When and how to "ignore" a singularity

[vato]

I am modelling a shipping container wall with rectangular openings. I'm using risa 3d, which, from my research on this site is a "lower" powered FEM program, compared to what yall mechanical guys use. I'm using shell elements for the wall and beam elements at the edges in the model. I have singularities at the corners of the openings which do show an increased stress as I decrease the mesh size in these areas. There may be singularities at the corner supports as well, but the stresses are so much lower than the opeing corners, that they don't show up. So, how do I deal with these infinite stress locations and get usefull results from this model. I'm trying to determine deflection, a realistic max stress in the corrugated wall, and perfomance of the boundary beam elements. Unfortunately I am way ahead of the corresponding real world load tests which we will be doing in the future.
thanks
an ps I have learned so much from this forum and it is indispensible to a one person office, thanks

 

[GBor]

Are you doing an entire shipping container, or just one wall? If you are just doing one wall, are your beam elements all the way around the outer perimeter? What are your loading and boundary conditions?

RISA3D is great for certain applications...just not sure this is one of them.

Garland E. Borowski, PE
Star Aviation

 

[vato]

I am modelling a wall only. I have a 2" square tube along the top, a channel on the bottom and angles at the ends/posts. I am loading the top and bottom beams, supporting the wall at the bottom of the posts. I am beginning to think that I am pushing the limits of risa. I have reproduced deflection in corrugated steel deck to within a 1/10th of published results.

 

[crisb]

Does it help if you apply a chamfer or radius at the corners? Does RISA have elements with midside nodes or are you stuck with 3/4 node shells? I find higher order elements perform much better in these scenarios. Can you use nonlinear material so that the maximum stress is kept to reasonable values?

 

[rb1957]

i wonder why you are getting singularities if you've got a panel with a rectangular hole in it bounded by beams ... unless (as the thought strikes me) the beam have bending stiffness (obviously, otherwise they'd be rods) but the shell elements for the panel don't. in this case there'd be nothing to restrain the beam bending freedoms (and they'd be singular).

some tests ...
1) fill in the hole (i don't think this'll fix the problem)
2) replace the beams with rods (just for giggles, to see what'll happen)
3) add full plate properties to the panel elements (maybe wack up their stiffness to see what happens)
4) add a beam (maybe several) across the panel (joining the cut-out frame to the edge of the panel) ... constrain the bending freedoms

are you only applying in-plane loads (there was a thread about the compression strength of corrugated container walls recently) ? ... even if you have no out-of-plane loads (and so nothing driving stresses into these out-of plane stiffnesses) FE codes don't like zero stiffness

 

[vato]

First off, thanks for the attention.
Crisb:
I'm modellilng a 40' long wall so a fillet or chamfer at the hole corner seems like a problem of another scale. I'm pretty much stuck with 4node shell elements and Risa3d does not do any non-linear analysis. I think this is ok, because we don't want to load the wall beyond any signifigant deformation (something that would crack applied finishes).
rb1957
1. I started with a no holes in the wall model.
2. I'm not sure of the difference between a beam and a rod. I have a choice of beam or plate elements. I can apply many different properties to either.
3. Little unclear on the full plate properties. My plate elements are as wide as the distance between vertical bends in the metal and about the same height.
4. I have messed around with this but it seems like, and I'm not entirely sure, that nothing is really stiff enough to erase the singularity which sorta makes sense.

I am only loading in the plane of the plate elements. No wind/lateral loads on the current model. Intuition says the model is acting correctly, except for the singularity.

 

[corus]

If it's a rectangular hole then the stress at the corners will be a peak stress which won't affect the overall displacement and should be considered only for fatigue purposes. Your shell/beam model won't be much good for that though unless you're only considering nominal stresses at a weld.

corus

 

[vato]

Thanks corus,
That is what I thought and we are not doing a fatique analysis. Can you guide me to some literature that would back this up? I am beginning to understand why it exists and why I can "ignore" it, but I need to have more of an understanding in order to explain it to my colleagues.
thanks

 

[corus]

Guidelines on stress classification are best found in Pressure Vessel Design codes such as ASME VIII or BS 5500. Maybe other countries also produce their own codes, I don't know.

