How Ansys Calculates Stress? Is stress independent of Young's modulus?
How Ansys Calculates Stress? Is stress independent of Young's modulus?
(OP)
I use Ansys finite element as software package. But I don't know how exactly does ansys calculate stress?
Ideally stress=P/A. So stress is independent of Young's modulus. But in finite element formulation we use stress=E*strain. So how does Ansys stress match our stress concept. Is there any situation when just changing the Young's modulus (keeping geometry etc..same)can cause stress to change in ANSYS?
Thanks!
Ideally stress=P/A. So stress is independent of Young's modulus. But in finite element formulation we use stress=E*strain. So how does Ansys stress match our stress concept. Is there any situation when just changing the Young's modulus (keeping geometry etc..same)can cause stress to change in ANSYS?
Thanks!





RE: How Ansys Calculates Stress? Is stress independent of Young's modulus?
FEM does not start with stress=E*strain. FEM uses [F]=[K]*[X] meaning you determine the global stiffness matrix,[K], as a function of geometric and elastic properties. You then apply loads [F] and solve for displacements [X]. Based on the displacements you can determine strains. To determine stresses, you pass it through the stress-strain elastic relationship.
The other question is really a mechanics of materials question, not a FEM question. So you should consider looking at a text related to that. But generically, if you have a simple part then the stresses are not a function of elastic modulus, provided the analysis is linear. This is not necessarily true if it is nonlinear (another topic). If you have various structural members and the solution is statically indeterminate, then yes the stress will be a function of member stiffness. But again, those are really mechanics of materials/statics types questions and not specific to FEM.
Brian
www.espcomposites.com
RE: How Ansys Calculates Stress? Is stress independent of Young's modulus?
RE: How Ansys Calculates Stress? Is stress independent of Young's modulus?
I tried an example of a cantilever beam with end load in ANSYS. I just changed the Young's modulus (scaled it by 100), keeping geometry, load etc.. same. But my stresses also scaled by the same order of magnitude I scaled E earlier. So my stresses also scaled by 100.
In theory stress in bending (My/I) depends again only on geometry and the loads. So this is not intuitive, that stresses depend on Young's modulus.
Is this correct? Is there any reason why this happened in ANSYS?
RE: How Ansys Calculates Stress? Is stress independent of Young's modulus?
RE: How Ansys Calculates Stress? Is stress independent of Young's modulus?
I applied the load as an end force. I am using beam element. I am looking at the stress in Y direction.
RE: How Ansys Calculates Stress? Is stress independent of Young's modulus?
RE: How Ansys Calculates Stress? Is stress independent of Young's modulus?
RE: How Ansys Calculates Stress? Is stress independent of Young's modulus?
/prep7
EX,1,29e6
nuxy,1,.3
block,0,6,0,1,0,.25
et,1,185
esize,.25
vmesh,all
et,2,154
type,2
nsel,s,loc,x,6
esln,s,0
esurf,all
esel,s,type,,2
sfe,all,2,pres,,100
nsel,s,loc,x,0
d,all,ux,0
nsel,r,loc,y,0
d,all,uy,0
nsel,s,loc,z,0
d,all,uz,0
allsel
/solu
solve
/post1
set,last
plnsol,s,x
Rick Fischer
Principal Engineer
Argonne National Laboratory
RE: How Ansys Calculates Stress? Is stress independent of Young's modulus?
This is what I did. Please correct me if I am wrong.
RE: How Ansys Calculates Stress? Is stress independent of Young's modulus?
Have you tried to do a hand calculation. Assuming that yout units are consistent:
Moment=1*1000=1000
Elastic modulus=(1*1^2)/6=1/6
Stress= 1000/(1/6)=6000
Strain= Stress/E=6000/10^6=6*10^-3 (Case 1) or
Strain= Stress/E=6000/10^8=0.6*10^-4 (Case 2).
RE: How Ansys Calculates Stress? Is stress independent of Young's modulus?
Rick Fischer
Principal Engineer
Argonne National Laboratory
RE: How Ansys Calculates Stress? Is stress independent of Young's modulus?
Whatever Rick did (2D beam), I repeated it, with Ricks macro..instead of doing it myself. The stresses do not change as we change the Young's modulus, if we have an end load for the cantilever. But for a fixed end displacement, the stresses do vary if we change the Young's modulus. I think this is because of the displacement boundary condition we applied. The fixed displacement at the end imposes different forces on the beam (indirectly, the force at the end for constant displacement becomes a function of Young's modulus) when we change the Young's modulus.
So what I can summarize is this: For a static linear elastic analysis with no change in forces, geometry of the model, even if we change Young's modulus, the stresses should not change. But for a displacement boundary condition (applied at the end) the stresses would change even for a linear elastic analysis.
Thanks everyone for helping me out. Thanks to Rick who did entire analysis and pointed out the correctness of the model we are analyzing. Feel free to correct me if still I am wrong.
RE: How Ansys Calculates Stress? Is stress independent of Young's modulus?
Might I suggest that a much more detailed knowledge of the theory of strength of materials is really essential before trying to use FEA.
Doug Jenkins
Interactive Design Services
http://newtonexcelbach.wordpress.com/