Plate Element Thickness Overlap Error

[gharli]

Hi All,

I am busy modelling a concrete tower with overall dimensions of 5.2m x 5.2m x 40m high.

The walls vary in thickness and shape.

At one of the corners of the tower, the attached image shows the geometry thereof.

The centre lines of the tower walls are shown in red, yellow, green and blue.

The intention is to model the tower using Quad8 plate elements with the above mentioned lines being the centre lines.

My concern is the potential “thickness” overlap of the red, green and blue elements (shown in the bottom hatched image).

For all FEM gurus out there, is this a potential concern and if so, what modelling techniques should one incorporate?

The tower will be buried and hence subject to huge lateral and downdrag forces. In addition, without going into every last detail, these nibs are critical to the functioning of the tower.

I’m interested in all opinions, image is here:

[link

http://files.engineering.com/getfil...0e-9110-6392d38645b9&file=Element_Overlap.JPG

]Link[/url]

Thanks,


_________________
Jones & Wagener

http://www.jaws.co.za

 

[corus]

This also happens when modelling I beams, for example, where if the flanges and webs of the beams are modelled with plate elements so they connect then you get an overlap of material. When the thickness of the plates is relatively thin to the overall size of plate then this shouldn't be of concern, though some suggest that gaps are left where the overlap occurs and the edges are tied together across the gap so no overlap of material occurs. This approach would be very time consuming though. In your case the thickness of material appears significant to the overall geometry so I'd have used 3D elements rather than thin shells.

 

[gharli]

Thanks Corus, point taken regarding thickness vs. length of element being a concern.

I'm reluctant to use 3D elements for 2 reasons:

1. Complexity of the model will obviously go up orders of magnitude (and hence processing time).
2. I'm after internal moments at the end of the day (for design purposes). If I use 3D elements I'd end up having to manually integrate the stresses at each design area...

Thanks for the reply!

_________________
Jones & Wagener

http://www.jaws.co.za

 

[corus]

Getting the bending stresses etc shouldn't be a concern as a lot of software provide means of integrating the stresses along a line to get the equivalent direct and bending components. It depends on the software you have though.

 

[ebdoep2]

It seems to me you are trying a square peg in a round hole. I would be reluctant to trust the bending moment numbers you would get from the plate solution because you are making them do something they were not really designed for.

But I also understand the convenience and computation factors. I would model a small but representative portion of the wall, one with full 3D analysis and the next with the simple plate and don't worry about the overlap. See how deflections and stresses compare in your critical loading case.

Maybe with a little luck the plate solution will get you through. If not make sure you use brick elements instead of tets in the 3D and that will save you massively on computation.

 

[gharli]

Hi All,
Just to close this thread out, for those who may be interested.

I’ve done a comparison of the deflections and bending moment for 3 situations:
1. Quad 8 plates with a normal face pressure.
2. Quad 8 plates with an “equivalent” normal edge shear stress (this would have clearly lead to more conservative results as a result of a longer lever arm but was done for interest sake).
3. Hex 8 brick elements with a normal face pressure. I had to manually integrate the stresses across the section as the software that I’m using (Strand7) doesn’t have that ability (if I’m wrong, please correct me).

A convergence study was done to determine adequate mesh densities.

Image showing 2D plates and 3D brick elements:

Graphed results:

Conclusions:
1. Although significant material thickness overlap occurs in the 2D plate model, the stress results are very close to that of the brick model.

​

a. Moment of 13.05kNm (2D) cf. Moment of 11.62kNm (3D). 2D plate is 11% higher.
2. Deflections are significantly different with the 3D model exhibiting a far higher stiffness to that of the 2D model.

​

a. Deflection of 0.291mm (2D) cf. 0.137mm (3D).

This is by no means meant to be a comprehensive study, but thoughts and comments are most welcome.


_________________
Jones & Wagener

http://www.jaws.co.za

 

[corus]

Personally I wouldn't read anything into the comparison as the geometry is plainly unsuitable for shell elements. I don't understand the representation of the 3D model by shell elements, that you've used. It could be that the shell parts are too long and as such are less stiff to give higher deflections. The agreement with stresses may just be coincidental.

 

[gharli]

Your points are noted and in addition, after some thought, having a single result that correlates doesn't give me the confidence to move forward on the 2D plate basis.

Having said that, I do believe that the probability of the results being so close considering the use of different formulation, different geometry, and manual integration of the stress block compared to straight forward output, is extremely low.

Thanks for the input.

_________________
Jones & Wagener

http://www.jaws.co.za