5 Replies Latest reply on Apr 12, 2019 2:11 PM by Joan Madera

    General Static Simulation

    Joan Madera




      I've taken CAD college courses which included SolidWorks; however, although they teach you how to "perform" different types of studies, they never teach you how to verify that your simulation is consistent with reality. Furthermore, as a student, there are simply many things in which I don't have the technical experience to declare whether it is acceptable or otherwise.



      I'm trying to perform a static analysis on the framework attached to this post. If memory serves, I can treat these as trusses. Each element is welded together. My intention is to gain a reliable understanding of the structure's current design with a typical load of 500 Pa per horizontal beam so that I can identify design points to improve. This is part of a medical air and vacuum system, so the structure is meant to carry heavy pumps and compressors.



      1. My current simulation results indicate a FOS of 69. Is this accurate? In my theoretical stress analysis courses, we rarely used a FOS greater than 3. Is my class consistent with industry? Could a fatigue analysis (due to vibrations from operating components, such as pumps and compressors) lead an engineer to increase the FOS by similar magnitude? After all, these systems are built to last decades.
      2. Could someone verify the fixtures I've chosen for the study? Are they proper? Do SolidWorks simulations not recognize weldments without having to label joints as "fixed geometry"? How would I model the ground as a supporting element?
      3. One clear indication that my simulation is wrong, I believe, is the fact that all those members experience 0 stresses. They should be experiencing torsion, moments, and buckling for the columns.
      4. I'd imagine that engineers perform hand calculations to verify consistency with results. If so, why simulate at all? Or is the purpose of simulation simply to act as a secondary confirmation of hand calculations? There are, however, many types of calculations which can't be performed by hand anymore. How do engineers verify those types of simulations?


      Thank you for your time!

        • Re: General Static Simulation
          Ryan Navarro

          Take a look at file attached, it should get you closer to the right path


          You definitely don't want to fix the ends of the individual beams as you've done. As you expected this is resulting in the zero stress in the other members.


          There are small gaps between some of your members and this is why the beam conversion fails in those areas. You should expect to have purple dots at all beam joints like in the revised study I attached. This can be accomplished either by correcting the geometry or manually editing the Joint Group and clicking on the individual dots to assign the various members to joints.


          Some of your members are also too short to be properly treated as beams. I attached a solid mesh approach as well. For this approach I manually bonded contacts across the small gaps to allow it to run, but again correcting the geometry is usually the preferred answer.


          Beam analysis (important to differentiate from truss which carries no moment) does not take into account local stress concentrations due to connection methods etc so if you are interested in those effects you must run either solid or shell mesh


          Check out the validation examples in the software under Help -> SOLIDWORKS Simulation -> Validation -> Verification Problems for tutorials you can work through and compare against hand calcs


          Hand calcs are useful but FEA can often reveal problems that would not be identified by any hand calc.


          I do believe it's pretty common to find structures/products with absurd FOS, not everyone is doing the engineering work to optimize their structures/products up front. They may simply select some common beam/material sizes and then test/validate at the end and if it passes that is sufficient. Often times this results in gross excess FOS but also minimizes the need for further analysis.


          You are right to be skeptical and I am glad you are on here asking these types of questions. FEA is a tremendously valuable tool and as you gain comfort in the software and analysis process I think you will find more and more applications where it will be useful.

          • Re: General Static Simulation
            Ryan Dark


            It might be typical for a Designer to use Simulation for guidance on how to improve a design by comparing the results of several designs directly to one another.  In that way you do comparative analysis where the exact accuracy with relationship to real life can be eschewed in favor of just making a comparative improvement.


