13 Replies Latest reply on Sep 5, 2014 12:47 PM by Jared Conway

    test example for convergence

    Magnum So

      Hi,

      I am trying to practice the convergence to make sure accurate simulation result. The following is the test example model:

       

      model : steel pipe( diameter 100mm, length 150mm) with an extension(30mm diameter, length 150mm)

      material: cast iron

      study: static

      fixture: fixed geometry at the end of extension

      force: 20000N action at the bottom of pipe

       

      Picture2.jpg

      Result:

      Picture4.jpg

      mesh density including

      coarse: 13mm

      default: 6.5mm

      fine: 3.2mm

       

      Sine the coarse to  fine mesh density cannot result in a convergence, so I have input smaller mesh density(2mm and 1mm) and then get a convergence.

      Based on this example, I have two questions:

      Q1. I have also input mesh density to 0.5mm, but the solidworks shows a mesh fail message, I am doubted as I always expect only large mesh size will cause mesh fail, right?

      Q2. The result is a convergence so it is accurate and reasonable. But, I have found that the total displacement is only 0.4mm due to the external force

      Picture3.jpg

      I have checked that the displacement is a convergence so it is also reasonable.

      The max. stress at the joint is about 550MPa which is over the tensile stress of cast iron, so this example result shows that a 20000N will deform the steel pipe and the joint of extension will break.

      But in reality, we cannot see the breakdown of a steel pipe with only 0.4mm displacement, right? 0.4mm displacement seems to be an insignificant value and may not result any crack or failure, so I am doubted that if my simulation concept is wrong.

       

      Hope this example will make more discussion here. 

        • Re: test example for convergence
          James Riddell

          Magnum,

          You didn't specify what your radius is between the 30mm & 100mm pipe but it does show one there.  I'd suggest local mesh control refinement at this radius, say on the order of 1/4 to 1/10 that size to give you some refinement in just that area and let the rest grow to a coarse mesh.  What's the shear stress in this area?

            • Re: test example for convergence
              Magnum So

              Hi James,

               

              The fillet radius on the joint is 10mm.

               

              XZ shear stress, the max. stress is around 40MPa

              p4.jpg

               

              YZ shear stress, the max. stress is around 150MPa

              p5.jpg

               

              Is shear stress much more important in this case? I used to focus on the von Mises stress only.

              The aim of example is to simulate the cracking of the joint, so which type of stress I should concern?

            • Re: test example for convergence
              J. Mather

              Magnum So wrote:

               

              ......and the joint of extension will break..

              Where did you get this information?

              • Re: test example for convergence
                Mikael Martinsson

                Can you post your model?

                 

                I find it difficult to understand that this pipe design, with the end of the 30 mm tube fixed, and 20000N (2 ton) would only deform 0,4 mm. How thick is the tube?

                Then I also wouldn't expect the 30 mm section to deform like a Z but instead bend like a C. But in your pictures above, the bottom end (force end) is perpendicular to the fixed tube end in your deformation plot. Did you add any more restraint or did you add a 0,4 mm displacement instead of a force?

                 

                Is it a linear or non linear simulation? The stress above yield is meaningless if it is a linear one, so in that case you can't predict failure.

                What is the material properties?

                • Re: test example for convergence
                  Valerio Valentini

                  I ran the model using 5 mm wall (shell), and refined the mesh at the radius, and got this (over 23 mm displacement):

                  Capture.PNG

                  I used the large displacement solver.  Clearly, these results must be interpreted that the part having failed a long, long time ago.

                  • Re: test example for convergence
                    Jared Conway

                    are you saying that you need to know the stress to a high degree of certainty at a singularity?

                    • Re: test example for convergence
                      Magnum So

                      Hi all, sorry that I have a trip before and cannot access the internet.

                       

                      For Ja.Marther,

                      Q: "Where did you get this information?"

                      A:The von Mises stress result show that the max.stress is at the joint position and the stress value is about 560MPa, this value is higher that the tensile stress of malleable cast iron, so I conclude the joint will break due to the action of 20000N force.

                       

                      For Mikael Martinsson,

                      Q:Is it a linear or non linear simulation?

                      A:I don't know how to define the simulation to be a linear or non linear. I just apply the "Static" study.

                      Q:What is the material properties?
                      A: I choose "Malleable Cast Iron" from the solidworks database.

                       

                      For Jared Conway,

                      My purpose is to find out how much stress the model could overcome and also make a convergence result at the joint position. But when I make it, I just feel that the result is unreasonable as the max.displacement is very small.

                       

                      For Valerio Valentini,

                      Sorry that I haven't showed the detail well, the following is the fixture of the simulation:

                      Besides the fixture on the small pipe end, I also apply a fixture on the inlet of big pipe to restrain the movement along the direction of action force.

                      pp2.jpg ! !

                       

                      I have attached my model file for all your reference. Thank you.

                        • Re: test example for convergence
                          Mikael Martinsson

                          Ok, the cylindrical restraint makes the results in your first mail more reasonable.

                           

                          This is a static linear simulation, based on your material choice.

                          So in areas where your stress goes above yield stress (275 MPa) the results are not real. (static linear works up to yield stress)

                          If you really need to understand if it's close to failure, then you need to do a non-linear simulation with the actual stress strain curve on the material your testing.

                          This requires the highest level of Solidworks Simulation.

                           

                          The high stresses occurs since the small short pipe takes all the bending, due to the cylindrical restraint in the large diameter.

                           

                          Von mises is best suited for ductile materials (elongation at break > 5%).

                          For brittle material you should plot max and min principle stress and compare to the tensile strength of the material.

                          Or you could use the FOS plot based on Mohr Coulomb criterion.

                          (I don't know the properties of this material, perhaps it is ductile)

                          • Re: test example for convergence
                            J. Mather

                            Magnum So wrote:

                             

                            For J.Mather,

                            Q: "Where did you get this information?"

                            A:The von Mises stress result show that the max.stress is at the joint position and the stress value is about 560MPa, this value is higher that the tensile stress of malleable cast iron, so I conclude the joint will break due to the action of 20000N force.

                            Static linear stress analysis results are only valid within the linear elastic deformation portion of the stress/strain curve.  Once you enter into the plastic deformation on the curve - the results are not valid, and in any case don't indicate fracture on the curve.

                            Based on experience you might be able to conclude that the part would in fact fracture, (referencing a general observation - not this particular geometry analysis), but it sounds like you know the part does not fracture and therefore you are calling into question the results that SolidWorks is returning.

                            A couple of things come to mind -

                            1. Factor of Safety below 1 is not the same as saying break or fracture.  (I wish there was a better term for this ratio.)

                            2. If you have experience evidence that conflicts with analysis results - you may need to do additional work to properly set up the digital model analysis to reflect the real world part.

                            If the von Mises stress calculation is (seems) unreasonable - you need to alter your analysis conditions or the interpretation of the analysis.

                          • Re: test example for convergence
                            Roland Schwarz

                            Auto refinement not working for this?

                            • Re: test example for convergence
                              Magnum So

                              Thanks! So "static" study is suitable for elastic deformation analysis only. I should learn more about non-linear simulation right now!