AMSE III Level D - Stress Intensities from ANSYS

[Drej]

I'm qualifying a structure to ASME III (NB) LEVEL D. The loading is seismic (DBE) and the loads on the structure are calculated using response spectrum analysis in ANSYS. There is a concern from the customer that the stress intensities calculated by ANSYS (and specifically required by the ASME code for qualification) are "non-conservative".

Has anyone ever come across this "concern" previously?

Cheers.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[vpl]

This might be better in forum569 or in a structural forum.

It's been a long time since I've looked at Section III, but isn't level D basically don't fall on anything important?

Patricia Lougheed

******

Please see FAQ731-376: Eng-Tips.com Forum Policies for tips on how to make the best use of the Eng-Tips Forums.

 

[TERIO]

I am assuming the concern is specific to response spectrum loading and not ANSYS in general. One thing that comes to mind is the SUMTYPE command. In the ANSYS basic analysis guide section on creating and combining load cases the statement is made that "unless SUMTYPE,PRIN has been requested, principal/equivalent stresses are not meaningful when computed from squared component values." It doesn't appear to say what is different using sumtype,prin that would make the stresses meaningful.

 

[Drej]

It was initially difficult to decide where to place the post, but having done some further investigation it may well be more applicable in the ANSYS/FE fora.

That said, forgive me for giving some detail here. The initial problem was generic to response spectrum analysis in terms of how the stresses are combined, and whether combining using either SUMTYPE,COMP or SUMTYPE,PRIN was meaningful in either sense for spectrum analyses. But it is now also a problem of how ANSYS is behaving. In ANSYS, the SUMTYPE,COMP and SUMTYPE,PRIN (as said) control how the stresses are derived/combined. If the SUMTYPE,COMP (default) command is used then one can view both component and principal stresses for the structure (SHELL63 elements). If the SUMTYPE,PRIN command is used then ANSYS does not give /any/ stresses for the solution, only strains. On the other hand, if the analysis is done with only pipe elements then ANSYS /does/ show (e.g. by issuing PLESOL,S,1) both component and principal stresses for SUMTYPE,PRIN. After lots of head scratching and running the problem in different versions of ANSYS (7.1 to 11.0) it is still the same. A mystery. It could be a bug.

Cheers.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[Drej]

Problem solved. After issuing SUMTYPE,PRIN the stress components/principals can be viewed using "PLES,NMISC,#" where "#" is the corresponding sequence number for the element. This is due to non-summable stresses not being directly available in the results file after the above SUMTYPE operation and loadcase combinations. Results (stress intensities, SINT) show that SUMTPYE,COMP is conservative for this problem using element-nodal values, and interestingly the nodal-averaged values for SINT are similar for both types COMP and PRIN.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com