Home › Forums › NextFEM Designer support forum › Linear elastic modelling of a slab
 This topic has 6 replies, 3 voices, and was last updated 2 weeks, 6 days ago by NextFEM Admin.

AuthorPosts

March 25, 2024 at 5:17 pm #5032Luciano JacintoParticipant
Dear NexfFEM admin:
I tested NextFEM against a square slab, fixed in the whole contour. The maximum positive moment given by NextFEM agrees with elasticity theory, but the negative moment seems to be very low. The model and the analysis details are attached. The version I’m using is the last one (2.3.2.1). Any help will be greatly appreciated.
Luciano JacintoAttachments:
You must be logged in to view attached files.March 25, 2024 at 8:20 pm #5035NextFEM AdminKeymasterDear Luciano,
thanks for your inquiry. Despite the theoretic shell behaviour is wellknown, numerical applications with shell elements need a lot of care in implementation, because results can vary on the base of adopted mesh, element formulation, and so on.
In particular, we use MIC4 shells for quad elements, which are integrated also along thickness. They have the advantage of avoiding stress concentrations and peaks, which are very unlikely in reality. You’re comparing a theoretical result (peak values, max and min) with an approximate solution – you get such a difference with 10×10 shell model, if you use a 20×20 you get Mmax=7.58 and Mmin=15.47 (hence you get closer).
Therefore, the way is to use more shells – unlike beams, their results are strongly meshdependent.
ps. other solvers (you can try with OpenSees) gives the same results.
ps2. you can get nodes on sides of the shells (to apply BCs) without counting them with
https://nextfem.it/api/html/M_NextFEMapi_API_getNodesOnSides.htmMarch 26, 2024 at 6:05 pm #5043Luciano JacintoParticipantMany Thanks for your very fast response. Thanks also for the free, basic version of the program. What I like best is its very simple interface with Python, making it possible to construct a model in few minutes (using templates). For me, the GUI is good to view results, not so much to build the model.
So, we may conclude that, although the implemented finite element has the advantage of avoiding stress concentrations and peaks (which is the case in many situations, for example concentrated loads on shells), if there is some real peak, we must use a refined mesh, with very small size.
March 26, 2024 at 8:38 pm #5044parhyangParticipanthi, let me add to discussions. It’s commonly doing mesh refinement at high stress/force areas only, below an example.
i reproduced a model using GUI, start from node by coordinate, draw single quad element, mesh uniformly then refined. Solver being used is OpenSees, rerunning with OOFEM given identical results.
Attachments:
You must be logged in to view attached files.March 27, 2024 at 9:19 am #5047NextFEM AdminKeymasterYou wrote:
“So, we may conclude that, although the implemented finite element has the advantage of avoiding stress concentrations and peaks (which is the case in many situations, for example concentrated loads on shells), if there is some real peak, we must use a refined mesh, with very small size.”Yes, and this is the desired behaviour. The element is linear (4 nodes); results in the middle of the span are quite good, while at fixed supports you have actually only 1 element to represent the transition from positive to negative moment.
March 27, 2024 at 12:45 pm #5050Luciano JacintoParticipantDear NextFEM admin and parhyang: Thank you both. Definitely, to estimate negative moments with some confidence in slabs at continuity supports we have to use finite elements with very small size near the supports (size in the order of magnitude of the slab thickness).
March 27, 2024 at 12:56 pm #5051NextFEM AdminKeymasterYes, this is not related to any program or solver; this is a general advice for shell modelling.

AuthorPosts
 You must be logged in to reply to this topic.