Learning Forum

[Elmano_6]

Hi Guys I am performing static-mechanical analysis in Ansys Mechanical 2020 R2 of the TPMS structure as shown in the picture. The body is fixed on the bottom plate (purple). A force is applied on the top surface (green) via FE-Force, so that I can change the angle of the force via additional coordinate systems later. The simulation runs smoothly and i get my results. However, since I see bigger differences between elements regarding the on-Mises-stress, I wanted to implement a convergence with an allowable change of 5 % with 3 refinement loops and a refinement depth of 2 and then rerun the simulation.
Now my problem: When I click on Solve I receive the error message:
Objects related to mesh nodes, elements and/or element faces or to a "Direct Assignment" are not supported for "Convergence".
I don' really know what that means. The body consists of two base plates and the TPMS structure in the middle, which were assembled in Spaceclaim and imported to Mechanical as scdoc.
What am I doing wrong? How can I get convergence?
I really appreciate your help.
Thanks in advance.

[Erik Kostson]

Hi

Can you show (add an inline image) the Mechanical Tree and your force and fixed support BC in detail?
If they are scoped to nodes like they seem to be from the image above than that is not supported for convergence as the message says. So scope force and fixed support to the faces.
Erik

[Elmano_6]

Hi Erik I hope this is what you need.

[Erik Kostson]

Hi
They are scoped to nodes and that is not supported for convergence as the message says. (It is impossible to refine the mesh during the convergence study if they are scoped to nodes since that node named selection will of course change when we refine the mesh, and it can not be updated automatically (named selection), so hence why it can not be scoped to nodes).

So scope only to geometry say e.g., face, edge, vertex,..

Erik

[Elmano_6]

Got it.
As mentioned, I want to add the same force at an angle (say 30┬░) on the top surface (like a tangential impact). With FE-Force (on nodes) and its connection to an additional, angled coordinate system, I am able to apply the force at an angle. If I use the "normal" force on the surfaces of the elements (see image), I can only apply perpendicular forces but cannot use a different coordinate system.
How would you suggest can the force be applied at an angle?

[Erik Kostson]

Hi

Under force, and define by, instead of vector choose components (and split your angled force to FX, FY FZ components).

All the best

Erik