6 Replies Latest reply on Jan 26, 2012 1:58 PM by Paul Kellner

    FEA vs hand calcs of a simple rod

    Charles Lee

      So, I've been using SimulationXpress for a while and one study made me question the results.  Anyway, I went back and created a simple square rod 1"x1"x5" and applied a 2000lb tensile load to one of the square ends.  The other end is fixed.  Simple hand calculations (F/A) say the stress should be 2000 psi ( 2000lbs/1in^2). 
      However, the SimulationXpress results (static study) yeild something vastly different.  I was wondering if someone could tell me what's going on here?  Am I missing something?   Then when I started playing with the mesh sizes (global size and tolerance), the stress values start going higher for smaller meshes.  Also, I changed the length to 20" and the stress values


      Couple things that I don't understand here:

      1. As the mesh element size decreases, the stress increases.

      2.  The stress is 5-80% over what it should be.... way outside an acceptable range of values compared to simple hand calcs

      3.  The length of the rod shouldn't influence the stress results.  Similar element sizes for a 5" rod compared to a 20" rod shouldn't yeild different stresses.  Some are right on and some are 8% off.  Why is this?  Should be the same calculations with an increase in the number of equations?

      4.  I've also tried this on a different machine which had an older license.  The results are different for same restraints, loads, and geometry but it's possible I can scratch this off to different compilers.  I'm not sure though, so I included the information here.

      5.  I've also tried this on a circular rod which gave me similar results, but the 20" rod was a lot closer to the hand calcs.  Is there reason to think that the separation of the load and the fixture would influence the results?


      Anyway, I've attached the results and any help would be appreciated.

        • Re: FEA vs hand calcs of a simple rod
          Roland Schwarz

          The increased load is dues to stress concentrations, which are the result of the way your part is constrained.  Whenever there is an absolute "fixed" constraint, such things will arise.  Hand calcs don't account for stress concentrations.


          Stress should go up as element size decreases.  If elements are too large, stress errs to the low side.  Reduce element size in regions with high stress gradients until stress stops increasing drastically.

          • Re: FEA vs hand calcs of a simple rod
            sandeep pawar

            As Roland answered, it's due to stress singularity. See attached.

            • Re: FEA vs hand calcs of a simple rod
              Charles Lee

              thanks guys.  So you're saying I should constrain it differently, adjust the mesh or just accept that I'll be getting errors around the restrained face?  Also, that still doesn't answer #3.... why is the length of the rod influence the stress?  Should be the same calculations with an increase in equations, right?  or am I way off?

              • Re: FEA vs hand calcs of a simple rod
                Paul Kellner

                How do your hand calcs match up in the middle of the rod? I expect exact.


                Why is the fixed base showing high stresses?

                Because it is fully fixed. Poisson's effect causes a 3D state of stress to be created as the tensile elongation along the long axis causes a contraction along perpendicular axes. Because it is fully fixed on the end, i.e. there is no compliance in a fixed restraint, as you decrease mesh size the stresses at the constraints will continue to rise because you have an impossible situation.


                In other words you have welded the end of the rod to an infinitely stiff base.


                Correct constraints on the base would be sliding on the face, two corner nodes in one direction in the end face plane and then one corner node perpendicular to that.

                • Re: FEA vs hand calcs of a simple rod
                  Mikael Martinsson

                  And just to add to Pauls answer, I attach a picture so you can see the result with his suggested constraints. (I understood that you have the Xpress version that only supports the "fixed geometry" constraint). Result is 2000 psi regardless of lengths as expected.


                  Restraints are tricky and I believe that Solidworks should have more focus on this matter in the simulation course. My only rule of thumb is to try to avoid the fixed geometry as long as possible.