Good afternoon,
I can’t select the mid-node of the shell (I attach the model) by the ID. I have identified the ID as 11056, but I don’t know why I can select it.
I can’t upload the file, I am new, is there a way to do that? Thank you
Thank you for your time.
Hi @FEAnalyst ,
Thank you very much, but I couldn´t select the node I want. I have done an analysis considering a pressure load, and the software defines the location of the maximum displacement. I want to define an additional force on that point, but I can´t by the way yo tell me. I share a link where you can download the file.
Thank you very much.
JJ
Try Tools → Find to highlight the node with that number. Most likely, it won’t be visible in the FE Model tab because when you use shells, they are internally expanded to solids, and new nodes are created:
To locate that point in the original shell mesh, you could check the undeformed coordinates of this node using the Query tool and then create a reference point at these coordinates to see which node is underneath it.
Or you can rerun the analysis with OUTPUT=2D so that the results are shown on the original (not expanded) mesh:
Just keep in mind that this kind of visualization doesn’t show bending stresses.
Ok, I understand. One question: what is the advantages and disadvantages of this phylosophy of Calculix, to expand for both (shells and beams). What other softwares work similar to Calculix on this way?
Is there any way to show nodes numbers?
Thank you.
JJJ
Unfortunately, this has barely any advantages and mostly causes issues - sometimes stress inaccuracies, but more importantly overconstraints and non-convergence when used with some other constraints and nonlinearities since this expansion is nonlinear.
That’s just a major limitation of CalculiX. It doesn’t have true 1D or 2D elements (apart from one true user shell element, but it needs a special definition and is linear).
However, in most cases, if you keep in mind some special considerations/limitations, it’s not such a big deal.
Other solvers typically have normal beams and shells. I guess it was just much easier fo the CalculiX author to implement it this way. But it might be better to discuss the details on the CalculiX forum where he also replies sometimes: https://calculix.discourse.group/
Not in PrePoMax, you can only search for them with Tools —> Find. But you could convert the results file to ParaView format and display the node numbers there.
not exactly the same since CalculiX use truly solid element with some treatment by number of integration point, advanced solid-shell element is available in Abaqus and Ansys.
Abaqus has so-called continuum shells SCx - volumes with shell formulation and plane stress (but only 3 DOFs) and even continuum solid shell element CSS8 with 3D stress state and special formulation for the thickness direction to better handle thin structures. Both types are typically used for composite modeling, but continuum shells are much more common. They can be stacked and are also superior in analyses involving contact (compared to regular shells).
From what I know, Z88 and Code Aster also have such volumetric shell elements. However, those are special-purpose formulation and these solvers also have conventional shells, while CalculiX has only shells that are actually solids with no special formulation (only some algorithms to handle expansion and dummy rotational DOFs).
I think this could be a very good implementation, and not depend on external applications.
it seems Ansys and Abaqus has problematic at shell part intersection for this element type i.e required truly solid element, CalculiX treated carefully at this condition using knot approach. Also, noticed a solid-shell element is highly recommended and the future to replace standard shell element (classical or conventional). Basically, it took advantage of solid element in face load or contact, nonuniform thickness or tapered, curved geometry, stress triaxiality and distorted element during large deformation but eliminated locking by mixed with shell formulation. Linear hexahedral being used in Ansys made it stiffer since use only one element trough thickness, recommended to use three layered or stack. CalculiX recommended to use quadratic shell element (quadrilateral or triangle) with composite options activated to increase number of integrations. Something is needed to concern is in boundary condition specifically on curved geometry, required to define in user local coordinate system.
Continuum shells in Abaqus are often beneficial (robust and accurate in most shell applications), but they are not recommended for very thin shells since their convergence can be slow. Also, their stable time increment in explicit dynamics depends on the thickness and may also extend the analysis time significantly compared to conventional shells. And there are some small limitations regarding the supported materials (no hyperfoam and low density foam models) and sections (no general shell sections where the section stiffness is provided directly).
There are some benchmarks in the Abaqus documentation where these element types can be compared, such as the Pagano plate problem and (hemi)spherical shell pinching.
in addition, OpenRadioss have this element type also, the solid-shell elements are:
OpenRadioss is explicit dynamics solver so it may have the same issue as Abaqus with continuum/solid shell element thickness affecting the stable time increment.
as i know, OpenRadioss have both implicit and explicit solver (linear & nonlinear) and needed to select and activated before in analysis setting.
Yeah, like LS-Dyna. But explicit solver is the key one and the main reason people choose this software.
