Altair RISE

A program to recognize and reward our most engaged community members

Nominate Yourself Now!

Connecting 3d mesh to 2d mesh

Hi,

I would like to analyse the wing the aerodynamic device of our formula student car.

Since we're using a foam as a solid core for the whole wing, I would like to mesh the foam as 3d elements and connect them with our 2d (Carbon Fibre) Elements.

I'm looking for an easy way to connect those elements to get sufficient analysis results.

Thank you very much for the help.

Find more posts tagged with

English

HyperMesh

Accepted answers

All comments

Altair Forum User

There are several techniques (glue, stick,...) to do that, depending to your solver.

But the most important thing to remember: if your connection area is too close to critical ones, your analysis results maybe not so good.

Altair Forum User

My solver is optistruct. Which technique is favorable here?

Altair Forum User

Hi Mathias,

one another way to connect solid and shells is with rigid elements like RBE2s or RBE3s with a layer of face elements on solid mesh.

Rahul_P1

Sandwiching: Having 1 or 2 layer of shell elements inserted between the solid elements at their junction. an extra layer of shell was created inside/between the solids helps create a smooth transient b/w solids and shells.

Using RBE2 to connect the shell and Solid elements. The independent should hold the Shell node and at least two dependent should hold the nodes on the Solid. Make sure you have nodes on Solid elements exactly of the PSHELL thickness.

Create skin of the solid elements and then connect the nodes of those skin elements with other shell elements.

Altair Forum User

Thank you very much for the help. I will try to use the advices you gave me and will give feedback.

Edit: Just another question: A friend of mine told me, that he created a 2d mesh at first and made a 3d mesh out of that existing 2d mesh. Is that possible? Sadly, he's not in town, so he can't show me the exact way.

Rahul_P1

HI Matthias,

You can do so in several ways,

you can create a 2d mesh, before solid meshing where the 2d mesh pattern will be maintianed,

Or you can drag 2d elements into 3d elements, here is a video tutorial about element offset panel used for this purpose - http://training.altairuniversity.com/modeling/hypermesh-related/introduction-and-use-of-the-element-offset-panel/

Altair Forum User

Hi Mathias,

one another way to connect solid and shells is with rigid elements like RBE2s or RBE3s with a layer of face elements on solid mesh.

How to apply this ?Any example?

Rahul Rajan_21763

Please refer attached screenshot.Assume bigger area meshed with hex element and thin section meshed with shell element.so there should be gap between shell and solid.Mesh carried out in mid surface for thin region.You can have same mesh pattern on hex and shell,then connect them with rigid element.

<?xml version="1.0" encoding="UTF-8"?>

Altair Forum User

If mesh is not same ?

Rahul Rajan_21763

You can try area connectors approach.But having matching pattern with rigid would lead in to good results.For Radioss solver please refer below link for connector creation.

https://www.youtube.com/watch?v=-HdECgBC_lM&list=PLQ7KUGFuVz4u5y3SvIEIU07427-gATaG6

Altair Forum User

Hi, what is thickness and density need to use for the skin elements(face elements of solid elements)

Altair Forum User

Hi, what is thickness and density need to use for the skin elements(face elements of solid elements)

as minimum as possible (say 0.0001)

Wiz211

as minimum as possible (say 0.0001)

I checked the influence of the thickness and noticed that if the thickness is too low the Connection is too weak.

I used a clamped 2D Surface as reference.

If the Skin element thickness was too low the displacement was too high.

I noticed that the Skin Elements need double thickness of the bending 2D Surface to result in the same Deformation like the clamped 2D Surface.

To not influence the System mass I gave the Skin Elements the same material but with a very low Density close to 0.

Giacomo2311

Hello,

i'm a beginner of Altair Hypermesh. I'm facing a fea analysis and i have a doubt about meshing.

I used 2d meshing for ctrical areas of the component i'm studying and i want to use 3d mesh for the rest of the areas not really stressed in the reality.

How can i combine / connect 2d mesh and 3d mesh?

Waiting for a feedback,

Thanks