Stress continuity across different bodies

[koenigsegg]

Hi all,

I'm currently building a relatively large structural model in ANSYS Workbench and I need your help in an intriguing issue that has come up.

Since this is a relatively complex geometry, I need to divide it into simpler "blocks" in order to have a nice structured mesh. To do so I am using the Slice tool in DesignModeler. From what I understand, as long as I define a Part that includes these simpler bodies, the mesh shall be continuous across their mutual faces. However, despite the fact that mesh is continuous, I am getting discontinuous stresses across the interfaces of the bodies.

Below are the links to two input files extracted from WB that show this behavior on a very simple example:

Original geometry (as a single Body/Part):

http://www.box.net/shared/rqp7cc8t69

Geometry divided in simpler bodies using the Slice tool (as multiple Bodies grouped in one Part):

http://www.box.net/shared/in0vu9jyvs

Does anyone have any idea of what is going on?

Thanks in advance for your replies.

Cheers

 

[jagad5]

I haven't tried this for awhile. You need to make sure that you still have a single body. You only want to define borders for mesh regions, not geometric discontinuities, which is what seems to have happened. Our firewall won't let me look at your pictures. Stress will be continuous if you have a single body. What type of contact did WB set up in the analysis?

Doug

 

[koenigsegg]

Hello Doug,

Thanks for the reply.

Actually, my purpose is indeed to have multiple Bodies grouped in a Part so that I can create a structured mesh. I don't know any other way of reaching this goal.

Here is an extract of the Ansys help file about this matter:

"Multiple solid bodies within a single part will be meshed with conformal mesh provided that they have topology that is “shared” with another of the bodies in that part. For a face to be shared in this way, it is not sufficient for two bodies to contain a coincident face; the underlying representation of the geometry must also recognize it as being shared. Normally, geometry imported from external CAD packages (not the DesignModeler application) does not satisfy this condition and so separate meshes will be created for each part/body. However, if you have used Form New Part in the DesignModeler application to create the part, then the underlying geometry representation will include the necessary information on shared faces when faces are conformal (i.e., the bodies touch)."

Apparently the mesh is conformal as there are no coincident nodes in the boundaries between Bodies. However the stress discontinuities are there...

As to your question about contact definitions, there is no contact definitions in the model which also indicates that the mesh is conformal...

Cheers

 

[seymours2571]

Koenigsegg,

Do the two bodies you have that have a conformal mesh between them have different material properties? That is one thing to check.

An alternative to creating a conformal mesh is to create contacts with the MPC method. From my understanding, this treats the two notes across the different bodies as bonded.

Steve

 

[jagad5]

If the multiple bodies are really part of a single body, with splits on the surface, then the mathematics forces the displacements and stresses to be continuous. I think that only two ways you could be getting a discontinuous stress distribution at these parting lines is for 1) two separate parts, 2) different materials.

But since WB didn't setup contact pairs, it appears that you only have one "piece" with multiple regions.

Doug

 

[koenigsegg]

Hello all,

Thanks for the prompt replies.

Steve & Doug, all the Bodies have the same material specified. However, one thing that I noticed was that, when I took a look to the APDL commands input file generated by WB, Ansys creates as many materials (with identical properties) as there are Bodies. But this is the only thing "strange" that I notice in the files. There is no apparent reason for the stress not being continuous.

Cheers

 

[seymours2571]

Are you using 1st order elements? If so the stress might not be continuous, but displacement would.

 

[koenigsegg]

Hi,

No, these are 2nd order 20 node elements (Solid186)

Cheers

 

[koenigsegg]

Does anyone have an idea of what might be happening?

Thanks in advance!

 

[seymours2571]

You may have to ultimately post either the zipped WB files or an input file.

 

[ansysfreak]

Dear

This is because of the non-averaging between material properties.
See the avred command for more detail.

Regards

 

[koenigsegg]

Hello,

Thank you for all of your replies. Ansysfreak, you are absolutely right! I completely forgot of that "minor" detail. Many thanks!

Cheers

 

[lediplomand]

Hello Koenigsegg and Ansysfreak,
I am currently confronting the same problem as you had with the Workbench Simulation.
Could you please explain me how you succeeded to resolve this problem ?
I made some reasearch on the "non-averaging between material properties" without any results.

Thank you in advance

Best Regards

Clement

 

[koenigsegg]

Hi Clement,

The way I went around the problem was to write an input file using the FE Modeler module in workbench (using this module, the software no longer assigns "different" materials to different parts) and importing it to the ANSYS Classic environment for the actual run. This is not the most elegant approach but in my case I needed the input file to run it in batch mode.

Probably you can get around the problem using a command snipet inside Workbench that disables this non-averaging behavior in the post-processing. Unfortunately I do not know what is the command for this action.

Cheers