How many nodes/elements/DOFs do you work with? 8

If you can use 2D elements, you should. They are far more efficient and you can extract more meaningful data. Using solid elements in place of 2D elements (where 2D elements can be used) is usually an indication of lack of experience (or should I say good experience). It also usually indicates a lack of a solid understand of mechanics of materials. Also, there is a bad history of people being familiar with software but not how things really work (known as a GIGO - garbage in/garbage out). A combination of these factors could cause the engineer to scoff at the model. In general, you should not use solid elements unless the model truly requires it. Maybe you can post a picture?

Brian

IMHO size is a thing of the past. We run (sometimes) horrendous models ... import pieces of an assumbly, tet (tet10s) mesh it (even the bits that are 0.06" thick !), join the pieces together with CBUSH, load and constrain, and push the button. Most like this take a day or so ... so what ? To make an efficient model would take a lot of analyst time (and calendar time).

another day in paradise, or is paradise one day closer ?

Disadvantages of using 3D elements when 2D elements can be used:

- Extracting bending moments, running loads, etc. are direct for 2D elements, but not for solids. This is usually reason enough to use 2D elements.
- Changing the thickness for 2D models is done in seconds. For a 3D model, it could mean a total rebuild. Thickness often needs to be a flexible design parameter.
- For 3D models, it is not clear if the mesh is reasonable and convergence is obtained. For plate bending problems, you will need a certain amount of elements through the thickness if solid elements are use. The order and type of the element will also matter quite a bit. By contrast, most engineers can eyeball whether a 2D mesh looks reasonable and converged.
- If a nonlinear analysis needs to be done (even a simple one), it could really blow up with 3D elements.
- Transferring files/data storage/run times/crashes/lag are still far more efficient with 2D models.

I could probably go on and on, but I think that is a sufficient list. 3D elements have their place, but if the 2D element is not in your toolbox, there is a big problem. The 2D element is the bread and butter element for some industries (especially aircraft). Less so for automotive. But really, we are not talking about a DOF issue (even though the OP posed it as such). The total number of DOF isn't the point. We are talking about the fundamental difference between solid and 2D elements. I don't think the engineer scoffed at him because of the DOF, he probably scoffed at him for the above reasons.

EDIT: For some situations what rb1957 said is definitely true. If you already have a CAD and need something quick, then a 3D model might get the job done. It will really depend on the process and the desired outputs. If you more of a designer/prelim FEM, then a quick CAD->3D model might be OK. If you are focusing on the analysis, then a 2D model might be better. But again, its not a DOF thing, and if you think the DOF alone is the distinction, then that is enough to question what is going on. It sounds like the OP is focusing on the DOF and not the fundamental differences between solids and shells.

Brian

Thanks Brian and rb1957. This has been enlightening. In my first real job as an engineer I did structural analysis using FEMAP and NX-NASTRAN, but years have passed and I've been stuck in Solidworks land until now. Solidworks seems to be taking over more and more. As a CAD design tool it's great, but I almost wish they didn't have Simulation capabilities because it practically forces you to use solids and it's very hard to inspect the model. The software has a "make simulation accessible to all users" objective, which IMO is a mistake, or at least leads to overreach --> most SW structural analysis I've seen is GIGO. I've decried the use of Solidworks static for analyzing all but the simplest parts to managers on many occasions, but they keep asking me to do it (and for complex assemblies no less!!) because it's cheap. I've finally managed to secure FEMAP and ANSYS licenses, even though only a fraction of what I do is FEA analysis.

In any case, it's obvious I need to brush up on my FEA understanding. Thanks for your perspective.

I agree ... in my experience designers (or draftees) have little experience in analysis (that's why they have more experience in design), and like you I "hate" the modern idea of packaging analysis software in with design tools. Not only are the users (typically) less knowledgeable about analysis, but these half baked analysis tools are simplfied to suit the design side of the software ... so to expand on your expression "GI" (limited user and s/ware) = "GO"

another day in paradise, or is paradise one day closer ?

I disagree with the argument that CAD software's should not have FEA modules.
Although I am not an expert in FEA, in my previous role as Product Development Engineer, I have extensively used Creo Simulate (FEA module in Creo) to solve a variety of design related problems. As a designer, it is tremendously helpful to observe how an object deforms under the application of forces. This not only builds an insight about the product, but also helps in doing comparative analysis. I have been in situations where we chose design concepts from comparative analyses. We had a dedicated FEA team elsewhere, but why my Manager preferred me doing it? Because it is quicker, easier and I can explain them in person what's going on. You cannot have dedicated FEA guys for each product design team and in the same facility.

I understand, but often the CAD-based structural analysis is limited (maybe you can only constrain a face, maybe you can only load limited cases. And maybe your situation is exceptional (at least compared to my experience) so my experience (and opinion) isn't applicable to your instance.

And Way too often I've seen models that are nice pretty cartoons.

For me, Design can make all the stress models they want, and guide their design with the results. I will not (generally) use them for certification; and will model the final design myself (or an analyst) with an FEA code. Hopefully we won't be too far apart.

another day in paradise, or is paradise one day closer ?

