Stuck? 
support@mecway.com
support@mecway.com
Mecway
FEA
Turn solid from step to shell in Mecway
Howdy, Stranger!
It looks like you're new here. If you want to get involved, click one of these buttons!
support@mecway.com
FEA
It looks like you're new here. If you want to get involved, click one of these buttons!
Comments
An unrelated point. Turn on Fit midside nodes to geometry in Meshing parameters otherwise the curves become faceted and stresses will be less accurate.
I was make the geometry only a surface in Ironcad. In internal solver evertything was ok, but in CCX I had again two mesh. Look at the pic, this is the same model in different analysis. In internal solver i had 676 nodes, but in CCX 1586.
In static 3d results are almost equal, but in buckling 3d the diference is very big.
For ccx, use the following cards, if using composites:
*EL FILE,GLOBAL=NO
S
Also, for ccx composites, add 'don't generate keyword' *EL File
There's an option to change the shell offset also. You should probably check to make sure that ccx expanded the solids the way you expected. You can move it around with the offset option.
Update; I downloaded your model. I see it's very thin. So it's hard to see the shell expansion ccx does. But it looks like it expanded about the midplane.
My experience with the mecway shells is not to use them. They are more like plate elements. For your curved cylinder, i would be surprised if they work right. Visually, the ccx results look good. I switched your model to nonlinear and ran it. It looked good as well.
For such a problem solution should be some kind of regular deformation pattern which can also guide you to discard bad solutions, imperfections in your mesh or any other pathology.
I'm intresting only in steel structures. If you say composites you mean plastic?
I don't read manual for Mecway, I don't know that I can't use internal solver for curved shells, thanks.
disla
I'm traing now free version so I can't use more nodes
My problem has a analytical solution
G = 0,605*E*t/r=0,605*210000*1/500=254MPa
a=254/50=5,08
You are close.
by composites i meant orthotropic shell elements. something like carbon/epoxy. i hadn't looked at your model when i wrote that. for your original model using ccx linear i get 51.85 MPa. With the refined mesh using ccx nonlinear i get 55.48 MPa so not a big change. On the modes, I'm not sure if you need to specify density. I'm not sure how it even solved with it being blank. The modal analysis won't solve but the buckling does. So maybe victor can clarify how buckling solves without a density value. From the equations I looked at online, it seems to be the same formula where the mass matrix is used. In any event, the first non zero mode has a buckling factor of 27.117 with your model using the ccx solver. For the refined mesh it's 5.71, using the ccx solver, and the mode looks completely different. so i imagine for that analysis you need a more refined mesh, like disla said. i didn't know you were using the trial version. so that's why i posted the results here. this is for the 1mm thickness you had defined.
anthony
You can recognize clearly a pattern which is also a good sign.
You don't need density for buckling. Though the eigenvalue equation is similar to the one for vibration, it uses the geometric stiffness matrix obtained from stress instead of the mass matrix.
Curved shells are OK with the internal solver, especially gentle curves like this where the ratio of radius of curvature to thickness is high. Twisted shells are not very good though.
There's no need to use formulas for cylindrical coordinates in the displacement constraints here because they're equivalent to ordinary global x,y,z constraints and are probably getting replaced by them internally anyway. But there's no harm in it if you're planning to extend this to something more complex later.
The radius is 499.5 mm which I guess is an error due to using the mesh of one surface. You can change it to 500 mm using Mesh tools -> Node coordinates or with a 0.5 mm shell offset if it matters.
CCX solution decreases with refinement, hopefully towards 5.08.
Internal solver solution also decreases with refinement, below 5.08 to values like 5.05.
I guess if you know the number of waves around the circumference, you might be able to use a small segment of the cylinder and mirror symmetry to capture exactly one wave with a low node count. Kind of risky though because that's excluding many possible wrong solutions.
as far as the internal shell elements. to me, the ccx stress results look like what you would expect. even when i refine the mesh, the internal results are a little odd. even for this model. the contour plots look off some. as far as the stress magnitude, the results are pretty close to ccx though. i didn't do much with the modes, since you seemed to have to chicken peck at an input setup and then get modes out.
I agree that choosing the Shift point by trial and error is a pain. That seemed to be a requirement of the ARPACK solver but somehow CCX doesn't need it. I don't know if it determines it automatically or somehow avoids using it. If you have no idea of the buckling factor, you can still start with a small value like 0.00001. In this case, knowing the theoretical solution means you can just pick Shift point to be a little lower than that. I set it to 1 and just left it there.
perhaps this helps in your evaluation. ccx nonlinear was able to solve up to the buckling load factor of 5.7. a value of 6 wouldn't solve though. the stress plot is with a cut-plane, so you can see the high stress on the inside of the tube.
Anyone with better shell experience in CCX can shed some light onto it?