General Mechanical

General Mechanical

Interaction of Two Bonded Parts in Static Structural

    • mark8899
      Subscriber

      Hello, 


      I am trying to simulate the bending of a composite skateboard, and I would like to define the supports as a pin and roller (located on the bottom edges of the "axles" as shown in the picture). Both are defined as remote displacements with free rotation, with one of the supports free to translate in the x direction. 


       


      However, the deformation plot looks like the image below, where the deck almost "wraps" around the trucks (axles):



      I would like the trucks to rotate with the deck. The following image is how I would like the simulation result to look: 



      What can I do to achieve this? It might be worth mentioning that the trucks and the deck are bonded with bonded connections. Thank you.  

    • peteroznewman
      Subscriber

      As a former skateboard rider, I am happy to answer this question!


      If the X axis is along the skateboard, the Y axis is vertical and the X axis is parallel to the wheel axles.


      I will assume you have one remote displacement on the rear truck that holds the axle on both sides of the truck. That one should hold X, Y, Z = 0 and Rx = 0 while Ry and Rz are Free.


      The remote displacement on the front truck axles should leave X Free and hold Y, Z = 0.  You can leave all rotations Free, or have Rx = 0 to prevent twist in the deck.


      Under Analysis Settings, turn on Large Deflection.

    • mark8899
      Subscriber

      Hi Peter,


      Thanks for your reply! I've made the remote displacements exactly as you have indicated. I think I see some improvement, but the same issue where the board "wraps" around the trucks still persist. (This is without large deflection)


      However, when i turn on large deflection, the model does not seem to converge. What can I do to improve this?


      I've attached my model for your consideration if necessary. Thanks again! 

    • peteroznewman
      Subscriber

      To get convergence, change the force to 500 N. At higher loads, element distortion errors begin. I also changed the Analysis settings to turn on Automatic Time Stepping and set the Initial, Minimum and Maximum Substeps to 10.


      The board wraps around the trucks because of the concave shape of the board. If you had a flat board made of isotopic material, it would not wrap around. However, the wrap around is highly exaggerated by the Display Scale Factor.  Change it to 1.0 (True Scale).


    • mark8899
      Subscriber

      That makes sense. Just changed it to an isotropic material with high stiffness and it did not behave the same way. Thank you!

Viewing 4 reply threads
  • You must be logged in to reply to this topic.