Issues with shell elements seperating

  • 59 Views
  • Last Post 03 October 2019
  • Topic Is Solved
RDelaCourt posted this 29 September 2019

Hello,

 

I am having some issues with surfaces separating in simulation (explicit dynamics). I have a tubular chassis with two different thickness (2mm & 2.5mm. Both geometries are grouped within their respected folders and then in one top level folder containing both.

 

I have shared the topology on the top level but the surfaces still separate in the simulation (before any contact has even been made also).

 

You have told me on here previously that If "shared topology" has been applied then there is no need to define connections within the solver. However I get the same issue regardless whether I include it or not.

 

Is this possibly an issue with my shell element creation process? I have tried to best capture some images below to help give you an understanding into my problem.

 

Thank you

 

Ryan

Order By: Standard | Newest | Votes
RDelaCourt posted this 29 September 2019

Using the "Show Contact" feature I can see that SC has correctly located the contacts

 

peteroznewman posted this 29 September 2019

Share topology, when it works, does not require any contacts to be defined.  You can tell that Share Topology is working after you Mesh by setting the element edge color to By Connection.  Black edges means 2 elements share that edge (most of the mesh), purple edges means 3 elements share an edge (T-intersection) and yellow edges means 4 or more elements share that edge. (+ intersection).

Share topology doesn't always work.  When it fails, you use Mesh Connections. These also don't require contacts to be defined. The same Edge color By Connection is used to check if there are any gaps.

When Mesh Connections don't work, then you must use Bonded Contact.  Use the MPC formulation because after a solve, you can display the connection elements to check how the parts were bonded (which nodes were used).

RDelaCourt posted this 29 September 2019

Thanks for the reply Peter, I will have a look into this and get back to you.

 

RDelaCourt posted this 30 September 2019

Hi Peter,

 

I had a look and the element edge colours are all red (single element). I also looked into applying an MPC based contact but I do not have it in my current version of Ansys (17.0). One thing I have noticed is the number of elements across the shell thickness face (Picture #3) I am only controlling the size of the mesh that is the rigid body wall that the car is crashing into. the chassis mesh is only;y defined as a global mesh with the relevance set to "zero"

 

I came across this previous post you answered:

https://studentcommunity.ansys.com/thread/how-to-get-three-elements-across-the-wall-thickness-of-a-thin-part/

My hope was to be able to increase the number of elements across the shell thickness but I had no luck (picture #5) my guess is that this is due to that fact that I am using shell elements as opposed to solid geometry?

 

RDelaCourt posted this 03 October 2019

Hi Peter, 

Apologies for taking so long to get back to you.

 

I was able to resolve this issue by taking your advice and using the mesh connections. I had previous had an issue with this in the past with the mesh generating. However I was able to resolve this by refining both Global and Local mesh elements as well as their respected tolerance limits.

 

As always, thank you for your help.

 

Ryan

Close