27 Replies Latest reply on Dec 6, 2018 10:05 AM by Bill McEachern

    Static simulation fails while real product succeeds

    B. Bijl

      Dear Forum,

       

      I'm running into a problem using solidworks simulation. To be very clear I'm not a professional using static simulations. I know the basics.

       

      A coupler plate for some machinery we have here needs to lift 2.5 Tons. To get a proper certificate it needs to lift up to 200%, meaning 5 Tons.

      It did this without any problems or deformations in the product. But when I try to simulate this in Sw, it shows that it should fail. The biggest stress areas Sw shows are logical though.

       

      Attached is the product.

      Below some screenshots:

       

      Coupler static.jpgCoupler static stress.jpg

       

      The hoist ears are welded on the bend plate. Can this be the issue?

       

      I would be very happy to get some advice from you guys on my problem.

       

      Cheers,

      Boris

        • Re: Static simulation fails while real product succeeds
          Dave Bear

          Hi JM Van Oossanen,

           

          Okay, just a couple of things to point out as a Rigger which I have past experience in.

           

          Why would you have this 'cut-away' present as it will only present itself as a weak point in the overall lifting structure?Nip.png

           

          Is the hole between the lifting fixture necessary as it appears that the corners are what may be showing the weakness?

          Corners.png

           

          But most importantly, what happens if you try your design with your lifting fixture running parallel to your lifting lugs?

          Brace.png

           

          Or, better still.....................

          Brace2.png

          Just as a side note, although it does happen, a certified lifting device will very rarely have any holes, cut-outs, perforations or such unless they are for a specific purpose.

           

          Just some ideas above for you to ponder.............

           

          Dave.

          • Re: Static simulation fails while real product succeeds
            Frederick Law

            Stress concentration.

            Safety factor.

            The area getting max stress are corners.  The sharp 90 deg on the lifting lug is welded to the bend part which will be a fillet.

            The fillet will never see stress that high.

            The sim never say part will fail.  It say max stress is higher then yield.

            Yield on material is minimum.  So material could have higher yield.

            Even if not, material will stretch and yield will go up.

            So the part will deform a little but won't break.

            If stress is higher than Ultimate, its another story.

            • Re: Static simulation fails while real product succeeds
              J. Mather

              JM Van Oossanen wrote:

               

              I know the basics.

               

              But when I try to simulate this in Sw, it shows that it should fail.

              Stress Strain.png

              Looking at a representative Stress-Strain curve note that linear static stress analysis is only within the yellow highlighted portion of the curve above - the linear elastic range.  Note the location of the Ultimate Strength and especially note the Fracture location on the curve.

               

              I assume your definition of "failure" is fracture of the part or perhaps permanent deformation in the non-linear plastic range of the curve (in which case run a non-linear analysis).

               

              I note that you did not indicate the calculated deformation in the high stress areas. (I can't open your files to examine as you are using a later release than I have.) In any case, keep in mind that your analysis is only within the linear elastic range.

               

              Consider further the image below.

              Hitch.PNG

              Imagine you were starting with a flat blank to press into this deformed shape.  This would be plastic deformation.  Permanent deformation.  Has the part failed in the process of forming from a flat blank into this permanently deformed shape?  (Or simply consider the force needed to make the bends (permanent deformations) in forming your bracket from sheet metal.)

               

              The term Safety Factor is an unfortunate misnomer.  It is simply a measure of Syield/Scalculated,

              the designer needs to define their measure of "failure".  Is it permanent deformation of a certain percentage?  Is it fracture?

              • Re: Static simulation fails while real product succeeds
                James Riddell

                1. You are not restraining nor loading the model in the same manner as it would be IRL.

                2. Define "it fails" - is your yield limit exactly the same as the actual material (including weld filler metal)?

                3. Your stress results DLR - I would expect a little better distribution of the hot-spot if the formed plate were fully connected to your clevis plates.

                  • Re: Static simulation fails while real product succeeds
                    B. Bijl

                    ''You are not restraining nor loading the model in the same manner as it would be IRL''.

                     

                    Well as close, those hoist lugs/ears are attached to a beam via a locking pin. Underneath it is a plate attached with bolts to the four holes. So that's exactly as I set it in Solidworks.

                     

                    It fails, since it may not deform plastically irl.

                      • Re: Static simulation fails while real product succeeds
                        James Riddell

                        B. Bijl wrote:

                         

                        ''You are not restraining nor loading the model in the same manner as it would be IRL''.

                         

                        Well as close, those hoist lugs/ears are attached to a beam via a locking pin. Underneath it is a plate attached with bolts to the four holes. So that's exactly as I set it in Solidworks.

                         

                        It fails, since it may not deform plastically irl.

                        B., No you are most assuredly not. You have the lift holes completely constrained. There is no pin or bolt that I know of that can 'lift' the bottom of a hole. A tell-tale for bad connection is the odd stress pattern at the ends of the lift lugs (clevis) that does not extend down the side at all. Your loading is not placed as a pin through those four bottom tab holes would be applied.

                         

                        Are you CERTAIN that you did not apply 5 tons to each of the tabs in the corners instead of total? That is the first place I'd look.

                         

                        I might have some time this weekend to look at your model if you haven't solved it by then. Feel free to PM me.

                    • Re: Static simulation fails while real product succeeds
                      B. Bijl

                      Thank all of you guys for the amazing feedback by the way!

                       

                      Really helpfull, and I'm glad to see such a active 'professional' forum nowadays

                      • Re: Static simulation fails while real product succeeds
                        Sergio Monti

                        B., please consider also:

                        - Fabricators usually use S275 sheets instead of S235, please check this

                        - Welded area .... this is a big deal! Unless you've done a normalizing or stress relief after welding, yield strength is much higher, despite ultimate strength is not - welded parts are usually more brittle

                        - Bent areas have been stretched beyond the yield point to achieve deformation. Therefore new yield point will be different from standard material

                        - Consider that a deformation of 0.1mm can increase the yield strength quite a lot, so may be you had deformation but you're not able to see it

                        • Re: Static simulation fails while real product succeeds
                          Bill McEachern

                          I did not read all the posts in any great detail and I am unsure if the issues is resolved or not. If an elastic plastic analysis is done where you load and unload the product it is often the case that the difference in shape is not noticeable as the load will redistribute till it is sustained and upon unloading the shape returns to the initial shape as far as the eye can see even though local yielding has occurred. No idea about this case but you can check this hypothesis by doing a NL elasto- plastic analysis - just assuming a low tangent modulus is likely good enough to confirm or refute.