When can I use Symmetry boundary condition 2

[Newuser2007]

Hi,
I have a model which geometrical symmetric but load is not symmetric. Can I use symmetry boundary condition? I am talking about planar symmetry not axisymmetry.

For eaxmple, a reactangualr plate area which is symmetric about its midplane. So I can model quarter of it and apply symmetry boundary condition on two edges. But my loading is not at the center of the full plate but load is on one quarter of the plate. So, loading is not symmetric but the geometry is.
Can I model the quarter of the plate with applied load at the center of the quarter model?

I am using ANSYS 11.0.
thanks.
Newuser2007

 

[prost]

Symmetry is a load and geometry constraint; in the case you have cited, you could not model one-quarter of the plate, use symmetry constraints, and have a good model of a plate loaded over one-quarter of the plate area. Say you did model one-quarter of the plate, used symmetry and put your distributed load over that one-quarter model. Then you would be modeling a distributed load over the entire plate, which is not what you are trying to model.

Think about two cases: Case 1--loaded over one-quarter of the plate area, and Case 2--loaded over the entire plate area. Are the deflection and stress the same in these two cases? No.

A good place to double check your work, and your intuition, is Roarks formulas for stress and strain

 

[SWComposites]

Since the load is not symmetric the stresses in the plate will not be symmetric, so you need to model the entire plate. Besides, computing resources are cheap, so its not worth the bother of modeling only a quarter section.

 

[rb1957]

could you describe your load as a symmetric component and an antisymmetric component ? ... then you could model 1/2 the structure and probably have 3 load cases ... the symmetrci loads, and two antisymmetric cases.

but then is it worth the hassle ?

 

[Denial]

Any (non-symmetrical) loading on a symmetrical structure can be expressed as the sum of a symmetrical load component and an anti-symmetrical load component. You can then apply the symmetrical load to the symetrical half-structure, and the antisymmetrical load to the anti-symmetrical half-structure. After that, you recombine the results from the two analyses with CAREFUL use of signs, to get the actual results for the two halves of the full structure under the full loading.

When computing power was in short supply, this was a useful ruse (and some software even had inbuilt facilities to make the approach a bit easier). But these days, as SWComposites says above, why would you bother?

 

[corus]

As prost says, a quarter symmetry model would in fact represent the whole of the plate under load. You could also use half symmetry to represent half the plate under load, with the load in the model applied to one quarter of the plate. Both these approaches may be acceptable if you can argue that the results will give you higher stresses (or deflections) than the true load over a quarter of the plate.

Contrary to the opinions above, I'd use symmetry to reduce the size of your model at any opportunity. Strictly speaking this case isn't valid as the loads aren't symmetric, however the results you get from using symmetry may be justified as being a worst case scenario.

corus

 

[fecad]

I would do with total plate to erase all confusions here.

cheers,
fecad

 

[Newuser2007]

thanks for all your advice. So I learnt that I can't do symmetry model unless both geometry and load are symmetric.

Now, what that anti-symmetric condition mean exactly ? Does it mean that the structure is geometrical symmetric but load is not? Like a plate where quarter of the plate is loaded. Then one models half of it and applies anti-symmetric bc . Is that right?

Does ansys or any other online resources discuss more elaborately on this symmetry /anti-symmetry thing?

 

[rb1957]

symmetric load/geometry means that the load/structure is mirrored about a plane of symmetry.

anti-symmetric load means that the load on one side of the "plane of symmetry" is the opposite to the other. This load condition places a different constraint on the boundary edge (eg for a symmetric boundary you can have out-of-plane deflection (ie in the symmetric plane); for the anti-symmetric case you can't ('cause on one side of the boundary it's deflecting upwards, and on the other it's deflecting downwards).

 

[rb1957]

read your reply again !

using a 1/4 model means you have two planes of symmetry ... i don't think anti-symmetric conditions apply, easily.

using a 1/2 model, read my previous post, ok ?

using a 1/4 model, then anti-symmetry means that two 1/4s of the full model (diagonally) are deflecting up and the other 2 1/4s are deflecting down; sort of like a flat panel loaded in bi-axial compression, buckling into the 2nd mode.

 

[Newuser2007]

rb1957, many thanks for nicely clarifying the sym and anti-sym conditions. That was really helpful.

May I ask another question??

How can I model situation like this:
a plate sitting on four beams(I-beam) or supports on all 4 edges. I tried to couple(or constraint adjacent region) uz(vertical) displacement of plate and support along the top flange of each I-beam(modeled with shell not beam element). This is practical as plate can't physically move down along those flange areas.Nice. But infact, the plate can move upward independent of the support underneath. How can I model that ? If I fix Uz or couple Uz, it constrains both vertical and downward movement , right? Is there anyway simple way to take care of this real life simple support condition?

 

[johnhors]

"Is there anyway simple way to take care of this real life simple support condition?"

No, this is not a simple support condition. Since you want to prevent downward deflection but allow unrestricted upward deflection then your model is non-linear. Gap elements or compression only springs can be used to model this, which I assume Ansys has in its element library.

 

[prost]

Wouldn't nonlinear springs restrict motion in one direction but allow in another? Nonlinear springs that are compression only, and will 'break free' from the structure for parts of the interface that are in tension?

 

[rb1957]

why not use the same node IDs for both ? if you want to get "fussy", you can use element offsets to physically separate the plate the the I-beam flange

 

[Newuser2007]

I looked at nonlinear spring elements in ansys. like combin 39. It requires coincident nodes. Now if I make a spring element at coincident nodes of support and plate, then how do I enforce that the support is grounded. I mean it does not go downward. I did a trial run but seems like the spring is compressing down which I don't want.

I want when load applied, the plate can't go down at the support but it can go upward if thats the case.

i am bit confused here on this.

 

[rb1957]

sounds more like a contact problem ...

can you make your non-linear spring virtually infinite stiffness in one direction and your finite amount (maybe close to zero) the other. possibly this is too extreme for the spring to handle

 

[chaboche]

I have a few comments, however I would urge other members to contribute, as I'm not sure if they will work:

1. Link10 elements support a tension only or compression only feature. I have had convergence problems with these elements in the past, but it may be down to the boundary conditions I had applied.

2. You may be able to define an elastic foundation stiffness associated with the shell elements. I'm not sure if this is associated with compression or tension or both, as I haven't used this feature before.

3. Instead of constraining the edges of the plate and applying loads offset, you may condider constraining the model where the loads are applied and applying a uniform pressure around the edge equivalent to the weight.

Hope this helps,

 

[NS4U]

check out: Matrix Structural Analysis, 2nd edition, by McGuire, Gallagher, and Ziemian

It has a good discussion and examples on how to analyze a symmetric structure with loading asymmetries.