Reply To: Unrealistic deformation

[peteroznewman]

Hi Patrick,

 

I'm not an Ansys Employee, so I can open your model. I noticed that you are using Ansys 19.0 which is many years older than the current version. Using the current version may help get a better result. Looking at your model, I see the three solid bodies meshed with quadratic solid elements. Because the bodies are very thin compared to the other dimensions, solid elements are not ideal.

Looking at the steel coil, it has only one element through the thickness. Two elements through the thickness is the minimum to get accurate bending results.

 

Looking at the inner layer, it also has one element through the thickness. The smaller elements of the inner layer follow the curvature better than the larger elements on the coil. While the nodes of all bodies are on the geometric surface, you can see the faces of the coil buried in the inner layer. It would be better if the elements were closer to being equal in size. The outer layer also has only one element through the thickness.

  

Because of the difference in element size between the large elements on the coil and the smaller elements on the tubes, the bonded contact will not be as accurate as possible.

I see you imported a STEP file to mesh these solid bodies. One way to get a better mesh is to import the geometry into DesignModeler or SpaceClaim and use the Shared Topology that is available in those systems. That will cause the meshes to be perfectly matched and connected at the shared faces then no bonded contact will be needed.

 

I see this website has "Failed to upload image with an HTTP Error: 504". I hope they fix that soon.

 

Another potential area of improvement is in the choice of the material model. The tubes are defined with Linear Isotropic Elasticity, but a Hyperelastic material model may give more accurate results. However, you will need to obtain the material constants for that model before you can use it.

 

Regards,

Peter