39 Replies Latest reply on Apr 17, 2012 6:53 AM by Peter Darby

    Factor of safety result causing concern.

    Yash Bhaskar

      Hi,

       

      I have been trying to simulate a physical tested clamp working safely under the load of 40KN with SWX simulation by the results value of this test is just freaking me.

      I don't know what to do with it, where I am going wrong. I have simplified the model for simulation but still unable to get the safe results.

       

      Looking forward for some desperate help. I have attached the model for further reference.

       

       

      Thanks in advance,

      Yash

        • Re: Factor of safety result causing concern.
          Jerry Steiger

          Yash,

           

          I don't have access to SW Simulation right now (and don't really have time to spend on it if I did have access), so I can't be much help. Plus I am not at all familiar with how it works, most of my FEA being done with ANSYS. I might be able to help a bit if you could show some of the results that you are worryied about and give some more explanation of your model, boundary conditions, and what you are expecting.

           

          It looks like your file was first compressed with rar and then zipped. A lot of people don't have the rar software, so it would be much better if you just zipped the files or let the forum software zip them for you.

           

          Jerry Steiger

          • Re: Factor of safety result causing concern.
            Angelo De Dominicis

            I've checked your model and the main issue there is the presence of geometric singularities due to sharp inner corners. Regardless of material properties or fabrication processes, sharp inner corners are not common or impossible in real parts, there will be always radii as small as they would be. Thus, results near sharp corners are not correct.

             

             

             

            Sharp edges in finite element analysis evaluate as infinite stresses due to a strain direction discontinuity just in the corners.

             


            In order to overcome this problem, estimate a real fillet radius (no matter how small) and apply proper mesh controls in the edges and face of such radius. Use curvature mesh control to mesh more than six elements at fillets. Check Peterson's Stress Concentration Factors, pretty good literature regarding these subjects.

             

            Regards

            • Re: Factor of safety result causing concern.
              Paul Becker

              Yash.  Although Angelo makes a good point about stress concentrations, I have run your model to convergence and the regions that are predicted to exceed yield go well beyond this corner. 

               

              FOS.jpg

               

              So the only suggestions I have are to double check your load magnitude, material properties, and the manner in which you are loading the part.

              • Re: Factor of safety result causing concern.
                Satit Nilyai

                Hi Yash, What are there at hole connect? Example pin, shaft,..Holes.jpg

                • Re: Factor of safety result causing concern.
                  Paul Becker

                  Several good points have been made here.  The area where over which the force was applied does appear to be inaccurate, given that the load comes from a cable running along the lower cupped portion of the part.  The load applied to the vertical face would result in more bending than the part would actually see.  Have you re-run with split lines to isolate the load to the actual area of contact?  Also, I'm assuming this was run as a linear static study.  That is fine, but be aware that any information on stress magnitude above yield is meaningless.  Also, the region of material that is predicted to exceed yield is likely exaggerated because due to the same reason... stresses are calculated from displacements and are extrapolated linearly from E, although in reality, the stress-strain curve does not follow a linear path post-yield.  This results in an artificially still part.

                   

                  Two questions going forward would be:  1) Is yielding still predicted with the updated, correct loading and 2) If so, what is the actual response post-yield.  If you need to know #2, then you will have to run this as a nonlinear static study using accurate data for the nonlinear stress-strain curve and material model.  If you are also talking about the effect of repeated loading, then you will need to take into account hardening, which can be specified in the nonlinear study properties.  This is likely what cause the part failure in the physical test Mikael described above, similar to bending a paperclip back and forth until it breaks. 

                  • Re: Factor of safety result causing concern.
                    Paul Becker

                    I ran it again with the load face limited to what I would roughly expect to be the cable contact area.  The restult actually looks worse than before.  Approximately 72% of the part is predicted to exceed yield.  Again, post-yield data must be taken as approximate, but I would say that it is not possible to reorient the force and have the results come out below yield.  Something else is up here.  Can you confirm the load and material properties?  Do you really have ~9000lbs on a 5" x 3/8" thick aluminum bracket? 

                     

                    Plot below shows volume of material above yield limit (~72%)

                     

                     

                    stress.jpg

                      • Re: Factor of safety result causing concern.
                        Bill McEachern

                        I didn't bother reading the whole thread but when things go post yeild the elements essentially turn to mush (dramatic reduction in stiffness -well for alot of materials. ?Some amterials like the 300 stainlesses it is much less dramatic. Just take a look at a stress strain curve to see how it behaves - mil hbk-5 might be useful). Thus stress risers can bleed out, load can align with the restraints reducing bending moments or allowing another laod path to take up a fraction of the load proportional to the stiffnesses. if you want to check the viabilioty of this design take the minimum section and just do P/A. If it exceeds the ultimate strength then the problem formulation is wrong if experimental evidence exists that says the device can withstand the load. Material properties maybe in error for example. Maybe the item is forged and has been mechnically work hardened during manufacture, etc.

