General Mechanical

General Mechanical

Convex to Convex Contact

    • vkm120991
      Subscriber

      Hello Everyone,

      I have a situation where a relatively smaller diameter cylindrical pin (Blue pin in attached image) makes contact with a larger diameter cylinder (Redcylinder in image attached). The contact happens between two convex surfaces and is a nonlinear contact where there is initial gap and gap is closed after some displacement of blue pin. Once gap is closed, the blue pin is expected to exert a pre-determined load of say 600N on the convex curvature of Red part. 

      I'm interested in stresses in the large red cylinder. I'm doing the following things:

      1. Red part as flexible material assignment; Blue as Rigid
      2. Contact as Red part (large cylinder, fixed); Target as Blue (small cylinder, moving). Using Frictionless contact
      3. Supports as shown in picture. Only one X displacement input as Remote displacement witih all other DOF set to zero. Remote displacement input as two time steps (T=0 and T=1 where X displacement = two times initial gap). Auto Timestep control with initial sub steps 20, min 10 and max 50.
      4. Once analysis is run, I'm trying to back work the the timestamp where my fixed support reaction is near 600N (desired force) and read out the stresses.
      5. Refined to a very fine mesh with 0.003" element size near contact regions using bod sizing. Tried with enforced quadriatic elements as well. 
      6. I'm ensuring penetration (from contact tool) is being checked and observing it in range of 0.0008- 0.0003
      7. Large deflections are already turned on.

      I have already tried out using Augmented and pure penalty, normal stiffness to 0.1 and slightly lower as well, tried "Nodal projected normal from contact" and other detection methods.

      Issues:

      1. Peak compressive normal principal stresses many times higher than yield observed on few nodes on the contact. However the tensile normal principal stress peak value is much less than yield. Due to high compressive on few nodes, overall model max Von-Mises exceed yield. [The principal compressive stresses increase with mesh refinement so this should be a singularity. I'm unable to remove it even with finer refinement.
      2. Not able to even out the contact throughout the length (observed by varying penetration along the length of red cylinder).

      Kindly help with your suggestion/corrections to my setup.

      I'm much obliged and thank you for your time .

      Regards

    • Aniket
      Ansys Employee
      1. Are you using a nonlinear material model? If you use a linear material model, stresses in the model can exceed the yield stress and use the same stress-strain ratio beyond the yield point.
      2. What do you mean by evening out contact through length?

      -Aniket

      How to access Ansys help links

      Guidelines for Posting on Ansys Learning Forum

      • vkm120991
        Subscriber

         

        Hello, 

        Thanks for the reply Aniket. I’m using a linear material model (i dont have non-linear material data at the moment). It is a ductile material.

        As can be seen in attached image, my cause of worry is the extreme surface level local compressive stress in principal stress plot which are bumping up the von-mises as well, no matter how much I reduce the local mesh size (upto 0.003″). 

        Regards to evening out: It is my interpretation that the very initial contact would be full line contact between the two surfaces. Upon further displacement, since blue pin is rigid, the red pin has to undergo local deformation. When ‘program controlled’ penetration is used, the results show the maximum penetration is more on the lower (vertical) half of the red cylinder. Once I override penetration tolerance to say 1/15th of smallest element size, the penetration plot seems more even along the length of the red cylinder. I have attached images as example.

        Thanks again for your time.

        PS: Peak Von mises stress is observed inside the thickness and not at the contact. Kindly let me know if this is expected behavior?

    • peteroznewman
      Subscriber

      Look up Hertzian Contact and equations show that the peak stress is expected to be below the surface.  That is true for linear materials.

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

      Making both sides flexible will help to even out the stress.

      You can add the simplest Plasticity material model: Bilinear Isotropic Hardening. All you need is the Yield Strength. Set the Tangent Modulus to 0.

      • vkm120991
        Subscriber

        Thank you for the link Pete! 

        I will try to add plasticity and get back with findings.

Viewing 2 reply threads
  • You must be logged in to reply to this topic.