## General Mechanical

#### Help with meshing!!

• Hannah Korte
Subscriber

I am very new to ansys and I'm really struggling with meshing. I am running a simulation on a small sector of a 1 inch ID corrugated hose with a braid. My sector is 1/6 of the full hose circumference and it is 0.765 inches long. I'm having issues creating a mesh on my intricate braid pattern that complies with the maximum amount of nodes and elements that ansys student can support. I have tried messing with the element size and trying different meshing methods but nothing seems to work. Each ribbon of the braid is made up of five 0.02" diameter cylindrical sweeps. I merged these 5 sweeps into one body. Please help with any suggestions to get my number of nodes down to 32,000 and elements down to 65,000!!!

• Hannah Korte
Subscriber

Here are some screenshots:

• peteroznewman
Subscriber

Hi Hannah,

I suggest you model the braid fibers using Line bodies.  Those can then be meshed with Beam elements and that is massively more efficient with nodes than meshing with solid elements. The corrugated material is thin walled so you should convert that to a surface model and mesh that with shell elements.

With the efficiencies of those types of elements, you can model a full diameter (or at least a half diameter) which you would want to simulate a simple bend in the pipe.

Does the braid just sit on the outside of the corrugated pipe or is there a solid filler (matrix) that holds the braids in place?  That would complicate things.

In the current version of Ansys Structural the node or element limit for the Student license is 128,000.

Regards,

Peter

• Hannah Korte
Subscriber

Hi Peter,

I see what your saying. However, I imported my geometry from solidworks, as I'm not well versed with modeling in SpaceClaim. Is there a way to convert imported geometries into line bodies?

The braid does just sit on the outside. There is a tiny bit of clearance in between the bellows and the braid fibers. It's supposed to help minimize the expansion of the bellows when subject to pressure (which is what I am trying to test).

Also, I messed with the mesh some more and got the nodes and elements down. The mesh is not very good but I wanted to run it anyway just to see what would happen. For whatever reason I am still getting the error that "Your product license has numerical size limits.." This doesnt makes sense because I have ran simulations before with more nodes/elements and have not gotten this error. Any ideas on what else this numerical size limit could be?

Thanks !

• peteroznewman
Subscriber

Hi Hannah,

SpaceClaim has some ability to convert solid extrusions to line bodies, but I don’t know if it will work on a swept solid body. If you are lucky, in SolidWorks there is a circle cross section and a 3D curve that the circle is swept along to create each individual solid braid strand. If that is the case, export the 3D curves as an IGES file and import that into SpaceClaim. Then you can turn those curves into Line bodies which can be meshed with beam elements.

In the current version of Ansys Structural the node or element limit for the Student license is 128,000 but that includes all the nodes and elements that are automatically created after you hit the solve button such as contact elements. So even though the node/element count in Mechanical statistics of the Mesh show it is below 128,000 that number undercounts the elements that are sent to the solver.  An accurate count is made in the Solution Information folder after the Solve button is pressed.

The Student license node/element number limit is not a count limit, but a numbering limit. What can happen sometimes is an initial mesh is made, the count is too high, so some mesh controls are edited to bring the count down, but some body does not get remeshed and it retains its original node number, which is too high. In that case, you can insert a Mesh Numbering object under Mesh and force the mesh to be renumbered to fix that problem.

Regards,

Peter