Calculate local stress in a plane not aligned to global coordinate system (Stress tensor rotation/projection)

[frank.rottgardt]

Hi,

I want to calculate local stresses in a point (node/element) in a certain 3D plane not aligned to the global coordinate system (free in space so to say) The Cauchy stress tensor needs to be rotated with a rotation matrix (normal vector of the new plane) and then the traction vector can be calculated. This vector represents the local stress in the new plane. It can be used to calculate the plane normal- and shear stress. Application: multiaxial fatigue problems.

I know this is not directly implemented in Inventor Nastran. But for a small number of nodes / elements that could be done manually with help of a Excel spreadsheet.
I have a rather dense mesh with element size down to 0,05 in hot spots. I have done a 3D non-linear static analysis with three different load cases. Load 1 - Unload- load 2 , resulting in local plasticity. Goal is to find stress and strain amplitude in the new plane as input for life-equations (Fatemi)

My understanding is that the matrix elements of the Cauchy tensor Sxx, Syy etc. can be extracted from the FEA result plot (probe) I read that these stresses are calculated in the 3D elements Gauss points.

Questions I have:

1. When I use the probe-tool, do the results for Sxx, Syy etc. are some kind of average of the 3D element´s Gauss points?
   
   
2. What do these values represent if I choose that stress shall be shown in Nodes (corners)
   
   
3. Are these values relative to the global coordinate system or the 3D elements local
   coordinate system?
   
   
4. Is there a simple way to plot stress (others than von Mises or principal stress) relative to other than the global coordinate system? Example: UCS
   
   
5. Is there a direct way to extract a Cauchy stress tensor without picking each single matrix value (there are 6) from the result plot, for instance looking them up in the FEA result file for each node? How and where, what to look after?
   
   
6. Is there an Inventor Nastran “receipt” for how to evaluate local stresses in a different plane (rotation/projection of stress tensor) - step-by-step instructions?
   
   
7. Does the Multiaxial fatigue module in Inventor Nastran use local stresses (se above) and can it be used with NL-static analysis?

My understanding is that stress tensors in the Stress linearization tool can´t be used for tracking local stresses on a plane? Have not used that tool – maybe a strange question.

Appreciate your help!

[John_Holtz]

Hi @frank.rottgardt 

1. Yes, the default is to display an average stress. The ribbon Probe then interpolates the result based on the position of the mouse. The model tree Nodes probe gives the (averaged) result at the nodes. See Tip 51 in the PDF document attached to my forum post Suggested Reading - Tips and Tricks on the Inventor Nastran forum.
2. See Understand Data Conversion, Data Type, and Contour Type in Nastran. The result from each corner of the element connected to the node is averaged.
3. Stresses for solid elements are based on the coordinate system that you chose on the Idealization. (The default is to use the global XYZ.) See How to define the material and stress axes in Inventor Nastran.
4. There is no option to rotate the results, other than the article in answer 3.
5. Use FNO Reader to extract the results you want from the locations you want. See Tip 56 in the Tips and Tricks document.
6. I do not know of any instructions. Best to use your favorite search engine to find the steps to perform a matrix rotation of the stress tensor.
7. Multi-axial fatigue uses von Mises stress (no direction), Maximum Principal stress or Maximum Shear stress (specific direction but not a local direction like you are asking). A fatigue analysis performs a linear static stress analysis and uses those results for the fatigue life calculation, so it cannot be used to read results from any other analysis type (such as nonlinear static stress). You will need to do the fatigue calculation manually.

Let us know if you have any questions.

John

[frank.rottgardt]

Hi John and thank you for the prompt answers!

Concerning 7)
Is there a way to make the Multi-axial fatigue analysis to accept (import?) results from a prior NL-stress analysis to start from (prestressed), even if the analysis will be linear from that point on? I have residual compressive stresses in the NL-file impossible to reproduce in a linear Multi-axial fatigue analysis.

Follow up question:
How does it come that the fatigue analysis gives me the possibility to use the strain-life method, where in / or close to LCF zone (2Nf around 2Nt) life gets more and more influenced by additional plastic strain. But at at the same time I won´t have any plastic strain in a linear analysis resp. my maximum stress is way to high because I won´t have yielding beyond Sy? Does that mean that Inventor Nastran will produce questionable life results at or close to LCF because of to small strain-amplitudes? 

Thank you, Frank

[John_Holtz]

Thanks Frank.

This is very interesting. As is often the case, Nastran has "some parameter or field, somewhere" that does the most obscure thing that I would never think to look for it. In many cases, the Inventor interface does not expose the setting for the user, so these things are largely unknown. 

Check out the parameter RSLTDATABASE which says it can be used to read results from a linear or nonlinear analysis for a fatigue analysis! I never knew this. (Parameters are the second to last branch in the Model Tree. RSLTDATABASE is available in the list.)

I am not that familiar with strain-based fatigue (E-N). My guess is RSLTDATABASE is how you get plastic strain to the E-N analysis. 🙂 Hopefully you have a good nonlinear example that you can use to test the E-N fatigue.

John