" by V. Adams