FAQ Structural Mechanics – Imported

FAQ Structural Mechanics – Imported

When I evaluate a result, why do I get the following error message : “You have a result that is atta

    • pgl
      Ansys Employee
      The message you're seeing is telling you that you're not allowed to scope a results object to a face that is shared between two bodies that are joined together as a multi-body part.When two bodies are joined this way, they share topology (the nodes that comprise that face are nodes that belong to both bodies). Thus, when you request what's known as an element-nodal result (like stress), which pulls results from element integration points, we wouldn't know which elements to pull from (from elements on body A or elements on body B), and these could be very different stresses! There is a workaround you can try, particularly if the materials are of a similar nature. You could select the face in question (so that it turns green), then right click in the graphics area and choose to create a Named Selection. Then, go to that new Named Selection in your tree and right click on it. Here you'll have the option to create a Nodal Named Selection from that face. This is a Named Selection of the nodes that comprise that face, rather than the face itself.Then, you can create a results object, and at the top of the details section, choose to scope it to a Named Selection rather than a Geometry Selection. In this case, you'll be able to scope it to your nodal Named Selection and see stress results on those nodes. You have to be careful about using this option particularly in the case that the two bodies have different materials with very different properties (like a rubber and a steel). In any case, just be sure to check your results carefully to ensure they make sense.
Viewing 0 reply threads
  • You must be logged in to reply to this topic.