4 Replies Latest reply on Mar 20, 2011 1:18 PM by Jerry Steiger

    Huge stress at face boundary

    Christopher Thorn

      Hi there, thanks for taking the time to help.


      I'm trying to simulate what happens to a flat steel blade clamped between two steel discs when a "centrifugal load" is applied to it.


      I've [badly] sketched out the rotor blade and how it is clamped between the rotor discs.




      The only model used in the simulation is the rotor blade. I am trying to simulate the centripetal force on the blade by making face 1 and face 2 fixed geometry. I have added an axis in the correct location and I am using this to define a rotation of the blade of 1200rpm.


      Whilst the simulation completes without errors, the highest stress concentration is at the tangent edge (indicated top right) between face 1 and the cylindrical face of the small cut out.


      Firstly, does it sound like I am correctly defining the restraints and forces in the simulation?


      Secondly, if everything sounds correct, is there any way to get rid of the massive stress concentration along the tangent edge? I have seen figures in excess of the yield stress of the material. I find it hard to accept that the stress in that location would be so high.


      Thanks again for your help,



        • Re: Huge stress at face boundary
          Paul Kellner

          Boundary conditions can be a big problem.


          When you fix the faces you are telling the nodes along the tangent edges of faces 1 & 2 that they simply can't  move at all. This is not what really happens when you clamp the part as you have sketched it. So the elements attached to those nodes have to vary the strain internal to the element from whatever it is away from the edge to zero at the edge where  the nodes are immovable. This sets up a singularity or a place where the stress is infinitely high. In other words, your boundary conditions are modeling a knife edge holding the pieces in place. \


          The clamp ring has some give to it along that edge and you should includ it in your model.


          You might also try boundary conditions where the face is constrained normal to it's surface and free to move in plane.

            • Re: Huge stress at face boundary
              Christopher Thorn

              Hi Paul,


              Thanks for the quick reply.


              Knife edge - exactly what I was thinking.


              Whilst the clamping disc will of course deform slightly, I've had very little success modelling two parts in contact using proper contact constraints. And I've found that the simulation takes forever to complete.


              In order to get a more accurate answer, however, I guess I will have to have another go and be patient.


              Holding the face normal to its surface sounds interesting - I will have a play.


              Best regards,



                • Re: Huge stress at face boundary
                  Abhay Naik

                  I get this problem at all times. There are many explainations to this posted on the forum....I agree with Vince's post here:




                  However, in your case, I think you should be able to split the boundary condition to different faces. I think instead of fixing face 1 and 2 in all directions, I would try to fix it in the direction perpandicular to the axis (same as perpandicular to the faces). I will fix the top or bottom face in vertical direction and horizontal direction.


                  I am not completely confident here...But I dont think the simulations will take any time here....



              • Re: Huge stress at face boundary
                Jerry Steiger



                This is much too late to help much with your original problem, but it may help on future problems. I'm not familiar with Simulation, as we just got a seat, but I think my ANSYS experience is applicable.


                Actually, I think it is a very nice sketch.


                Paul has given you very good advice. Fixed faces are an abstraction that never really exists in the real world. The first thing I would be inclined to do is to split the face that bears on the hub, so that you get the correct contact. (It looks like there is clearance between the tangent line and the edge of the hub.) This may make your stresses a little more realistic. I would also fix one face and let the other one move along the axis.


                Actually, the first thing I would do is to simplify this to a 2D analysis. You've already done the 3D analysis (or you could use a hand analysis) to get the force on the blade. The 2D analyses will run much faster. I would model a small bit of the hub and use contact with light springs to keep the blade from moving along the axis. You can also use symmetry to model just half of the blade.


                Jerry Steiger