                        Either way a non-linear analysis is required. You can't figure it out with a linear analysis as no load redsitribution can occur whether it be material, geometric or contact induced.

                          • Re: Factor of safety result causing concern.
                            Yash Bhaskar

                            Hi Bill,

                             

                            If I am not wrong,  what you are really trying to say is that, this is something which is beyond the scope of static analysis and I need to go for non-linear analysis for this one.

                             

                            Thanks & regards,

                            Yash

                              • Re: Factor of safety result causing concern.
                                Bill McEachern

                                In order to find out whether doing an NL analysis is even worth while I would take the area where indicated in the pciture and do P/A to get a stress, where P is the applied load. If this stress is above the ultimate of the materail there is no way this part will survive. This analysis assumes that the thing bends enough to remove all bending moments and the load is directly lined up with the restraints, which may be a  non-conservative assumption  - so if this doesn't work then I would go looking at the problem formaulation. Something isn't right. I would lokk at the actual test set up, how it is held inthe test righ, how is it loaded and with what, what is measured and how they are otherwise qualified. If youw ant to predict a test result modl lthe actual test with fideltity.

                                cable fitting area pic.png

                            • Re: Factor of safety result causing concern.
                              Yash Bhaskar

                              Hi Paul,

                               

                              I also ran it the way you did, in some of early efforts and as the result was more worse so I didn't considered it. I have also googled a lot to confirm that the material properties and the load conditions are correct or not. What I found that these strain clamps are actually designed for various standards starting from 20KN and goes upto 50KN.

                              I have also attached the snapshot for the material propeties of LM6 which I got,

                              LM6.jpg

                              You have also made a point about the Non-linear analysis, can I just know what make you to consider this as a non-linear analysis?

                               

                              Thanks & Regards,

                              Yash

                                • Re: Factor of safety result causing concern.
                                  Paul Becker

                                  Hello Yash.  I mentioned nonlinear analysis due to the material yield.  Otherwise, it is a straight forward linear static problem.  If yielding is occurring in the model, then any post-yield data is basically meaningless (see Bill's reply above.)  If you want to find out what happens post yield and get a more accurate picture of the stress distribution post yield, then you would need to run it as a nonlinear study with a plasticity material model and NL stress strain data.

                                  • Re: Factor of safety result causing concern.
                                    Mikael Martinsson

                                    Hello again.

                                    Where do you find the information about these clamps? Would be interesting to read more about them.

                                     

                                    I did a new study with a split surface to better simulate the actual load from the cabel. The result was similar to what you experienced, worse than before. A nonlinear study is mainly interesting if the part is designed to yield under maximum load. For a part like this it sounds strange.

                                     

                                    A P/A calculation in the narrowest section, according to Bill's proposal, gives approx 40 000 / 583 mm² = 69 MPa which is far below UTS, TS and FS for the material. Looking at the simulation, this section isn't the "worst" one, but a lot of the material has stress levels above yield. In a section more close to the force, simulation predicts that almost all the section yields at 40 kN. (see pictures below.)

                                     

                                    Stress1.JPGStress2.JPG

                                      • Re: Factor of safety result causing concern.
                                        Bill McEachern

                                        What consitutes failure? Bent or broken? If bent still works then  NL study will allow the load to redistribute the bending and hte thing should survive. If bent part is NFG under the applied loads.

                                          • Re: Factor of safety result causing concern.
                                            Mikael Martinsson

                                            Agree.

                                            And reading more carefully I find that Yash actually answered this in an earlier reply. Quoting "The only input I have is the model is working safely up to 40KN, the cracks develops after the load value increases beyond 40KN.". Not sure if it's a crack due to overloading or a crack due to fatigue, but still the result from a NL study would be very interesting. Unfortunately we don't have the "premium" package.

                                          • Re: Factor of safety result causing concern.
                                            Yash Bhaskar

                                            Hello Mikael,

                                             

                                            Results posted by you are very interesting, what different method you followed in this??

