General Mechanical

General Mechanical

‘End Time’ Problem

    • Muhammed
      Subscriber

      Hi everyone,


      I'm trying to make a bullet impact analysis. However, the program gives the results in the middle of the analysis. I'm increasing the 'End Time' step by step. End time was 5e-4s and now 5e-3s. But bullet doesn't go anymore or bounce from the target. It must go further. What's the problem with that. Any help is appreciated. Thanks in advance. 




    • Sandeep Medikonda
      Ansys Employee

      Muhammed,


      The elements are distorting so much that the time step is falling down significantly. Since the Minimum Time Step is set to program controlled in your Analysis settings, the value will be chosen as 1/10th the initial time step. So once your time step falls beyond this value your simulation is failing. Now, you can decrease this value manually for the solver to proceed. However, you are not addressing the bigger issue by doing this and the simulation will be very slow.


      Alternatively, you can introduce some mass scaling to overcome the problem as well. i.e., Automatic Mass scaling introduces additional mass into the system to increase the computed CFL time step. However, introducing too much mass can lead to non-physical results.


      You also would need to focus on some kind of erosion criteria for removing excessively distorted elements. Under Erosion Controls of the Analysis Settings, I would recommend turning on Geometric Strain Limit and use the default value of 1.5 or you can also use the Minimum Element Time Step as erosion criteria (you can combine as well). From the image you shared, your projectile looks like it is being modeled as a flexible body, so basically the elements are getting crushed upon impact, hence it is recommended to use some kind of erosion criteria for the analysis to proceed.


      P.S: Please post any explicit dynamics questions in the Structural Mechanics category in the future.


      Regards,
      Sandeep

    • Muhammed
      Subscriber

      I don't know which number should I choose for the Initial Time Step. Do you have any recommendations?

    • Sandeep Medikonda
      Ansys Employee

      The Initial time step when left on Program Controlled, the time step will be automatically set to ½ the computed element stability time step. The Program Controlled setting is recommended. But you can always reduce the Time Step Safety Factor. You can read about the CFL time step here.

    • Muhammed
      Subscriber

      Thank you, Sir. I will try.

    • Muhammed
      Subscriber

      I turned on Geometric Strain Limit and use the default value of 1.5 but the results didn't change. In my work, the size of the target is 245mmx245mm and the thickness is 4.5 mm. At first, element size for the meshing of the target was 1 mm. After I changed it to 2 mm and the problem was solved. Now, I made it 1.5 mm and the results are still OK. Is it can be an acceptable solution?

    • Sandeep Medikonda
      Ansys Employee

      Muhammed,


      It is very hard for me to answer that. FEA is a mesh dependent analysis, so if you don't see a significant difference in the results between 1.5 and 2mm, I would be tempted to say that. But in general, a mesh convergence study needs to be performed for any problem. Peter has a very good post where he refers to an ASME V&V10.1 document. You would have to go through this and draw your conclusions accordingly.


      Regards,
      Sandeep

    • djtan
      Subscriber
      this has helped me with the issue i also encounterednn
Viewing 7 reply threads
  • You must be logged in to reply to this topic.