Stress continuity across different bodies
Stress continuity across different bodies
(OP)
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
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





RE: Stress continuity across different bodies
Doug
RE: Stress continuity across different bodies
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
RE: Stress continuity across different bodies
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
RE: Stress continuity across different bodies
But since WB didn't setup contact pairs, it appears that you only have one "piece" with multiple regions.
Doug
RE: Stress continuity across different bodies
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
RE: Stress continuity across different bodies
RE: Stress continuity across different bodies
No, these are 2nd order 20 node elements (Solid186)
Cheers
RE: Stress continuity across different bodies
Thanks in advance!
RE: Stress continuity across different bodies
RE: Stress continuity across different bodies
This is because of the non-averaging between material properties.
See the avred command for more detail.
Regards
RE: Stress continuity across different bodies
Thank you for all of your replies. Ansysfreak, you are absolutely right! I completely forgot of that "minor" detail. Many thanks!
Cheers
RE: Stress continuity across different bodies
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
RE: Stress continuity across different bodies
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