As you may have noticed from my other posts, i’m going through the Linear static course on enterfea.com by Lukasz Skotny, using only PrePoMax. I’m finding it to be a good way to test out all of PrePoMax/CalculiX and (possibly) learn it’s limitation.
An example in the course is about a bolted cantilever beam, made from shells, which i’ve modelled with midsurfaces in Solidworks, then imported into PrePoMax. The vertical beam has a thickness of 4mm, while the horizontal is 3mm. I’ve set up the model like Lukasz’, except i’ve meshed the vertical C-section profile with TRI’s because quad-dominated causes bad ratios around the bolt holes, that i wasnt able to mesh nicely.
The BCs for the bolts are realised by applying a reference point in the middle of the 4 holes, then restraining TX,TY,TZ. The bottom edge is constrained in TZ only.
The 2 shell parts was having rigid body motions until i set the TIE constraint between the 2 parts to have an offset of 2mm (4mm/2 = distance to surface of vertical part, once expanded).
I’ve doublechecked the geometry, and i believe it matches that of the course, as well as the material data etc. Only differences i can tell are:
The mesh on the vertical part
CalculiX shell elements vs. FEMAP true shell elements
Possibly, the way the connection between the 2 parts are handled.
I feel that the results from the course model (1.9mm) is a bit much off from my model (2.5mm).
I’m still new to using shells in CalculiX, so i wonder if this is me doing something wrong, or simply a limitation to the solver, somehow.
It won’t improve the deflection results but I would advise moving the beam 2 mm away from the column to account for the shell thickness (tie constraint will still work with proper tolerance).
Assuming that everything is set in the same way as in the course (I can’t check it because I don’t have access to that course), what may actually help is refining the mesh (CalculiX sometimes requires more fine mesh than other software to obtain the same results).
If OUTPUT=2D the fields in the expanded elements are averaged to obtain the values in the nodes of the original 1d and 2d elements. In particular, averaging removes the bending stresses in beams and shells.
I see - so move this beam 2mm away from the vertical one?
Is that because the expanded shells from the horisontal edge will end up having TIE constraints to both the inner and outer surface of the vertical beam, with the 2mm offset from midsurface?
Tie constraints and contact account for shell thickness so it’s advised to prepare the geometry with gaps that will be closed when shell thickness is included. Thus, usually, a gap of t/2 is used for each connection. Another options is to use offset in shell section definition.
Yes, although i suppose this will change the overall geometry of the vertical c-profile quite a bit, losing 4mm in X direction and 2mm in Z? Hmm. Modelling with gaps seems a little cumbersome.
Are you using linear or parabolic “shell” elements? Especially elements used for the vertical beam should be parabolic to account for the local bending of the beam wall.
