3 Node Triangular Shell Elements 1

[kellnerp]

I am doing a side study of the behavior of the various shell elements I have at my disposal. When I use triangular 3 node shells I get some peculiar behavior.

I modeled a long thin strip and put one row of triangles down the length. It is restrained as a cantilever. Here is a list of the odd behaviors:

1. I must constrain all dof or the model is underconstrained. UX, UY, and RZ should be enough but they aren't.
2. The reactions in the UY direction (same as load) are not equal.
3. There are moments about the free edges of the strip.
4. If I use displacement loading the reactions are unequal.

When I add midside nodes to get 6 node shells there is similar behavior but to a lesser degree.

Any thoughts? I have a guess.

TOP
CSWP
BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[gwolf2]

See Sleipner Disaster on a web search. It is the most expensive FE mistake I know of relating to these elements.

gwolf

 

[gwolf2]

p.s. Please name your code - sounds like nastran, you have to constrain dofs even when they are not used by the element.

 

[kellnerp]

Wow, 3.0 on the Richter scale and no airliners involved.

Results indicate that the current ACI code provisions are very unconservative.

and

The bearing capacity of a thinner wall depended also on the length of the wall. At some point in the optimization process it was discovered that, given its thickness, the length of the tricell walls was to long. The solution to this problem that was proposed was to go back to the model of the element mesh and add a triangular element in the sharp tricell corner. The alternative, making the walls thicker again, would increase the weight of the GBS and the total amount of concrete again. The triangular element filling in the tricell corners solved the problem by reducing the length of the tricell walls between its supports. The amount of concrete necessary to fill in the corners on the construction site was limited..

It is not clear whether they are referring to a triangular finite element or a triangular shaped portion of the structure. I take them to mean the latter.

Apparently in the scope of this project there was considerable review and risk assessment. The engineering team also prided itself in engineering out weight.

Anyway this is kind of off the topic. The software I am using also has a quad element made up of two triangular elements and it is also exhibiting the kind of behavior I am seeing with the 3 node element.

I am just testing elements anyway, not using them in any particular projects. I am still curious as to the inner workings of these elements.



TOP
CSWP
BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[GregLocock]

Yup, the tricell was a structural component of the rig, not necessarily modelled with 3 node elephants.

Cheers

Greg Locock

SIGlease see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[johnhors]

The software I am using also has a quad element made up of two triangular elements

uh? Really? If so, then its not a quad element, its two triangular elements. What code is this?

 

[corus]

I've seen early codes that used 4 triangular elements to define a 'quad' element. These were 'in-house' codes and full of bugs, needless to say.

To get back to the original questions

1. You need to constrain all dofs even if there is no load in that direction.
2. Reaction forces won't be equal at all nodes but will be distributed in the shape of a parabola. I think this is because a rectangular section is less stiff towarsd the free edges. Refer to shear stress distributions in beams.
3. You may see moments at the free edge due to the mesh density even when theoretically they should be zero. Finite elements are by no means perfect.
4. Whether you use displacements or loads, the problem is equivalemt, and the same answer as 2 applies.

corus

 

[rb1957]

personally, i think the only thing 3 noded triangles are good for is target practice. they are horrible elements; and a quad made up of two tris is horrible^2.

 

[johnhors]

Why stop at two triangles?

Join three together and have a pentangular element?

Of course this is nonsense!

 

[pja]

The stiffness matrix for the workhouse quad shell element in ANSYS (until shell181 came along) SHELL63 consists of a superposition of the stiffness matrices of 4 DKT (triangular) elements. Many commercial codes have shell elements like this..which is what I think he was talking about.

 

[kellnerp]

uh? Really? If so, then its not a quad element, its two triangular elements. ...

See Cook 3rd ed., pp. 242ff on macroelements.

I have four choices for formulation of four node shell elements:

QUAD 2 element (2 triangles to form a quadrilateral)
QUAD 4 element (4 triangles to form a quadrilateral)
QUAD element (4 node quadrilateral element)
QM6 (4 node quadrilateral element)

Default is the QUAD 2 formulation.

