General Mechanical

General Mechanical

How do I apply a constant load with same velocity to reach desire deformation in ANSYS Workbench?

    • StevenChoong
      Subscriber
      I'm currently working on my academic project and it is required to perform a simulation about ASTM D575-91 (Method B) using ANSYS. I'm totally new to ANSYS, hoping someone can help me out. nThe compressive load (50-kN load cell) was applied at a rate of 12mm/minute until the specimen thickness became 10mm. The origin thickness is 12.5mm. Shape is cylindrical with 28.6mm diameters.nIs it better to use Static Structural or Transient Structural? And how do I define the condition? I tried YouTube but nothing similar is found. n
    • peteroznewman
      Subscriber
      nBest to use an Axisymmetric model. nhttps://forum.ansys.com/discussion/10021/axisymmetric-mechanical-model-tutorialnThe Y axis is the axis of rotation. In a CAD program, DesignModeler or SpaceClaim, draw a rectangle in the XY plane with one corner at (0,0) and the diagonal corner at (14.3,12.5). Create a surface from those four curves. SpaceClaim does that as soon as you go back to 3D mode.nIn Workbench, use Static Structural. Once the geometry cell has that rectangular surface, and before you open the model in Mechanical, look at the Properties of the Geometry cell and set the Analysis Type to 2D.nOpen the model in Mechanical. Click on the Geometry item in the Outline and in the Details window, set the type to Axisymmetric.nApply a Fixed Support to the bottom edge of the rectangle. Apply a Displacement to the top edge of the rectangle and set X=0 and Y=-2.5 mm. This is creates a condition as if the sample can not slip on the surfaces. If you want to simulate the condition where the surfaces have zero friction with the sample, then leave X Free in the displacement and replace the Fixed Support with a Displacement where you set Y=0 and leave X free. In a more complicated model, you can add two surfaces and make frictional contact with the top and bottom of the sample.nIn Static Structural, ignore the time. In this 1 step solution set the end time to 2.5 seconds so one second will represent one mm. Under Analysis Settings, turn on Large Deflection. You will also want to turn on Automatic Time stepping and set the Initial, Minimum substeps to 100.n
    • StevenChoong
      Subscriber
      n
Viewing 2 reply threads
  • You must be logged in to reply to this topic.