4 Replies Latest reply on Aug 28, 2012 10:42 AM by Anthony Botting

    Deviation between practical results and SW simulation results

    monika kodikara

      Dear All


      This model was created using SolidWorks 2011 and I am using SolidWorks Premium. I got 2 different answers for the displacement of the 2mm sheet from the SolidWorks simulation and from the practical test. Max. displacement from the simulation is 0.672mm and the max. displacement from the practical test is 2.8mm. Used  Material  is Aluminium 2024 T3 and the properties of actual material and solidworks library material  are equal. Applied pressure was 3 bar. Simulation which I did was attached herewith. Can anyone please help me to find the reason for this deviation?

        • Re: Deviation between practical results and SW simulation results
          Josh Brady

          You haven't attached the simulation.  However, I am going to guess that you put a "fixed" constraint around your outside edges.  As your plate "balloons", it will pull the edges inward toward the center.  The capscrews do not prevent this.

          • Re: Deviation between practical results and SW simulation results
            monika kodikara

            Dear Josh


            Thanks. I have attached the simulation with the assembly file itself. You can see it by clicking the study 1 tab at the bottom left corner.

            • Re: Deviation between practical results and SW simulation results
              Anthony Botting

              Hi Monika:

              I opened the assembly. Usually (but not always) the primary issue is the boundary conditions. Where it is "fixed", the Simulation assumes absolute rigidity, which is not as in real life. Hence, the plate assembly will be much more stiff than actual. It will deflect much less than shown by lab test data. Also, I noticed the "Global contact" is set to "bonded", which glues the plates together where they contact. This 'bonding' tends to stiffen-up the assembly considerably.

              I noticed there are at least two planes of symmetry as well, so you could use a 1/4 symmetric plate assembly. This will reduce meshing and computation time substantially.

              I would approach this by:

              1. Create a new Configuration and section the model (cut off three quarters and leave one quarter for analysis).

              2. Install symmetry boundary conditions on the cut (exposed) faces.

              3. Install "no penetration" contacts between surfaces of the two plates that come into contact.

              4. Install "fixed" fixtures on only the inside surfaces of the bolt holes (not quite realistic, but this may be close enough).


              Try a sample run on this. It will take a while to run due to the "no penetration" contacts (compared to without them). The assembly should be much softer. If still too stiff, it might be because it does not acount for the elasticity of the screws. They can actually stretch.

              To add another step, I would install "Bolt connectors" between the plates to account for the elasticity of the bolts (but remove the fixed restraints on the inside bolt hole surfaces of the 2mm  plate). I am assuming here that the 5mm plate has screw threads, but the 2mm plate does not.


              I hope this helps!