shell elements 6

[tsankar]

Hi,
I have just started using Pro/Mechanica FEM software. I have some basic confusion regarding the use of shell elements for the analysis of thin structures. Can anybody elaborate why the use of solid elements will not yield good results in analysing thin plates/structures?.

Also Pro/Mechanica offers only a limited range of elements. Rigid links are not available in Mechanica and we have to model beam elements of high stiffness or springs of high stiffness instead. The rotational degrees of freedom of the spring end have to be supressed where it meets a solid element. Is there any other means of modeling this?.

Thanks,
TS

 

[brad]

Structures generally undergo some amount of bending. Solid elements cannot handle bending modes directly; rather they react bending my means of the normal stresses through the section.

Think of a cantilever beam. Solid elements beneath the neutral axis react a compressive stress; those above the neutral axis are tensile. This net couple then reacts the applied moments. A limited number of discrete solid elements through the thickness tends to not capture this (important) behavior well.

There are several other issues which revolve around the "whys" of this question. I acknowledge that this is only a cursory answer, but it is the general skeleton on which the larger discussions are built.

--
Implied from the above discussion:
Solid elements could work in "thin shell" structures, but you'd need several elements through the thickness. One needs to make several elements through the thickness, yet still make sure that there are reasonable aspect ratios. Usually once these two items are addressed, there are far more degrees of freedom in the model than if a shell element were used.

Brad

 

[vasu77]

what is shear locking

 

[rahulsrp]

hi
actually my project is in thin shell analysis.
you cannot use regular elements for thin shells because
as thickness decreases elements tends to become more
stiff and causes shear stress locking.
one way is to use reduced integration for shear terms
if you need more information please be free to write

rahul

 

[brad]

I was afraid my cursory response wouldn't be enough . . .

What is shear locking?

This is not intended to be an exhaustive discussion, so my apologies to the hardcore solid mechanicians; this is intended to explain in easiest terms this phenomenon.

Take the example which I earlier gave of the cantilever beam. Solid elements cannot "bend", per se.

So for a single solid element in cantilever bending,
(where the x's are the nodes)
Let's presume I hold the left vertical face fixed and apply a bending moment to the right side:
The original and deformed configurations would look like:

ORIGINAL DEFORMED

x x x x

becomes
x x x x


If this is a fully-integrated 1st order element, the "bending" displacement plays itself out as a contraction of the bottom portion and an extension of the top portion of the element. Hence, the bending mode effectively can only be reacted by a shear mode in the element.
One could calculate the strain at the top and bottom of a cantilever beam. If a solid element in bending has a strain of +e on the top face and -e on the bottom face, the energy due to this is much less than the energy due to shearing of that same amount. However, the solid element can ONLY react this load condition via shear. These parasitic shear stresses result in an overly-stiff element. For first-order fully-integrated elements, this can introduce significant error for a coarse mesh. This overly-stiff behavior is referred to as shear locking.

Rahulsrp suggests using reduced-integration elements to avoid this; however, they present their own unique problems in that they have no hourglass stiffness. They have no way of resisting this shear behavior, therefore they have spurious zero-energy shear modes, which can propogate through the mesh.

The way to get around these issues:
1) Use 2nd order elements
2) Use a finer mesh--a fine mesh will eventually converge to the "correct" solution
3) Some codes have special fully-integrated elements which account for this behavior. They are sometimes referred to as "incompatible modes" elements.

And despite rahulsrp's statement, you CAN in fact use solid elements for "thin" structures; you just need a fine enough mesh and need to be able to maintain reasonable element ratios (after all, "thin" is a relative term). As previously stated, once one has addressed these two issues, it is generally much more computationally expensive to use "solid" elements instead of "shells".

Just so there is no confusion: one CAN use solids for these thin structures, but I would recommend using shell elements instead for most cases.

Brad

 

[tsankar]

Bradh's explanation was very helpful. Now Iam presented with one more question. How to choose an aspect ratio for my mesh?. Mechanica gives me an option of specifying the aspect ratio for the elements it will create using its automesh feature. How can I choose a proper value for this?.Does this depend on how we expect the stresses etc to vary in different directions in our model?. I have gone through some text books to find out an answer. But I haven't got the clear picture yet. Can anybody elaborate?.

Thanks,
TS

 

[rahulsrp]

hi
as suggested by bradh you can use solid elements.
but it unnecessary involves more computational work.
instead you can use selective reduced integration means
use reduced integration only for shear terms.
you can find good explation in T.J.R. Hughes book
on Linear Finite Elements Method.

rahulsrp

 

[brad]

tsankar,
I can only answer the aspect ratio in general terms, apart from Mechanica. I believe that my general statements apply to Mechanica also, but as it has been a long time since I've used that code, I can't be 100% sure.

Finite elements end up being sorted out mathematically through their idealized shape (in the case of a quadrilateral element, it is first idealized as a perfect square). This idealized shape is then "linked" to the actual element geometry through shape functions. This is significant because these shape functions break down if the actual geometry of the element seriously diverges from the idealization. This results in "bad answers"

The number that I have most heard for a reasonable aspect ratio is <5.0, meaning the longest edge of an element should not be greater than 5 times that of the shortest. Obviously, one would like this number to be as close to 1.0 as often as possible (meaning all edges are the same length--closer to the idealized shape). However, that is generally not practical. The general rule is always build the best meshes in the areas of greatest concern.

One thing about Mechanica which may effect details of deciding aspect ratio (although I don't think it does) is the fact that Mechanica utilizes polynomial elements. I don't think that p-elements change any of the statements which I have made on this posting. However, if somebody who knows Mechanica feels differently, PLEASE correct me on this point

 

[tsankar]

Thanks Brad. That was great.

Cheers,
TS

 

[Andrea Mino]

I know the limitation about ratio of the tickness and the model dimension( > 1/10).
Does someone know if exist a limitation about the ratio of the tickness and the minimum element dimension ?
Thanks,
AM

 

[brad]

Minoand,
There does not exist a limit for this, to my knowledge.
Often people refer to the 1:10 thickness:element dimension, but this is in fact a reference to the thickness and model dimension.
I have not encountered a reference to any limits such as this with regards to element formulation (note that some classes of problems may however have a limit; I just don't know of a general &quot;rule&quot.

Brad

 

[sreul]

Hi,
I am using Pro/MECHANICA now for more than 8 years. And I am a CEP partner of PTC and an authorised trainig provider. So I know Pro/MECHANICA very well.
Tsankar, MECH works with p-elements and not with the conventional h-elements. P-Elements increase the polynomial orders from 1 (equivalent to linear conventional finite elements) up to 9th order ! This results in a lot of advantages:
- each solid element can handle bending, torsion and shear
- the element limits can vary for the
- aspect ratio up to 1:30 !!!
- edge angles from 5 to 175 deg !!!
- edge turn up to 95 deg (p-elements follow exactly the underlying geometry, so a hole or similar can be represented as a minimum by four (4!!) element-edges
- therefore tetrahedal automatic meshing is no problem; stresses and displacements can be recieved as precise as you wish by defining a numerical quality (convergence) of e.g. 5 %
- that is thin structures can be calculated very good; example: we calcualted structures with 1 mm thick walls and an diameter of about 800 mm with 110,000 solid elements and 4.8 Mio. DOF !!

To rigid connections: since Version 2000i2 (actual is version 2001) rigid connections can be defined and used. The use of beams is not necessary any more.
Answers this some of your points ?

Best regards, sreul