Mesh change between FEA analysis types?

[Nathanwest58]

TL;DR Summary

Depending on the type of FEA analysis being done i.e. static, modal etc, should the mesh be changed?

Hi all,

Sorry of this is a silly question but it is one that recently came to mind and I cannot seem to find an answer to it: "should I change my mesh depending on the type of FEA analysis I am doing?"

My feeling is that I should not change it, but that is a total guess on my part.

Any further information or insight would be greatly appreciated.

 

[jrmichler]

FEA analysis packages normally give you a choice of element types. The analyst has the job of selecting the element type, followed by mesh size. Different element types will have different optimal mesh sizes.

For linear static analyses (modal analyses are linear static), everything I have read on the subject seems to say that there is very little difference in end results and run time between different element types. Getting the mesh right is more important than choosing the optimal element. Also, correctly specifying forces and restraints is more important than element type.

Nonlinear dynamic analyses are different. In those, the element type is a critical variable. I once spent about three months chasing down a blind alley because I was using an element that was not suited for the sheet metal forming problem I was working on.

 

[FEAnalyst]

The choice of mesh density depends on what you want to get from analysis. Whether you are interested more in the global response (that’s often the case in dynamic analyses) or the local one (that’s common in static stress analyses). In the latter case you will need proper local mesh refinement. Here are some examples:
- you won’t need very fine mesh in rotating disc analysis
- the mesh in drop test will likely be rather coarse (to reduce the calculation time)
- in modal or linear buckling analyses you will need sufficiently refined global mesh to capture all mode shapes but with no need for large global or local refinement
- if explicit dynamics simulation is performed, mesh size influences stable time increment and thus has huge impact on calculation time and you will have to avoid extreme refinements in such cases (even though you can compensate this effect with mass scaling)
- however, in static contact or fracture mechanics simulations the mesh will need significant local refinement (cases like spur gear analyses)

That’s just about the mesh size but there’s also a lot of discussion in terms of which type of element to choose for particular analysis. This topic is too broad to discuss it in general here (due to large number of element types in advanced FEA codes) but software vendors usually share various benchmarks, advice in the documentation and even whole courses on this topic.

 

[Nathanwest58]

Thank you both for your answers, but I realize now that I was not clear at all in my original post.

Let me restate the question: "If I wanted to run multiple FEA on the same geometry/part (i.e. static, modal) should I alter the mesh from one analysis type to the next?"

After reading your answers it seems that I probably should alter the mesh, examine the results of either analysis and alter the mesh accordingly.

 

[FEAnalyst]

It really depends. Many products require a whole set of different analyses. We usually keep the mesh relatively unchanged within a single study (even if it consists of multiple simulation types). But for example, if we decide to check fatigue as well then we may have to apply further refinement in critical areas. For modal analyses, there's usually no need to change the mesh unless it's too dense. Another thing is that several simulation types are often involved in a single run if the software allows for that. In such cases, the mesh can't be changed. For example, consider this scenario:
- step 1 - static preload
- step 2 - linear buckling
- step 3 - nonlinear buckling

Or this one:
- step 1 - static preload
- step 2 - natural frequency extraction
- step 3 - static load
- step 4 - next natural frequency extraction
- step 5 - dynamic release of load

All these steps are performed using the same mesh.

 

[Tom.G]

I once spent about three months chasing down a blind alley

Billable Hours?
(or is that Proprietary Information?)

 

[Frabjous]

Billable Hours?
(or is that Proprietary Information?)

Before the advent of modern meshing tools, spending 6 months getting a complicated mesh to run properly was more common that you would expect.

 

[jrmichler]

Billable Hours?
(or is that Proprietary Information?)

Nope. Grad student working on sheet metal forming about 1993. I had the experimental data, and needed FEA analysis. A number of papers on sheet metal forming had all used ABAQUS and the same element. ABAQUS has a huge book full of elements, so I just used the same element that everybody else used. I tested the software by simulating a tensile test. The FEA results matched the experimental results, so I went ahead with blankholder friction, then further steps until I simulated the full moving drawbead.

The FEA results differed from the experimental results by about 30%, plus the deformed geometry was wrong. A faculty member who had got his Ph.D. in sheet metal forming using ABAQUS with that element said it was experimental error. My error budget, and the deformed geometry said otherwise. So I dug into it and found that that particular element was not suited for sheet metal forming due to something known as hourglassing. I found a workaround that gave useable results. The longer models took over 200 hours CPU time on Sun workstations. These models ran in the background (graduate computer lab), so got about 16 hours CPU time per day. And the entire system was rebooted on the last day of every month.

Typical result of one FEA run. The solid black is really four elements thick, and is moving from left to right.