Hello,
When You preapare shell models, how You find proper direction of shell thickness?
For eg. I made an 2 examples- square shell pipe,w ith 2mm wall: 1) 40x40 2) 36x36
In one case typing 0,5 offset give result that shell thicknes was directed from external surface to the inside of pipe. In second example situation was opposite (if I wanted to hafe thickness from outside to the inside I had to type -0.5)
I have one more question here-
In both cases I added the same BC (1 end fixed) and load (as surface traction at second end)
So- both model (with thickness) have external dimension 40x40, but results for both models were much different (stresses and displacement):
1)
Both results are shown only from compresion/tensile stress from bending (not shear stresses)- and values from calculation “by hand” is approx 136 MPa.
For comparision, shell model with 38x38 dimensions (also 2mm wal thickness, sa it also gives external dimension as 40x40, but offset is 0) gives that results:
So, despite stress concentration at the corners, it looks the closest to the hand calculation- ecepcialy when we use Saint-Venant’s principle (of course in bending it is a bit contoversial).
Could you tell me if You use some of approximations- 1 or 2, in YOur calculations, or You always try to build model, to have shell surface as center of shell thickness- as in 3rd example?)
Check the surface normals. You can use View → Color Annotations → Face Orientations for this purpose. If needed, there’s also a tool that can invert normals for selected faces: Geometry → CAD Part → Flip Face Normal.
Normally, I don’t use shell offsets - I prepare midsurface models for shell meshing.
since the case have a box shape and sharp corner it’s not the same for both models. someone can do simple check of total areas and sectional inertia.
offset definition outward direction will have smaller properties compared to actually. In opposite, an offset definition inward will have larger value of sectional properties.
mid center models will have the same values of sectional areas but not for sectional inertias. approximation model much depend on width to thickness ratios.
offset inward/outward and mid center will have no difference for modeling without a sharp corner i.e box shape has round corner of two times thickness and mesh around corner being refined.
Thanks, I see the point. I didn’t known that in case with offset outward (exampe 2), that missing part will take a count in FEA also- of course in that case inertia will be smaller, due to “lack of material” at corners.
Do You known if, in case of inside direction, when acctually in corners we have small areas with 2 faces on each other, will this be consider by FEA as additional area? Crosssection and innertia in my opinion should be the same as a real 40x40x2 profile (without radius at corners)- but how this “interference” will be calculated?
I think there is a third option in which the cross section is exact. It requires an original step non squared 36x40 and one should offset shells in different directions to avoid overlapping in the corners.
By other hand you should be careful when looking at stresses on shells common edges. As the nodal value is averaged, Stresses may be nonsense if the shells axis are not pointing in the same direction. You could be averaging sxx with syy for example. It is better to look at element values.
Thanks, I also conisidered this way of preparing model- I just make a calculation in that case, and the results looks the best, comparing to the manual calculations:
It looks that this method, and midsurfaces method (mayby only commone edges could be problematic), are the best- and the worst is method with offset inward- which gives smaller results than expected- but is the easiest way to make a number of models
I would consider it a good practice to look at stresses in elements since they are calculated per integration point in each element. The node values are extrapolated and can sometimes lead to mistakes.
No, this is not possible. Are you sure the normal is the cause of the error? Usually, when the mesh is created, all elements of a single surface have the same orientation. So not only one element is to blame.
You could try to remesh the existing mesh using Model → Tools → Remesh Elements
Yep Sure. I have used the Calc_em suggestion and plot colors. It was an isolated element used as wall, made of just one element.
I have fliped outside in the mesher software and “reload using mesh cooordinates form file”.
Thanks anyway. That could maybe be a future feature.