                                            When I tried he model with NL analysis my results are still very higher than the yeild stress as you can see in the below pics

                                             

                                            fos 1.jpg

                                              • Re: Factor of safety result causing concern.
                                                Mikael Martinsson

                                                Yash.

                                                Not sure what you mean by "different method". I made a split line on the surface where the force is applied to better simulate the actual contact surface from the cable. The result scale is also modified so the yield limit starts in the yellow color span. Then I made section views to see how much of the section area estimated to be above yield limit.

                                                 

                                                Interesting to see the NL simulation. UTS for the material is 290 MPa, and there are only smaller areas with stress peaks above this limit. But now you also have a bigger cut-out in the middle of the bracket so it is a bit different than linear simulations done before.

                                                 

                                                You mention that the result still are higher than yield strengt of material, and that is what we have seen from the beginning. NL simulation show what happens after yielding up to the materials UTS. The part will suffer a permanent deformation under 40kN load.

                                                  • Re: Factor of safety result causing concern.
                                                    Yash Bhaskar

                                                    Mikael,

                                                     

                                                    I also made a split line for better surface contact of cable as suggested by Jeremy Feist above in his post, but the my results where not similar to yours, thats why I asked what different method you did i.e. apart from split lines.

                                                     

                                                    The big cut out was always there in the part as "Cut-Extrude38" feature, but it was actually suppresed in my upload as in some of my early efforts I used simplify the model for simulation option and the cutout got suppresed in that process.

                                                     

                                                    If possible can you just send me the report of your effort for the above result.

                                                     


                                                    • Re: Factor of safety result causing concern.
                                                      Paul Becker

                                                      Notice that the load Yash has applied above is normal to the selected surface, rather than oriented downward.  This may results in a somewhat smaller net downward force, although it may not be significant.  Yash, in your NL analysis, did you use a linear elasitc material model?  Other than the cutout in your part, did you increase the thickness or may any other changes to the geometry?  Regardless, it sill appears that your part is exceeding yield over a large percentage of it's volume.

                                                        • Re: Factor of safety result causing concern.
                                                          Yash Bhaskar

                                                          Hi Paul,

                                                           

                                                          I tried the "Selected Direction" option with the load pointing downwards before applying it normal to the face but the result was worse. Thats why I posted the "normal to face" result.

                                                           

                                                          Yes, I used linear elastic material model, do I need to change it?

                                                            • Re: Factor of safety result causing concern.
                                                              Paul Becker

                                                              The NL analysis using a linear elastic material model is equivalent to running it as a linear static, large displacement problem.  You may get more accurate results in some respect, but you are faced with the same issue of post-yield data being meaningless and potential exaggeration of stresses due to extrapolation of the linear stress-strain curve.  If you want to study post-yield behavior, then you will need to run using a plasticity model and input a nonlinear stress strain curve.  I looked around for some NL date for LM6, but didn't see anything.  Just for a "what if" test, you could try using a tangent mod of 0.8E and see how it affects the results.

                                                • Re: Factor of safety result causing concern.
                                                  Yash Bhaskar

                                                  Hi All,

                                                   

                                                  Wasn't able to get to the forum for a long time , as I was busy with the year  end closure and some continuous business tavelling. But thankfully got an oppurtunity to see the physical testing for the above product with lower dimension tested for the load of 25KN only.

                                                   

                                                  I am attaching the pics and videos of the process, lets see what help these can be for us.....IMG0083B.jpg

                                                   

                                                  Cheers,

                                                  Yash

                                                  • Re: Factor of safety result causing concern.
                                                    Peter Darby

                                                    Out of curiosity I did a quick search for the alloy and believe LM6 is a cast alloy spec for aluminium?

                                                    http://www.hadleighcastings.com/uploads/LM6%20Alloy%20Detail.pdf

                                                     

                                                    If it is cast then the material properties are most likely influenced by the cast integrity of the final part and local imperfections - there is likely to be variabllity in the nominal properties from variances in the alloying and cast process.

                                                     

                                                    If you are working with high stresses and safety/risk is of high concern then the properties should be determined from samples taken from a cast part - a standard for mechanical properties for this alloy would nominate the properties and tests required. The foundry undertaking the casting should have good process control, records and traceability.

                                                     

                                                    The elongation at break from the properties you've shown is 3.5%; this would seem to indicate a brittle material with potentially little ability to deform to redistribute concentrated stress areas before a brittle type failure. Impact loading would also be an issue. What safety factor are you assigning to the minimum material yield properties to arrive at a maximum allowable design stress. There should be some sort of standard for this product what do these indicate as appropriate?