Mesh generation on membrane surface with shape optimization

Product Support
, ,
1

Hello everyone,

I am stuck at a point in a project (spoke wheel membrane roof) and hope someone here has encountered this before.

Problem:
During the mesh generation, the following keeps occurring:

"An error occurred during mesh generation: mesh input could not be generated."

The affected part is a membrane surface (geometry type quadrangle, stiffness type membrane, orthotropic material, d = 1.0 mm), which is part of a form-finding calculation (form-finding add-on active, pretension of supporting/tension cables and tension ring as separate load cases).

What I have already ruled out:

  • FE mesh quality criteria relaxed to the respective maximum values (α = 5°, ΔD = 15), additionally failure criteria (curvature of membrane elements, aspect ratio, corner angle, Jacobi) significantly increased
  • Element shape set to "Triangles only", "Triangles for membranes" active
  • Model check for duplicate nodes/lines with tolerances from 0.1 to 10 mm
  • Surface area plausible (approx. 500–700 m², no zero or negative value)
  • Isolated test surface rebuilt with 4 new, straight lines between the same 4 corner nodes → same error
  • "Connect" applied to surface + boundary objects
  • "Split surface with cutting lines" → creates 4 partial surfaces, error remains in all
  • Integrated objects and result mesh temporarily deactivated
  • Member subdivisions reset to default values (10)

Questions for you:

  1. Does anyone know this error in this form with membrane surfaces that have a strongly skewed initial geometry that has not yet found form?
  2. Is there a setting or object property that can block the mesh generator which I have not yet considered above?
  3. Is it advisable to smooth the initial geometry more strongly before form finding, or should the mesh generator also be able to handle distorted quadrangle surfaces?

Version: RFEM 6.14.0010

I would be grateful for any hints.

Best regards
A

image
image1302×946 131 KB

image
image1706×872 379 KB

3

Hi @aaaaa

I would definitely start by subdividing the surfaces a bit more frequently. See what happens if you make 12 surfaces around the perimeter.

If that doesn't help, feel free to send me your model via private message, and I'll take a closer look.

Best regards
Fabian

4

Hello Fabian,

At the beginning, I divided it into all 45 segments. I think the cause lies elsewhere. I've attached the model with 12 surfaces in this reply, as I can't send private messages yet.

I would be very grateful if you could help me with this matter; I feel like I've already tried everything.

St_12_Fl..rf6 (5.0 MB)

Best regards,
A.

5

Hello @aaaaa,

apparently there are problems with building the stiffness matrix, which is due to the material definition. You correctly set the shear moduli in z to 0. However, exact zero values can cause problems, so they need to be handled differently. This is done automatically for materials of the type "fabric," but your material is a custom base material with an orthotropic material model.

You have two options, with the latter being the one I recommend:

  1. Set Gxz and Gyz to 1e-6 or similar
  2. Adapt a library material of the type "fabric"

image
image1602×1059 47.3 KB

Then the meshing should work as well.