Meshing a sheet with a hole 1

[ripubcn]

Hi everybody,

Let me explain my problem with meshing a sheet with a central hole.

I’m modelling a tensile test of a blind riveted connection (3 parts: 2 sheets and the setted blind rivet). I’m using SOLID185 (bricks) and linear isotropic material model.

I want to mesh it with hexahedrons but Ansys doesn’t allow that option with that kind of geometry. I know that if I do two symmetry plans then I can use the option “Sweep”, but I don’t want to do it in that way because afterwards I have to simulate other geometry (more than 1 rivet) which doesn’t have symmetry.

I opened the geometry with Ansys WB and I meshed automaticadly and the result was totally OK (well, I wanted more density of elements around the hole but to start it’s enough). You can see the result in the attached file.

How can I transfer that mesh to the geometry that I already imported to Ansys? Any other idea to mesh it with bricks directly in Ansys?

Thanks a lot,

Ripubcn

 

[seymours2571]

Ripubcn,

Because of the round hole I don't know if it could be possible to have a 100% brick mesh. The hex mesh you have should work fine, unless you need some additional refinement at the hole. If so, just add sizing to the edge of the hole.

Were you looking for a 100% brick mesh or am I way off base with understanding the problem?

Steve

 

[ripubcn]

Thank you for your answer Steve!

I don't want a 100% brick mesh, just with hexahedron it would be fine. I think too it's not possible to mesh it with a 100% brick mesh.

The result that you can see in the attached file I got it in "Ansys WB" and my problem is I want to do it with "Ansys Classic" but there I only can do it with tetrahedron...
that's the reason why I'm traying to import that mesh from "Ansys WB" to "Ansys Classic"... or finding out other method to do it directly in "Ansys Classic".

Thanks again for your answer!

Ripubcn.

 

[timkwan]

You can create a similar hex-shaped mesh in the ANSYS Mechanical APDL (aka Classic) GUI. To do so, manually select the source and target areas for a Sweep operation.

The alternative is to create a mesh pattern using MESH200 (dummy) elements with the desired pattern on the source and target areas first. Select an element shape with the appropriate number of nodes by modifying the dummy element's key option. After that, sweep mesh with the corresponding solid element.

 

[seymours2571]

Ripubcn,

Okay I think I understand now. Setup the problem in Workbench by meshing it and applying boundary conditions. Then highlight either the "Static Structural" tree item or the "Solution" tree item and click Tools > Write Input File.

This will create an input file that can be read by Ansys classic. The input file will only contain the mesh, nodes, and boundary conditions. It will not contain the underlying geometry.

Hope this helps,

Steve

 

[ripubcn]

Thanks timkwan for your answer!

I have allready tryed with "Sweep" operation but it was impossible to got it (i think it's impossible, if you read what ansys help says, at the end of the message)

maybe (probably) I'm doing something wrong... First I tryed just with "Sweep" without a previous mesh, and then I tryed meshing with MESH200 before "Sweep"...you can see in the attached file waht I tryed.


In the Ansys Help says:

"The volume cannot be swept if any of these statements is true:

If LESIZE is used with the “hard” option, and the source and target areas contain hard division which are the not the same for each respective line, then the volume is not sweepable.

The volume contains more than one shell; in other words, there is an internal void within the volume. (A shell is the volumetric equivalent of an area loop - a set of entities that defines a continuous closed boundary. The SHELL column in a volume listing [VLIST] indicates the number of shells in the volume.)

The source area and the target area are not opposite one another in the volume's topology. (By definition, the target area must be opposite the source area.)

There is a hole in the volume that does not penetrate the source and/or target areas."

Thanks again!

Ripubcn

 

[ripubcn]

Thanks Steve!

I didn't see it your answer! Ok, I will try with that but the problem it's I'm not really get used to Ansys WB. Anyway, thank you very much for your advises!

Ripubcn.

 

[timkwan]

The second sweep you tried should be the way - however, you need to create 1 mesh pattern, and then copy it to the other areas with the same topology. After that, you can issue the sweep mesh command.

 

[ripubcn]

Timkwan, you are totaly right! Finally I get it! (see result in the attached file)

How I did it:

1.- Meshing manually all lines
2.- Meshing lateral areas with a 2D element (I used SHELL93 but I supose it´s better with MESH200 because you don´t have to clear the 2D previous mesh when you finally have the 3D mesh)
3.- Meshing the top face and copy the pattern to the opposite face ( Modeling > Copy > Area Mesh )
4.- Meshing the volum with a 3D element (SOLID185)
5.- Clear the 2D pre-mesh

Next step I will try to improve the mesh with more density near the hole and with more than one element in the axial direction.

Thank you for all your advises!

Ripubcn

 

[cbrn]

If I understand it correctly, you need it meshed in Classical environment.
No problem:
- preferably use "mesh200" to create a nice quad mesh on the first plate surface. The surface will have to be "free-meshed" since it doesn't have "3 or 4 boundaries" and there isn't any concatenation that can be used to revert to a "3 or 4 boundaries" situation. Moreover, you very likely need much more elements around the hole than along the plate's perimeter.
- copy the mesh to the other 3 (or 2, it depends on how you built the model) plates' surfaces
- on all the corner edges of the plates, set a number of divisions equal to the number of "through-thickness" elements you desire
- mesh the plates with the "sweep" method.

Suggestions by the other users are pointing you in the same direction, it seems.

Regards
- mesh the plates using sweep-mesh, and set