How Small is Small deformation

[PaulRomanos]

Hey,

I'm a relatively recent graduate (6 months) and have been using structural FEA for a year now. I think I understand most of the basic theory behind it but I just have one practical question that I can't seem to find an answer to in books.

I understand that a static linear isotropic FEA simulation depends mainly on 2 assumptions

- Linear behavior, i.e equivalent stress < yield strength
- Small deformation

My question is simply how small is small deformation ? the first assumption is relatively easy to check knowing the yield strength, but how can we check for the second one?

Thanks in advance,
Paul

 

[inline6]

linear material behaviour is when stress and strain are proportional.

small deformation means sin(THETA) is approx = THETA

 

[GregLocock]

The bloody awful answer is that you really need to run a non linear model to see if your linear model was good enough.

In practice you'll find that linear is good enough in cases where you aren't expecting plastic failure, in the normal scale of structures, made from steel.

You may find rules of thumb for this in your particular industry. As an example in the automotive world the vast bulk of FEA jobs are linear, including durability. But most cpu cycles are spent on non linear, doing crash.

Cheers

Greg Locock


New here? Try reading these, they might help FAQ731-376

http://eng-tips.com/market.cfm?

 

[PaulRomanos]

Thanks for your replies,

Greglocock:

The only problem is that I don't have access to a non-linear solver at work. We use CATIA V5 and we don't have the non-linear module. However even if we acquire it, I'd still like to be able to check my assumptions before running non-linear analysis .

inline6: Could you be more specific about what theta is and where this approximation is used in FEA?

I know for example that small deformations assumption are used in 2 instances:

1- in shell bending where there's decoupling between plane deformation and transverse flexure for small deformation
2- In the definition of strain where eps=du/dx is just an approximation for the more general non-linear strain definition.

Is there somewhere else where it's used?
My real question is what are some practical and numerical limits to check for this approximation?

 

[hacksaw]

you can answer those concerns only in the case of simple elastic structures without joints, well even that is not entirely true, for example consider the case of buckling

the sine function example is meant to illustrate the limitations of a linear approximation in any situation not the fea method

generally any deviation in the structure from equilibrium opens the door to non-linear effects

 

[Drej]

Large deflection relates to activating the non-linear geometry capability available in most implicit codes (given as 'NLGEOM' in ANSYS and ABAQUS), and which is 'built-in' to the Explicit formulation (within LS-DYNA for example). This 'effect' accounts for several type of geometric non-linearities such as 'Large Strain/Rotation' and 'Stress Stiffening' - a classic example being the displacement-dependent stiffness of a guitar string.

Unfortunately, in a lot of cases there is no definite general answer that you can give to this question, only rules of thumb (and experience) as mentioned, and therefore to truly see if your model is influenced by NLGEOM effects you will need to enable this capability to find out.


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

 

[jean15paul]

Are you looking for the theoretical answer or a rule of thumb? For a rule of thumb I've heard the "grey-beards" at my work say that you want your deflection to less than 10% of your thickness, in addition to making sure you're in the linear stress range for the material. For example if you're analyzing a 0.1 inch plate, then you'd like your deflections to be less than 0.01 inches. If your deflection is more than 10% of your thickness, then you should consider running your model geometric nonlinear to make sure that the small deflection assumption applies.

I've looked on a couple of occasions, and I haven't been able to find a source for this rule of thumb. I think it's just based on experience.

 

[rb1957]

that rule sounds like deformations out-of-plane for a plate in bending (my version is 50% thickness).

the point is do the deformations affect the loadpaths in the structure ? ie if you're looking at a beam or plate in bending, when does the out-of-plane deflection change the problem from a straight beam/plate to a curved beam/plate ?

greg's solution is the most pragmatic ... but then we'd use NL all the time (and these days why not ?)

a simpler idea is if the stresses look reasonable (less than yield) then your displacements are probably "small".

 

[bxtsafe]

The "Large Deformation" option (or "Large Displacement" option in some FE packages, for example Ansys) should be used usually in 2 cases:

- When the displacements of the structure nodes are very large. In these cases, the formulation of the shell elements for bending is no longer valid. I mean... in these element's formulation there is an aproximation: dy/dx=tan(theta)~=theta . This approximation is valid just when there are small displacements. When the large displacement is turned on it's considered that dy/dx=tan(theta). This option should be used when doing FEA of rubber parts, nonlinear elastic analyses, plastic analyses or when the structure displacements are large. It's also recommended to turn it on when the displacement of a plate in out-of-plane bending is bigger than 75% of it's thickness.

- The strain used in the linear FEM formulation is eps=du/dx . However, its an approximation. The real formula, that is used in the nonlinear FEM formulation, have high order terms. These high order terms are considered in the computation of eps when the large displacement is turned on. It's recomended to turn it on when we expect to find large strain, as in rubber parts FEA, in nonlinear elastic analyses or in plastic analyses.