Why displacement formulation always lead to over stiff representation of the structure? 2

[JBlack68]

To all,

While doing some reading on FE related matters I came across the statement: displacement formulation always lead to over stiff representation of the structure

While I am fully aware of the issue of elements such as the 4-nodes tetra (the famous TET4) being too stiff and requiring a fine mesh to be effective/accurate why is the general statement made above ?

I understand from that statement that all displacement-based elements are inherently too stiff: Why is that? Is it in opposition to the hybrid formulation of the element stiffness?

Thanks
Regards

 

[Mustaine3]

What's the source of this general statement?

I'm working with Abaqus since many years and I've never heared of that - and this does not only include Abaqus.

 

[JBlack68]

It was in an (old) book issued the NAFEMS organisation
incidentally some "random" web searched produced this link
[URL unfurl="true"]http://www.twi-global.com/technical-knowledge/faqs/structural-integrity-faqs/faq-what-is-reduced-integration-in-the-context-of-finite-element-analysis/[/url]

where the statement is repeated

 

[rb1957]

Ithink it goes to the basic formulation of the elements. There is a basic assumption underlying how an element produces results. In a 4 node quad the typical assumption (most common displacement based elements) is displacement is linear, the alternative assumption (in rarely found stress based elements) is that stress is linear. I think this is a Beta/VHS type of thing ... one is notionally better but one rules the market place. In 8 node quad the assumption is that displacement is quadratic and this I think gives "better" results.

another day in paradise, or is paradise one day closer ?

 

[Denial]

In very basic terms, my understanding of the basis for this statement is as follows.

Imposing a restraint on a structure will never decrease its overall stiffness, and will usually increase its overall stiffness.[ ] When you set up an FE model of a structure you discretise it into a set of finite elements.[ ] Within each of these finite elements you impose a (mathematical) restraint that its displacement field will be described by a set of parabolic or cubic or quintic or hyperbolic or whatever equations.[ ] Left to its own devices, the element's displacement field would prefer to adopt a slightly different displacement field.[ ] So this mathematical restraint will "artificially" stiffen the overall structure.[ ] If the assumed displacement field is a good approximation to the actual displacement field, the amount of artificial stiffening will be small.

 

[gravityandinertia]

It's much simpler than you think.

When we discretize our geometry into some number of elements,that number of elements is always significantly less than the number of atoms/molecules that actually make up the material. As a result, fewer degrees-of-freedom in the model, make for a more stiff model than reality which has more degrees-of-freedom to move.

When we are building FEA models, and performing convergence checks, we are trying to determine the size of the mesh that is small enough to represent the actual system to our desired level of precision.

 

[Mustaine3]

It was in an (old) book issued the NAFEMS organisation
incidentally some "random" web searched produced this link

http://www.twi-global.com/technical...on-in-the-context-of-finite-element-analysis/

where the statement is repeated

That section may point toward volumetric locking, where fully integrated elements might have to many 'constraints' when the incompressibility needs also to be enforced.

 

[JBlack68]

Thanks to all for the input. I think the original statement I queried must be an "historical" thing. As most (all)general FE code used elements based on a displacement formulation - I have never used the so-called hybrid formulation, in the original work done (years and years ago) when computer power limited the number of elements one must have noticed (benchmark type of study) that the error and convergence rate was such that the "over-stiff" structure became apparent. I do not think that one will find a "mathematical" proof that a displacement formulation lead to an overestimated [K] matrix.

 

[ESPcomposites]

I thought Denial provided a good description. The FEM has less DOF than an actual structure. It has nothing to do being a "historical" thing. It is well known that displacements based FEM solutions are overly stiff (based on the physical nature of the solution). You just mitigate this by using enough elements to get a result that is within a few percent of the actual response (convergence). The "historical" difference is that it was more difficult to obtain convergence with less computing power. In the early days, they were using models with about 10-100 elements to keep the solve times (and set up times) manageable - hence more awareness of it being "overly stiff" by nature. Nowadays, you usually plenty of elements to obtain displacement convergence and its not such a big that it is still "overly stiff".

Brian

http://www.espcomposites.com