How Ansys Calculates Stress? Is stress independent of Young's modulus?

[koolraj]

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!

 

[ESPcomposites]

Take a step back first.

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

http://www.espcomposites.com

 

[koolraj]

Yes...i got it...thanks!!

 

[koolraj]

Hi again..
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?

 

[bkal]

Did you apply the load as a prescribed displacement or a force / moment? Is you model using beam or plane or solid elements? If it is plane or solid elements and you are looking at the stresses at the supported end, then they might be affected by the boundary (depending on how have you defined it). Which stress component are you condiering?

 

[koolraj]

Thanks for reply.
I applied the load as an end force. I am using beam element. I am looking at the stress in Y direction.

 

[bkal]

From what you said your stresses should not be Young's modulus dependent. Could you send a sketch indicating what you have done (and what is Y direction) and also a summary of input parameters and results.

 

[sundaram15887]

Koolraj : As ESPcomposites pointed out , Finite Element Method uses a series of steps before calculating strains and Stresses. I would to add that stresses and strains which are expressed in the matrix form are related by the constitutive matrix which includes all the elastic constants of the material under consideration. Again depending on the element type (and displacement field), the software uses this constitutive matrix to generate a strain displacement matrix implicitly, which relates stresses and displacements or bending moment and curvature depending on the load cases applied. So essentially the stiffness of the structure changes if any of the elastic constants are changed.

 

[rickfischer51]

I did the same thing. I ran the model, noted the max stress and deflection, then decreased E by an order of magnitude. The stress stayed the same but the deflection was 10 times higher. This makes sense. y = PL^3/3EI, so deflection is inversely proportional to E. s=Mc/I, so E has no effect. Put another way, decreasing E by 10 times raises deflection and strain by 10 times, bur sigma = e*E, so 10 * 1/10 =1. Check your boundary conditions. Don't apply point loads. If you completely fix the fixed end, you get Poisson's effects that your hand calcs don't deal with. Also, your hand calcs are for Sx, so plot Sx

/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

 

[koolraj]

Hi all.
This is what I did. Please correct me if I am wrong.

 

[bkal]

Apologies for this, but are you sure you are checking stresses and not strains? Can you specify what exact parameter (in ANSYS terminology) are you qouting as equal to 0.007088 and at which location is it (i.e. at the support?). It seems that for the higher E value you get that value lower, which implies strains or even displacements of the tip of the cantilever.

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).

 

[rickfischer51]

That's not what you did. It is a cartoon showing what you think you did. What do your hand calculations say? A beam 1 unit long by 1 unit wide by 1 unit thick? Not very beam like.

Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[koolraj]

Hi..Sorry everyone. I did everything again.
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.

 

[IDS]

What you have said is correct for a simple example such as a cantilever, but consider what happens if you were to attach a spring to the loaded end. If you now increase the stiffness of the beam (leaving the spring unchanged) it should be obvious to you that the distribution of the load between the beam and the spring will change, and hence the stresses will change.

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/