When can I use Symmetry boundary condition
When can I use Symmetry boundary condition
(OP)
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
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





RE: When can I use Symmetry boundary condition
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
RE: When can I use Symmetry boundary condition
RE: When can I use Symmetry boundary condition
but then is it worth the hassle ?
RE: When can I use Symmetry boundary condition
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?
RE: When can I use Symmetry boundary condition
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
RE: When can I use Symmetry boundary condition
cheers,
fecad
RE: When can I use Symmetry boundary condition
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?
RE: When can I use Symmetry boundary condition
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).
RE: When can I use Symmetry boundary condition
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.
RE: When can I use Symmetry boundary condition
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?
RE: When can I use Symmetry boundary 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.
RE: When can I use Symmetry boundary condition
RE: When can I use Symmetry boundary condition
RE: When can I use Symmetry boundary condition
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.
RE: When can I use Symmetry boundary condition
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
RE: When can I use Symmetry boundary condition
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,
RE: When can I use Symmetry boundary condition
It has a good discussion and examples on how to analyze a symmetric structure with loading asymmetries.