General Mechanical

General Mechanical

Bolt Pretension Origin

    • calebniles
      Subscriber

      Hello,


       


      I am trying to evaluate the effect of torquing a bolt on a clamp assembly. I can't share the whole simulation due to confidentiality. I have a base into which are tapped two holes. The clamp begins flush to one side of the base, with the other side raised a few mm. My bolts on either side have bonded contacts with the base, and frictional contacts with the clamp itself.


       


      I would like to specify a bolt pretension on each bolt. I've been looking at tutorials on how to use pretension and I understand that ANSYS defaults to applying the pretension load at some point on the cylindrical face of the bolt. Since the contact between that cylindrical face and the base is bonded, this results on the bolt pretension pulling in opposite directions in the middle of the bonded contact. I am looking for a solution, and with my limited knowledge of ANSYS have two ideas.


       


      The first, and ideal solution would be to change the point at which the bolt is split by the pretension so that it pulls in opposite directions above the bonded contact. This seems like the most accurate way to model the problem. I have included screenshots of where the pretension currently splits, and where I would like it to on my custom coordinate system.


       


      The second would be to delete the bonded contact and maybe include a fixed support at the bottom of the bolt, but that definitely doesn't seem as legit as the first method.


       


      Does anyone know how to change the origin of my pretension? I have found videos on youtube that mention that possibility but I haven't been able to find a description of how to actually do it.


       


      Thanks for your time

    • peteroznewman
      Subscriber

      You should split the cylindrical face at the top face of the part with the hole so that the lower part of the shaft can be bonded to the hole and the shorter cylindrical face above that can have a Bolt Pretension load.


      The Bolt Pretension software will automatically split the body in the center of the short cylindrical face in order to put one node on the shaft side of the split and one node on the head side of the split so that it can pull them together with the assigned force. It helps if the mesh in that region is small enough so there is at least two elements along the shorter cylindrical face so that the body split can be successful.

    • SaiD
      Ansys Employee

      Hello,


      You can create a new coordinate system but going to the model tree--> Coordinate Systems --> Insert --> Coordinate System. The x-y plane of that new coordinate system will be the plane used to split the bolts and the z-axis is supposed to be parallel to the bolts' axes (so you can define the new coordinate system accordingly).


      When you use the Insert --> Bolt Pretension and choose the bolts where bolt pretension is to be applied, under Details of "Bolt Pretension" you should see an option to define Coordinate System. Here, you can choose the new coordinate system that you have defined, and the location where the bolts are split will change accordingly.


      Ansys employees are not allowed to download any files from the forum, including images. If you need additional clarification, could you use the Insert Image option while posting?


      This is not part of the question you are asking, but remember that bolt pretension and assembly load should not be applied simultaneously. Bolt pretension is generally applied in step 1 and in the subsequent steps the bolts are Locked while the assembly is loaded.


      Hope this helps,


      Sai


       

    • calebniles
      Subscriber

      Hello Sai,


       


      Thanks for your response! That is what I had hoped would be the solution, but I am having trouble executing it. I have already made a new coordinate system, I am just not sure how to define the coordinate system of the pretension. I've included a snip of the details of my pretension and can't find where to specify the coordinate system.


       




      Thank you for your tip about inserting images.


      Caleb

    • SaiD
      Ansys Employee

      Hello Caleb,


      In Ansys, if the Bolt Pretension is scoped to a cylindrical surface, the local coordinate system is defined behind-the-scenes. I think that is what you have done, due to which you don't see an option to define the coordinate system.


      Instead, if you scope it to the solid body of the bolt, by default it will choose the Global Coordinate System, but you can change it to the new coordinate that you have defined. 


      So just try scoping the Bolt Pretension object to the Solid Body of the body instead of just the cylindrical surface.


      Hope this fixes it!


      Sai


       

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