How does Nastran evaluate stresses? 4

[sushi75]

Hi everybody!

As FEA is not limited to displaying nice colors, it's important to understand what's behind...

If we consider a QUAD4, and looking at the the .f06 file, there are 5 values of stresses per element: one at the centroid and 4 at each node location.

What I try to understand, is how these values are obtained. From my understanding, the stiffness matrix is calculated at the 4 points of interpolation (Gauss points).
Then I guess Nastran evaluates stresses using nodal displacements.

But how come the value is given at centroid? Is is an extrapolation of the value at Gaussian points to centoid using shape functions?

Also, the nodal displacements are given in the global coordinate system, so there should be a change of coordinate system to get the values in the element coordinate system, right?

I'm a bit confused about how Nastran "works". I think it's important to understand fully what the values given in .f06 mean to interpret the post processing as best as possible!

Thanks for your help!!

 

[rb1957]

first, congratulations for questioning the pretty colour pictures we can make; we aren't artists.

2nd, yes the element centroidal value is some average of the nodal results (themselves some sort of extrapolation of the gauss points).

if you really want to understand the element, read the user manual, read texts on how the math for quad elements works.

I think it's really important to study how well they work, and when they don't work (hint, they hate a bending stress field).

another day in paradise, or is paradise one day closer ?

 

[SWComposites]

Find and read the Nastran theory manual.

IIRC 4 noded quad only has gauss point in center. Nodal stresses are extrapolated out from center and are much less accurate.

 

[csk62]

You mean the plots aren't just nice pictures for .ppt presentations?

Your answer will be found by studying FEM theory, specifically Gaussian quadrature and how it is translated to nodal values.

 

[sushi75]

Thanks for your replies!

Does any know where I can find such documents? I could not find any relevant guide investigating MSC website,hanks only user guides but nothing about the maths behind.

Hopefully this stresses output will become cristal clear so that interpretation of results will be easier to justify!!

Thanks!!

 

[inline6]

https://simcompanion.mscsoftware.co...D_NASTRAN_DOCUMENTATION&channel=DOCUMENTATION

 

[inline6]

https://simcompanion.mscsoftware.co...t=MSC_MD_NASTRAN_DOCUMENTATION_2004&actp=LIST

 

[rb1957]

what is the confusion of the "interpretation of the results" ? why the need to justify CQUAD4 results ?

it is a different question if you're being asked to justify your model, which has less to do with the inner workings of a CQUAD4 and more to do with your mesh. If this is what you're after, there are downloadable reports to show you how (I think from NASA, maybe MSC ... how to qualify/quantify the quality of your model)

another day in paradise, or is paradise one day closer ?

 

[sushi75]

Thanks all for your useful tips!

Well, my intention to understand how stresses are calculated is to be confident in the results displayed: stresses can be averaged, extrapolated, at node, centroid (all fringe options actually).

So it's not really about the quality of the model, but more understand how results from .f06 files are created and can be post processed!

 

[rb1957]

one thing to be wary of is effective skin ... FEM is fully effective, so if you've got a skin/stringer in compression, extract the compression load (GPFB, or axial element load + 1/2 bay adjacent skin bays) and apply it to the effective section by hand. you may need to worry about shear buckling (how diagonal tension redistributes load over the structure).

another day in paradise, or is paradise one day closer ?

 

[stressebookllc]

It is dangerous to dismiss nodal values as inaccurate.

Nodal values are extrapolated and averaged for a good reason, to account for geometry and adjacent element contributions.

http://blog.3dvision.com/2008/04/18/nodal-versus-elemental-stresses/

http://www.stressebook.com

Stressing Stresslessly!

 

[sushi75]

Thanks stressbookllc!

So if understand well, the nodal stress is the average of the stresses evaluated at gaussian points of the elements this node is connected to.

And the elemental stress is the average of stresses at its nodes.
So the elemental stress is averaging stresses evaluated at gaussian points twice, right?

Not so obvious I think!

Cheers

Tom

 

[rb1957]

I think the element does it's calculations at the gauss points and that the precise location of these points is "irrelevant".

element stresses are usually the average of the nodal stresses of the element.

nodal stresses are usually the average of the different stresses at a node (from the different elements).

I think it's more instructive to delve into when the elements are producing accurate results and when they're not; which elements are "good" and which to avoid.

another day in paradise, or is paradise one day closer ?

 

[stressebookllc]

This is how I understand it:

Nodal values are calculated based on the Gaussian point values and the shape functions, and element geometry etc. per element.

Then the final values at a single node shared by multiple elements is the average of the different element contributions at that node.

The element centroid values are the average of nodal values. Its not exactly a double average at the centroid, its a better representation of the continuum stress field considering the adjacent elements as well.

If there are huge jumps in these values, then its an indication of a bad element topology, singularities or other discontinuities in the mesh or gemoetry, or even properties for that matter.

This complexity and potential for misinterpretation of mesh quality and results is one of the reasons why aerospace relies heavily on free body section loads and moments and well established hand analysis methods.

http://www.stressebook.com

Stressing Stresslessly!

 

[IceBreakerSours]

There are threads that have dealt with this question effectively and comprehensively. Always google before you ask.

However, I wish to add a note:

In the traditional displacement-based finite element analysis, two kinds of quadrature points are employed: Material or Gauss integration points and surface integration points. While this isn't really needed and, depending on what you do for a living, may even be a distraction, I suggest coding a simple element and a material if you wish to 'get it'.

Carlos Felippa (one of the key figures in the early years of FEA) has uploaded perhaps the most comprehensive course notes on FEM (will require time/patience) and Klaus-Jurgen Bathe's videos and notes are famous as well (but the lectures are fast-paced).

Are you new to this forum? If so, please read these FAQ:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[olduser]

In response to tomstress' original question:

Firsty, now that NASA has made nasa nastran open source you can take a look at the code and the programmers reference manual to see how stress is calculated in the public domain version of nastran. You can find the the download by searching for nasa/nastran on GitHub.

Secondly, nastran users only know about node point locations. Nastran has a table called the BGPDT (Basic Grid Point Definition Table) that defines the location of all grid points in basic coordinates, and generally this table is used by the post processor to define the location for displaying grid point stress. It is then the post processor that performs some weighted average of all element stresses at a given node point. It this average that is used to paint the pretty pictures.