That’s why you need a good control on orientations. Now it’s clearly not ok.
Mecway.
That’s different. GLOBAL parameter applies to shells. GLOBAL=NO is default for SNEG, SMID and SPOS. That’s fine as long as they point where you want them to. If you let the program orient them automatically and you can’t see them, you may end up with something like your photo.
How did you set them in Mecway ? By just specifying points defining the CSYS for the *ORIENTATION, or does Mecway have a more convenient way to define it in cases like this one ?
I thought it also meant that shells always give the results in local directions. At least in Abaqus, that’s the case. Of course, one can just do the transformation in postprocessing. Perhaps that could help here.
However, since displacement and Mises stress are ok, and I can read the hoop stress using cylindrical transform (looks good too), then I guess the meridional stress is likely also correct, and I just can’t read it properly for now (I can only look at the untransformed S11 and S33 stresses, but the orientations are unclear). It would be good to find a way for that in PrePoMax, but I can even skip it if it turns out too problematic.
I know that Victor is very aware of the importance of orientations and has managed to eliminate several bugs by working on them carefully over several versions. In Mecway, you can define orientations with explicit functions f(x,y,z) for each direction. In shells, the normal is fixed, but far from being a limitation, it allows, if you get the direction of a common axis right, the homogeneous distribution to be completed automatically.
We should convince Matej to implement a new feature to visualize and distribute Orientations. Not only for shells, also for ortothropic materials and laminates.
Whom might find it interesting playing a little with the boundaries of these formulas might find this GMSH script useful. It will generate whatever you like of dimension for a corrugate pipe according to the geometri described in the formulas.
Once imported ex. in PrePoMax it can be decided either it should be shell or solid to be used. In the script it can also be decided if linear or second order element should be used. Depending off the size of the piecake cut One should/could adjust the number of elements.
Personal I don’t understand why the mean radius ‘a’ doesn’t exist in the deflection formula.
//+
SetFactory("OpenCASCADE");
//+
n_corrugate = 5; // number of Corrugate
a = 132.2; // mean radius of the corrugated pipe
b = 40; // radius of the bead
t = 1; // material thickness of the pipe
phi = 15; // piecake cut in degree
//+
rad = Pi * phi / 180;
flipflop = 0;
//+
For i In {0:n_corrugate-1}
n = 5 * i;
Point(1 + n) = { a, 0 + 2*b*i, 0};
Point(2 + n) = { a, -(b-t/2) + 2*b*i, 0};
Point(3 + n) = { a, (b-t/2) + 2*b*i, 0};
Point(4 + n) = { a, -(b+t/2) + 2*b*i, 0};
Point(5 + n) = { a, (b+t/2) + 2*b*i, 0};
If ( flipflop == 0)
Circle(1 + n) = {3 + n, 1 + n, 2 + n};
Circle(2 + n) = {5 + n, 1 + n, 4 + n};
flipflop = 1;
Else
Circle(1 + n) = {2 + n, 1 + n, 3 + n};
Circle(2 + n) = {4 + n, 1 + n, 5 + n};
flipflop = 0;
EndIf
Line(3 + n) = {2 + n, 4 + n};
Line(4 + n) = {3 + n, 5 + n};
Transfinite Curve {2 + n, 1 + n} = 30 Using Progression 1; // 30 = number of elements on bead
Transfinite Curve {4 + n, 3 + n} = 1 Using Progression 1;
Curve Loop(1 + n) = {4 + n, 2 + n, -(3 + n), -(1 + n)};
Plane Surface(1 + n) = {1 + n};
EndFor
For i In {0:n_corrugate-1}
n = 5 * i;
Extrude {{0, 1, 0}, {0, 0, 0}, rad} {
Surface{1 + n}; Layers{10}; Recombine; // 10 = number of elements on mean radius
}
EndFor
//+
Mesh.RecombinationAlgorithm = 1;
Mesh.RecombineAll = 1;
Mesh.Recombine3DAll = 1;
Mesh.Renumber = 1;
Mesh.Algorithm = 6;
Mesh.Algorithm3D = 1;
Mesh.SecondOrderIncomplete = 1;
Mesh 3; // Generalte 3D mesh
SetOrder 2; // 1 for linear, 2 for second order elements
Coherence Mesh; // Save mesh in MSH format
Save "CorrugateTube.unv"; // Save mesh in UNV format
Good reflection!! I think it does indirectly from the validity range of the parameter my (4 to 40).
@teeps , when I use the following data
n = 5, b = 40 mm, t = 1 mm, P = 2000 N, e = 210000 N/mm^2, ny = 0.3
analytic it will give the deflection of 1.048 mm
In Calculix I obtain following
a = 132.2 => ny = 39.99 => deflection = 1.058 mm
a = 1322 => ny = 3.99 => deflection = 1.499 mm
In case I’m right it seems the validation space for deflection formula should be narrowed/adjusted.
@fgr As to mentally accepting the apparent lack of influence of “a” on the deflection one could argue by comparing with a corrugated but not rotational plate. Here the deflection would be proportional to the integral of the line moment along the integration path. The line moment would be proportional to the height “b” of the corrugations and the line (force per lenght of plate) load pulling the structure. In the case of a body of revolution the generated hoop stresses are proportional to the ratio b/a. This also means that when a→inf or b→0 there will be no such “geometric stiffening”.
The formula uses the total force as P. This also means that the line load is proportional to 1/a which is also what happens to the geometric stiffening, so this essentially means … 
.
This doesn’t really explain why there is discussed a validity range for parameter “my”. One has to study the source of the formula to understand that. Often it is a shortcut in the integration such as x=sin(v). Here it could also give rise to a discrepancy that outwards b is equal to inwards b giving a deflection asymmetry - which also ceases as a→inf or b→0
To get a better understanding one should study the source of formula 6b of Table 13.3 in “Roark’s Formulas for Stress and Strain” as discussed by @Disla and @Calc_em above.
When you compare FEM calculations to analytic solutions you may want to consider the effects of discretization and also the finite element formulation. For most analytic calculations the integration is along a single path, so the best FEM reference for such comparison in my opinion is a 1D model with rotational symmetry.
@teeps In this case with the corrugated tube I can’t agree with you. Due to what I could name as lack of Euler stiffness in the structure it will be my opinion that the influence of radial stiffness can’t be neglected in the axial stiffness of the corrugated tube.
@fgr I agree that they are coupled. If you understood my philosophical approach that way I have been unclear in my descriptions.
I also agree that “a” is supposed to affect stiffness, and following my own line of thinking it does, which may also be confirmed by FEM studies as mentioned by yourself.
A better understanding of the deflection formula from the Roark collection and why the influence of “a” was left out requires insight in the mathematical treatment behind it. This was the essence of the discussion.
It could be interesting to see if other sources on bellows have treated this better. The companies specialized in making bellows, might have a better formula.
Here is an article which quote an expression (formula 3) for stiffness being propotional to radius (a). This differs from Roark formula which claims stiffness is (largely) not depending on radius (a) and from FEM results showing deflection increase, i.e. stiffness decrease with increasing radius (a).
The aim of the article itself is not a parameter study in the elastic regime so not super relevant but the formula 3 is for linear elastic conditions (neither force load nor plasticity limit load are present and small deflections).
…