sandwich with layered shell elements

[SandwichMaker]

Hi, i'm new for this forum and a quite new user of Ansys, so I apologize for any newbie-error i'll post...
I'm trying to model a sandwich square plate, simply supported on all four edges, under a constant z-pressure load, static linear elastic analisys. The section of the plate is made of four layers: lapideal-carbon fiber prepreg- cork - carbon fiber prepreg. The thickness of lapideal and cork layer is much bigger than the thickness of fiber reinforced layers (10 mm versus 0.1 mm).
The first thing I've done is to model a quarter of this simple structure with shell layered elements: shell99. I set the proper real constants with the right sequence of layers and materials, set the proper boundary conditions (2 lines Uz constrained, 2 lines symmetric) and applied a constant pressure over the lapideal layer. The results match my Matlab Analisys (based on J.N. Reddy layerwise theory) only when thickness of layers are the same. In the real case of big differences between the layers thickness, the two solutions diverge.
The probelm is:
with shell99 elements the deformations (i'm looking for results epelx,epely,epelxy,epelxz,epelyz) are considered linear and continuous trough the thickness, while my analisys tells me that the slope of the deformations in a x-y point and plotted along z-axis are linear but changes across one interface and the other.
A possible solution should be abandone the too simple shell analisys and model my geometry with 3d elements, but the difference between the thickness of carbon and cork layers constrain me to use a enormous number of elements (if they are sized to model the carbon layer, their size forces me use a unnecessary big number of elements for the cork or the lapideal layer!).
The question is:
Is it possible to connect parallel layers of shell elements. This permits me to obtain piecewise linear deformations through thickness with a relatively simple model.

I apologize for my english, maybe it's a little difficult to understand!

 

[SandwichMaker]

Another information about the problem. The ansys theory reference for the shell layered elements says:

"Assumptions and Restrictions:
Normals to the centerplane are assumed to remain straight after deformation, but not necessarily normal to the centerplane."

So I thought:
If i could superimpose more shells, I'll obtain a piecewise linear variation of displacemtens (and then deformations)!

The ansys answer is in the shell91 guide:
"FigurL9e 91.5 SHEL1 Common Node Elements"
it says that i could "also define two elements that share the same nodes but have different settings " that "specifies the nodes to be at the top, middle or bottom surface of the element". I tried to mesh the same area with 2 types of shell91 elements, type one with nodes at top and type 2 with nodes at bottom. But the program says that I can't mesh a already meshed area (obviously).
Anyone knows what the guide means with the tecnic of "sharing common nodes"?

 

[SandwichMaker]

hello.
After some tests I found the way to "share common nodes"in shell elements. It is possible create two parallel shell layers along the thickness of the laminate, here is my procedure:

1 define two types of the same layered shell (for example shell 99), changing the element options so that the first element has "node offset option" (K11) set to "top" and the second to "bottom"

2 create two coinciding areas (for example copying an area with zero offset)

3 mesh area1 with elem type1 and area2 with element type2

4 merge the nodes (numbering ctrls>merge items>merge nodes)

Now the model is formed by two shells in the thickness direction! Loads can be applied like a classic single-shell model.
Unfortunately, results are the same as using a single multilayered element! I have not appreciated the change of slope of through-the-thickness dislpacements...

So, the only way it profiles is to use a number of shell layers with a z-offset separating each from the other.
Is my intention to model the shells with K11 "nodes at midsurf" and mesh a surface with shells for every layer, separating the layers by the distance filled by the shell thickness. The problem is how to bond together those parallel-through the thickness-shell layers.
I'm trying with contact elements and MPC approach, but it seems to be a little difficult and the ANSYS guide is not very helpful/clear about my specific problem. Anyone has experience with this kind of element bonding?

thanks

 

[SKJoe]

Hi,

my english is not very well too, so i hope that i understood...

there is my advice to you : to increase accuracy of solution you dont try to mesh an area with 2 elements.

just try to increase number of layers - you can divide the ply of thickness of 0.1mm by lets say 2 layers the ply of thickness of 10mm by 20 layers...

Regards,

Lubo

 

[SandwichMaker]

Hi, SKJoe.
Thanks for the advice. I've followed your advice, and obtained strong variations on the stiffness of the structure. The plate become less stiff increasing the number of layers: the center point UZ is now 10 times bigger.
I'm a little suspicious on this result
However, the through-the-thickness displacements and deformations still remain linear and continuous; but it was obvious because, like I said in the second post, those elements calculate linear, contiunuous displacements by definition...

I think the only way is a 3D maped Hex mesh, but the layer of prepreg is so thin that I'll have to mesh it with elements too small compared with those that I'll use for mesh the thicker layers: the problem is the "aspect ratio" of prismatic element, the side-to-side dimension coul not exceed 1:20 ratio. But everyone knows it!

Tanks a lot for the reply , it has been very useful to understanding the way of model such plates!

 

[SKJoe]

Hi,

i have some additional notes for you...

1, in fact increasing of accuracy of soution is not depend on number of layers directly, but depend on number of integration (Gauss) points per thickness - you can use less number of layers with more integration points and vice versa. for one layer is it possible to set from 3 to 9 integration points.

2, you can try to use SECTION instead REAL, for me is it easier to use section command. i dont know if it is possible to vary number of integration points via real command.

3, you can try to use different element type : SHELL181 (it has membrane options) instead SHELL99...

4, you have not mentioned ratio between thickness and deformation. if thickness is comparable with deformation you must perform nonlinear solution instead linear.

regards,

lubo

 

[SandwichMaker]

Hi,
SKJoe your advices open me everytime a new way in modeling and meshing. I'm studying the structure with the shell sections menu and it's much more easy control the through-thickness geometry. Thank you!
Some specs you requested:
-now meshing with shell181
-calculating small deflections, principally because I'm comparing the results with linear elastic results
-displacement/sandwich thickness ratio is manteined between 0.05 and 0.01. I could say I'm working with very "small deflections"
-for the moment I'm not interested to geometric nonlinearities
-my plate dimensions are 1x1x0.003 [m]

Now I'm going evaluate the continuity and linearity of strains through Z in the center of the plate.

I've also modeled a plate with solid layered elements like solid191, with mesh 40 divisions on X&Y(decreasing dimension in proximity of the center point of the plate) and 6 divisions on Z. The number of elements was huge and taked 2 hours of computing time. With this model I've finally appreciated the piecewise variation of strains along Z but maybe with shell and sections control I'll achieve the same results (the center deflections with shell 181 matched the huge solid model result!) with a thousands times simpler model!

Cheers

 

[SandwichMaker]

Hi,
I've got some good results.
Shell elements are not suitable for the problem. Meshing the plate with solid181 gave me the right solution. It requires a more expensive model in terms of operation time but I could say it's the only way. I've meshed my four layers with the same 60x60x1 elements using the layer option to stack the laminated faces: 60x60 mesh on the plane X-Y, 4 elements along the thickness (Z direction, a element for every layer).
This is the way the plate is meant to be meshed.