Stress linearization
Stress linearization
(OP)
All,
I am begining to learn the process of stress linearization (in general). Do y'all have any suggestions in terms of references I should start with? I will need to use this technique to perform some analyses on 3-D FEM(s). After reading some of the information on this forum, it seems the largest hurdle is figuring out how to seperate the membrane and bending stresses from the outputs available in the finite element code being used. I will be using ABAQUS which apparently has this capability built in. However, Im hoping to extend this methodology to the software I am most familiar with which is NeiNastran. Has anyone had experience with stress linearization in NeiNastran? If so, I would love to discuss.
Best to all.
I am begining to learn the process of stress linearization (in general). Do y'all have any suggestions in terms of references I should start with? I will need to use this technique to perform some analyses on 3-D FEM(s). After reading some of the information on this forum, it seems the largest hurdle is figuring out how to seperate the membrane and bending stresses from the outputs available in the finite element code being used. I will be using ABAQUS which apparently has this capability built in. However, Im hoping to extend this methodology to the software I am most familiar with which is NeiNastran. Has anyone had experience with stress linearization in NeiNastran? If so, I would love to discuss.
Best to all.





RE: Stress linearization
Consider that this is just a mathematical operation, you'll be able to do it by hand or to automate it with some macro language built in your software.
However what you should really study in depth, because it's a much more difficult task that cannot be automated into a software, is how to separate primary from secondary stresses, and peak stresses from the total stresses. The only way to somewhat automate this is by plastic analysis, but if you want to stay elastic, then it's a matter of experience and reasoning (and 3D analyses make this task much harder).
There are many threads in this forum about the subject: you could start from there, then try some worked examples.
prex
http://www.xcalcs.com : Online engineering calculations
http://www.megamag.it : Magnetic brakes and launchers for fun rides
http://www.levitans.com : Air bearing pads
RE: Stress linearization
1) locate a stress classification line (SCL) - of course, you need nodes located along this line.
2) for extract the "nodal" stresses for all six stress components (3 normal and 3 shear?)
3) manipulate these stresses to seperate the membrane and bending stresses (i.e. membrane is the constant part accross the cross section and bending is the linearly varying part across the cross section).
Please correct me if im wrong. I also noticed that the principal stresses are used in some way which i did not understand.
RE: Stress linearization
3)There's not so much to manipulate: by averaging each one of the six components along the SCL (note: the averaging procedure must account for the positions or distances along the SCL of the used nodes), you obtain the six components of the membrane stress and similarly for bending (averaging the moments of each component about the middle of the SCL).
You'll generally combine those 6 components into a single quantity to check the stresses against a failure criterion. The Tresca criterion requires determining the 3 principal stresses to obtain the largest difference of them taken 2 by 2.
To be noted also that the bending stress alone is not really useful, as the check will be on the membrane+bending stress. Now by the procedure above you obtain two different membrane+bending stresses, one at each end of the SCL, and of course both need be checked.
prex
http://www.xcalcs.com : Online engineering calculations
http://www.megamag.it : Magnetic brakes and launchers for fun rides
http://www.levitans.com : Air bearing pads
RE: Stress linearization
RE: Stress linearization
jt
RE: Stress linearization
RE: Stress linearization
The peak stress is used to calculate the fatigue life of a component for which SN curves are normally used. These curves are based upon calculated (linear) stresses within a specimen, and hence must be compared with linearly calculated stress results from the FE model. Using Abaqus with non-linear (post yield) stresses would be wrong for this case.
corus
RE: Stress linearization