Mesh continuity over different areas

[sjorskremer]

Hi all,

I'm generating a geometry that consists of many different areas with varying sizes. As a result, some lines and keypoints do not exactly coincide, and I am unable to merge them. When I proceed to mesh all the areas, the nodes and elements are not continuous across area boundaries, which could lead to inaccurate results.

I've attached a screenshot of both the area and element plots that illustrate the problem for a relatively simple case.
I have already tried using mapdl.aglue() and mapdl.nummrg(), but unfortunately without success.

Does anyone have experience with this issue or ideas on how to tackle it?

Thanks in advance for your help!

Sjors

[germa89]

Well, I would probably break the bottom area on the contact with the top area, so they both share at least one line which should generate a decent mesh so you can use NUMMRG (to merge the line and its nodes and keypoints). This should probably be enought, but you can check applying forces on the top area and see if the displacements match the expected pattern.

If not, you might need more advanced approaches depending on whether you are using SHELL or SOLID elements.
I suspect you might be using SHELL elements, in that case it is recommended you constrain the nodes degree of freedom using CP to couple degrees of freedom (not appropriated for large displacements), contraint equations CE or multipoint constraint MPC elements (appropriate for large displacements and shell-solid interfaces).
If you are using SOLID elements, things are easier since you can use NUMMRG, LGLUE, AGLUE, or VGLUE.

[germa89]

Pinging @mikerife for fact checking.

[sjorskremer]

Thank you for your response!
The problem that I have is with a 'slightly' more difficult geometry than I initially posted:

I have made functions which creates geometries of plates and T-stiffener profiles. Combining the different geometries will make up the entire structure that I'm modelling (see the figure for an area plot of the ideally straight geometry). As you can see, each geometry is made up of smaller areas. This is because I give the stiffeners and plates a deflection (half sine wave). The deflection points are represented by splines, ultimately creating the smaller areas.

A problem occurs when a longitudinal and transversal stiffener intersect (see the second and third figure). I want them to be connected, but as the lines don't coincide, I am unable to merge / glue the lines or areas together. This means that the mesh is not continuous over the different areas at this intersection. (I am using SHELL181 elements btw)

I might have to change my modelling approach to mitigate this, but if you have any suggestions which might fix it I am happy to hear them! :)

[germa89]

If meshes are non-coincident, you need to use MCP184 to fix meshes. It requires a bit of setup, but nothing too complicated.

On the other hand, you could made all the nodes to match by carefully splitting the geometry. This might be quite manual, and very geometry dependent.

So it is up to you.

FYI @mcMunich @mikerife