General Mechanical

General Mechanical

Topics relate to Mechanical Enterprise, Motion, Additive Print and more

contact issue

    • AMIT MOOND
      Subscriber

      Hey !!

      I was trryting to do static analysis in which two clamps are tighntened with the help of bolt over a thin mettalic sheet. The only load here is bolt pretension i.e.15000N. The contact betweeen the thin metallic sheey and clamp which i am using is frictional and no seperation.

      If frictional : the clamp will move apart in space somewhere and it is not behaving as it should be(attaching a image for frictional contact properties)

      I have tried with .3,.5,.8 as friction coeficinent but did not work.

      Then i tried to use no seperation here. Also used dispcament contraints in two directions.(attaching a pic for the same)

      here the clamps will remain at its position but still bolt at15000N is not enough to tigheten the clamp.

      any comments

    • Akshay Maniyar
      Ansys Employee

      Hi Amit,

      Can you insert a contact tool and check for the initial information? May be status for some contact is open or far open.  Also, can you post an image of contacting surfaces and loading? You can also check the below course on 'Preventing rigid body motion'. 

      Preventing Rigid Body Motion in Contact\

       

      Thank you,

      Akshay Maniyar

      How to access Ansys help links

      Guidelines for Posting on Ansys Learning Forum

       

    • AMIT MOOND
      Subscriber

      Please find the inital surfaces details:

      here i have provided pin ball radius also.

      For loading conditions,there are tw bolts and bolt pretension applied on both the bolts. whole assembly is fixed at two flanges.

      {{{Initally i tried with linear material properties but the bolt load was not enough to capture the tightening the clamp. Thein i thought of using the non linear material properties, now at the smaller load step the clamp is tightening but the solution is not converged.}}}

      Why main doubt is why frictional contact is not behaving as it should be.?

       

    • Akshay Maniyar
      Ansys Employee

      Hi Amit,

      As per the images you have attached, it looks like there is a gap initially between the faces which are having frictional contact. So, you can try changing the interface treatment to 'Adjust to touch' and see if it helps. 

      Convergence issues can be very tricky to solve. Can you check what is the exact error you are getting? Also, review Newton-Raphson Residuals to locate the highest residuals, which reflect possible problem areas. Are there loads or supports applied in those problem areas, or are the areas part of a Contact Region? Double-check the model setup as it affects the problem areas.

       

      Thank you,

      Akshay Maniyar

      How to access Ansys help links

      Guidelines for Posting on Ansys Learning Forum

       

    • AMIT MOOND
      Subscriber

      Thanks Akhsay,

      The gap here is visible only because of mid-surface and solid body. I tried to use the frtictional contact "Adjsut to Touch".

      For linear analysis, the solution is converged but bolt pretension load(which is 15500N) is not able to tighten the clamp. If i check working load in bolt tool then it is showing the 15500N. Also the stresses are coming at the bolt shank location only. 

      please check the image 

       

      As you can seee here, if i take the non linear material properties then the results are very different which is at a very minimal load. The solution was not converged with non-linear material which i need to check as you commented.

      do i need to make changes in contact also. 

    • Akshay Maniyar
      Ansys Employee

      Hi Amit,

      As per as I understand from the images you shared, it looks like there is some issue with the contacts. I have some suggestions which you can try.

      1. If you have contact between a shell and a solid body, so did you consider the shell thickness effect?
      2. Please check the initial contact information properly and see if it is correct or not. You can check the status, penetration, or gap. If you find some things wrong with contact then make changes accordingly.
      3. For the frictional contacts which have some gaps, try using contact stabilization damping with the 'Add offset, ramped effect' interface treatment.
      4. Make sure that you have large deformation ON and that you are using enough number of substeps.
      5. If a large friction coefficient is defined (>0.2) consider using an unsymmetric solver.

       Please check the solve.out file properly for the warnings and error messages for finding the exact issue. You can also use contact trackers and Newton Raphson residuals to find the problematic region.

      Thank you,

      Akshay Maniyar

      How to access Ansys help links

      Guidelines for Posting on Ansys Learning Forum

       

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