General Mechanical

General Mechanical

How to make part of a body rigid

    • edoardo
      Subscriber

      Hello everyone,


      I have a problem in simulating a flexible pivot (see the image below). The top plate is fixed, while the bottom plate has a force applied on the edge in -y direction. I need a solution to make the bottom plate rigid (as you can see I get an unrealistic result). I was thinking of splitting the body in 2 pieces, is that possible? In that case, what condition do I need to apply between the 2 parts? Any other possible solution?


      I hope my question makes at least a little bit of sense. Forgive me for my lack of knowledge, I'm new to Ansys (using 16.0). If you need any more files/infos let me know. Thanks in advance


      Edoardo


       


    • peteroznewman
      Subscriber

      Hello Edoardo,


      The best version of this model would be built by having the three surface bodies to represent the flexures. The fixed body doesn't need to exist. Just fix the ends of the flexures where they would connect to the fixed body.  The moving body can be a rigid body. Just make it so by changing the setting under the Details for that solid body. Use three fixed joints to fix the end of each flexure to the rigid body.


      Make sure you turn on Large Deflection under the Analysis settings.

    • edoardo
      Subscriber

      Hello Peter,


      thank you for your prompt answer. I have a few more issues.


      1) After defining the moving body as rigid, I wasn't able to apply a force on it (I could instead apply a force on the flexure). Instead I applied a remote force with success. Is there any difference between them?


      2) Now it seems that I can't mesh the rigid bodies ( I tried with "Full Mesh" on Rigid Body Behavior but Ansys couldn't solve the model). Is there a way around?


      3) Finally, I got a couple errors I'm failing to solve (one about the mesh, the other about boundary conditions):


      Thank you in advance.


      Edoardo

    • edoardo
      Subscriber

      Hello, 


      sorry for being redundant: does anyone know how to solve some of my issues? Thank you


      Edoardo

    • peteroznewman
      Subscriber

      Hello Edoardo,


      1) Remote force is acceptable.


      2) Rigid bodies only get a mesh if a frictional contact is defined. They don't need a mesh to solve.


      3) You have not replaced the flexure solid bodies with surface bodies that are assigned a thickness property. Do that next.  Don't use mesh refinement.

    • edoardo
      Subscriber

      Hello Peter,


      thank you again for your answer.


      I'm having trouble changing the solid bodies to surface! Where can I do that? Is the fillet going to be preserved? (I need to modify it to see how the deformation of the model changes).


       

    • peteroznewman
      Subscriber

      Hello Edoardo,


      No, the fillet would not be preserved if you choose to use midsurface. In fact, you have to delete them to perform the midsurface operation. You can do that in SpaceClaim under the Prepare tab.


      Fillets the size of one wall thickness are not going to change the deformation significantly but if you want to study very large fillets, then you will need to keep the solid body.

    • edoardo
      Subscriber

      Ok, I'm slowly getting there. I still need some confirmation with the Overconstraint error I showed you some posts ago. I found a workaround by using a remote point for the bottom plate while creating the joints. See picture for more clarity. Do you think it's okay?



      Thank you again 


      Edoardo

    • peteroznewman
      Subscriber

      It's a Warning not an Error, and you can ignore most of these kinds of warnings.  It look okay.

    • edoardo
      Subscriber

      Sorry for bumping this thread, but I have a new question related to it. My purpose here is applying a fixed remote displacement to the bottom plate (let's say 20mm in direction -y, while others dofs are let free). While I mantain this value constant, I wanna increase the thickness of the leafs, to get to the point that the material won't yield. 


      The problem is that as I enlarge the leafs, the maximum stress value won't change. How is that possible? I was expecting it to get lower, as I increase the thickness of the leafs. Any ideas?


      Edoardo

    • peteroznewman
      Subscriber

      Did you try double the thickness of the leaf?  I would expect the stress to increase with thickness since you have a fixed displacement.


      Is this the model that has the solid elements with the blend radius at the bottom or the shell model?


      Please attach the archive if you want me (or anyone else) to take a closer look.

    • edoardo
      Subscriber

      I made some changes in the geometry and forgot to update the leafs to shell model, it works as you said. Thank you for pointing out the thickness matter: it makes sense that if I increase the thickness, the structure is more rigid and so I should expect an higher stress under the same displacement. The problem is that I'm used to think with forces rather than displacements

Viewing 11 reply threads
  • You must be logged in to reply to this topic.