Highlighted

FEMAP Stress Linearization Tool - Different values

Solution Partner Creator Solution Partner Creator
Solution Partner Creator
Hello every body!
 
One of our french users observes non-negligible differences between the stresses displayed at the nodes (here von Mises, averaged corner data in the figure below, but the other display options also show differences) and the corresponding stress evaluated by the tool.
Does the value "stress" on the graph correspond to the requested invariant, von Mises here? Should the values at the ends of the line not correspond to the calculated values by NX Nastran in our case ? How are the stress tensor values treated at these ends before the computation of membrane , bending and in our case von Mises stress ?

Could you help me to understand why this difference ?

 

Values at node :

  • Contour :  460.8 MPa
  • Stress linearization tool : 371.7 MPa.

 

Many thanks !

Marie

 image.png

2 REPLIES 2

Re: FEMAP Stress Linearization Tool - Different values

Siemens Phenom Siemens Phenom
Siemens Phenom

 

The ASME spec used to create the Stress Linearization Tool is designed around membrane failure of pressure vessels.  The line along which stresses are linearized should be from the inside tothe outside of a pressure vessel, and needs to meet these requirements - 

 

ASME_SCL_REQs.jpg

If the above requirements were met, there would be no discernible difference.

 

Why the values are different -

 

The methods used to recover von Mises stress are different in FEMAP's contouring vs. the Stress Linearization Tool.  In the sample model provided for testing, a concentrated load and the resulting high stress gradient around it can be used to understand the differences -

 

SL_VM.jpg

 

In FEMAP, NASTRAN reports a von Mises stress for the node in question, from both of the elements connected to it.  Default contour options in FEMAP then average this value to create the color contour display -

 

NX_NAST_VM.jpg

 

The Stress Linearization Tool requires the Stress Tensor at every point along the SCL.  An interpolation routine is called in FEMAP to find the stress tensor at that location.  It uses a similar approach, all of the tensor data is averaged at the nodes, and a value is interpolated out of that field.  In this high stress gradient area, the shear stresses go from +17,000.0 to -17,0000, averaging to 0.0 at the SCL, reducing the calculated von Mises stress there.

SL_AVG_YZ.jpg

This value is then used in the Stress Linearization Algorithm to compute a von Mises value, and is transformed to the SCL for linearization calculations.  We  have discussed different methods for interpolating the tensor in a mesh, i.e. within a single element only, however this would lead to wild swings in this coarse mesh, and in the coarse mesh from the original query. As outlined above, for a proper SCL, the shear stresses should not be the driving influence on stress, SCL transformed in-plane stresses that drive the calculation of linearized stress.

 

An excellent discussion of Stresss Linearization in general, and the impact of situation where the SCL goes through an extremely high stress gradient can be found here -

 

https://pveng.com/home/fea-stress-analysis/linearization/

 

 

 

 

Re: FEMAP Stress Linearization Tool - Different values

Solution Partner Creator Solution Partner Creator
Solution Partner Creator

Many thanks,Mark, for these quick and clear explanations !

 

Regards

Marie