"Use Corner data" option in FEMAP 3

[sir0co]

Hello all,
I have a doubt related to postprocessing results in Femap. I've made some estructural linear analisys and I've found that exist great differences in stress values in some little areas (where stress concentrates) if you active or not the corner data results. Actually, without corner data results I can get some reasonably good results and with corner data results I get little peaks of high stress (maybe 100 MPa higher), specially in some vertex(even in areas with a fine mesh).
Do you recommend me having into account all data for postprocessing results? Or maybe this high stress peaks in little areas don't exist in the real model with this values?
I have to say that without corner data results I get a more 'homogenous' stress concentration in these areas a with a lower value...
Thanks so much in advance.

Jose

 

[mechfeeney]

It could be your mesh refinement in those areas. Typically bogus values will appear as stress concentrations if the mesh is too coarse in the corners. Do a total model or local area mesh refinement and observe the changes until it converges. Compare with hand calculations too.

 

[sir0co]

Thanks so much for the answer. Unfortunately it´s not easy in this case making hand calculations because of the complexity of the model, but it has sense bogus values in corners due to a coarse mesh. Actually, when I turn on "Corner data results" I find fast stress transitions along the same element until a high peak in the corner, what doesn't seem very logical in most of cases.
However I would like to know the convenience of having in account the "corner data results" in these cases. Maybe it's more realistic to activate only the elemental data results when mesh is not very refinated??

 

[mechfeeney]

Yes, if the results are changing as a function of your mesh size, then the mesh is clearly not refined enough. Additionally, if the stress values are changing drastically from one element to the adjacent element, these are clear signs of a unrefined mesh. You can locally refine these areas, or you can do a brute force and refine the entire model.

 

[sir0co]

Thank you, I will have into account your advice, but only refining the local area because my model is quite big (about 120.000 nodes) and it would take much processing time.
Best regards!

 

[rb1957]

this sounds odd to me ... importing corner data should allow FeMap to average the four element results at a common node and base fringe plot on these (as opposed to using the element centroid stress).

dumb question ... you have checked for coincident nodes ? (and removed them)

 

[sir0co]

Hi rb1957, the answer to your question is yes. As well I've tried to be very careful with this model, trying to get quad maped meshes of quality in every component. The real thing is that I'm a bit surprised with some results because of the great differences in some areas between elemental data and corner data postprocessing.
At last, I have the feeling of not to be getting realistic or accurate results...

 

[rb1957]

is this a fuselage under pressure ?

 

[sir0co]

no, is something much simpler. It's a kind of structure with a tubular beam reinforced in the base with a few triangular gussets. The thing is that if I consider "corner data" in postprocessing the stress is much higher in some corner gussets than if I don't consider them, but only in a very little area (little peak with fast stress transition inside an only element). As well the difference between the values obtained is quite high, so I'm not very convinced about these results.
What do you recommend me, to have in account 'corner data' being conservative or trying to remesh with a fine mesh in this area and check again?

 

[mechfeeney]

Tubular beam? What type of elements? If solids, how many through the thickness? Do you have pictures?

 

[sir0co]

I've used plate elements (quad planar in Nastran)for meshing both the tubular beam and triangular gussets.
On the other hand, I don't have pictures in this moment because it's an enterprise project and I'm at home right now. Tomorrow I will upload an image(A picture is worth a thousand words...)

 

[sir0co]

Hi, I've uploaded a pair of pictures of the problem.
In the first one I have the postprocessing only considering elemental data results. The stress distribution is smoother in the area close to the inferior corner and the maximum von misses stress is 263 MPa, what is under the Yield tensile strenght for S275 Steel. Safety factor is very reduced, but well, anyway.

http://files.engineering.com/getfile.aspx?folder=61caba93-2bcf-4e51-b843-4a88fd87a714&file=1.bmp

On the other hand, I have the postprocessing considering averaged corner data results. In this case I get a maximun stress of 324 MPa, what is over the Yield tensile strenght. As well, the stress transition is faster in the corner element.

http://files.engineering.com/getfile.aspx?folder=27be8820-acc5-4337-bf73-bb349bb697f6&file=2.bmp

The difference of the max values between this two postprocessing results is more than 60 MPa (what is a lot!), and that's the reason because I'm a bit confused and can't believe in the accuracy of the results...

 

[rb1957]

3 noded triangles ?

