General Mechanical

General Mechanical

contac178 contact behavior

    • dfsdf dfsdf
      Subscriber

      I'm trying to model a contact behavior, which is in the tangential direction, for FN < 0 and the absolute value of the
      tangential force (FS) less than μ|FN|, contact "sticks". For FN < 0 and FS = μ|FN|, sliding occurs. When it’s sliding,the tangential force is μ's.(μ' is the the tangential stiffness and s is the sliding distance)

      I've checked the contact behaviors of contac 178 and there is no suitable behavior for my case. Now I have to set keyopt,10,0 to use the standard unilateral contact, but the output data of the tangential force always equals to 0.

      I wanna know how to model this contact behavior. Can I modify the contact behavior or Do I have to write a friction law?

      Any information will be appreciated :)

      Thank you!

    • John Doyle
      Ansys Employee

      What is the physics that causes the external load to increase proportional to the sliding?

      Rather than trying to program something into the contact algorythm, can you create a tabular load for tangential force that is a function of sliding distance?

      • dfsdf dfsdf
        Subscriber

        Thank you for your reply!

        I think it's because I didn't express it clearly, so I’ll try to simplify the problem.

        The external load is a random force.

        When this external load F <  μ|FN|, it sticks. When F =  μ|FN|, sliding occurs. When F >  μ|FN|, it's sliding and its frictional force equeals to μ|FN|.

        I searched ANSYS contact behavior and I think the frictional contact behavior almost meets my requirements.

        But for conta178 element, there is no frictional contact behavior to choose.

        Can element conta178 use the frictional contact behavior? or I have to write my own contact behavior.

        Thanks for your reply again!

         

      • dfsdf dfsdf
        Subscriber

        Now I set KEYOPT(10)=0 to use the standard contact behavior. But the output data of the tangential force always equals to 0.

        I can confirm there is a normal pressure.So I checked the output data of MU, and I found it equal to 0. It's wired because I set MU equals to 0.2

    • dfsdf dfsdf
      Subscriber

      Now I set KEYOPT(10)=0 to use the standard contact behavior. But the output data of the tangential force always equals to 0. I can confirm there is a normal pressure.

      So I checked the output data of MU, and I found it equal to 0. It's wired because I set MU equals to 0.2😣

      I think maybe this is the main reason.

    • John Doyle
      Ansys Employee

      How are you post processing the friction coefficent?

      From Table 178.3 and 178.4, it should be available via ETABLE as an NMISC item via   'ETAB,lab,nmisc,8'.  Make sure you also execute 'OUTRES,all,all' prior to solving so the info is saved to the rst file.

      It is also worth mentioning that CONTA178 is node-node contact and really should only be used for small sliding.  You might want to consider CONTA172 (for 2D) or CONTA174 (for 3D) if you anticipate large sliding.

      Also, this might just be a book keeping issue.  Make sure that your material attribute number is set to "3"  (via "MAT,3") before creating the CONTA178.

       

      • dfsdf dfsdf
        Subscriber

        Thank you so much!!

        I didn't use the MAT command :(  Now I write MAT,3 in my file and it works.

        When it is sliding, I output the data of Fsz(ETAB,lab,nmisc,3), it does equals to MUFn which is consistent with the fritional contact behavior.

        But I wanna make the Fsz equals to tangential stiffness times sliding distance which is a changing force.

        Therefore, the fritional contact behavior can not satify my need.

        I tried to write my own contact interaction(USERINTER)  but there is no example for reference. I have trouble writing this.

        Do you have the USERINTER example? or I can just modify the contact behavior.

        Hope you coule give me some advice.

        (I'm a beginner and I don't speak English. I apologize in advance if I have caused you trouble :()

Viewing 3 reply threads
  • You must be logged in to reply to this topic.