News: Need training? HyperSizer Training Videos are available now! Learn more here: https://hypersizer.com/trainingevents/e-learning/

Author Topic: Shell Orientation variation in components  (Read 2206 times)

JanPio

  • Client
  • **
  • Posts: 24
    •  
Shell Orientation variation in components
« on: May 30, 2018, 10:33:09 AM »
Hi,
I got two questions regarding shell material orientation (orange arrows in FEM Viewer):
  • How does the material orientation of a component influence the sizing in general? In my understanding, the sizing-results are not wrong. I just have to take care that plotting 90-degree-results will always show me the results perpendicular to the orange arrows, i.e. adjacent components might show results for different directions. Is that right?
  • I checked shell orientations in the FEM-Viewer and noticed that the arrows point in different directions even within the boundaries of components (cf. attachment). Does this cause sizing errors or plotting errors?
Thanks,
Jan

James

  • Administrator
  • *****
  • Posts: 252
    •  
Re: Shell Orientation variation in components
« Reply #1 on: May 30, 2018, 10:50:33 AM »
Hi Jan,

1. Material orientations define the Nx load direction, x-buckling span direction, the 0-degree fiber direction, ribbon direction of honeycomb core and the stiffener direction.
See: https://hypersizer.com/help_7.3/#FE-Shells/shell-orientation.php%3FTocPath%3DFeatures%7CFEM%2520Interface%7CShell%2520Elements%7C_____3

2. For HyperSizer analyses, all loads are transformed into the material coordinates. Then the loads are summed-up based on the selected statistical loading method. So it's very important that these are consistent within a component. It's a best practice for the material vectors to be consistent within an assembly.

I hope this is helpful.

-James

JanPio

  • Client
  • **
  • Posts: 24
    •  
Re: Shell Orientation variation in components
« Reply #2 on: May 30, 2018, 11:12:01 AM »
Hi James,
from the manual I got what the shell orientation is used for. For our case, I forgot to mention: we use Orthogrid panels.
Assuming a consistent shell orientation within each component: Am I right that with, say, a shell orientation in the circumferential direction of my cylindrical fuselage, the 0deg-results (stiffener spacing, height, etc) are valid for the circumferential direction (and the 90deg-results for the cylinder axis direction)? So the sizing was not wrong, I just have to remember this when plotting 0deg- and 90deg-results because the "labeling" is wrong? This information would help me to decide if current results can be used or have to be thrown away...

Besides that: I understand that varying shell orientations within assemblies (and particularly within components) is highly critical. I will change that.
Thanks,
Jan

James

  • Administrator
  • *****
  • Posts: 252
    •  
Re: Shell Orientation variation in components
« Reply #3 on: May 30, 2018, 11:16:11 AM »
I'd say you're okay as long as your "radius of curvature" and "axis of curvature" selections are correctly defined for your curved panels. See the curvature options on the Sizing Form > Buckling tab.

-James

JanPio

  • Client
  • **
  • Posts: 24
    •  
Re: Shell Orientation variation in components
« Reply #4 on: June 18, 2018, 07:27:09 AM »
Hi,
if I see it right there might be a bug during import:
we use cylindrical coordinate systems (COS) to align the element COS to. The FEM import correctly recognizes the following:
  • the local coordinate systems (visible in FEM Viewer)
  • the assignment of a local coordinate system to elements
But it seems as if information on the COS type (cartesian/cylindrical) is lost. I tested a panel, where local cylindrical COS #15 (axis = panel cylinder axis) is used for the left half (cf. pictures):
  • ANSYS: the x-axis (black) is in downward circumferential direction
  • HS: the x-axis direction points upwards circumferential for the first 5 element rows, then changes to downwards. My guess: HS assigns COS #15 to these elements but treats it as cartesian. That means, for the lower part of the shell: x-axis-projection is used (downwards). Upper part: x-axis-projection gets too small (or even a point), so the y-axis of COS15 is used as the elements' x-axis. Many FEM-programs such as ANSYS also use this method).
  • HS FEM-Viewer "Create or change local COS"-form: here I also cannot find any indication if a COS is of cylindrical or cartesion type.
Even more confusing: plotting, say, N11 in the FEM-Viewer, it shows the correct ANSYS result, i.e. for the actual x-direction, not the one depicted by the arrows! So my understanding is that, for the sizing process, HS uses the actual N11-result for the components but assuming it is the value for the direction shown by the arrow (which is wrong by 180° in this case, and by 90° in the case of my first post).
Can you confirm this?
Thanks,
Jan