General Mechanical

General Mechanical

Soften the contact

    • jonsys
      Subscriber

      To avoid some of the high stresses at the contact region, I was wondering what are some possible ways to soften the contact between two faces?
      (Adding a rubber layer between/more substeps or what?)

      Regards,


      1

    • Sandeep Medikonda
      Ansys Employee

      Hi Jon,


      Adding visco-plastic materials will dissipate energy. This is up to your end application and engineering judgment.


      You can also add numerical/contact damping into your solution to reduce the high forces but note that artificial energy is being added to achieve this. So, even if your problem converges a lot of artificial energy might not be what your physical problem experiences.


      From a contact perspective, think of it as placing imaginary springs between the 2 bodies. So, if a body is penetrating another a spring force proportional in the opposite direction is being applied. Now, how forcefully is this spring pushing back on one body depends on the contact stiffnes (can be controlled from contact settings) and could define the contact stresses being developed on that surface.


      Hope this helps clarify a little bit.


      Regards,


      Sandeep

    • jonsys
      Subscriber

      Hello Sandeep,


      thank you for the reply.



      • by numerical/contact damping do you mean to add "Stabilization Damping Factor" under Advanced of Details of Contact? what does that factor represent?

      • At the other paragraph, do you suggest to use a "Normal Stiffness Factor"? how does it affect a contact an increasing Factor for example? what are some suggested values for this Factor?


      Regards,


       

    • Sandeep Medikonda
      Ansys Employee

      Hi Jon, Yes Stabilization is like adding dampers to the springs, so it helps contain large displacements for small load increments. Their purpose is similar to weak springs and should be carefully monitored since they add artificial energy. Note that stabilization damping factor also helps with Rigid body motion. This section is from the manual:



      A contact you define may initially have a near open status due to small gaps between the element meshes or between the integration points of the contact and target elements. The contact will not get detected during the analysis and can cause a rigid body motion of the bodies defined in the contact. The stabilization damping factor provides a certain resistance to damp the relative motion between the contacting surfaces and prevents rigid body motion. This contact damping factor is applied in the contact normal direction and it is valid only for frictionless, rough and frictional contacts. The damping is applied to each load step where the contact status is open. The value of the stabilization damping factor should be large enough to prevent rigid body motion but small enough to ensure a solution. A value of 1 is usually appropriate.



      About the normal stiffness factor, it primarily controls the amount of penetration between contact and target surfaces.


      Higher normal stiffness values decrease the amount of penetration but can lead to ill-conditioning of the global stiffness matrix and to convergence difficulties.


      Lower normal stiffness values can lead to a certain amount of penetration and produce an inaccurate solution.


      Ideally, you want a high enough normal stiffness that the penetration is acceptably small, but a low enough normal stiffness that the problem will be well-behaved in terms of convergence. I typically go with about 0.1, especially when I run into convergence issues.


      Once again, this is from the Manual:



      Enter the Normal Stiffness factor. The usual factor range is from 0.01-1.0.



      • The default value of 1.0 is appropriate for bulk deformation.

      • If bending deformation dominates, use a smaller value (0.1). A smaller value provides for easier convergence but with more penetration.



      Hope this clears your questions.


      Regards,


      Sandeep

    • jonsys
      Subscriber

      Sandeep,


      thank you for your clear answer.


      Regards,

    • vkm120991
      Subscriber

      Hello Sandeep,

      Thanks for the insights. 

       been trying to simulate the standard Hertz/Boresi contact cases for regular geometries (like two parallel cylinders pressing; sphere on plane etc ) for which there is clear theoretical backing to predict the contact stress. When doing this, I initiallly left program controlled stiffness updated for each iteration and this give me good agreement. Convergence was also very smooth. So does this mean, I should not further try to soften the contact by reducing the factor for stiffness? 

      1. What are the general guidelines under which we should start using non-program controlled stiffness?
      2. For typical contact problems lets say gear to gear contact / cam to follower contact/ contacts between pin joints of a mechanism, what is the best approach with normal stiffness? 
      3. Ansys user guide only gives range of normal stiffness that can be used (as you mentioned) and also default penetration tolerance of 10% element depth. But is there a typical best practice as to what is acceptable penetration for the above mentioned typical problems which we encounter in all mechanical assemblies? The basic starter course on contacts in Ansys eLearning suggests even 3% penetration of local deformation /element size is high enough. 
      4. My particular use case is where I'm interested to study if failure due to contact can occur between the pin/links of small hand held devices , say a hand held dremmel under loading. I'm already using slow loading in steps, augmented lagrange, large deformations and other standard best practices. I noticed that the contact pressure (and subsequent equivalent stresses generated) are much dependent on the stiffness value (& penetration) that I choose.

      Much obliged for your time & insights.

       

      Thanks

Viewing 5 reply threads
  • You must be logged in to reply to this topic.