I try to analyse the ovalisation of a bended tube. To reach my goal i made a three-point bending model where i bend a tube made of plate elements. (pic5)
Now i want to analyse the behavior of my tube when the tube changes the profile from circular to oval.(Pic 6)
For that, my idea was to maka a plot where i make a realation between Curvature and Moment (Mz).
Something like: y Axis = Curvature ; and x Axis= Mz(x)
Do you have any experience in doing such a thing?
Ps.: some genereal questions cuz i am not that expierienced, do you think my element size is small enough to make a analyse about the curvature of a tube?
You look as though you have made a good start with this model.
If you want to avoid things like APIs etc, then perhaps you want to use the Charting pane (or List | Output | Results to Data Table, then copy/paste to Excel) so you can look at the (average, and difference in) Y displacement of nodes at the top and bottom centre of the tube; and also the difference in Z displacement of nodes at the front and back of the tube. The average of the Y displacement gives the "general bending", The difference in the Y displacements (top and bottom) and Z displacement (front and back) will give you the oval character (ie. minor and major dimensions of an ellipse). And generally all of these results should be vs Set Value = proportion of applied load, from which you can derive the moment.
Regarding mesh refinement, the rigorous approach is to refine the mesh until the important answers don't change "significantly". Given this physics is dependent on local buckling at the bend point, the model you have shown is excellent as a test model to establish procedure, but you probably should refine the bend zone to a mesh which would start at 2 then maybe 4 times finer than what you have. Mesh | Editing | Element Refine is one relatively simple way to do this if you haven't got some local geometry in that zone where you can use mesh controls (eg. Meshing Toolbox -> Mesh Sizing) to produce local refinement.
You can ask NASTRAN to output curvature information for certain solution sequences. In FEMAP, preview the NASTRAN input file in the Analysis Set Manager. You can then click "Edit Preview", and edit the output requests. For this run, I set up STRAIN to be output as curvature at the centroid and corners of shell elements. I also set it to go to the PRINT file so that I could show the following data. If you set it to PLOT, it will go to the .op2 file and FEMAP will read it for graphical post-processing. In the printed version, 0.0 is Mid-Plane Strain, and Curvature is reported at -1.00000000.
Update, you can do this in FEMAP without editing the NASTRAN input file, in the Analysis Set Manager, under NASTRAN Output Request, you can turn on strain, and set to curvature output in lieu of fiber strain -
Sorry for the late reply, i had to finish my exams.
Thank you so much for your detailed help. I will now continuing working on my project and will try realize your tipps and hope i can get some good results. I must admit that i am not that experienced when it comes to postprocessing.