von Mises Stress for Hexahedral Elements

Experimenter
Experimenter

Hello,

 

I’m a newbie to the world of Femap and have been wrestling with ensuring I understand what it does when it presents von Mises stresses for hexahedral elements, based on outputs of the SESTATIC solution in NX Nastran. I’m using Femap v11.3 and would sincerely appreciate any help to clarify the following:

 

1.    What is Femap literature (i.e. help files, reference guides etc.) when referring to "corner data"? Are these data at Gauss (Quadrature) points or are they those at elemental nodes?

 

2.    What is the difference between the “No Element Averaging” and “Centroidal Only, No Averaging” options in the Data Conversion section of the Contour menu within the Postprocessing Toolbox?

 

3.    Are von Mises stresses calculated first at Gauss points (by Nastran or Femap) and then interpolated to the elemental centroid when either option is selected? Does the same occur when they are extrapolated to the corner nodes? Or do the direct stresses get interpolated or extrapolated first, respectively, and only then do the von Mises stresses get calculated at these locations?

 

4.    Should the maximum von Mises stress for a specific element ID and a specific results’ set identified in an output-envelope, be different when it is extracted directly for that element ID for the identified result-set?

 

List->Output->Query-> element ID for a specific set of linearly combined stress results gives a different (i.e. lower) value for the von Mises stress when compared to the value identified as the maximum value obtained by Model->Output->Process->Envelope->Max value (All Locations); the enveloping identifies the element ID and set of linearly combined results that is queried for the output-list of to extract and compare.

 

Thanks in advance,

Nal

3 REPLIES 3

Re: von Mises Stress for Hexahedral Elements

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Dear Nal,

1.- For all the questions related with the solver NX NASTRAN enter in FEMAP and go HELP > NX NASTRAN, then the bible of FEA will be in your hands: please note FEMAP is a pre&postprocessor working with any FEA solver of the market, then all questions related to results, element formulation, solvers, etc.. the best source to find the answer is the NX NASTRAN USERs GUIDE.

Regarding your question "corner data" means the "corner grid points". With NX NASTRAN you can request to have stress, strain of forces output at element center (by default) or at corner grid points using the STRESS, STRAIN, and FORCE Case Control commands as follows:
STRESS(CORNER) = {ALL or n}
STRAIN(CORNER) = {ALL or n}
FORCE(CORNER) = {ALL or n}

Where { } indicates that a choice of ALL or n is mandatory, but the braces are not included. Only one type of element output (center or corner) is supported per run. Corner data is different to Gauss points.

 

2.- This question is fully related with FEMAP, is the way how you postprocess results coming from the FEA solver:

  • Elemental Contour Discontinuities > No Averaging: this is only active when you select ELEMENTAL results under F5 > DEFORMED & CONTOUR DATA > CONTOUR OPTIONS.
  • When you choose Elemental contouring, you can specify which discontinuities in the model to use in the contouring to obtain an accurate representation of the results. This type of contouring is very useful for multiple material models as well as models with plates with that intersect at large angles or have varying thickness. Stresses will not be averaged across these values. The resulting graphics may not be as “smooth” as nodal contouring, especially at material breaks, but it provides a more accurate representation of the results when discontinuities exist in the model. In addition, element contouring allows you to view both top and bottom stresses of plates on one plot, as well as an addi­tional output vectors.
  • Element contouring has the added feature that if you select No Averaging under Element Contour Dis­continuities, the pure data at the element centroid and corners is plotted without any manipulation. This provides a graphical representation of the pure data coming from the FEA solver, without any postprocessing manipulation of FEMAP.

elemental-contour-discontinuities.png

Ah!, sorry, reading your question again I note you are using the MESHING TOOLBOX, well:

  • if you want to plot the stress at the element centroid only choose "Data Conversion = Not average, Centroid Only" and Contour type = Elemental, then you will have only ONE value per element (one color per element). In the classical method this means to activate NOT AVERAGING under Elemental Contour Discontinuities, in this case the data conversion option selected is useless (Average, max o min, the result is the same), because only one value per element exist, the elemental centroid one.
  • If you choose "Data Convergion = No Element Averagingand Contour type = Elemental, then FEMAP do not average results between neighbour elements, but only inside each element.

The basic question is: you need to plot nodal & elemental stress results, I always suggest to use DATA CONVERSION = AVERAGE, and also USE CORNER DATA = ON, using F5 and the classic method is more clear, more simple to understand.

 

3.- You can request to the NX NASTRAN solver to compute stress output location at GAUSS points instead the center and at each of the corner points, take a look to my post here (this question is getting very popular lately, please FEMAP developers, put this option in the FEMAP GUI!!): 

https://community.plm.automation.siemens.com/t5/3D-Simulation-Femap-Forum/How-to-select-in-FEMAP-Str...

 

4.- Probably, this could happens when FEMAP process and manipulate any output set, you can test yourself using precise numbers, if you detect any error please report here with anexample. For instance, when creating Linear Combinations some vectors cannot be linearly combined. When FEMAP reads output from your analysis, certain vectors are identified as being not “linearly combinable”. Examples of these are Principal Stresses, Von Mises Stress, and Total Displacement. Instead of combining these vectors, FEMAP recalculates them based on their lin­early combined components (if all necessary components exist). This recalculation is only possible when you com­bine entire output sets.

Best regards,
Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director
IBERISA • 48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog Femap-NX Nastran: http://iberisa.wordpress.com/
Highlighted

Re: von Mises Stress for Hexahedral Elements

Experimenter
Experimenter

Dear Blas,

 

Thank you for responding so promptly and with such detail. I thoroughly appreciate your explanations and will have to digest your information in the context of my use with particular focus on your suggestion in item 4. I agree especially with your call for a GUI or some entry form in Femap to have it create the request for stresses (and strains) at the Gauss points. This considering that NASTRAN has the option available and the user should be enabled by Femap to tap into this.

 

Much appreciate your help.

 

Best regards,

Nal

Re: von Mises Stress for Hexahedral Elements

Experimenter
Experimenter
Dear Blas,

You m unable to detect errors and am led to believe there is none at this stage; this is in relation to your advice on item 4.

My sincere thanks to you again.

Best regards,
Nal