2D FEM for plate bending

[pt75]

Hello,
I'm trying to set up a software tool for plate bending analysis that in the future should account for non linear and plastic deformation, too.
At present I've implemented the calculations as described here 2D FEM, in a rectangular domain. In order to validate the tool, I used a 1cmx1cm square section bar, 1m long, with prescribed displacement zero at corners, and prescribed load at center, comparing the maximum deflection with that calculated with Bernoulli beam formula.
Unfortunately, the results are very different, being the formula value 10 times bigger of the simulated one.
So my question is:
Is there some methodological flaw in my model? Can a 2D model like this used in this way? Or should I look for a bug in the implementation?
Thank you very much for your help.

 

[klaus.]

Are you a student ??

 

[Erik Panos Kostson]

I think it is better to start with some standard and common tests (bending of shells and membranes - single element test and multiple elements) that are really good for trying and testing a FE script/tool/programme.

https://www.nafems.org/publications/browse_buy/browse_by_topic/benchmark/p01/

https://www.nafems.org/publications/browse_buy/browse_by_topic/benchmark/p18/

PS: The link refers to 2D elements that can be used for plane 2D FEA and not bending of plates which has a different formulation, which say could be achieved by combining the membrane action of a plane stress CST formulation of a TRI3 (as the link describes), and a separate bending action/formulation of a TRI3 which can be quite involved. So it can have two parts.

Thus do a plane membrane stress/strain 2D benchmark (only UX, and UY dof, no out of plane dof or rotations) for your programme (plenty of those in the above benchmarks)

 

[Shu Jiang PEng SE]

You may use constant-strain triangle (CST) elements for the simulation. The type element does not work well, especially used for to simulate “soft” material. You can try using Quadratic triangle (LST) element or other type element.

 

[prex]

Is there some methodological flaw in my model?

We don't know your model, how could we judge?

Can a 2D model like this used in this way?

Yes

Or should I look for a bug in the implementation?

Likely yes

prex
[URL unfurl="true"]http://www.xcalcs.com[/url] : Online engineering calculations
[URL unfurl="true"]https://www.megamag.it[/url] : Magnetic brakes and launchers for fun rides
[URL unfurl="true"]https://www.levitans.com[/url] : Air bearing pads

 

[Erik Panos Kostson]

As mentioned if you want flat shell elements that usually can have both inplane membrane actions and bending you would need to add the bending part to the 2d plane formulation shown in the 2Dfea link in your post. A good explanation on how to do that can be found in.

Development of Membrane, Plate and Flat Shell Elements in Java - ...
PDFciteseerx.ist.psu.edu › viewdoc › download
by K Kansara · 2004 · Cited by 12 · Related articles
membrane elements developed are the constant strain triangle

 

[IDS]

If properly formulated a plate bending element should give deflection results close to a beam element and classical beam bending theory.

Are you sure your units are right? Results out by a factor of 10 are always suspicious, especially if you are using SI units.

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[Erik Panos Kostson]

If you have the plane stress element implemented then you can check bending against beam theory for a beam made of plane stress elements deflecting along the thick direction and in plane. The discussion below (from another post by me) is on the similarity for a beam elememt and plane stress and flat shell representation of cantilever and pinned member in plane bending.

"think it is better to start with a simple elastic bending test. The uploaded figure shows a linear elastic cantilever beam element with an end force (top element in the image), a linear elastic plane stress QUAD4 mesh in the middle (cantilever also), and finally a flat shell/plate (cantilever) QUAD4 mesh at the bottom of the image all giving the same end-displacements (

https://imgur.com/a/6IYawiG),

as it should be.

If you look on stresses though at an inbuilt/fixed end on a shell/2D mesh, there is a stress singularity there which is mesh dependent, so it would be better to compare NL-FEA results for a pinned-pinned beam and look at the plastic hinge forming in the centre/mid span instead (there is no singularity there).

If we do that there is no mesh dependency and the stresses are the same for all meshes (beam, plane stress, and flat shell/plate - see uploaded image below), thus the force needed to go plastic at the centre, is the same for all meshes there, at least for geometrically linear analysis like in this example.

https://imgur.com/a/vMlmhqd

"

 

[Erik Panos Kostson]

I hope it goes well with your work. If you feel confident with linear FEA and have implemented the elements you need, and decide to do material nonlinear, then there is a very good benchmark in the Strand7 verification manual.

The benchmark is about calculating (material nonlinear analysis/arc length sub-steps, no geometric nonlinearities, in order to compare to easy hand calcs.) the plastic hinge in the centre of a pinned beam (modelled with beam elements) with a point load midspan (in plane bending). Section is square solid (B:10 mm x H:10 mm), and 1 m long. The plastic point force at midspan (to hinge the centre) is thus 1000 N (plastic force=(B^3*Yield stress/Length). E=1E5 MPa, v=0, Yield = 1000 MPa.

The results are the same for the beam elements and the shell elements (1000 N for the plastic hinge to form at the centre). Picture (Y axis is point force magnitude, and x is deformations in Y at midspan, curve goes almost flat when hinge forms, at about 1000 N, as in theory):

https://imgur.com/a/ynQZDYO

&

https://imgur.com/a/vDvsFYs.

All the best

 

[bkal]

It seems to me that there is a confusion between plate bending and your FE set-up: your link points to 2D membrane elements, I am not sure how do you intend to use them in a plate bending case. In addition, your example (0.01m*0.01m x 1m) hardly looks like a plate bending problem. Could you send a sketch of your example showing loading and boundary conditions, your FE mesh and also the results you are comparing.

 

[gugaluz]

Hello pt75,

The link you posted presents the formulation for Plane Stress or Plane Strain, not plate bending element. The formulation for Plate Bending is much more complex. Anyway, did you fixed your problem? Answer here, otherwise.