Actually I finished testing the shells that I have available and the QUAD element with the QUAD2 option (2triangles) is the worst, not because I can't get it to converge, but because it converges on a lower stress than the hand calc. The plain old 3 node shell does converge to the same stress that the others do, which approaches the hand calc to withing a fraction of a percent. The other formulation of the 4 node QUAD give a higher stress than the 2 triangle formulation, but still underestimate the stress.

In order to compare stress to the hand calc with a cantilevered strip 1 wide and 10 long and .5 thick the top fiber stresses are averaged across the width. The stress distribution approaches parabolic for most of the elements but for the 4 node QUAD it look more like qartic when the element count goes way up.

I would feel comfortable with these shell elements except the 4 node quad.

Thanks Corus, you hit it.

PJA, that is the formulation I am talking about. They don't specify which formulation for the sub triangles so I have no way to tell if they are DKT or not.

TOP
CSWP
BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[gwolf2]

>It is not clear whether they are referring to a triangular finite element or a triangular shaped portion of the structure. I take them to mean the latter.

It means both! One triangular shell was used to model the new connection between concrete tubes. From memory, the stresses were 60% out the wrong way.

As I understand it, someone please correct me if I am wrong: The insurer was as I recall Det Norske Veritas, and their analysis division OK'd the potential customer's analysis. The problem was that the insurer's analysis division used the same mesh as the customer instead of making a new model. They of course fell into the same hole, OK'd the design, and ended up 400,000,000 somethings worse off

Triangular elements are agents of the Devil..............

Must have been spectacular for any passing whales as they watched it drop past. I heard it was doing around 100 mph when it hit the bottom of the fjord.

gwolf

 

[kellnerp]

I found the paper describing blow by blow a hind sight analysis of the failure. The analysts apparently all knew each other (Denmark is a small country) by whoever wrote the paper didn't always make statements about FEA that were clear. That suggests a second hand source.

There was more to it than a misplaced 3 node element. Apparently they substituted a new-fangled rebar retention system for the tried and true bent rebar. The T shaped end caused a stress riser which seriously weakened the concrete around the end of the rebar.

There was also the fact that the support which failed was designed before the superstructure. When the superstructure was finished it was overweight and they had to lengthen the tubular members. The analysis of the lengthening was done in a hurry when it was not clear who was responsible for what. This was more than an inappropriate use of a 3 node element.

They apparently detailed off the Global Analysis (GA) too and they limited the number of drawings and hence details that had to be figured because of the size of the project.

In the words of the report, before the failure they did nothing wrong. All the boxes were checked. It was only after the failure that it was determined that something was wrong.

It would be interesting to see a snapshot of the mesh in the area you are talking about.

The one thing I found during my testing is that in a "hot" area you want more than one element along an edge or face, especially if there is a big stress gradient. Higher order elements can reduce the amount of refinement needed. But you still don't want to rely on just one element in a critical area.

TOP
CSWP
BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[corus]

It seems to me that what the disaster emphasises is the need to not rely solely on the results of a finite element analysis. I always thought this compewtericestation electrickery of design and analysis would bring doom.

corus

 

[kellnerp]

Sliepner did do tests IIRC. They did everything right.

My final thought is that you should take the time to know your tools. I can get good answers from 3 node elements. Let's face it, that was the first plate/shell element available and was used on aircraft way back in the punch card days.

Deflection will converge with a very coarse mesh, but stress is another thing. How many people running the current rash of "instant" FEA don't take the time to check things out.

TOP
CSWP
BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[rb1957]

Too Damn Many ...

 

[gwolf2]

Kellnerp,

I've had a look around and I can't find the mesh picture which I remember. It was definitely hardly any (probably just one) element in the critical area.

"I can get good answers from 3 node elements."

Agreed, if you check carefully and generally know what you are doing. I sometimes make outrageous models which break a few of the good codes of practice, but I know what I'm doing and often have a small test analysis to back it up.

Anyway, interesting new information on the Sleipner disaster. David Hibbitt of ABAQUS fame used to do a great after dinner speech on FE cock-ups. Maybe there is food for a new thread "Worst analysis I ever saw"............

gwolf

gwolf