Preliminary study: 2D–1D connection using LIAISON_MAIL

marcelo

Hello everyone,

I am currently working on a preliminary study involving the connection of a 2D structure to a 1D structure in Code_Aster 17.4 (Windows 11). I used LIAISON_MAIL to establish the connection between the two parts.

As an initial check, I wanted to verify whether the connection was being defined correctly. Without any loading, the model behaves as expected and no deformation is observed.

However, when I apply gravity, an unexpected rotation of the structure occurs. This behavior was not anticipated at this stage of the study, and I am trying to understand whether it is related to the way the 2D and 1D structures are connected, or to another aspect of the model definition.

At this point, this is only a preliminary study, and I am mainly interested in validating the modeling strategy and the LIAISON_MAIL connection before proceeding to a more complete analysis.

I would appreciate any suggestions regarding possible causes of this unexpected rotation or recommendations for checking whether the 2D–1D connection has been correctly defined.

Thank you in advance for your help.

input.comm

6kB

run.export

151B

MESH: .med file

jeanpierreaubry

marcelo
i do not understand what you expect from LIAISON_MAIL in this case
did you read the doc?
in fact i do not understand at all what you want to do

marcelo

jeanpierreaubry hi,
My intention was to connect (transfer forces and combine stiffness) the shell structure (2D) with the beam element structure (1D). I was actually under the impression that LIAISON_MAIL applies only to 2D and 3D elements; however, I couldn't find another solution for this type of condition. How could this be handled? Since the upper structure provides stiffness to the lower structure—which acts as its support—this connection is essential. As I mentioned, this is a preliminary study...

*Judging by the output log, the coupling occurred without issues, which might have led me to believe I took the right approach—or perhaps I just can't see where I went wrong...

jeanpierreaubry

marcelo
try to print the masses, the sum of the reaction and the individual reaction at support
you will see that they do not match
this should be done all the time as a check

jacob

https://codeaster.gitlab.io/doc/docaster/manuals/man_u/u4/u4.44.01/Chargements_de_type_Dirichlet_.html#mot-cle-liaison-elem

LIAISON_ELEM

jeanpierreaubry

jacob
looking at the mesh
i doubt this will do

marcelo

jeanpierreaubry Exactly; given my current level of experience, I can't seem to come up with an alternative or establish that connection between them. I need a more experienced perspective. If the geometry were vertically or horizontally aligned, I would project the structural elements onto the shell—I believe that would align the nodes, making it easier to set up the constraint... It doesn't strike me as a complex problem, but unfortunately, I lack the know-how to work around it.

jeanpierreaubry

marcelo
i understood what you want to do, it is a gangway, is not it?
i doubt this can achieved with LIAISON_MAIL which to my understanding is to glue edges together
i have done quite a few studies of this type
i used:

1- one single mesh with plates and beams, with common nodes
the trouble with this is the offset of beams relatively to the plates is not handled correctly
the plates lie by default in the neutral fiber of the beam
one can use an offset of the plates in the plate properties, it is tricky to use

2- giving an offset to the beams themselves can be achieved
but it is quite high level use of beams, POU_D_T will not do that
i did this theoretical analysis for somebody but i believe i do not own the copyright of this workflow which is very tricky
this study was to model stringers attached to the skin of a ship or an airplane with the offset
and it was a collaborative work with some other engineers hence the copyright

marcelo

jeanpierreaubry You were close; actually, it involves a cable tray system where the 18 cables running beneath the trays need to be supported by an angle-iron structure—specifically in an area where the elevation changes (as in this case study).
The tray system provides a certain level of rigidity—values for which are even provided in the structural component supplier's tables—but due to safety requirements, I was asked to design a supplementary structure, with the constraint that I could only use 2" x 2" x 1/4" L-shaped beam.

I realize this can't be handled via a simple LIAISON_MAIL, but I wanted to consider a different way to transfer the load from the shell to the beam structure. The angle-iron assembly supporting the trays adds strength, and that is what I want to verify; however, I haven't been able to come up with a strategy for doing so.