I agree, with both of you. Having the ability to do quick stress/deformation/thermal/frequency analyses of simple parts integrated into a CAD package is great to have. The problem comes when people mistake SW for a full-up analysis tool and attempt to predict the response of assemblies with fastener joints, composite layups, what have you.

I feel like the only way to use SW successfully for anything but the most simple analyses is if a trained analyst is using it, aware of the boundaries of its capability and religiously keeping within them. This requires skill. In which case you may as well be using an actual analysis tool...

Again, my case against packaging CAD programs with analysis tools is that it leads to overreach and expectations the honest engineer has to constantly combat: "Why do you need ANSYS? Solidworks can do thermal and structural analysis of this spacecraft detector system, can't it?" Or the young engineer who believes the cartoons they make. Oy vey.

My most accurate and useful FEA model was for an airconditioning compressor. We weren't limited in the number of nodes on a PC, but by the speed of solution on a 286 with a maths co processor. It had approximately 150 nodes. Mode shapes matched for the first 5 modes, and frequencies were within coo-ee.

Sadly the idea of producing correlated models seems to be a dying art.


Cheers

Greg Locock


New here? Try reading these, they might help FAQ731-376

In the initial stages of method development, I prefer to have smaller number of DOFs (thousands or tens of thousands) so I can iterate fast (which is why I try to avoid fancy analysis techniques such as ALE as much as I can). Towards the later stages, tens of millions of DOFs are quite regularly experienced.

*********************************************************
Are you new to this forum? If so, please read these FAQs:

I see two different themes here and would like to speak to both.

First, I see someone talking about the skill of the user. If I had to evaluate someone's FEA skills, I would do it two-fold. First, can they apply the correct theories/elements/etc to get a valid solution? After that would be, do they understand the underlying assumptions enough to be able to get an accurate answer as quickly as possible through the use of alternate element choices, minimum necessary DOFs, problem simplification, etc? The second one to me matters, but at the same time the user has to be skilled/experienced enough to know how much "human time" it will take to get enough savings in "machine time" that benefits the company. For example, a run between 8 and 24 hours long generally doesn't make a difference unless in a queue of other work because it will finish after hours either way. So applying human time to reduce a 24 hour run down to 8 doesn't make sense, however making a 48 hour run take 24 hours shaves a day off a project which is a benefit to the company if it takes you less than a day to reduce that run time.

The second theme I see here is whether CAD-based tools have merit. I have a lot of experience here because I work for a software reseller that sells both SOLIDWORKS Simulation and Abaqus, so I see both sides of the coin. SOLIDWORKS Simulation isn't nearly as limited as some believe, they just haven't been trained properly. It has functionality for solids, shells, and beams. As well as the ability to constrain things in many different ways. Even loadings can be non-uniform if you use the tool correctly. The problem is the lack of understanding of this tool. As was mentioned, someone with analyst level knowledge who has been trained on this tool, will find for simple problems (think static analysis or frequency analysis of a component, or small assembly) it can be superior to a tool like Abaqus due to it's much fewer steps to setup. That aside, it's main purpose was never intended to replace an analyst tool, only provide designers with a feel as they design something. "If I use this diameter shaft, what is my ballpark on deflection?" That's what it's intended purpose is for, and that's the way my company sella it, because for more than that, we offer Abaqus. Other resellers that don't have Abaqus to offer may push SOLIDWORKS Simulation for more than its intended use, and that's a shame.


As you move into complexity of many parts (I'd say around 25+), difficult material models, highly non-linear contacts, and the items that cause convergence issues, SOLIDWORKS Simulation becomes difficult to manage and a product like Abaqus starts to show its superiority. The extra steps involved in setting up the model are paid back through the stability of the solution and the robustness of the available options.

But it takes years to of experience in FEA/solid mechanics/industry specific knowledge to be competent with FEA. And your skill set is going to be most specific to the software package you use regularly and what your peers use (knowledge base). Basically, by the time you are actually competent in FEA, you are usually better off and more efficient to just use a robust FEA pacakage. The CAD based simulates definitely have some advantages in certain scenarios, but they are more theoretical than practical solutions because of the above mentioned reasons. What really happens is someone sort of familiar with FEA and someone who sort of familiar with analysis knowledge tends to use the CAD based approaches because of the low learning curve. The results are really hit and miss, hence the bad reputation. On the flip side, the skilled FEA guys go directly to a robust FEM they are very familiar with.

20 years ago the CAD based FEA packages were looking really promising, but it didn't really pan out as hoped. I first learned that way, but I did a decent amount of GIGO. This was because of the low learning curve which made me *think* I could do real analysis (when I was not actually qualified). The reality is that 3D models have the intent of form/fit/function/production/etc of parts. FEA models are MATH models that only resemble the CAD model. They are farther apart than many people realize. In an ideal world, you would have access to both, be able to learn both, have the equivalent knowledge based, etc. But from my experience, that is not what happens. Just my experience the last 20 years, but I have not seen a skilled analyst use a CAD based solution. Clever analysts can usually come up with efficient approaches and the overall process (checking, validating, peer approval, data extraction, flexibility) becomes more efficient with a robust FEA solution, largely nullifying the perceived benefits of the "push button" CAD based FEA. But again, just my personal experience and I am sure there are some good analysts that uses the CAD based FEA as well.

