The Ansys Innovation Space website recently experienced a database corruption issue. While service has been restored there appears to have been some data loss from November 13. We are still investigating and apologize for any issues our users may have as a result.
General Mechanical

General Mechanical

Topics related to Mechanical Enterprise, Motion, Additive Print and more.

Hertz contact simulation (cylinder on flat)

    • s310413
      Subscriber

      Hi everyone, I'm new on Ansys. I'm trying to simulate a cylinder (radius=6mm, E=200GPa nu=0.3) on flat Hertzian contact under 185N normal load. According to Hertz theory I should get a contact pressure of around 330 MPa but I don't manage to get it on Ansys. I attach some details of the analysis, please can someone help me to find the mistake or anyone has suggestions? Thanks a lot

    • Ashish Khemka
      Forum Moderator

      Hi,

      Please search YouTube for a video titled 'Hertz Contact Simulation using Ansys Workbench 2019 R3' and you will get relevant instructions.

      Regards,

      Ashish Khemka

    • s310413
      Subscriber

      Hi,

      thanks for your response. I tried following that video suggestions but I still get 1000 MPa. In the video a normal displacement is applied while I have to apply a normal load so maybe the problem is in defining the load condition. Any other ideas? Thanks

    • Ashish Khemka
      Forum Moderator

      Hi,

      Can you check the following post as well for suggestions? Modeling Hertzian Contact Stress in Line contact by two cylinders (ansys.com)

      In addition, have you cross checked your hand calculations with any of the online calculators?

      Regards,

      Ashish Khemka

    • peteroznewman
      Subscriber

      Hi Gabriele, this is an online calculator I like to use.

      https://amesweb.info/HertzianContact/HertzianContact.aspx

      I put your data in but you did not specify the Line Contact length. If I use 10 mm it calculates a maximum Hertizan contact pressure as 328.4 MPa. If I use 1 mm it calculates a pressure of 1038.5 MPa.

      It looks like you have created a 2D analysis. Did you choose Plane Stress or Plane Strain?  Plane strain is calculated based on a unit depth, so if you are working in mm, then the Plane Strain contact pressure is expected to be the 1038.5 MPa result.

      • s310413
        Subscriber

        Hi peteroznewman, I think you guess the problem. Actually I was trying to replicate a paper in which the author uses a 2D simulation and selecting plain strain. So I chose plain strain getting 1038 MPa as you said. So do you have any suggestion to get 328 MPa in a 2D simulation or the only way is a 3D simulation? Thanks

        • peteroznewman
          Subscriber

          If the physical problem has a 10 mm depth with a 185N normal force, and you build a Plane Strain model that has a 1 mm depth, the force in that 2D model should be in N/mm or a value of 18.5 N/mm and then you will get 328 MPa of contact pressure.

        • s310413
          Subscriber

          That was the mistake. Thank you!

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