CTRIA3 Elements

[richardmorris]

I’m trying to de-idealise results from a very large existing aircraft FE Model. The model contains a number of TRIA3 elements in the fuselage side skins and I can’t quite workout how these elements are working. If you de-idealise them using the grid point forces as you would a QUAD4 it would suggest that these elements to a large extent simply carry end load along the edges, as the end loads are equal and opposite along each edge and therefore there doesn’t appear to be any shear forces involved. So instead of representing the shear capability of the skin they appear to have the effect of introducing additional end load carrying stiffeners. In certain instances, were there is a gap between existing stiffeners these elements seem to bridge this gap and in effective change the load path from what would be expected. Looking at various web sites what comes through is that these elements are ‘over stiff’, I could reduce the thickness down to virtually zero to remove the end load capability, but then in effect I would be introducing a hole.
Has any body come across a similar problem and found a solution to using these elements to effectively transfer shear but not end load.

 

[rb1957]

from my experience 3 noded triangles "suck, big time". perhaps not too technical an answer but ...

it sounds like you've noticed "issues" with the internal loads, not only of the triangles, but also on their neighbours. perhaps, if you wanted to make them shear stiff (and endload soft) you could trick the material matrix. i'd try this out of a test panel to see how it works before committing to this approach.

i expect that most of these are in areas of mesh transition. i'd investigate remeshing quads and tris to remove the tris, this'll produce kites, but i think they're better than tris.

good luck

 

[SWComposites]

Yes, 3 noded triangles are usually too stiff, and they can only represent a constant strain value across the element, so may have difficultly modeling a shear strain field. I can't imagine why someone would mesh a fuselage with triangles, especially if one also wants to have nodes along the stringers and frames. Aircraft fuselages are often modelled with shear elements representing the skin and beam elements for the stringers and frames; this avoid having the skin elements carry axial loads.

 

[richardmorris]

Thanks for the replies, If I understood you correctly, I’ve just tried reducing the E value in the material card to practically zero and I get the same results as with the panels not being there, altering the G value made no difference at all. Basically, it seems to have just one mode of balancing itself, so changing the E value or thickness just changes the magnitude of the loading not how the element reacts. (i.e. it does not appear to be like a plate were as when you reduce the thickness more of the load is taken by membrane and less by bending)

The area I’m looking at is the side skin below the canopy on a fighter, so it’s not your standard stringer/frames configuration where every thing tends to be at right angles to each other. On the actual structure, stingers/ stiffeners are not all horizontal and they do actually come together at certain positions to produce a ‘point’. Also the canopy posts are not vertical (looking inb’d/out’bd) so again when in attaches to the frame you do actually have a triangular piece of skin.

The stingers are modelled using rods for the stringers and shear elements for the skin. I suppose if you just consider a triangular piece of skin on it’s own it can’t be balanced by pure shear on it’s edges alone. So would it be safe to say I’m never going to be able to get any ‘reasonable’ results using this combination of element types.

 

[rb1957]

maybe the best thing is to remesh this panel to either remove the triangle or to leave a small triangle in the middle ?

you might look at a 6 noded triangle, these behave much better.

 

[fkmeyers]

If you are using Nastran, use the CTRIAR elements as they are decent and unlike CTRIA3 which is a constant strain element, they are linear strain.

 

[vonlueke]

richardmorris: Alternately, can you just convert your model to tria6 and quad8 elements? Like fkmeyers suggestion, no remeshing is required, and this eliminates the tria3 elements.

 

[pbd999]

I don't think the CTRIAR is a linear strain element. The way I understand FEA theory is that with only 3 nodes available to create the shape function, you get a constant strain element. The CQUADR and CTRIAR are better than the old standbys CQUAD4 and CTRIA3, but the biggest difference between them I think is that they have 6 degrees of freedom at each node rather than 5 by including the "drilling" stiffness.

Paul

 

[fkmeyers]

CTRIAR and CQUADR elements are basically CTRIA6 and CQUAD8 elements with a transformation that converts the mid-side node displacements (x and y) into vertex drill DOF (membrane). For bending they use the same approach as the CTRIA3 and CQUAD4. The is true in MSC, NX, and NE Nastran versions. There are papers written by MSC and NE available. The CQUAD8 and CTRIA6 are parabolic elements. I think pbd999 is confusing what K6ROT in Nastran does which is to simply add a loosely coupled drill stiffness which is not the same. I think there is a paper on this for NE Nastran which explains exactly what they do on their website

http://www.nenastran.com.

You may have to ask them directly for it since it basically gives the theory behind the element.

 

[pbd999]

I asked someone at MSC this question and here was his response, "The CTRIAR element is exactly the same as the CTRIA3 element except for the drilling dof (rotational component of motion normal to the plane of three connecting grid points) of the element, hence this makes it a constant strain element."

NE/Nastran may be different...I have never used it...

 

[fkmeyers]

This just proves that MSC is no longer the company it was and those who are still there really do not know their own product. To prove my point I created a simple cantilever beam in MSC Nastran 2005. The beam was 10" long x 1" high and 0.1" thick. I meshed it with 80 CTRIA3 elements and made a 2nd model with 80 CTRIAR elements. The CTRIAR model was within 5% on displacement and stress from beam theory. The CTRIA3 model was off by more than 60%. If the CTRIAR was EXACTLY the same would this be the case? A nice consequence in the CTRIAR model is you get a vertex drill rotation that matches beam theory as well. I recommend you go back to MSC and educate them on their own product. This is one of the reasons we are using NE Nastran now. They seem to know their own product.