Tek-Tips is the largest IT community on the Internet today!
Members share and learn making Tek-Tips Forums the best source of peer-reviewed technical information on the Internet!
-
Congratulations cowski on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!
FEA software for extremely high aspect-ratio structure 2
- Thread starter 2lai
- Start date
-
1
- Thread starter
- #3
SWComposites
Aerospace
And just what are you going to do with the "3D stress distribution"? Why do you care about thru-thickness stresses in such a thin plate? How is it loaded?
- Thread starter
- #6
- Thread starter
- #8
Sorry I don't understand the definition of "2D elements". Does it mean to simulate any cross-section of the laminate, or the maximum mesh for each layer is 1 like shell model? The 1st approach is not working since the boundary condition is applied to the edge instead of top and bottom of the laminate
Use shell elements (sometimes called plate or 2D elements) as rb1957 and SWComposites advise. In any decent program you can specify the number of layers and the properties of each layer. The edge boundary condition can be achieved with rigid links or a short plate at right angles to the edges.
- Thread starter
- #10
-
1
- #11
ESPcomposites
Aerospace
I think you may find some differing responses to this.
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
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
I would agree with Brian (ESPcomposites) about treating CAD/FEA bundled packages with caution. These tend towards the generation of solid elements which are only applicable for certain types of structures just like beam and plate elements are only applicable for certain types of structures.
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
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
ESPcomposites
Aerospace
And just to add to that, these types of tools do have some nice features that even high end tools don't necessarily offer. The parametric interface naturally supports that.
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
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
- Thread starter
- #14
I did quick Solidworks simulation using both solid and shell mesh. The test laminate consists of a 5-layer stack including one layer with 2 different materials. The modulus of these 2 materials are 8 MPa and 110 GPa, respectively. In addition, a control laminate is constructed where the 110 GPa material is replaced by 8 MPa material.
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?
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?
BlasMolero
Mechanical
Hello!,
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:
Best regards,
Blas.
~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director
IBERISA
48011 BILBAO (SPAIN)
WEB:
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:
Best regards,
Blas.
~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director
IBERISA
48011 BILBAO (SPAIN)
WEB:
ESPcomposites
Aerospace
Blas, a couple items:
"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
"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
BlasMolero
Mechanical
Dear ESPcomposites,
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:
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:
ESPcomposites
Aerospace
Blas,
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
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
BlasMolero
Mechanical
Dear Brian,
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:
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:
- Status
Similar threads
- Question
- Question