GIRDER MODELLED BY SHELL ELEMENTS 1

[SKJoe]

Hi,

i am modelling simply suppoted girder ( it is not main goal, it is only in order to verify use
of shell element for another problem ) by shell elements shell 181 in ansys subjected to uniform pressure on the top flange 5N/mm2( cross-cection is an I-shape, thickness of this flanges and web is 50mm, width of web is 700mm, width of flanges 200mm,lenght of girder is 3800mm )

i want to get normal stesses in the bottom flange (bottom layer of shell - along the path), but there is level of stress 177N/mm2,analytical solution is 188N/mm2... this deviation seems to me be large.

in the help file for shell181 is also said :
"Bilinear elements, when fully integrated, are too stiff in in-plane bending.SHELL181 uses the method of incompatible modes to enhance the accuracy in bending-dominated problems."

it seems this increase of accuracy is not enough... i also dont know what this expression "Bilinear elements" means...i only know expression „bilinear material“

there are some discontinuity in normal stesses on the interface flange - web as well - probably effect of shear locking, but how to obtain correct value (it is needed for the another problem...) – may i simply „kick out“ this value from averaging ?

i hope there will be someone able to help me...thanx

 

[jte]

SKJoe-

Can't help you with Ansys issues... But perhaps you are facing a more generic issue: I suspect that you may find your error not in the FEA, but in the analytical solution. If you are determining the stress based on a beam formula (Stress=Mc/I) then you may be neglecting the contribution of shear to carrying the load. Shear always exists and will influence the results, but generally to a neglegable extent when the length of the beam exceeds 10*(height). In your case, the beam would have to be 7000 mm for you to comfortably neglect shear. Thus, it is possible that if you account for some of the load being carried by shear (max stress occurring in the middle of the cross section) you may find that the analytical solution for bending stress at the extreme fiber is reduced a bit...

jt

 

[SKJoe]

jte,

you are probably right, but if i am modelling this girder by beam4, beam44 or solid185 i obtain level of stress 187-189 N/mm2.....?

 

[prex]

When using shell elements for problems where bending is of importance, the result is critically dependent on where you put the midplane of your elements.
If you correctly put it at the midplane of the corresponding plates, then you get a number of deviations from the results of the theory of beams:
1)the moment of inertia of the flanges is correctly evaluated (this is not a deviation for this case)
2)the height of the web is one flange thickness higher, and this overestimates the section moment of inertia
3)stresses are evaluated at flange midplane, not at flange outer fiber, and this underestimates the stress.
If you put the midplane of your elements for flanges at flange outer fiber, then the above deviations are of course bigger.
I'm surprised by the deviation you state between FEM and beam theory, as I expected a bigger one.
I'm afraid there is no general rule to cope with such deviations: one suggestion, that may be valid as any other, is to place your elements in such a way that thicknesses and section area are conserved.
Anyway, wherever you place the elements in a reasonable way, you'll inevitably have to analyse your results for consistency (and if you can use normal beam theory for your actual problem, just do that, FEM will sometimes complicate things in place of making easier the analysis).

prex

http://www.xcalcs.com

Online tools for structural design

 

[SKJoe]

prex,

according to 2)in your answer i have done my model by this way : i lowered hight of web to 650mm, i set up bottom surface of shell elements for top flange as reference surface and set up top surface of shell elements for bottom flange as reference surface.
level of stress is now correct !, equals to 188N/mm2 as i have mentioned above...thanx a lot !

but still seems to me be strange that after this correction is stess accurate, but deformation is higher(4.998mm)than analytical solution (3.596mmm)
according to one sentence published everywhere : if using deformation variant of FEM, then defomations are the most accurate and stresses are less accurate because they are numerically derived from deformation functions..

anyway thanx a lot !

 

[prex]

The discrepancy in deflections is now enormous!
Don't know what exactly means the reference surface of shell elements you mention, but now your beam should have a depth 50 mm lower: however this doesn't explain the difference in stiffness.
In fact you have now a section with the same effective area as the original one: this seems to have a good influence on stress values, but ruins the deflections.
As I told above there is no general rule to fully resolve this kind of issue.

prex

http://www.xcalcs.com

Online tools for structural design

 

[jte]

SKJoe-

The results you are getting with beam elements don't surprise me. Do the beam elements you are using include shear, or are they based only on long beam theory where bending is the hugely dominant player?

As prex pointed out, with shell/plate elements you must model your geometry at the mid-thickness to get very accurate results.

What I'd be curious about is how your problem changes if you double the length of the beam. If you modelled the whole beam originally, just put some symmetrical boundary conditions on one side of the model and you've effectively doubled the length. Now re-do your hand calc's and compare results. My suspicion is that your FEA results will be closer to the hand calcs.

The issue is that while the max stress is matching, your deflections are not. Since the max shear stress is not co-located with the max bending stress, you won't see the difference in the FEA vs hand stress calc's. But the shell element FEA inherently includes shear in its calc (What is your FEA indicated Von Mises or Tresca or membrane stress at the neutral axis?). So while you are (presumably) neglecting shear in your hand calc's, the FEA is not. This may be the cause of the difference you are seeing.

jt

 

[feadude]

are you looking at top or bottom of your shell element stresses?

 

[SKJoe]

jte,

1) in ansys i use shell 181 and it has ability attach offset "section of element" - it means if offset section is set up to midle-plane, then applied thickness (lets say equals to 50mmm)is divided to 25mm in positive direction of normal of shell element and 25mm in negative direction,
if offset section is set up to bottom-plane, then appied thickness is considered in negative direction of normal of shell...if top, then in positive direction, furthermore i can set up that quantities will be stored in midle-plane - it means that result for midle-plane will not be averraged from results from top and bottom-plane...

so i simly assume that if there is added in ansys this sort of function (ability to set up offset section)quantities are calculated in accordance with this function

2)i have made model with doube length : numerical result are : sx=795,8N/mm2, uz=66,639mm, analytical : sx=792,5N/mm2, uz=63,77mm - as you said (thanx for recalling me...)

3)but there is still one issue, which hasnt been answered yet(from beginig if this topic) :

there are some discontinuity in normal stesses on the interface flange - web as well - probably effect of shear locking, but how to obtain correct value (it is needed for the another problem...) – may i simply „kick out“ this value from averaging ?

regards

 

[prex]

SKJoe,
concerning your point 1) in last post, does this offset feature mean that the nodes for connecting, for example, the web to the flanges, may be put at the surface of the shell element, instead of being at the midplane? If so, it would be necessary to know more about the theory of that element to discuss your results, but I guess it is a too complex argument for a forum.
Consider also that the flange of a beam in bending is subject to membrane stresses only (no bending in the plane of the flange), so that it should be unrelevant to consider mid plane or surface stresses, they should be all substantially the same.
Concerning your point 3), it would be necessary to know more about the discontinuity stresses you see: as you are using shell elements, you should not see the local discontinuity stresses that certainly exist at web to flange attachment. So I can't really see what kind of discontinuity may cause those stresses, except of course that the shear stress falls to nearly zero in going from the web to the flange.
Once again I guess it will be difficult to discuss here such a topic in depth.

prex

http://www.xcalcs.com

Online tools for structural design

 

[feadude]

1.top flange is in bending and axial because there is uniform pressure applied to it (load).
2. top flange and bottom flange should not have uniform stress across the thickness because the outer fibers of each flange will see the maximum stress.