Issues with FEA of ship section in ANSYS APDL

I've created a 3D model of a ship section in Rhino and imported it into ANSYS where I glued the areas together and meshed the model. The problem I'm having is that when I apply the hydrostatic pressure along the outside of the hull, significant deformation occurs. I've tried various boundary conditions from constraining all degrees of freedom at either end of the structure and constraining the transverse frames and stiffeners along the structure. I've attached pictures to show the deformations I am encountering, any help would be much appreciated as I can't progress with my project until this is sorted.

 

Giving an opinion with that data is like trying to guess the future with a crystal ball. What can be seen seems to indicate that the buckling of the sidewall plates occurs, more plate thickness is needed or, better, a greater number of longitudinal reinforcements or longitudinal reinforcements with a greater modulus of resistance.
If the model is correct, it can only be that the structure is weak.
Check again and again that the contour elements are well defined and the fasteners of the knots are correct.

 

It is not wholly clear what you mean by significant deformations. What values are you getting?

Can you show/describe your model at said locations in better detail....element types, element size, and how you are applying the loads etc.

 

Besides explain to us "element types, element size, and how are you applying the loads etc.", please have a look at your structure that presents several things, different, with respect to a normal structure:
- There are no transversal beams on the intermediate decks.
- the longitudinal reinforcements in general are very small compared to the frames and do not seem to be properly attached to them.
- Those vertical reinforcements, what purpose do they have?
- the top of the double bottom, does not reach the side?
You should concentrate on making a more "normal" structure layout before starting to calculate anything. Once you have designed the correct structure, you can make the 3D model and then calculate scantling with the software you like the better. S0ftware can't design the structure.

 

I forgot to mention that the modelled section is between 2 watertight bulkheads, as for why the vertical stiffeners are there and appear to be attached to nothing, the bulkheads are normally there but have been removed to show the interior of the section a bit better. The frames and stiffeners are both attached to the walls/bottom however I tried many different ways to connect them both directly to each other without much luck.

Shell element type is being used (SHELL181), the full section is 12m in length, 9.5m depth and 11m beam. The longitudinal stiffeners have heights of 0.25m, spaced 0.8m apart, the girders are 0.5m with the same spacing and the transverse frames have a spacing of 1m along the length of the section.

Since the model involved a lot of overlapping areas/gluing them in order for a solution to be obtained, it has resulted in there being a lot of individual areas along the outside of the hull (all the rectangles seen in the standard screenshot), I think this may have something to do with the problem I'm having. I am applying the pressure to the outer nodes of the hull by using a function of P=pgh (with the draught being at 6m). Obviously the model shouldn't be deforming under such standard conditions, but I was thinking it was maybe because of all these new areas being formed rather than one, larger area being used.

I've attached images of the model constrained at both ends, with the nodal displacement values along the bottom. As you can see, having a maximum nodal displacement in the vertical direction of 0.011895m at the bottom and horizontally of 0.002213m is not really ideal!

 

1) Can you not apply the pressure at the plate centre, rather than at the nodes?
2) Make a simple model of a flat plate with known dims, make it simple support and then built-in. Apply the same hydro pressure. This is a standard and simple calculation you can also do by hand. Thus to compare the model and your hand clac's, are they the same, ergo, is your modelling and application of the boundary conditions and applying the loads, correct?
3) a deflection of 2.2mm is not much!..i assume that is less than plate thickness!?

 

Yes, you are correct that the deflection actually isn't much compared to the plate thickness. I was able to set the displacement scale to 1:1 in the settings so that the deformed shape wasn't being exaggerated and it seems to be displaying it correctly with no significant deformations. I am still relatively inexperienced with APDL so I appreciate the help, thank you!

 

The purpose of the deformed shape plot is to highlight on an exaggerated scale what is going on. You then check what the values are in those regions. Since any deformation, when a scale is applied, will look extremely bad. But it is a visual aid only. The values, beit displacement, stress etc, is what you then need to review.

Don't let the tail wag the dog!!

 

I do not know if it makes any sense to talk about small or large deformations (how the hell!) of a structure that, imo, presents serious deficiencies in its conception.
Why are there deformations on the side, very close to the neutral axis, and there are no deformations on the upper deck ?. Strange.