FEA software for extremely high aspect-ratio structure
FEA software for extremely high aspect-ratio structure
(OP)
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.
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.





RE: FEA software for extremely high aspect-ratio structure
RE: FEA software for extremely high aspect-ratio structure
RE: FEA software for extremely high aspect-ratio structure
i'd use a laminate material property to combine the different plies, i'm guessing you've got different ply directions.
RE: FEA software for extremely high aspect-ratio structure
RE: FEA software for extremely high aspect-ratio structure
RE: FEA software for extremely high aspect-ratio structure
RE: FEA software for extremely high aspect-ratio structure
RE: FEA software for extremely high aspect-ratio structure
RE: FEA software for extremely high aspect-ratio structure
RE: FEA software for extremely high aspect-ratio structure
Just my opinion, but some of the CAD/FEA bundled programs should be treated with caution. The risk is that you have users who are not necessarily familiar with stress analysis, with the apparent ability to generate a FEM.
Again, my opinion, but every FEM user should have a basic understanding of what a spring, beam, shell, solid, etc. element before trying to solve an engineering problem. From there, one could then move on to composites, etc. BUT only after a thorough understanding of the classical methods. Perhaps after that, one may consider a nonlinear solution. Otherwise, the risk is a GIGO scenario.
The challenge is that many companies/managers do not necessarily understand what "stress analysis" really means, but it does not start with FEM analysis and certainly is not a CAD to FEM approach.
The ironic thing is that once you really do have the ability to create a quality FEM and do quality stress analysis, you are not likely going to use something like the Solidworks bundle. This starts to beg the question of its true value, though I think for some problems, it can be useful.
Brian
www.espcomposites.com
RE: FEA software for extremely high aspect-ratio structure
If you are restricting yourself to solid elements, you are not necessarily using the right tools in your "FEM toolbox" for the job.
I will further agree with Brian than even if you are using one of these bolt-on packages, you should still understand a) solid mechanics and b) FE theory otherwise you are setting yourself up for a world of hurt.
For the structure you have which is very slender, solid elements are most inappropriate. Plate/shell elements will outperform solid elements every time. Some FE packages make use of solid elements for laminates and there are situations where this will offer advantages over plate/shell elements (with a computation cost) but for very thin structures, plate/shell elements with a laminate tool (showing ply information) is typically the best way to go. Be aware that plate element can have different formulations as well which will affect your results. (thick plate theory vs. thin plate theory for example)
It is also very important that the tool you choose should have good post-processing capability for showing results at each ply layer, maximum and minimum results throughout the laminate and ideally, an enveloping function to determine worst-case situations over multiple load cases.
Analyzing composite structure using FEA is a fairly advanced topic. It is a good idea to work through some of the mechanics by hand for simple loading situations and simple laminates to improve understanding of the problem.
Regards,
Aaron
RE: FEA software for extremely high aspect-ratio structure
However, (again my opinion), one should be well versed in the core usage first. That way, you can understand how to get the benefits of a CAD/FEM tool, while side stepping the pitfalls (which are many). For example, stress concentrations for various geometric configurations might be a good use for a CAD/FEM tool. Real composite analysis? Perhaps not.
Brian
www.espcomposites.com
RE: FEA software for extremely high aspect-ratio structure
If using solid mesh, the deformation in the test laminate is about 30% less than that in control laminate. However, if using shell mesh, the deformation in the test laminate is about 5% higher than that in control laminate.
Moreover, the absolute deformation is sensitive to mesh size.
Is this the fundamental limit of CAD/CAE, as Brain and Aaron mentioned? or something that I miss?
RE: FEA software for extremely high aspect-ratio structure
The question "which FEA software is the best" posed by 2LAI in my opinion is not correct, this is not a question of FEA software names, but the element type & analysis to use to model this problem to obtain accurate results.
Fisrt at all, this problem should be treated as nonlinear by the geometry, you have a very low thikness (0.2 mm), then you will have large displacements, so you need to account (depending loadings & constraints) for in-plane effects, stress stiffnening/softening effects, etc.. as you see this problem could be extremely nonlinear by the geometry.
Second, depending the element type used, you need to setup your mesh correctly. My fisrt model will be always 2-D Shell CQUAD4 elements (more when the problem is a laminate!!), you can use an element size of 4x4mm (20 times the thickness!!), and you will have a mesh of 500x250 = 125000 nodes & 125751 nodes, ie, more than 750000 DOF!!!. Please caution, for a nonlinear problem this is an important value, you will have to investigate loads & boundary conditions in order to see if any simplification by symmetry is possible to apply to the model.
As you see, to mesh the model with 3-D solid elements is not very adecuate for this problem, please have in mind that you need to set a minimun of two solid elements in the thickness, then you will end with millions of nodes & elements, not practical at all. And not to mention that this is a composite laminate problem, then depending the number of plies you will need to use more or less layers of solid elements, ...
In fact, you have different Modeling Methods to mesh Composite laminate problems:
1.- Using 3-D solid hexaedral CHEXA(8) elements for the core, and laminate 2-D CQUAD4 elements for the face sheets.
2.- Using plate 2-D CQUAD4 elements, which utilize classical plate theory to represent the core and face sheets, all in one property.
3.- Using a 2-D CQUAD4 laminate element which will encompass the face sheets as well as the core all in one property.
