0
$\begingroup$

I'm quite new in NASTRAN enviroment, and I am wondering how to use failure criteria which I can define when creating my isotropic MAT1 material for 1D elements (like CBEAM).

From the Quick Reference Guide, (MAT1) I am able to define 3 stress limits during the material creation.

What type of related output should I expect? Can I obtain failure indices or security indices? (like PLY composites) I've tried to launch a SOL101 but I can't figure out how to obtain these values, unless they are in the colums of F06 file named M.S.-T and M.S.-C (I can't find a reference in the guide, though!)

Other types of SOLutions effectively use these stress parameters? I'm actually interested in SOL111.

Thank you in advance for any help.

$\endgroup$
1
$\begingroup$

Any NATRAN solution should output the margin-of-safety factors if you output the stresses. Whether they are meaningful for any particular analysis is up to the user to decide, of course. For example, they probably are not meaningful for a vibration analysis since the mode amplitudes are arbitrary, but they would be meaningful for a forced response or transient dynamic analysis where the displacements represent something physical.

The definition of the stress output should be described for each element type.

For example, for a CROD element the margin of safety is defined as (ST/SA) - 1.0 when SA is positive, and -(SC/SA) - 1.0 when SA is negative, where SA is the calculated axial stress in the element, and ST and SC are the allowable stress in tension and compression given on the corresponding MAT1 card.

(Ref: https://docs.plm.automation.siemens.com/data_services/resources/nxnastran/10/help/en_US/tdocExt/pdf/User.pdf section 4.20)

For composite shell elements, the margin of safety is calculated for each layer - Google will find you references to the details.

| improve this answer | |
$\endgroup$
  • $\begingroup$ Thank you very much for the response: the link at the NX NASTRAN guide seems to be more complete about these concept than the MSC one. However, my SOL111 analysis of my beam still give me only a table with real/complex stresses and there is no reference at all to the margin of safety in the result, even if values are correctly inserted in the bdf file. (Yes, many reference about composite shell elements can be found, but I am interested in beams for now). $\endgroup$ – marcoresk Jul 23 '17 at 15:51
  • $\begingroup$ IIRC the "complex stresses" in Sol 111 represent the magnitude and phase of the individual components of the stress. You can get the magnitude and phase (not the real and imaginary components) with STRESS(PHASE). Note, the different stress components at one point can have different phases in a damped structure, so combining them into a single value (max principal, von mises, etc) to find a "margin of safety" is not trivial. NASTRAN takes the position that this is "post processing" not "analysis," since exactly what you want to do with the data is (or should be!) problem dependent. $\endgroup$ – alephzero Jul 23 '17 at 22:36

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.