8 Replies Latest reply on Sep 21, 2014 4:45 AM by Leonardo Presciuttini

    Higher stresses for fillets rather than sharp corners? Simulation error?

    Alex Gardner

      I have a question here about something that doesn't seem to make sense to me. When I make a pressure vessel, and put a uniform pressure on the inside of it, I get higher values for the stresses for an internal pressure on rounded corners than I do for the same exact scenario with sharp corners? Can anyone explain this? I can't understand how these result could be correct. Attached is a picture of the pressure vessel and the corresponding results. The fixture and loading are exactly the same for each case. There is a uniform pressure on the inside of each vessel which is exactly the same for both cases. In fact, there is less surface area in the second case, therefore the net force on the inside of the vessel should be less....

        • Re: Higher stresses for fillets rather than sharp corners? Simulation error?
          Zhi Lu

          The results you have was "correct".

          The stress you were looking at was Von Mises stress (yeild equivalent).  If you look at the center/inside node where the maximum stresses occured and compare the two results, you will notice slightly lower hoop and radius component stresses, but much higher axial stressed in the case of your filleted model.  You may "feel" the results were wrong, or not real, but it was parcially becouse you applied a non-realistic loading to the model.

            • Re: Higher stresses for fillets rather than sharp corners? Simulation error?
              Alex Gardner

              Could you explain your answer a little bit more what you mean by my loading being unrealistic? And also why the axial stresses would be higher for the filleted case? I would agree that having no entry or exits to a pressure vessel is unrealistic, however, the general shape of inside of the vessel is what I am concerned with at this point in design. I could build this vessel using two parts made on a lathe or mill, bolt them together, and internally pressurize it with a fluid.   I do have a more detailed version of this (which I can't share do to ip reasons) that bolts together, but I can't test it as an assembly because I don't have the Simulation Professional so I am trying to approximate it as a single part just to get an idea of the stresses. I'm just trying to get an idea of what the internal shape of the vessel needs to look like to optimize the design.

                • Re: Higher stresses for fillets rather than sharp corners? Simulation error?
                  Zhi Lu

                  The model in the png files apears just a ring rather than a whole "pressure vessel".  Can you realy apply pressure only on the cylindrical face of the ring without anything on the fillet?  Where is the ends of the "vessel" (where the pressure would results in high tensile stresses in axial direction)?

                  In order to see the fillet to axial stress effect, you can take a section plot and watch the stresses changes in your filleted case.

                  Your model apears short like a ring.  If you make a test model with a relatively longer "vessel", such effect may become more clear.

                    • Re: Higher stresses for fillets rather than sharp corners? Simulation error?
                      Alex Gardner

                      Zhi,

                       

                      I have attached a picture that better demonstrates how I applied a uniform internal pressure. I didn't just apply a pressure in the radial direction, I applied a pressure to all the internal surfaces of the vessel. I cannot slice open the model in the "results" section of the simulation, to look at the results,  so I sliced open the actual model and reran the study to show what i am talking about. There are bolt holes at the bottom which are fixed, and the pressure is applied uniformly to the inside of the ring. In these results, the stresses were slightly lower for the filleted model rather than the one with sharp internal corners. I am still trying to understand how in the first case (non sliced) my stress results could have been higher, but I cannot slice open the model to see the stress distribution. Maybe if you have Simulation professional I could attach the files and you could check it out and show me what you mean.

                       

                      Pressure Vessel 2.png

                        • Re: Higher stresses for fillets rather than sharp corners? Simulation error?
                          Zhi Lu

                          Now I see what your was doing.

                          To see the inside, rather, to run your FEA, you can cut your model into a 1/4 one and utilizing symmetrical constrains.   It will also help you refine the mesh while keep the size of the model small.  With a 1/4 model, you should be able to refine mesh at one of the corners to check the convergency of the model (try used node stress plot, not element average, as shown in your another post).

                          Also check where the maximum stress is located.  It may be at the "bolt holes", rather in the pressured inside opening.  Look at indevidule stress conponents can also help you understanding more about your case.

                          • Re: Higher stresses for fillets rather than sharp corners? Simulation error?
                            Jared Conway

                            alex, i would recommend linking all your posts together so that if someone finds one they find the others because you're essentially asking the same thing in each. in the end, i'd recommend getting some guidance on setting up the simulation and helping you interpret the results.

                    • Re: Higher stresses for fillets rather than sharp corners? Simulation error?
                      Leonardo Presciuttini

                      Alex, I cannot understand your model and I do not see the mesh, so I will try to offer you a general answer.

                      What you ask is perfectly possible. When you have sharp corners the solution of the elastic equilibrium problem may not converge on the finite element method. This is because the analitical solution may lead to infinite stress when the sharp corner is acute. Therefore the FEM solution may give higher and higher results when the mesh gets finer and finer. Instead, with gentle fillets, the FEM solution does converge. This is why a 'good' solution with the fillets may lead to higher stresses than the solution (necessarily 'poorer' than the former one) with corners. The correct choice between the two models depends from which engineering problem you are considering.

                      If you look at fatigue damage the fillets may be more appropriate (but not necessarily). If you are looking at risks of plastic collapse the sharp edges mwy be more appropriate.