Orphan Mesh to Geometry

[mattwood123]

Hi all,

I am modelling a triaxial test for a soil sample using 3D point data which is measured using cameras. I have used MeshLab to mesh the points and create an STL file, which I have then converted to a .STP file. However, when trying to do an analysis on the mesh, it seems to give no deformation whatsoever. I repeated the exact conditions on a regular cylinder that I created in Abaqus and it worked perfectly, however the mesh seems to be unaffected by the displacements. The mesh is a solid and I have also attempted to convert the mesh to geometry using the plugin on abaqus, but the plugin is not appearing in my GUI for some reason, so I haven't had the opportunity to try it.

Does anyone have any experience with imported meshes on abaqus that would be able to give some advice?

Thanks,
Matt

 

[FEA way]

Hard to say what's wrong without seeing the model, maybe some features like boundary conditions or loads were incorrectly applied to the mesh. Try running a frequency analysis on it, see if it's not hollow, check the number and type of elements and so on.

Regarding the plug-in, it has to be unzipped and placed in the abaqus_pugins folder in one of the specific directories (including your work directory).

 

[mattwood123]

I followed this video exactly with the only difference being that I imported my cylinder in as a step file with a predetermined mesh.

https://www.youtube.com/watch?v=9CxTP0MSBg0

When I run the job, it runs, but then gives me the error message: 'There is no valid step data available on the database. If the analysis is running, the database must be closed and reopened once the results have been initialized. The requested operation has been cancelled'

 

[FEA way]

Step files can't store finite element mesh. You would need a different format to import orphan mesh. INP would be the best. But even if you import STL with a surface mesh, you will still have to convert it to geometry (using the plug-in or Geometry Edit --> Face --> From element faces) and remesh it with solid (volume) finite elements.

 

[rb1957]

I think the STP file can include node mesh, and elements ... OP said that's what he did ... admit I think it would be unusual.

but having the model defined (nodes and elements) doesn't require the underlying geometry to be defined (geometry is just the shape, FEA meshes this with nodes and elements).

but why would not having a geometry "model" prevent the generating of nodal displacements (how I read the OP's OP) ?
if you have the FE model (nodes and elements, et al) and run the analysis, then there should be results ... no?

is it possible that you ran with no loads ??

"Hoffen wir mal, dass alles gut geht !"
General Paulus, Nov 1942, outside Stalingrad after the launch of Operation Uranus.

 

[FEA way]

I've seen some attempts to convert FE meshes to STEP. They end up as geometry divided into small segments. That's also how Abaqus would recognize it and still require meshing. Apparently, the OP just converted STL to STEP, getting hollow (surface) geometry with a bunch of triangular faces.

Abaqus supports so-called orphan meshes (no geometry, just FE mesh) but they have to be imported in specific formats like INP or ODB (Abaqus output database). As I said before, STL can also be used this way but as a surface (shell) mesh only.

 

[mattwood123]

Hi all,

Thanks for your help. I managed to download the plugin on the 2022 version of Abaqus, as it didn't work on the 2021 version for some reason.

After converting to geometry, I used the virtual topology tool to merge the faces of the mesh and that seemed to work for me.

However, I'm not sure if I have removed too much detail from the shape as it was not a perfect cylinder to begin with, although I did get the deformation that I was looking for.