3D Design

3D Design

Impose a distance between two objects

    • Babeth
      Subscriber

      Hello !

      I model fall/impact tests and I don't find how to impose a precise distance between two objects and be able to easily modify this distance (make it become a parameter for example), using Spaceclaim.

      Is this possible ?

      Thank you,

      Elisabeth

    • peteroznewman
      Subscriber
      Hello Elisabeth If the distance you are talking about is between the object falling and the surface it will impact, you don't use distance to simulate falling from that distance. Instead, you put the two objects in contact and assign an initial velocity to the falling object to simulate the drop height. For example, the impact velocity in m/s for a drop height h is sqrt(2gh) where g is 9.8 m/s^2 and h is in meters. It should be simple to make that velocity a parameter in Mechanical.
      If you want to know how to set up a parameter for a dimension in SpaceClaim, check out the video in this discussion:
      https://forum.ansys.com/discussion/29473/why-is-spaceclaim-layout-slightly-different-from-any-tutorial-that-i-can-find#latest
    • Babeth
      Subscriber
      Hello Peter Thank you ! I was wasting a lot of calculation time simulating all the fall...
      I was also calculating the time of the fall, to have a value for end time in analysis settings. What will become this value if the objects are already in contact ?
      Regards Elisabeth
    • peteroznewman
      Subscriber
      Hello Elisabeth Most of the damage is going to happen on a millisecond time scale. A good feature of these simulations is that you can set a short End Time such as 0.010 seconds and look at the results, If things still seem to be happening, you can type in a longer End Time and restart the simulation from the end of the last one without starting from 0.
      How you do that depends on the solver. In Explicit Dynamics, it is by typing in the Start from Cycle entry in the Analysis Settings and it has a list of points at which it can restart from. In Transient Structural, there is more work to do, you have to preconfigure the Analysis settings to Retain the files after full solve, otherwise it deletes some temporary files at the End Time. Then to restart you set that in Analysis Settings.
      For either solver, you can Pause the simulation to look at results. Do not hit the Stop button on the simulation, that tells the solver to discard everything!
Viewing 3 reply threads
  • You must be logged in to reply to this topic.