stresses at perpendicular shell elements. problem? 1

[BP846]

hello,

I am modeling a structure with shell elements and I am having very high local stresses in the areas
where perpendicular shells are connected as you can see in the attached file. In the real strucutre
the webs are welded to the rest of the structure.

I've heard that perpendicular shell elements give pessimistic results. Is this issue relevant in my
model? Should I use a more detailed mesh?

To understand what I am talking about please look at the attached pdf.

My question is how relevant these modeling issues are, and which is the best way to model this
kinf of problems.

PD: The results shown in the attached file are from a random analysis.

thanks

 

[rb1957]

it looks like the thickness of the web is of the order of an element side. the 2D shell web is applying it's load to a single node, creating high stresses. the 3D solid web is distributing this load along the element side, lowering the stresses.

note the 3D solid web and the 2D shell body do not join as you might expect/desire. 3D elements have not moment freedoms at the nodes, so the 2D shell elements of the body have no where to react this load. so i think this is probably the least accurate model. the 3D solid web and body is probably the best representation of what you have, since the web and the body are compatable.

 

[Naffoussi]

if you want to use a solid elements for webs and shell elements for the vertical "body" you have to create a skin property (plate with 1E-4 m) for your solid elements (and try to put more than 1 element for the solid thickness)this allows the connection between shell and solid element thru the skin...the stress found is maybe a true one.

When you use only shell elements did you just merge nodes or you have put a rigid element between the perpendicular parts?

did you try to use C-WELD elements to join the perpendicular shells?

sorry for my english level

 

[inline6]

You need a minimum of 4 HEX8 element through the thickness to capture bending stress. With solids the mesh is probably too coarse to pick up the peak stress. With shell you need to use the correct averageing of stresses it looks like you are averaging all which should not be done across T junctions.

What kind of analysis are you doing? is it a strength/proof load of fatigue analysis? Looking at the solid model proportions it looks like shells should do the job if you use the correct averaging and ignore stresses in the virtual overlaps. A much finer solid would also work but may be more costly from time point of view. Either way you should be getting results that are much closer

 

[irq]

BP846: Could you provide a plot without avaraging, results in the centroid of each element? It looks you are using Patran and most likely Nastran - there is a special MPC there to connect solid with shell and couple the different dof already mentioned by rb1957

inline6: What is the origin of 4 elements of HEX8 thru the thickness? The minimum of 3 elements seems to me more intuitive (tension-neutral axis-compression). Have you ever compared 3 and 4 elm. solution? Are the differences significant?

 

[BP846]

hello,
nodes are simply merged. I've never heard about cweld elements, don't they make the structure stiffener?

irq, yes, i am using Patran/Nastran. About averaging, I'am not very used to Patran, could you help me with this? how can i plot results wihtout averaging?

 

[BP846]

about solid/shell conection, I used shell elements coincident to the solid faces to transmit the moments to the shell elements of the wall

 

[inline6]

transverse shear distribution through thickness peaks at middle so you want a node at neutral axis. 4 elements are required because of parabolic distribution and this reasonably captures it. It is just a rule of thumb. With higher order elements you could do two elements.

In patran do a fringe > Plot Options > Averaging Definition > Domain

 

[rb1957]

would it be easier to RBE the solid nodes to the shell nodes ?

 

[BP846]

what is the advantage of using c-weld elements in perpendicular shell elements? instead of merging the nodes?

 

[rb1957]

i haven't heard or the CWELD elements, but maybe they're NSTRAN's answer to this reasonably typical problem (joining 3D elements to 2D).

personally i'd strongly advise against merging nodes, 'cause i think you're creating a pinned joint at the interface.

 

[BP846]

rb1957, I was asking about using cweld to joint shell elements with other perpendicular shell elements as compositecurves said. In this case there is no pinned joint am i right?

 

[Naffoussi]

hello,

BP846, Are u using Femap ??

 

[BP846]

i am with Patran and Nastran.

 

[rb1957]

i would assume that CWELD elements (whatever they are) would allow a moment connection.

i was talking about merging nodes directly (what i thought you'd done originally) between 3D and 2D elements. connecting the two elements with say CWELDs or RBEs isn't (in my imnd at least) "merging nodes".

 

[Naffoussi]

when he merge nodes, a very important stresses are found on the perpendicular shell connection (maybe it's a true one)

 

[irq]

In plot options you can set none for domain and centroid for extrapolation to plot result stress at element centroid w/o averaging.

Use shell-to-solid element connector (RSSCON Surf-Vol) from Elements/MPC to couple the different dof's between shell and solid and have the things done. It is much easier than RBE2 or RBE3 (you do not need to specify any dof's, the constraints are set automatically) and model exactly what you are looking for.

CWELD is general purpose connector in MSC.Nastran to enable a quick connection of the disimilar meshes without node alignment etc. MSC says that it is more accurate than RBE2/RBE3 but I have never checked it.