Every method have pros and cons, but with the model dimension of your problem, the best method is the Laminate. Also The laminate element can provide stress on a ply by ply bases as well as ply specific failure indices. Ply bond failure indices are also available with the laminate.
Here you are a sandwich composite tutorial (Honeycomb Panel) solved step-by-step using FEMAP & NX NASTRAN FEA code:
h
Best regards,
Blas.
~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director
IBERISA
48011 BILBAO (SPAIN)
WEB: http://www.iberisa.com
RE: FEA software for extremely high aspect-ratio structure
"Fisrt at all, this problem should be treated as nonlinear by the geometry, you have a very low thikness (0.2 mm), then you will have large displacements, so you need to account (depending loadings & constraints) for in-plane effects, stress stiffnening/softening effects, etc.. as you see this problem could be extremely nonlinear by the geometry."
That is not correct. The problem can very well be linear (and many times is). From the nonlinear deformation standpoint, most structure is "built up". For example, a composite cylinder, I-beam, etc., would generally be considered linear. Flat plate deformation, what you be thinking of, is generally a less common type of structure since it is so inefficient.
The effects of stress stiffening/softening do not necessarily occur just because of the aspect ratio and/or being composite. They "may" occur, but many times do not. Again, consider a cylinder or I-beam. That is not a likely scenario for stress stiffening. A problem like a "drum" would witness stress stiffening, but is not as common. But one cannot say that it will have these without first understanding the model. It is better to first understand why these effects may occur than to just toggle the nonlinear geometry button.
"Second, depending the element type used, you need to setup your mesh correctly. My fisrt model will be always 2-D Shell CQUAD4 elements (more when the problem is a laminate!!)"
Just because it is a laminate, does not mean that it would require more elements than an isotropic material. Many times the density should be comparable, but that will depend on the objective of the analysis.
Brian
www.espcomposites.com
RE: FEA software for extremely high aspect-ratio structure
In real life everything is nonlinear, and dynamic!!. Then is up the user to check if the obtained analysis results are accurate or not, one method is to compare the linear & nonlinear solution, and then you will see the accuracy of your FE model, you have the answer in your hands.
I invite everybody to be professional as much as possible, not to be happy with ONE solution, but to double-check results using different solutions (linear & nonlinear, static & dynamic) and also different element types (beam vs. shell vs. solid), check if the results are "mesh-dependant", questioning loads & BCs, etc.. Yes, I know it its difficult, but this is the tool we have, FEM/FEA, really powerful when used correctly!!.
Best regards,
Blas.
~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director
IBERISA
48011 BILBAO (SPAIN)
WEB: http://www.iberisa.com
RE: FEA software for extremely high aspect-ratio structure
Here are some other items that should be given consideration:
- "Engineering", by its very nature, is about making quality assumptions and idealizations. A "FEM engineer" may make run many combinations, but a "stress engineer" has no need to. He/she already has a good understanding of the problem and knows the proper way to idealize it as a FEM.
- We have a finite amount of time to solve problems. In my opinion, one is better off spending time to understand the physics/engineering of the problem, rather than running combinations of static, dyanamic, beam, shell, solid, linear, nonlinear, etc. You could go on for a very long time with this approach. To me, it would also indicate a lack of understanding the problem.
- It is not practical, nor necessary, to run many combinations, etc. The engineer may identify that a particular problem may have a DISTINCT form of non- linearity and address that. But I would discourage "random" types of parametric studies.
- In the end, the aerospace programs (as advanced as they are) do not run all of these combination type scenarios. This may or may not be indicative of other industries though since I do not have experience outside of the aerospace side. We rely on basic engineering and utilize the FEM to enhance our results at times. One must already know how to approach the FEM or else it is not started. Rather, the physics of the problem would be better understood and the FEM would only be used to help numerically solve the problem. The FEM will likely let you down if you do not already know what to expect and what type of solution to run, element to choose, etc., since the understanding has not caught up.
As I mentioned before, I don't think it is a good idea to start every problem by assuming it must be nonlinear or has stress stiffening/softening, etc. One should already understand if the problem has these effects and then very selectively identify each type of nonlinearity, etc. Just because we "can" run every possible combination and compare the results, does not mean that we "should".
Brian
www.espcomposites.com
RE: FEA software for extremely high aspect-ratio structure
www.Roshaz.com
RE: FEA software for extremely high aspect-ratio structure
To clarify I am not questioning anybody here, I want to be constructive, I don't like problems (I have a lot solving real life engineering problems!!), I just try to be of help using the "classical" approach, it seems not lucky, sorry.
Best regards,
Blas.
~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director
IBERISA
48011 BILBAO (SPAIN)
WEB: http://www.iberisa.com
RE: FEA software for extremely high aspect-ratio structure
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
www.espcomposites.com
RE: FEA software for extremely high aspect-ratio structure
RE: FEA software for extremely high aspect-ratio structure
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
www.espcomposites.com
RE: FEA software for extremely high aspect-ratio structure
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
RE: FEA software for extremely high aspect-ratio structure
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
www.espcomposites.com
RE: FEA software for extremely high aspect-ratio structure
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).
RE: FEA software for extremely high aspect-ratio structure
RE: FEA software for extremely high aspect-ratio structure
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
www.espcomposites.com
RE: FEA software for extremely high aspect-ratio structure
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) ??