×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Are you an
Engineering professional?
Join Eng-Tips Forums!
• Talk With Other Members
• Be Notified Of Responses
• Keyword Search
Favorite Forums
• Automated Signatures
• Best Of All, It's Free!

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Strains in shell and birck elements

Strains in shell and birck elements

(OP)
Hi to everyone,

I am an aerospace stress engineer and I need support in the following question:

I modeled a beam fixed-free, two times, in hypermesh:
First, with shell elements and the second one with brick elements.
Then, I applied the same vertical load at each free side of beams and I ran the model with a sol101 in Nastran.

Now, I'm looking the output with hyperview and I see somethings doesn't feel right:
I have, in the same points, the same stress values in beam direction (and in the other directions) for both the beams, and these values are also in according to the values that I find using the classical beam theory.

The problem is that I find at the same points different strains between the two beams (shell and brick).

So I did this check:

i applied the stress-strain relationship (sigma =E*eps) to find the stress in beam direction by the strain in this direction:

the stress calculated by the solid beam strain (in beam direction) are in according to the stress values for classical theory and in according with the stress result by the FEM.

But, obliviosly, the shell beam strain output and stress strain relationship give me a wrong values.

Why does this happen?

Replies continue below

RE: Strains in shell and birck elements

shear strains (in the beam, not in the 3D model) ?

it does seem "odd" to model something (a slab ?) as a shell and also as a solid. The shell collapses the thru thickness freedom (that the 3D model models); a shell has not analytical thickness, the 3D model has actual thickness. The fact at the stresses are consistent says that the shell element code is correctly accounting for things not modelled.

I imagine your stress/strain relationship is "wrong". In the first place there are probably 3D strains. In the second place I'd apply (or at least read up) the element coding ... how does the element convert strain to stress, both shell and 3D. Remember these elements typically assume a strain function (linear of a 4 node shell, parabolic for a 8 node shell) and stress is calculated from strain. And not necessarily stress = E*strain ... often they hide "easter eggs" there, factors accounting for other effects.

"Hoffen wir mal, dass alles gut geht !"
General Paulus, Nov 1942, outside Stalingrad after the launch of Operation Uranus.

RE: Strains in shell and birck elements

what I think you should be doing, if you're learning a code, or just getting used to it, is run some single element tests to see how the elements respond to different loads.

"Hoffen wir mal, dass alles gut geht !"
General Paulus, Nov 1942, outside Stalingrad after the launch of Operation Uranus.

RE: Strains in shell and birck elements

Shells are tricky in terms of results interpretation (especially when it comes to the components of stress and strain tensors). Depending on the software, they may use local directions (so, for example, σ_x in a shell model may not be the same thing as σ_x in a solid model), output can be displayed at different integration points through the thickness (or in form of an envelope) and split into the membrane and bending contributions, there might be additional output variables approximating results that can't be calculated directly because of the way shells are formulated (e.g. transverse shear stress estimates) and so on. You should be really careful when comparing the results obtained with solid and shell elements.

If you want us to help more, please share the results.

RE: Strains in shell and birck elements

(OP)
Sincerely Thanks to everyone for the support.
I have just founded the solution; I was looking only at membrane strain and not at bending strain component (as FEA way He advised to do).

RE: Strains in shell and birck elements

" Remember these elements typically assume a strain function (linear of a 4 node shell, parabolic for a 8 node shell) and stress is calculated from strain."
Elements in solid mechanics use displacement and rotation interpolants in elements. In post-processing, the definitions of stress resultants (bending, twisting, shear, normal forces) - which are functions of derivatives of displacement and sometimes also rotation - for the applied dimension reduction model (bar, beam, plate, membrane, shell) are used to evaluate the stress resultants in each element and at nodes. Finally, normal stresses and shear stresses are evaluated by utilizing their definitions (functions of bending, shear etc.). Stress invariants (e.g., von Mises stress) are calculated in the final steps before display of results.

In the 3D model, no dimension reduction is performed and thus 3D kinematical (displacement-strain) and constitutive (strain-stress) relations are directly applied to give normal stresses, shear stresses and invariants.

Mixed models deviate from this, but they are rarely applied in commercial FEA software.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

• Talk To Other Members
• Notification Of Responses To Questions
• Favorite Forums One Click Access
• Keyword Search Of All Posts, And More...

Register now while it's still free!