Learning Forum

[joepa_2017]

I have been aiming to use conformal meshes on my simulations that involve a layered material where the layers have different mechanical properties. In setting up the model, I used DesignModeler to create a shared topology. This involved selecting all of the bodies in the model and then selecting, "Form New Part." I have noticed, however, that while the mesh is conformal, there are contact elements and a bonded contact created at the boundary between the layers. If I create a shared topology in SpaceClaim, there aren't any contacts created. The results are also slightly different after running the simulation (nothing too drastic, but minor differences).

Is there any advantage to choosing one method for creating the conformal mesh over the other? I guess it comes down to deciding if those contacts would add any benefit to the simulation or not. I'll also note that I just use the default bonded contact settings that DesignModeler creates. In reality, there probably would be some kind of bond between the layers, but I'm not very concerned with the properties of that bond at the moment.

[peteroznewman]

Read this post about Auto Detect Contact on Attach. It is, in my opinion, one of the worst defaults in Workbench.

If you had this unchecked, then you didn't get any contacts created when updating from DesignModeler.

If you had that checked, then you should delete the contacts that are created automatically. They should not be there, they are not needed and are just slowing down the solution.  There is no advantage to those contacts, they are a cancer on the model.  In my next post I'll tell you how I really feel : )

[Sonambk]

Hi Peter,

I am also trying to have a conformal mesh between a solid and a shell element. For modelling, I have left a gap to the midplane of the shell elements of exactly half the shell thickness. Also, I have shared the topology between shell and solid body and even glued the contacts using MPC formulation. Still, I am not getting matched nodes, when viewed in thick shell and beam model. 

[peteroznewman]

@Sonambk,

You have two discussions asking the same question. The post above is the third time you have asked the same question in yet a different place. Don't do that, it wastes my time. I am going to lock one of your discussions (or you can delete it). If you get an answer to your question it should be in the remaining discussion.

 

[joepa_2017]

 @Peter

Thanks for that info. It's odd to me that DesignModeler and SpaceClaim treat the contact region differently when creating a shared topology. From what I can tell, it seems like DesignModeler does fine with making the shared topology, but it does add quite a few contact elements. Anyway, thanks for clearing that up for me.

[joepa_2017]

 Hi Peter, 

Let me know if I should make this a new post; I wanted to ask a follow up question. After turning off Auto Detect Contact on Attach and updating the geometry in my project, a "Contacts" icon still appears under "Connections" in Mechanical. "Contact region" no longer appears under "Contacts," however. Is this what is supposed to happen? Or should there be absolutely nothing beneath "Connections"? 

 

[peteroznewman]

Joe,

If you configure the Workbench Option to uncheck the Auto Detect Contacts on Attach, then you would have a No not a Yes in the image on the left.  You have to restart Workbench for the option to take effect.

When you have that option unchecked, on a new project, you will get no contact created in the connections folder and my Details of Connections shows a No not a Yes for Generate Automatic Connection on Attach.  If you have an old project where there was a Yes created under the old option setting, you have to change the Yes to a No in Mechanical on that old project.

I get no contacts in the Connection folder whether I am coming from SpaceClaim or DesignModeler.

[joepa_2017]

I am observing the same thing if I start the model over again from scratch. If I try to simply switch out the geometry and create a shared topology in SpaceClaim, then I observe what is shown in the left photo. I think I can get this to work as desired now.

 

Thanks!

[peteroznewman]

If you have an old project where there was a Yes for Auto Detection created under the old option setting, you have to change the Yes to a No in Mechanical on that old project. Then in the next attach, there will be no contacts created.

[joepa_2017]

That does work. Now, I have the issue of the solution converging when using bonded contacts but not converging when using shared topology. Why would that happen?

[peteroznewman]

Probably because the mesh size is different on each side of the interface between the bodies and the bonded contact can connect them, while for shared topology, the mesh size has to be identical on each side of the interface.  The model might need smaller elements to converge.

In Mechanical, on the Solution Information folder, set the Newton-Raphson Residual plot count to a non-zero value like 3 or 5. After a solve fails to converge, look a the N-R Force Residual plots. The maximum value is where smaller elements are needed to help it converge.

[joepa_2017]

Just thought I'd update. I've been working on figuring this out for a few days, and I still only get a converged solution when using bonded contacts. The Newton-Raphson residuals show that the issue is not at the interface of the two materials, and reducing mesh size at the problematic spot doesn't necessarily help the solution go further before diverging. 

I'm a bit puzzled as to why bonded contacts make the solution converge better than shared topology, especially when the issue is not at the interface to begin with. There must be some change in how the problem is formulated. Maybe, I have no choice but to stick with contacts.