Preprocessing

Preprocessing

How to avoid pyramid elements to solve the explicit dynamics by using autodyn solvier

    • Jung Myungjun
      Subscriber

      Hi, good afternoon


      now i am modeling bullet which has conical shape for penertration analysis


      However, it seems that a pyramid elements are formed during the mesh generation.


      So when I solve the model, I get a warning message like "pyramid element not supported by the solver, 000 pyramid elements are split into tetrahedral elements." and it takes too long to finish(more than 2days even though simple model).


      I think this is due to the mesh, but I do not know how to solve this problem.


      if one of you know the solution. plz let me know..


       

    • Sandeep Medikonda
      Ansys Employee

      Jung, 


      Right click on the Mesh and Insert a Method, Insert a Method and change it to MultiZone. In this try to use the sizing controls:



      This should work but if not try to use Tetrahedrons and select Path Independent under the Algorithm.


      Hope this helps.



      Regards,
      Sandeep
      Best Practices to post on the Student Community

    • peteroznewman
      Subscriber

      Jung,


      The solver automatically splits Pyramid elements into Tet elements, so that is not a problem. The long solution time has little to do with the Pyramid elements. It has everything to do with the shortest element edge length in the model.  You can replace all Tet elements with Hex elements with the same edge length and the model will still take 2 days to solve.


      The Explicit Dynamics solver calculates a critical time increment from the edge length of the smallest element in the model. One way to cut the solution time in half is to double the element size of the smallest element. But that reduces the detail in the solution. Another way to cut the solution time in half is to artificially increase the density of the materials in the model by a factor of four, but that changes the physics of the problem.


      You might consider cutting off the tip of the projectile in the geometry editor to remove a region that will be filled with small elements, thus increasing the length of the shortest element edge length in the model.  It's good to follow Sandeep's advice and try to make Hex elements because Tet elements often have one edge much shorter than the other three. That short edge is going to dictate the critical time increment.


      The only way to reduce solution time without giving up detail or changing the physics is to use a computer with lots of cores and use an HPC license.


      Regards,
      Peter

    • Sandeep Medikonda
      Ansys Employee

      Indeed, and you can use this check to look for the smallest element that is causing the problem. Smaller the value here, smaller is the time step:


       



      From the picture you provided, it doesn't look like your model is that big. There must be just one small element somewhere. Also, are you using any kind of erosion criteria?


      Regards,
      Sandeep

    • peteroznewman
      Subscriber

      @Sandeep, the Mesh Metric you show is perfect. I didn't know about that, thanks!


      @Jung, if you cut 5 mm off the tip of the projectile, you also have to move the projectile 5 mm closer to the body so there is no gap. Check the mass of the projectile before you cut off the tip, and add that mass back into the projectile by extending the back face until the mass matches the original.


      I recommend you rename the Title of this discussion to "How to reduce solve time for Explicit Dynamics model" since that was your actual desire. The current title is a bit misleading to others who might benefit from the information in this discussion.

    • SaurabhD
      Subscriber

      This was truly enlightening. I am learning ANSYS by whatever there is in Public Domain. Could you please let me know where (source?) can I find such intricate details about the ANSYS Meshing?


       


      Hoe does increasing the density of the material reduces the time for explicit solver?


       


       

    • peteroznewman
      Subscriber

      The maximum time step in Explicit Dynamics is calculated using the speed of sound in the material.  The slower the speed, the larger the maximum time step, the fewer time steps are needed to get to the end time.  The speed of sound is reduced when the density of the material increases.

Viewing 6 reply threads
  • You must be logged in to reply to this topic.