From BS EN 13445 (the later version of BS 5500):
C.2.5
peak stress
that part of stress which is additive to the respective primary and secondary stresses, to form the total
stress
NOTE 1 Peak stresses do not cause any noticeable distortion and are only important to fatigue and brittle
fracture in conjunction with primary and secondary stresses.
NOTE 2 Peak stresses also comprise deviations from nominal stresses at hole edges within tube-hole fields
due to pressure and temperature, in which case the nominal stresses are derived from equilibrium of forces
considerations.


corus

 

[mtnengr]

Any structure that has a re-entrant corner will produce a very large stress concentration. The peak stress of a 90 deg. corner is infinite based upon M. L. Williams' study (JAM ~ 1957). Any FEM based on classical elasticity will predict larger and larger peak stresses as the radius of the fillet becomes smaller and smaller at the juncture point.

The problem with this type of analysis is that we start with the assumption that the stress tensor is symmetric. Most FEM programs make this assumption. The shear stress is assumed to be symmetric, Txy = Tyx. Resissner (QAM ~ 1947) demonstrated how to handle the edge stresses of a plate that had a zero shear stress along one corner and a finite shear on the other face.

Grioli (Acad. Press 1962) provides a detailed elastic analysis when it is assumed that the stress tensor is nonsymmetric. This author Citerley, (J. Franklin Inst 1966) demonstrated how to impose this non-symmetry condition using Lagrangian multipliers.

The engineering approach would be to establish the basic state of stress adjacent to the re-entrant corner using any verified FEM program and then apply well established stress concentration factors obtained from Peterson's Stress concentration book.

 

[prost]

Even without reading Grioli, it still seems like nonsense to say the stress tensor is not symmetric for a linear elastic, isotropic material--strass tensor symmetry is one of the fundamental assumptions when deriving what an 'isotropic material' is, is it not? There can be linear elastic materials which are non isotropic, right? But when you use 'linear elastic' materials in FE software, almost all of them assume the material is isotropic, and therefore the strain/stress tensors are symmetric. It's just an engineering model for real life behavior; all models have problems with reality.

Is Grioli saying that isotropic linear elastic materials have non symmetric stress tensors? That seems to contradict the fundamental assumption, the isotropy. It's as if you make the assumption that the process is 'isentropic' then claim the entropy did increase.

Wish I had the book so I could see for myself just what Grioli is talking about. Is this the Grioli book?
Mathematical theory of elastic equilibrium: (recent results) (Ergebnisse der angewandten Mathematik) (Unknown Binding)

It's Academic Press, 1962.

 

[xerf]

Some remarks:

The symmetry of Cauchy's (i.e. true) stress comes from the conservation of the angular momentum (assuming no couple tractions) and has nothing to do with any material formulation.

Some stress measures are not symmetric, for example the first Piola-Kirchhoff stress tensor (sometimes referred to either as the nominal stress or as the transpose of the nominal stress) is not symmetric.

Some of the symmetries of the elasticity tensor [E_ijkl] are shown assuming the symmetry of the stress and strain tensors.

 

[mtnengr]

Prost: Your identification of the ref. Grioli is correct. See pg 107 of that ref. Fichera had posed three classical problems of elasticity. One is the mixed boundary value problem--a displacement specified on one surface and zero stress tractions on the adjacent surface. Grioli presents the integration method of M. Picone. Symmetry of the stress tensor is not assumed.

This method was employed to the end grain problem of a cylinder supported at its outer surface. The cylinder is cooled and thermal stresses result. At the wall interface, assuming a symmetric stress condition, infinite stresses are predicted. The same is true for a bi-metallic strip. The Picone method suggests otherwise.

Xfer: Thank you for a more complete explanation regarding symmetry.

 

[vato]

Wow,
I have some reading to do now. I will post my current analysis soon and perhaps we can discuss some specifics. This is a new area for myself and I really appreciate everyones thoughts. I am analyzing thin corrugated metal and I have discovered another stress concentration where the corrugation transisions to flat. I haven't found any direct reference for dealing with this type of discontinuity yet although I am confident that the metal will deform and we aren't dealing with any cyclic loading or crack propogation, yet. Again, thanks to all for the time and I hope this discussion continues.

 

[JAE]

vato,

Not to try to cover what the excellent posts above discuss...but one aspect of RISA's graphic output (the stress contours) is that you can identify only certain ranges of stress on the plot window to get a better look at stress gradations in the low stress regions and ignore, temporarily, the hot spots at the corners.

On the plot window, under the selection of the type of stress/moment/etc. it lets you set a range. So this alters the contours to read more detail in just the range areas you are concerned with.

 

[mtnengr]

Vato: The structure you are now describing is either a curved plate or a shell. Discontinuity stresses can occur when there is a sudden change in the radii of curvature. 1/rphi for a flat plate is zero. You need to separate the curved corrugation and flat plate into two distinct elements.

If modeled correctly, any FEM program should be able to give the correct results.