Bug in hydrostatic pressure and position dependent position on shells

Victor

Mecway Versions 1-6 have a bug with shell elements that have either hydrostatic pressure or normal pressure as a function of position. It uses the position of the shell's node plane instead of the face to evaluate the pressure. This will be fixed in version 7.

The attached model demonstrates the effect. It's a 0.1 m thick plate with the top surface under 0.05 m of water. The pressure there should be:

P = density * g * h

  = 1000 kg/m^3 * 10 N/kg * 0.05 m

  = 500 Pa

  

But, due to the bug, it uses the depth of the shell midplane, which is 0.1 m below the surface. The pressure it applies is:

P = density * g * h

  = 1000 kg/m^3 * 10 N/kg * 0.1 m

  = 1000 Pa

which is reported as a reaction force of F = 1000 Pa * pi m^2 = 3141 N.

  

This example is chosen to highlight the error. It won't be so big in a typical case where the shell is thin compared to the depth of fluid.

Andrea

OK!
So next release is coming soon?

Have you other news about it?

Victor

I don't have a timeline for version 7. But some things it has are distributed moment loads on faces, pressure XYZ can be a function of position, stress linearization doesn't require nodes to be on the SCL line, and more features work with CCX.

Sergio

Great news Victor! Can you look for some way to move the option of reduced integration elements from a "program option" to a "file option"? Now can be a little problematic if we forgive to swich of the option on models that don't needed it.

Regards

Victor

I'm still not clear on when reduced integration should and shouldn't be used so I don't want to commit to having it saved with the model yet.

Sergio

In my humild opinion, the more logical from the point of view of the FEA would be in the material, because one would like that all of element of the same material behave the same. If it would be in model, then all materials/components would have this behavieur and very often this is not true. Other place were it has some logic would be at the mesh definition, as we choose the shape and grade of the element, the integration point sounds logical to be here also, but then the problem arise in case of imported meshes that has no definition... so there would not be oportunity to add it.

Now that I has writted, I found that also in the material could be the same problem, sometimes we add the materials in the CCX custom content. Even if that definition were in the Component defintion (that again, it has his logic), we could also work without components and again no way to define it. 

My votes are on the Component. Now that they can be hidden/unhidden in the postprocessor, they are usefull and there is no way to create it as custom content, so one will almost always define it.

Regards

Andrea

I sometimes use reduced integration elements in plastic analysis to reduce computation time. Reduced integration uses a lesser number of Gaussian coordinates when solving the integral. This involves 8/20 nodes brick elements and 4/8 node shell elements. So using tetra for the most of times is not possible to use reduced integration elements.
Someone recommends:
"Therefore, in some cases, particularly non-linear problems such as plasticity, creep or incompressible materials, it is actually advisable to use reduced integration instead of full integration. The slight loss of accuracy is counteracted by the improvement in approximation to real-life behaviour"

Obviously there is a less accuracy on results and can lead to hourglassing. Take care to use reduced integration in buckling analysis or in stress analysis if you want to capture peack stress because is necessary have more elements.
To change elements I use "Scite" or a simple txt editor simply using "replace".

Victor

Thanks Andrea. That helps a bit. It still seems like a bit of a black art. It's looking like it should be set by both element shape and component.

Andrea

Here a good explanation of the basic problems related to reduced integration elements

http://optimec.ca/news/how-to-model-bending-and-bending-dominated-problems-in-abaqus/

kwip

In almost all cases elements of type C3D20R are the Elements of choice.

Stress gradients (not speaking of singularities) are resolved by refinement anyway. One major advantage of those Elements is their superconvergent behavior, thus the stress Inter-/Extrapolation works best.

Pls. compare "Barlow, J., Optimal stress locations in finite element models. Int. J. Num. Meth. Engng. 10 , 243-251 (1976). " ... the latter publication shows that from the interpolation perspective the best locations are the 0.577...  spots which are the gauss point positions of reduced integrated quadratic elements.

regards