General Mechanical

General Mechanical

Solver pivot warning

    • thanhttdt
      Subscriber

      Hi everyone, when I practiced as a tutorial 



       


      there was an error (see picture).


      Could you please give me some instruction to solve this problem?


      I also attached project file here for more detail


       https://drive.google.com/drive/folders/1wUlFFu7-1UYM4SXxIP62eQicv63nWQkG?usp=sharing


      Thanks in advance,


    • peteroznewman
      Subscriber

      Hi,


      The problem is the ribs are not connected to the plate. You can see this in Mechanical where the free edges are colored red.



      There are several ways to correct this. One way is in SpaceClaim, to use Shared Topology. In SpaceClaim, here is the current setting:



      Change Share Topology to Share.



      Now the mesh shows that the nodes along the intersection of the plate and ribs have "triple" connections. This is what you want.



      The solver will now solve.



      ANSYS 18.2 archive attached.

    • thanhttdt
      Subscriber

      Hi peteroznewman 


      Thanks for your kind support and very clear illustration. 


      Best Regards,

    • Kai
      Ansys Employee

      Hi, 


      Some general explanations on what "pivot error" means in FEM.


      The pivot or pivot element is the element of a matrix, or an array, which is selected first by an algorithm (e.g. Gaussian elimination, simplex algorithm, etc.), to do certain calculations. In the case of matrix algorithms, a pivot entry is usually required to be at least distinct from zero, and often distant from it. (source: https://en.wikipedia.org/wiki/Pivot_element). A negative or zero equation solver pivot value usually indicates the existence of a singular matrix with which an inderminate or non-unique solution is possible. In ANSYS when a negative or zero pivot value is encountered, the analysis may stop with an error message or may continue with a warning message, depending on the various criteria pertaining to the type of analysis being solved. You may also read ANSYS Help > Mechanical APDL > Basic Analysis Guide > Solution > Singular Matrices to access more details.


      Regards,


      Kai

    • glfakatkar
      Subscriber

      Iam also getting similar error. I have modelled in Geometric modelling and not in space claim. I have applied share topology option. But still Iam getting the error. How to apply shared topology correctly in geometric modelling and how to verify it.


      Thanks in advance.


       


       

    • peteroznewman
      Subscriber

      Try linking a Modal analysis to your Static Structural and solving that. Look at the mode results. If there are modes that have a zero or almost zero frequency, there is a part that is not connected to the other parts that have the Fixed Support.  The mode shapes will show the one part floating about so you can identify it, then take corrective action, such as adding Bonded Contact, to connect that part to the other parts.


      It is better if you start a New Discussion, and include a link to an old discussion for reference. When you start a New Discussion, you are the owner of the discussion and get notified when a reply is posted, and you get to decide when your question has been answered. The original poster is getting notified of these new replies, not you.

Viewing 5 reply threads
  • You must be logged in to reply to this topic.