modal analysis, shell vs solid

[Michele667]

Hi all,

i'm performing a modal analysis on a piping system. i discovered that natural frequency values change if i use shell elements instead of solid.
Is this possible?
I checked everything: from material used, till constrain and contacts.

First prototype built (shell elements used), had problem of resonance even if the value of the natural frequencies for pipes were far away from excitation of the force, calculation tell me 35.8 Hz while force is near 47Hz.

Just for curiosity i changed my model using solid elements for the pipes instead if shell, and i discovered that the pipes have a frequency in the field of the frequency of the force, 45.8Hz.

the only thing i see different is that while with shell elements bonded contact are generated between edge, with solid elements i'm supposed to put contact between faces arising the whole stiffness, is this thought correct or should i look for other reasons?

thanks in advance

 

[hacksaw]

the simple answers is yes there is a significant difference, it has to do with the shell elements being more flexible

more specific answers will require response from those more involved with the calculation methods.

 

[Twoballcane]

Off the top of my head, I think there is an aspect ration that you have to follow which is thickness to length. If the aspect ratio is small you go with shell, if large, you go with solid. You can also do some hand calculations to find out what the Fn is for a long pipe and see which one correlates better. FEM is GIGO, you have to correlate to somthing to make FEM valid.

Tobalcane
"If you avoid failure, you also avoid success."

 

[corus]

If you use a coarse mesh then the model tends to be stiffer and hence produces a higher frequency. If you've used solid elements then my guess is that you have too few through the thickness and the model is tending to be over stiff.

Tata

 

[Michele667]

Hi all, thanks for the answers, you clarify me one face of the problem.

Yes, solid element size is about 3mm along thickness of the pipe that is 0,7mm: so this lead to say that the resonance value i calculated is more probably a coincidence.
Furthermore the ratio thickness by lenght is about 0.7/500 minimum. So shell elements seem to remain the correct one to use.

But nothing about contact? i mean, don't they play a relevant role on FEM analysis?

thanks again for your support

 

[TheTick]

What about element size? Keep reducing element size until the numbers stop changing. Too coarse of a mesh can produce erroneous results, whether solid or shell.

 

[Michele667]

I don't think that my mesh is so bad, please have a look to jpeg; yes maybe i can further reduce element size, but at what cost for processor? is there any advantage for a simple modal analysis?

 

[SWComposites]

"But nothing about contact? "

Contact between what? different parts? Are you saying you have contact between the surface of the pipe and some other part? If so, how specifically have you modelled it?

 

[TheTick]

Solid mesh is definitely on the coarse side, even if you're using P-tets. What software are you using? Does it have automatic mesh refinement? (Likely not available for modal analysis, anyhow.)

Any idiot can finish a test if he's not worried about getting right answers. More time processing is the least of your worries if your results aren't right.

Run again with a mesh refined by a factor of about 1.5. If your results are comparable, you're OK. If not, keep refining.

 

[corus]

Contact doesn't apply in modal analyses as you're just obtaining the 'characteristic' modal shapes and not specific displacements. You'd need to run a full dynamic analysis with prescribed loads/displacements if you wanted to include contact.

If you're only interested in the pipes then why have the rest of the structure there as relatively speaking it must be fairly rigid compared to the pipes and could be replaced by imposing fixed restraints, perhaps?

Tata

 

[Twoballcane]

I do agree with corus for modal analysis, however, once you do a vibration analysis, I find that having a contact fixed in direction, but free to rotate (even though you think it should be fixed in dir and rotation) is more realistic.


"so this lead to say that the resonance value i calculated is more probably a coincidence."


I'll have more faith in hand calcs than the FEA. IMHO, FEA are the pretty pics you show to management to communicate what you calculated by hand. Don't become complacent with FEA, if you can not do the hand calcs, you shouldn’t do the FEA. In any case, you should have a good idea what the frequencies and mode shape (stress, strain, deflections…etc) should be before you do the FEA.

Tobalcane
"If you avoid failure, you also avoid success."

 

[Twoballcane]

Actualy let me take that back on the modal analysis (sorry corus). I find that if your cantacts are fixed in directiona and rotation, you will get higher Fn, and if contacts were fixed in direction and free in rotation, you will get lower Fn. From test data I have done in the past (such as covers on a electronic box that is fastened on all four sides), I find that fixed direction and free rotation is more realistic.

Tobalcane
"If you avoid failure, you also avoid success."