            1. A Factor of Safety of 69 is quite high.  Fatigue of a vibrating load may raise the FOS but generally not as much as 69.  Given the yield stress of the applied material (Plain Carbon Steel: 220 MPa) compared to the induced stress on the model (3.2 MPa) that Factor of Safety is consistent with the boundaries applied to the model.  Whether those boundaries represent the real life scenario is the real question.  Looking at how you have fixed the model I would say that this model is not setup right so don't believe that FOS.
            2. These fixtures are wrong.  They are stopping the model from bending under the loading at the ends of each of the cross members.  In a general sense you have to think of fixtures as, "Where in real life am I going to hold this design?"  If this object sits on the ground you should only be fixing joints at the bottom that would interact with the ground.  When using beam mesh elements like you have you don't have an ability to create No Penetration contact with an object (ability to lift off but not push through an object).  So, the best thing you could apply is a Roller/Slider that disallows both lift off and push through motions in the direction normal to the ground.  Either that, or convert your model to solid geometry and use a Virtual Wall
            3. That is a good insight and definitely an indication that the model is not setup in a good way.  You would see all sorts of bending in this model right up to the fixture points.  The fixture points just happen to be in wrong locations.  I think that might be because your beam mesh is not connecting the cross members to the rest of the structure and you have fixed those pieces in an attempt to stabilize them.
            4. Engineers will perform sanity check calculations against FEA models but FEA models can be self checked to a degree.  With solid and shell meshes you would reduce the element sizes applied to the model to see how the stress results change and eventually converge.  That is one self-check.  Hand calculations are typically the secondary check to FEA given FEA can do mode complex geometries quicker than hand calculations can these days.


            In your own model it does appear there are some connection issues between the cross members of the beams.  I suppressed all the trims in the model (they are not needed for beam analysis) then I edited your "Joints" definition and changed the "Treat as joint for clearance" to Less than 1".  Making this change then having the joints recalculate attached the cross members to the rest of the structure so the top and middle fixtures could be removed.  The results seem to be more in line with what I might expect from something sitting on a floor.



            The changes made on the model reduced the FOS down to 39.  So, you can see how setting up the boundaries in an analysis mean a great deal.

            • Re: General Static Simulation
              Joan Madera

              Thank you both for replying. This information is very helpful. I spent a lot of time learning how to perform a solid mesh instead of a beam mesh and replicate the simulations you provided. I've performed the same simulation three times.


              1. Beam mesh with joints edited to take into account the small gaps and fixtures at the bottom corners of the structure.

              2. Solid mesh with contacts and a fixtures on the bottom surfaces of the structure.

              3. Solid mesh with contacts and virtual wall.


              What I noticed is that, while the beam mesh shows a FOS of 38, the solid meshes both indicate a FOS of 16. I was searching for more information about choosing the most adequate simulation technique for my purposes. If I'm not mistaken:


              Beam Mesh

              • Bending Moment Diagrams
              • Faster

              Solid Mesh

              • More accurate
              • Includes stress concentration due to joints


              So the beam mesh assumes the entire structure is a single continuous medium (like our skin) while the solid mesh recognizes that the structure is composed of individual components joined by some method (like our bones). Is this distinction correct? Furthermore, Solidworks doesn't recognize that the joints are bonded by welding, does it? And to simulate the effect of bolted joints I'd have to change the model to include said joint structure, yes?


              I'm going to attempt to analyze this structure by hand with academic techniques to compare with Solidworks.

                • Re: General Static Simulation
                  Ryan Dark

                  Hi Joan,

                  Yes, that description of how beam versus solid elements behave is correct.  The beam element is a 1-Dimensional object (a straight line) that has the properties of the beam profile applied to it via equations and not physically modeled.  The result of this is that beam mesh models calculate very quickly but do not encompass the complexity of the joints that connect them together.  To analyze the stresses in the joints specifically you would need to use solid elements that then can bond specific edges to corresponding faces not unlike what a weld does.  Bolted joints are likewise complex and need to have solid elements used to analyze a bolted joint.

                • Re: General Static Simulation
                  Joan Madera

                  Hello again,


                  Could you look over these simulations to determine whether I set it up correctly?


                  There a two files:

                  • "Adjustable Joint Assembly_BOLTS.zip" (File 1) most accurately represents the fixture and loading conditions.
                    • I'm interested in determining the stresses in the cross-member and the holes.
                    • I used the Bolt Connection feature, as the member is intended to be bolted as shown.
                    • Most of the weight will be supported by the adjacent beams themselves. The bolts are expected to experience minimum stresses as their function is merely to hold the beam in place and adjust its position along the length by sliding.
                      • Pre-stress on the bolts is 0.
                  • "Validation 1.zip" (File 2) is meant to validate File 1. My professors have stated that a simulation must be validated -either from an empirical test, theory, or a simpler simulation operating under similar conditions.
                    • This simulation is meant to mimic the File 1 simulation.
                      • Rectangular supports represent the adjacent beams from the File 1 simulation.
                      • Bolts are replaced by fixture on cylindrical faces.
                      • Virtual wall replaces a boundary not physically represented in this set-up.
                    • If I yield similar results on this simulation as on File 1, then that means that the simulation is valid under the conditions considered, correct?