Learning Forum

[Gabriel Coêlho]

Hello everyone,

This is my first post in this forum, so sorry if I am using it wrong.

I am trying to model a portion of a bearing (static), as shown below. I am trying to model the sphere as a rigid body and the rest as flexible. When i try to solve, I get the following error: All bodies under this part must have the same setting for stiffness behavior.  Please modify this setting on each body. I don't understand why. On Spaceclaim, the parts are defined as different components. Any thoughts?

[Sampat Kumar]

Hi Gabriel,
What are the boundary conditions that you have applied? Please let me know.

Regards,
Sampat

 

[Gabriel Coêlho]

Hello, thanks for the reply.

I've set a fixed support on the lower flange and a force through a remote point to the upper flange, as shown on the figure below.

[Sampat Kumar]

Hi Gabriel,
Please unshare the shared topology under the workbench tab in SpaceClaim and perform the shared operation only on those parts that are to be shared by using the share option under the workbench tab in SpaceClaim. You can hide the other parts of the geometry that are not to be shared while using the shared topology on the specific part. Make a separate component of the rigid and flexible parts under the geometry in the SpaceClaim. It looks like all the geometry components are under "Geom" in your case. Both components should be under "geometry."  

Regards,
Sampat

[Gabriel Coêlho]

Hi Sampat, 

I've done what you suggested, and it seems to work, I can now define the sphere as rigid with no "?" on geometry on the tree.
But now, although the individual components have share topology (see figure below with the exploding view), Mehcanical is creating contect between the parts of each component, which in my understanding should not be created if these parts have shared topology. This makes the nodes between the parts not coincident. Any thoughts on that?

[Sampat Kumar]

Hi Gabrial,
Please use the By Connection option to see if the shared topology has been performed or not. Always try to use share and unshare under the Workbench tab in the SpaceClaim. The pink color shows the shared one. Yes, if you have performed shared topology between the parts then it shouldn’t make contact between them. please verify the connected part in the SC again if they are shared or not and let me know. 

Regards,
Sampat

 

 

[Gabriel Coêlho]

Hello, Sampat

I've used the BY Connection on Mehcanical and the result is this:

On Spaceclaim, I define Share Topology on each component individualy, and not on the assembly itself. The result is shown below:

 

[Sampat Kumar]

Hi Gabriel,
Thanks for your patience,
It’s supposed to be updated in the mechanical. Just for information, I think you would have updated your model by selecting “update geometry from the source” in the Ansys Mechanical, after performing the share totpology option in the SC.

There is no need to perform the sharetopology individually. You can hide the ball and perform the Share topology option in the SC on the whole body part, then do the reverse visibility and perform the Share topology on the ball only.

After performing the Sahre topology, you can show all the body and click on the unshare (just to check which geometry parts are shared or not; don’t click on the green tick; it will perform the unshared operation) under the workbench tab to check which parts are shared or not. Then, click Update the geometry from the source in the mechanical. According to your geometry and shared topology operation, there should be two connections in the Ansys Mechanical. Please let me if you have chekced all these points and still facing this issue, then we can check others things also. 

Regards,
Sampat

 

 

[Gabriel Coêlho]

Dear Sampat,

Your solution finally solved the problem.

Thank you.

[Sampat Kumar]

Hi Gabriel,
I appreciate the confirmation. Others who experience difficulties of such type in the future will benefit from reading this topic.
Regards,
Sampat