 

[sir0co]

4 noded quads, as you can see in the pictures

 

[rb1957]

ok, i was picking up on "triangular" gussets.

i think your pix clearly show what is happening. in pic 2 you have imported nodal stresses, so the program can plot them. ie the stress peak at the corner node is imported and plotted. in pic 1, using only element data, the program doesn't extraploate well from element centroid to the edge (i think it is extrapolating from one element centroid to the next and projecting this tragectory into the corner.

pic 2 is the better set of results. the fact that the FEA is predicting localised yielding isn't too much of a concern ... hand calc would never calculate it, the yielding wouldn't be evidient or detrimental to the structure. it is also due to the rigidity of the joint inherent in FEA; in reality there is a finite stiffness between the gusset edge and the shell (rather than the infinite stiffness moidelled by sharing the node).

 

[mechfeeney]

Your nodes are pretty distorted around that corner. Try the localized refinement around those corners.

 

[rb1957]

scrub (maybe) that infinite stiffness comment ... on 2nd look you have different nodes on the tube and on the gusset, joined by a finite stiffness spring or an infinite stiffness RBE ?

 

[mechfeeney]

Yeah....there is some funky interface he's got going on.

 

[sir0co]

Hi, thanks for your answers!
I think it was really a refinement mesh problem in that area. Actually, I've remeshing the gusset with a smaller element size and I've observed that both elemental centroid results and nodal results converge in similar results, so you were right when said that pic 2 shows better results.
In another hand, nodes in left side of the gusset are common to the ones of the tube and I've connected low nodes of the gusset with the base using RBE2 elements with 6 DOF fixed (in NX Nastran it represents infinite stiffness elements, so it's the same that sharing the node). Would you have modeled it in other different way? Maybe extending the gusset until the base and sharing common nodes?
As well, you have said something interesting: "the fact that the FEA is predicting localised yielding isn't too much of a concern ... hand calc would never calculate it, the yielding wouldn't be evidient or detrimental to the structure". Why do you think that this localised stress wouldn't take place in a real model only because a hand calculation doesn't take it into account? If what you say is true, I should rethink many concepts realated to postprocessing and validating a model using FEA...

Mechfeeney, I consider distortion in that elements is not very high. In fact checking both the alternate taper and internal angles I get some good enough ratios (internal angles < 30º and alternate taper < 0.05) so I think the main problem was not elemental distortion but mesh size.

http://files.engineering.com/getfile.aspx?folder=ed40db25-7d8c-4830-8ce5-85cc4a651393&file=3.bmp

As well, you comment that there is something strange in that model. What are you referring to exactly? Well, I have to recognize that I'm relatively new in fem and maybe I'm making something wrong...

 

[BlasMolero]

Dear Jose,
Remember, when you define the "NASTRAN Output Request" you have an option at the base of the form that you can switch ON/OF named "element corner results", when ON then FEMAP will write the following in the nastran case control:
FORCE(PLOT,CORNER) = ALL
STRESS(PLOT,CORNER) = ALL

If OFF the nastran input will be as follow:
FORCE(PLOT) = ALL
STRESS(PLOT) = ALL

You can request corner outputs (stress, strain, and force) for CQUAD4 in addition to the center values with the STRESS, STRAIN, and FORCE Case Control commands. Corner results are extrapolated from the corner displacements and rotations by using a strain rosette analogy with a cubic correction for bending.

When you select "element corner results", output is computed at the center and four corners for each CQUAD4 element, in a format similar to that of CQUAD8 and CQUADR elements.

In summary, what I try to tell you is the SOLVER computes stress at the corner nodes, then is mandatory to activate "use corner data" when postprocessing stress results in FEMAP, not to ignore this data at all because the stress results are too high.

Another history (but closely related) is the quality of the mesh: I saw your pictures, not too bad, the mesh density in a finite element model has important implications for both accuracy and cost. I am of those that spend all the time required to prepare geometry (splitting surfaces, using pads, washers, etc..) to have the BEST quality mesh as possible, with the less distortion as possible (in case of shell elements the ALT TAPER to be less than 0.5 always!!). How fine a mesh you want depends on many factors. Among them is the cost you are willing to pay versus the accuracy you are receiving.

Compare solutions using different mesh sizes, you can always establish error bounds for a particular problem by constructing and analyzing multiple mesh spacings of the same model and observe the convergences, this is the way, comparison of results!!

And for linear analysis I prefer to state using CQUAD4 elements instead high-order CQUAD8, in general the results using CQUAD8 are better than those using the CQUAD4, yes, but results using CQUAD4 can, of course, be improved by increasing the mesh density to approach that of the CQUAD8 in terms of number of DOFs, and solution is faster.

Well, this is what I can share with you, good luck!.
Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/