I even considered projecting the lower structure onto the contact faces as a shell and creating a LIAISON_DDL constraint, but I didn't go through with it because I didn't think it would work... I'm open to suggestions.

jeanpierreaubry

marcelo
the group CABLES looks like sharing its elements with the group BANDJ
which is assigned as DKT with thickness of 3.8, this is strange

in addition i doubt that FORCE_ARETE on CABLE is really doing what you expect

finally when a command ends with no error or warning this does mean that it does what you expect

in your case all the LIAISON_MAIL seem to be done but what are they actually?
only a close look at the mess file would tell, as far as i know there is is no graphical tools allowing to view that
i suggest you try on a very small model with less than 20 nodes so as to look which one is actually link to which one

i have modeled quite often the this sort of grating
i used DKT with a dummy thickness giving the same EI and a dummy RHO giving the same surfacic mass

nevertheless if i read well the doc LIAISON_MAIL is met to glue edges

marcelo

jeanpierreaubry Yes, the CABLES group corresponds to the underside of the tray assembly—which is where I would apply the load—so CABLES is part of the BANDEJ group (the entire assembly). That’s how I learned to do it: I define the groups in the Salome Mesh module and then apply the conditions.

I’m not using FORCE_ARETE; in fact, I’m following your advice and checking only the mass due to gravity to verify that the connection has been established.

"Finally, when a command ends with no error or warning, it means it does what you expect"—I understand that perfectly.

I am also convinced that LIAISON_MAIL isn't the right solution for my case, unless I perform some geometric manipulation. However, I haven't yet found a way to connect the two parts... how would you approach this problem?

jeanpierreaubry

marcelo
humm
i made a typo!!!!!!!!!!!!

"finally when a command ends with no error or warning this does NOT mean that it does what you expect"

i would do a single mesh
or 2 meshes with SUPERPOSE and common nodes where they join

marcelo

jeanpierreaubry I used SUPERPOSE, but I'm not getting anywhere. The "MAIL" keyword is still in the code, but you can disregard it.
Also, how do I make the "common nodes where they join"? That’s the X of the matter... Salome has a lot of features, but I haven't made much progress in my learning.

MODEL LINK

jeanpierreaubry

marcelo
with SUPERPOSE every times code_aster find 2 nodes sharing the very same coordinates it merges them into one single node

so you have to build geometries and meshes according to that

and please try to make meshes wit a sensible number of nodes related to the problem

marcelo

jeanpierreaubry Ok, thanks... but in my case, I left a 57 mm gap between them. Would the SUPERPOSE still work under those conditions? Even with correlated meshes...

jeanpierreaubry

NO!!!!!!!!!!!!!!!!!!!!
there is no solution to your problem unless you modify the meshes

marcelo

jeanpierreaubry I see, but I have one last question before I work out the new geometry/mesh. Would I need to incorporate the L-profile structure into the 2D geometry? I admit I’m actually struggling to explain how I would create this geometry or separate the components to tackle the problem. Please take a look at the image to see if I’ve interpreted it correctly:

In this case, I would have the same mesh elements being shared. So, I would perform the SUPERPOSE operation between the SHELL group (which corresponds to the entire assembly, including the 1D elements) and the BEAM group (a member of the SHELL group). Afterward, I would perform the LIAISON_MAIL. Would that be the correct approach?

jeanpierreaubry

marcelo
how many times should i say that LIAISON_MAIL does not give the correct answer
it is clearly written in the doc
i suggested you do a mesh around 20 nodes to get convinced of that

AsterO'dactyle

Hello,

In code_aster, a distinction is made between what pertains to the geometric framework (2D, 3D) and what pertains to finite element modeling.
This is the difference between MAILLAGE (mesh) and MODELE .
All codes should do this; it would prevent misleading confusion!
In short, if you want to link meshes, LIAISON_MAIL is designed for that. If you want to link models (beams and plates, for example), you must use LIAISON_ELEM (which is poorly named—it should have been called LIAISON_MODELE; we contributed to the confusion!).
In the case of LIAISON_ELEM, we’re linking degrees of freedom between different models. The degrees of freedom are the same between beams and plates, however, linking degrees of freedom isn’t as straightforward—it’s a real modeling challenge.
I admit I didn’t understand how you wanted to link the two models.

jeanpierreaubry

AsterO'dactyle
the trouble is that marcelo wants
to LIAISON a large number of nodes of beams to a large number of nodes of plates
where the beams are lying in a plane parallel to the plane of the plates with some perpendicular offset
as far as i know this is not possible
however LIAISON_MAIL is done without any error or warning
but a simple load with PESANTEUR gives a very large discrepancy between the dead weight and the PESANTEUR calculated sum of REAC

marcelo

jeanpierreaubry Exactly.
However, as I understand it, it would involve the connection via LIAISON_MAIL; I couldn't see any other way... I even tried to interpret the suggestion you gave me to try and solve the problem... but I still haven't found a solution.
Based on the way you taught me, I understood it as I drew it in the image; however, as I interpret it, the connection between them is still established via the connection between meshes.
The main concern is that my deadline is right now—September 4th.

Reducing the number of elements is the least of the problems... that is easy to do.