plates perpendicular to each other 2

[netjack]

I am trying to model a structure made from plates and supporting bars. Think about 2 rectangular plates connected to each other by supporting plates and bars that are perpendicular to 2 plates. As far as I know, if I connect plates perpendicular directly on the same node, I end up with very flexible structure than real. Nastran manual says put a bar element at the corner to compensate. Do you have any suggestions or design tips for this analysis.

 

[dubourg]

I get very good correlations between FEA and experiment when using shell perpendicular to each other (either Nastran or Ansys). Why is it so flexible in your case ? Are you using shell elements and perpendicular beams to these shells ?

 

[austim]

I would have expected reasonable results without the corner beam elements, PROVIDED that your plate elements are 3D plate bending elements, and not just simple 2D membranes.

 

[brad]

Depending on the software, what version of the software, and what specific controls/parameters you are using, this could be an overly-compliant situation. Shells do not by their formulation have "drilling" degrees of freedom (in-plane rotation). Different codes handle this fact differently. If this is not addressed by the code and/or the user, this may result in overly-compliant answers (for particularly-posed problems) when compared with "reality".

The problem which netjack has posed is an example of this very behavior. Imagine two flate shell structures, one of top of another, both with normal in the z direction. If I connect these two structures with a beam element which is oriented along z, there is no means in the "classic" shell formulation to react moment about z from the shells.

Most codes have some means of addressing this problem, either via "artificial" stiffness in this dof (often done automatically), or through automatically constraining this when it occurs.

Other ways to address this: connect to more than one element, or use elements to distribute these loads.

 

[netjack]

I am using standard 3D shell elements. I will also use beams but currently i am concentrated in plate joints. This drilling dof problem as bradth mentioned appears in Nastran practical guide and also in one of Aerospace company's ýnternal research group documentation. Do you think solid elements can give satisfactory answers as long as you provide fine mesh instead of shell elements. If this is the case, I want to try to open a simple L profile both by shell and solid elements.

 

[brad]

As long as the mesh is fine enough, that should work. Note that, using Nastran, you'll need several solid elements through the thickness (as I expect they'll see bending). If you don't have enough through-thickness shells, you'll get an overly stiff response.

One other thing--
Although I am not a current Nastran user, I understand that MSC has recently introduced something called SNORM. One of my former colleagues has been playing with it. I have heard good and bad things about it, but it is my understanding that this in some way addresses issues with drilling degrees of freedom (although I think you may need to use K6ROT in conjunction with it). As I said, I don't know the details myself, so don't take this as anything definitive--maybe look into the user guide on this.

Brad

 

[TonyA]

There seem to be 2 issues. 1. Plates perpendicular to each other forming an L - the reason a bar is recommended is that you cannot model accurately the torsional stiffness of the intersection line otherwise. In practice it will be welded, bolted or have some corner radius which will contribute a torsional stiffness. Put this in via the bar. Trying to match analysis natural freqs with test on thin walled structures often shows how critical this is and may well be true for statics in your case.

2. Plates parallel connect with bars rods etc. This opens up the drilling dof problem with the plate. You cannot use SNORM,K6ROT etc. to constrain a rod perpendicular to a plate. The rod ends need to be connected by a 'spreader' type of technique using rigid elements to transmit the drilling moment into differential translations in the plate wherever you choose. SNORM is a technique in Nastran used where the plates are essentially connected in the same plane, but small unpredictable angles between them introduce stiffness into the drilling dofs by terms coming from the adjacent edge bending stiffnesses. That means the drilling stiffness term which should be zero is non zero and cannot be eliminated by AUTOSPC. The result is a spurious small stiffness which may have effects ranging from negligible to mechanisms. SNORM 20 degrees seems to be a very robust default.

 

[Ron]

Check your model and make sure all the common nodes have been merged after meshing. This will cause the problem you described in some software applications.