FEA software for extremely high aspect-ratio structure 2

[2lai]

Hi,

I am going to do mechanical simulation of a laminate with extremely high aspect-ratio, i.e. 2 meter length, 1 meter width, and 0.2 millimeter thickness. I am wondering which FEA software is the best to deal with such model?

Thanks for the input.

 

[ESPcomposites]

Blas,

Thanks for sharing your opinions, they are welcome. I wanted to add some other opinions as well. As long as we are all respectful, that is fine. In this particular case, 2lai is still a newer user (from what I can tell). In that sense, it may be better to encourage fundamentals rather than "advanced" topics too early.

John,

Thanks for the comment. I think we are the same page as far as how we view FEM. In my case, some of my vantage point stems from practicing poor habits early only (relying too heavily on the FEM). Later, I realized it to be more effective to use FEM as an enhancement, but not as a crutch.

Brian

http://www.espcomposites.com

 

[2lai]

Thanks all for the input. It is interesting that I've run FEM for about a decade with solid mesh only! Regarding to the laminate, I probably have to do nonlinear simulation since the material properties of individual layer are temeprature dependent. With shell mesh, the static and nonlinear analysis generates different results. I guess it is more like an mathmatics issue rather than a physics one.

 

[ESPcomposites]

2lai,

For most stress analysts, the beam and shell elements are the "bread and butter" element choices. Solid elements are not as common since they are not a particularly good choice for many models. However, for some models, solid elements are required. The fact that you have never used a beam or shell element indicates that you may want to further expand your knowledge of FEM.

As Blas mentioned, in reality all models are nonlinear, though many can be idealized as linear. You say "With shell mesh, the static and nonlinear analysis generates different results." The way this is worded, it does not make sense. Since you can have a nonlinear static analysis, are you implying the analysis is dynamic? What is the form of non-linearity? Geometry (and what type), material, or other?

Composites, just as every other material, have temperature dependent properties (i.e. nonlinear). However, it is uncommon to analyze it is nonlinear just because of this. An exception would be a bond line anlaysis in a joint where the temperature dependent properties and plasticity significantly affect the response. But for general analysis, it is far more common to analyze with room temp properties and then apply "knockdowns" to to account for strength differences. Applying temperature dependent properties at each lamina, and solving as nonlinear, is probably reserved for a research solution.

Based on your comments, I would recommend further investigation into the analysis approaches of composites and FEM. Everything you have indicated seems to be far from the "norm". I think one of the more difficult things about composites is knowing what is important and what is not, and how to incorporate that into a FEM. If your company or industry does not have a lot of background in that, you can easily go in the wrong direction. If you don't have the right software (i.e. shell elements) and/or the direction based on industry solutions, it will be difficult to get a useful result. Good luck.



Brian

http://www.espcomposites.com

 

[2lai]

Brian,

In my case the coefficient of temperature expansion, cte, of individual layer is temperature dependent rather than linear. I used to do nonlinear analysis to estimate the stress evolution during thermal cycling. I don't know what is the best way to solve this problem using static analysis at several discrete temperature.

2lai

 

[ESPcomposites]

2lai,

If you really find it necessary to capture the nonlinear CTE mismatch, then you have no choice but to run a nonlinear analysis.

But the question is why are you doing such a thing? Sure, we understand that this may occur, but couldn't a linear approximation suffice? From an industry perspective, it would not be common to try to capture these forms of nonlinearites (unlike perhaps a research project).

Then, the next question becomes, how are you using these stresses? Some argue that these stresses relieve due to matrix creep and matrix cracking will even occur, but not have a significant affect to the laminate strength. So to go beyond this and try to capture a nonlinear CTE effect starts to question the value.

The other question is how are your allowables generated? Are you using lamina or laminate based properties and are you designing for structures with holes, bolts, or to allow for impact damage? If so, then may want to use laminate (and not lamina) based allowables, which may have the CTE mismatch "absorbed".

As you can see, there are some additional things to consider. One would have to further understand the problem and the objectives of the analysis to go much further. But what you are proposing does seem to be out of the norm, at least as an engineering solution.

Brian

http://www.espcomposites.com

 

[rb1957]

a solid mesh of something very thin would produse a begeesus (ie big, really big) number of elements, no?

a 2D mesh (shell, plate) elements would produce a much more reasonable number of elements.

what's the loading ? in-plane would probably produce reasonable linear results, out-of-plane (ie pressure) would immediately become geometrically nonlinear.

don't forget, your in-plane allowables are probably much less than ftu, fsu ('cause of buckling).

IMHO, keep solid elements for solid pieces (ie big, thick, chunky) and 2D elements for thin structures.

good job on testing your model ... i'd've thought the the 8 MPa material would be negligible compared to the 110 GPa. its only effect would be to space the 110 GPa plies (like core in a sandwich panel) and so increase the bending stiffness (from 1/4 squat to maybe 1/3 squat ... ie the bending stiffness of this membrane is always going to be low).

 

[2lai]

I created a simplified model whose dimension is about 1% of true laminate. The pressure loading is in perpendicular to the laminate. Will be interesting to know the difference between static and nonlinear solvers in dealing with the geometrically nonlinear problem.

 

[ESPcomposites]

I believe you mean to say difference between "static linear" and "static nonlinear". You seem to be implying that a nonlinear analysis cannot be static.

Whether or not you see a difference will depend on the boundary conditions, loading, etc. You should already have an idea of whether there is a significant geometric nonlinearity before running the model (and not the other way around). I think this has all been said before by now, but best of luck.

Brian

http://www.espcomposites.com

 

[rb1957]

there are essentially two types of static (and pretty much anything else) solution ... linear and non-linear. There are (at least) two primary non-linear effects ... material (yielding) and geometrical (large displacement).

spo,ething interesting i've noticed with fuselage models. you can model a shell (no stringers or frames) with 2D elements and get the expected results (hoop stress, etc). adding frames produces the expected results ... much higher radial stiffness at the frame location, unframed results mid-bay (if you have enough elements). adding the stringers is where things get wierd ... use rod elements and you get (essentially) the same results, use beam elements and all of a sudden each stringer bay (the skin between strginer and frames) starts acting like flat plates (with ridiculous displacements) ??