3D Design

3D Design

Interference fit in cylinders

    • hassam

      i am trying to create an interference fit betwwen two cylinders on Ansys and as soon as extrude the seconde cylinder they get merged



      and shows it as one single body. Pictures are attached for refference. how should i go by this problem.

    • peteroznewman

      Click on Extrude 17 and review the settings in the Details window. You want to Add Frozen to avoid having the new extrusion merge with the first extrusion.

    • hassam


      Thank you very much for your help. I have managed to import the model now and need to follow theses steps to perform my pressure analysis on Ansys. Need your guidance through the process

      b) If geometry, boundary conditions and material has a certain symmetry we ALWAYS use it reduce the problem size. Here an 2D axisymmetric (rotational symmetric approach is good).

      c) The overlapping contact hast to be ramped (i.e. slowly increasing) to give accurate results. You will have to first get the stresses induced due to heat and in a second loadstep you will apply the loads (here pressures)

      d)Please carefully study the chapter about FEM convergence, element quality etc. To get excellent contact pressure results you should try to make the contacting elements as quadratic (in 3D cubic) as possible (close to 100% element quality)

      I need to create two simulations in DM (one with the minimum overlapping, one with the maximum interference)

      Looking forward for your reply



    • peteroznewman

      There are two kinds of 2D models you could make. Axisymmetric and Plane Strain.


      If you create geometry for an Axisymmetric model, it must be in the XY plane, the axial direction must be the Y-axis and the radial slice must be on the positive X-axis. In your 3D solid above, the faces in the ZX plane would be what you would want in the XY plane where Z is replaced by Y.

      In Workbench, right click on the Geometry cell and get properties. In the properties window, you must set Analysis Type to 2D before you attach the geometry to the Model in Mechanical. I am repeating what I said above but it seems you haven't been successful yet.

      Once the model opens in Mechanical, you must click on the Geometry branch, and in the Details window the row 2D Behavior has a pull down and you must select Axisymmetric.

      An axisymmetric model only needs one edge (say the bottom edge) to have a Y Component of Displacement set to zero and X free and the whole model is properly constrained.

      The axisymmetric model has a specific length and there will be end effects near the top and bottom of the assembly that will differ from the center of the axial length.

      Plane Strain

      The faces in the XY plane of your 3D model could be used as a 1/4 model of the Plane Strain. It is good that you have two additional planes of symmetry. You set X = 0 and Y free on the edge on the Y axis, and you set Y = 0 and X free on the edge on the X axis.

      Once the model opens in Mechanical, you must click on the Geometry branch, and in the Details window the row 2D Behavior has a pull down and you must select Plane Strain.

      The depth is infinite, so there are no end effects in Plane Strain.  This represents what you would see halfway along the axial length of a long part.


    • Keyur Kanade
      Ansys Employee

      To help others on forum, please mark this topic as 'Is Solution' as original issue is solved. 

      For other questions please create a new thread. 

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