General Mechanical

General Mechanical

SIMULATION OF HONEYCOMB STRUCTURE

    • LidiannedePaula
      Subscriber

      Dear guys,

      I'm Lidianne, graduate student from Brazil. I need help in simulation of honeycomb structure in static structural. Can you help me, please? The software don't accept solve the model, that is in the figure: 

    • peteroznewman
      Subscriber
      Dear Lidianne I suggest you slice the solid geometry on the horizontal flat face to have a larger surface area. Also, you can try eliminating the rigid surfaces, holding the bottom faces Fixed and applying the Ux Displacement on the top faces. That should allow it to solve.
      Also, try meshing so there are 4 elements through the thickness as shown in this video.
    • LidiannedePaula
      Subscriber

      Thank you for yours tips! I eliminated the rigid plates and the problem is solved. But, I wanted validated my model comparing with results of a article that solved though explicit dynamics. Is possible achieved the same results with static structural?
      My computer isn't very good for solve it in explicit dynamic.
    • peteroznewman
      Subscriber
      You can solve this with Static Structural.
      See this discussion for a link: https://forum.ansys.com/discussion/comment/123876#Comment_123876
    • LidiannedePaula
      Subscriber
      Thank you! I achieved understand the different between static structural and explicit dynamic.
      The model for the article is this. They used shell elements in the model and so did I.
      I'm having trouble generating self-contact. Is this correct? Some surfaces are selected at the top and others in the bottom. I couldn't keep a correct order. I also needed to select the same surfaces in target and contact of self-contact.
      Attached is the my project. Please consider only "A" and "B" of the project.

    • peteroznewman
      Subscriber
      I downloaded your .rar file, but you put in the .wbpj file which is not useful on its own, it needs the _files folder of the same name. If you open the .wbpj file in Workbench, use the File Archive menu to save a .wbpz file. That is an achive that has all the information needed to open on another computer. Please attach the .wbpz file to your reply.
      Did you download my file in this discussion? https://forum.ansys.com/discussion/2522/defining-self-contact-in-static-structural/ It is the third post in the thread and has a .wbpz file that you can open. The correct procedure to setup contact for Static Structural is tricky. It would be easier to show you in a video meeting.
      As I mentioned before, Explicit Dynamics requires no effort to setup contact. You get that automatically, but as you learned, you can wait a long time for the solver to compute.
      There are some changes you can make to your Explicit Dynamics model to make it solve in less time. You can edit the density of the material to artificially reduce the time it takes to solve. For example, if you multiply the density by a factor of 25, the solution will take 1/5 of the time to compute the solution.
      Another change is to increase the minimum element size. Look at the Mesh Metric called Characteristic Length. If you can increase the minimum length by a factor of 4, the solution will compute in 1/4 of the time.
      If you do both those things, the solution will take 1/20 of the time to compute. If you also move the displacement 5 times faster, you can cut the end time by 1/5 so if you do all three things, the solution will compute in 1/100 the time.
Viewing 5 reply threads
  • You must be logged in to reply to this topic.