How to analytically validate a large deformation analysis? 7

[noelieboy]

Dear all,

I am involved in writing a 3D large deformation finite element code, that uses 8-noded brick, linear elastic elements ONLY. I need to validate my solution against a simple problem that is solved analytically. For example a long thin (3D) rod that is held and one end and somehow highly loaded at the other, such that there is large deformation in the rod. Does anybody have such a sample problem with an analytical solution?

Or anybody got any other suggestions?

Experimental testing isn’t really an option.

Kind Regards, and Happy New Year!

 

[xerf]

My advice is to look in the documentation of a decent commercial FEM software. They usually include benchmark/verification examples of FE results compared to analytical/experimental solutions. In general the verification examples are quite specific so it would be difficult for me to indicate all the details of such an example.

You can google for the online documentation of ABAQUS.
It includes 2 manuals:
- ABAQUS Benchmarks Manual
- ABAQUS Verification Manual
where you can find typical verification problems.

For example:

http://lcadm.rrzn.uni-hannover.de:2080/

 

[prex]

For solutions of beams, circular plates and rectangular plates under large deformations you can look in the site below.

prex

http://www.xcalcs.com

Online tools for structural design

 

[israelkk]

http://users.cybercity.dk/~bcc25154/Webpage/largedeflection.htm

 

[GBor]

You may want to try

http://www.nafems.org

 

[prost]

Because of the inherent difficulties associated with large deformation analyses, there are only a handful of analytical large deformation solutions, unfortunately.

Maybe if you told us the material you wanted to model? A rubber? A nonlinear viscoelastic material?

I might have a few large deformation analytical solutions to help you if the material type is the same.

 

[noelieboy]

Firstly thanks to all that have replied thus far, very useful information. I am modelling a highly porous/ honeycomb/scaffold type structures. The actual material property type is limited to pure linear elastic, due to the limitations of the FE software we have developed. However I need to validate the solver for large deformations/buckling effects that occur. I am looking at the abaqus benchmark example of "2.1.2 Geometrically nonlinear analysis of a cantilever beam" from version 6.5. However, they do not give any information as to what the analytical solution should be for this particular example. The also found that "the element type C3D8 gives a very stiff responses", which unfortunately is the same element type as I use (8 node cubic element"

Does this imply that my choice of element type will probably limit my large deformation modeling capabilities? certainly looking at figure 2.1.2-1 it appear so (apologies to anyone without access to the abaqus benchmark manual 6.5)

Dear Prost,
My FE solver is limited to 3D linear elastic 8 noded cube elements only, while this constitutive behavior is probably a very simplified version of any true material behavior under large deformations, it is what I am looking for, for the purposes of my project, and is what I need an analytical solution for. If you think you have any model + solution that may be of use, I would be most appreciative

 

[JakeRAD]

The problem with large defomations is that a non linear material needs to be used to properly simulate the deformation. In your case an elasto-plastic material will be required. I'm assuming a non linear analysis is executed.

The best analytic solutions are available for simple beam cases, usually cantilever beams with a distributed or point load.
The nesh density is an important factor of high deformation analysis, so make your mesh properly dense.

 

[GregLocock]

Wow.

I've never heard that before. Are you telling me a Slinky doesn't operate in the elastic range? or a leaf spring? Because when we design springs we use geometrical non linearity, but assume materals are linear.



Cheers

Greg Locock

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[corus]

Looking in the Benchmark manual you'll find that there is a reference to the analytical solution, or at least who derived it. The solutions they give indicate that their results are close to that analytical solution so therefore you could use the results from Abaqus to verify your model.

The C3D8 elements won't give the correct result as they are linear and only one element is used through the thickness of the cantilever in their example, ie. for that element the stress is constant. In that case the element is overstiff, as they say. That doesn't mean to say the element is crap, it's just been used inappropriaitely.
In reality you'd be a fool to use only one element through the thickness for a bending problem.

As Greg points out, the problem is non-linear because of the large deformation, not because of material properties, which are linear.

corus

 

[torpen]

Hello,

You can do a single element test for a start and so check some work conjugate stress and strain measures for large strains.
The 8-node brick element has unit dimensions. The stress-strain relation is linear.
One face is fixed and on the opposite one a displacement is applied in such a way we have a uniform tensile state of stress.
To validate the results we view the end reaction force, stress and strain states (for several strain measures if available) to a given displacement.
And we compare them to a very simple analytical solution.

You can check with an another test (cantilever under intermediate load for example) wether the components of the stress tensor (of the elements at the end of the beam) do not change as result of a rigid body rotation.


Regards,

Torpen

 

[prost]

Perhaps my question should have been-what kinds of nonlinear materials do you have access to? This is not a trivial question, since if you don't have access to a particular material constitutive relationship inside your FEA program, then you'll have to develop the software to model that material yourself.