In my point of view and in my line of work the (original) discussion is moot (2D or 3D etc.), and this is why the answer to the OP is extremely industry / line of work dependent

I understand the necessity of using 2D elements and their advantages, but where I currently work, 2D elements are almost never possible.
I mainly analyze assemblies made of injection molded parts, or complex CNC machined parts (plastics and metals), since these technologies are very (well relatively) geometrically unrestricted, the designers really come up with very complex geometries (highly varying wall thicknesses, intricate connections, highly curved surfaces, etc.) that are generally impossible to 2D mesh, I rarely even try 2D meshing (even symmetry is not always possible to utilize) and most of the times go straight to try and HEX mesh (pure hex is possible in rare occasions because of the complexity of the parts) and if this is not possible - I strive to get a good quality tet10 mesh.

So I guess this is very industry specific (or even work place specific) and the #of DOFs answer you'll get will vary.

Generally - I try to stay below 100K nodes when I setup a non-linear contact problem, and if I had more computer power (hardware and license) this number would have gone up because as gravityandinertia mentioned, most of the jobs are ran overnight, and if I just want to see if the setup is OK I temporarily reduce (a lot) the node count to see that everything converges, and re run the fine mesh setup overnight in any case.

historical analysis relies on 1000-5000 elements for aircraft flying today - whereas we started saving so much weight with better FEA models and accuracy that those old aircraft are getting significant lighter weight updates on their primary load structures.

it always depends on the budget, accuracy aimed for, and level of modification and purposes.

I worked with from 2000 elements (for a finemesh shell fatigue model) to 10million elements (for a complete vehicle with superelements for transient modal response analysis to calculate final fatigue life results).

it will always depend on your analysis and you'll know what you need with diverse experience.
per static, the reality is that you may reduce your model only to an analysis region of interest. so, until you get what you need and your boundary conditions are flexible (either as a representation of the attaching structures at the boundaries or just flexible boundary conditions with different dof applications at different boundary locations), try using as least as you can while maintaining the real behavior of the structure.

I'll give one example:
- for a thermo-elastic analysis, one may go as far as modeling the whole structure.
- but in reality, you may cut the model at any location depending on where you want the accurate results and how much accuracy you need.
- if you cut the boundary at a location and place RBE2 elements at this location and define the boundary material's thermal expansion coefficient to these RBE2 elements, you will have an issue of being too conservative and not conservative enough depending on your increasing and decreasing temperature for the thermo-elastic analysis.
- instead of placing those nodes the RBE2 elements, if you only define a flexible boundary condition that will allow the structure to expand freely, you might have just aimed at the perfect simple thermo-elastic model.
- just think about how structure expands with different materials used in a wing structure and think about all above statements. now, you most probably saved the analysis time by %30 to %90.
- replicate this example per static analysis. how the structure would deform with the complete model modeled as is, how it deforms if there are SPCs applied at the cut nodes. you will get some extra stiffness if you cut the model too short for static analysis under mechanical loads.

***remembering Kirchhoff's Rule for structural analysis, try to maintain the structural circuit up to some level as much as you can - either by using representative CBAR elements, or using some of the shell mesh from the rest of the model to have flexible boundaries where Kirchhoff tries to circulate your model

Spaceship!!
Aerospace Engineer, M.Sc. / Aircraft Stress Engineer

the good thing about FEA is that the error converges. the more nodes it has, the more accurate the result will be. if the model have simple geometry, u can simplify the number of nodes, but if it has complex geometry, the more nodes the better. I have read that a multi-million dollar project failed just because the engineer didn't put in enough of nodes and the concrete tower which supposes to be floating sank to bottom of the sea.

disclaimer: all calculations and comments must be checked by senior engineers before they are taken to be good.

oh dear Mr onlinetutor ...
"the more nodes it has, the more accurate the result will be" ...
assuming that the model is not fatally flawed (with constraints as an example)

another day in paradise, or is paradise one day closer ?

Don't worry GregL, I work on the order of 1000 nodes for a full automobile body. (concept model with mostly beams and very coarse shells)

This was going to be a different perspective, but I see mlevett3 beat me to it.

I regularly use FEA in my work, with between 2 and about 5000 nodes. Working on long uniform structures means a 2D analysis is usually suitable for final design, and a staged non-linear analysis can be completed in seconds, which allows a wide variety of different scenarios to be modelled. At the lower extreme, modelling a single beam, or a few beams, is a perfectly good way of doing a cross check on a more detailed analysis.

Occasionally I need to do a 3D analysis, but even here the upper limit on model size I have used is about 500,000 nodes

Doug Jenkins
Interactive Design Services