41 Replies Latest reply on Aug 18, 2014 11:14 PM by Jared Conway

    simulation result not symmetric

    Magnum So

      Hi All,

       

      I have tried a static study in simulation to learn thermal expansion

      model dimension: 200mmx50mmx50mm with a T leg

      material: alloy steel

      fixtures: fixed geometry on the T leg bottom face

      external loads: temperature 50 Celsius (ref temp at zero strain=20 Celsius)

      mesh: standard mesh

      Picture2.jpg

      The max displacement is 5.676e-002mm.

      I expect that the four edges should have the same max. displacement but the probe shows that they have different value. So is there any tolerance in solidworks simulation?

        • Re: simulation result not symmetric
          Knut Fiskergard

          The difference is very very small. (0,5%?).

          I don't do much thermal work, but I think this is what you should consider to be equal.

          The result is affected by the mesh (is it absolutely symmetric?) and numerical round-up/-down during calculation and extrapolation of the shown result.

            • Re: simulation result not symmetric
              Magnum So

              I don't know how to make sure that the mesh is symmetric. I have tried different method to extrude the above model and found that the number of total nodes and total elements change every time. So I cannot avoid such non-symmetric result, right?

                • Re: simulation result not symmetric
                  Knut Fiskergard

                  I think you should not expect the results to be symmetric - as a hand calc would be.

                  I don't think Simulation has the tools, as for example Ansys has, to take control of the meshing.

                  FEA is a numerical approximation. Highly dependent on element size (density), quality, round-offs......

                  In structural analysis one would check for convergence of the result. How much does the result change if you make the mesh a bit finer in areas with stress concentrations? If the change is less than 3-5%, if that is an acceptabel criteria, the solution is said to have converged and the result is reliable. (you don't want to run with to many elements either)

                  I would say your results are symetric.

                   

                  BTW- meshing is not dependent on how you generated the geometry. It is an independent operation.

                    • Re: simulation result not symmetric
                      Nicholas Luyster

                      Hi Magnum,

                       

                      Knut is right.  The mesh will not be symmetrical.  SolidWorks Simulation has too much automation to make a symmetrical mesh.  In this case, a difference of .5% is effectively zero. FEA is not that accurate.  

                       

                      All the best,

                       

                      Nick

                      SolidWorks Simulation Training

                        • Re: simulation result not symmetric
                          Magnum So

                          Thanks!

                          I have tried to increase the model length from 200mm to 2000mm, found that the difference in four edges displacement has increase to be 1.5%

                          Does it mean that an increase in model scale cause an increase in 'tolerance' in FEA? 

                           

                          In professional field, how to simulate stress issue or thermal issue in large-scale model? Or Solidworks FEA result is just for a reference?

                            • Re: simulation result not symmetric
                              Jerry Steiger

                              Magnum,

                               

                              Most engineers would be very happy with results within 1.5%. Our assumptions about the model and the boundary conditions are usually not good enough to worry about differences that small.

                               

                              Jerry S.

                              • Re: simulation result not symmetric
                                Knut Fiskergard

                                In professional field FEA is the standard method because of the complexity of the tasks, and then add non-linearities (ex. material yielding). But in time you get experienced in different ways of analyzing the result, and always remember the assumptions you made! Change a boundary condition slightly and you could get quite a different result.

                                 

                                It looks like you have added your thermal load on an edge. If this was a structural load, the results would not be reliable close to the edge (st.venant principle). Don't know if it will have a similar effect on a thermal load??

                                 

                                This model does not seem to take long to solve. If you have used Simulation default element size - what happen if you manually set an
                                element size about half of what you have used?

                                • Re: simulation result not symmetric
                                  J. Mather

                                  Magnum So wrote:

                                  Or Solidworks FEA result is just for a reference?

                                  What does the F in FEA mean?

                                  What other reference do you have?  Actual physical testing/measurements against which you can compare your digital model analysis?

                                  In the physical models that you have tested - is there any measurable variations between tests?

                                    • Re: simulation result not symmetric
                                      Knut Fiskergard

                                      I sense a retorical question here:

                                      "What does the F in FEA mean"

                                      F stands for Finite - how does that answer Magnum's question?

                                        • Re: simulation result not symmetric
                                          J. Mather

                                          Yes, I was presenting a rhetorical thought question to the OP.  Trying to provoke a logical thought process about why the reported results aren't perfectly symmetrical.

                                          A Finite number of elements/nodes are defined.

                                           

                                          Imagine being a spider with a different type of "vision" than human.  This special spider can only "see" code.  It is tasked with building a web (mesh) within a given volume.  The hard part for the human, with only the usual human visual experience, is to imagine the difficulty of "seeing" this code and selecting a start point for creating their web and creating it in such a way ("seeing the code") that it will be perfectly symmetrical to the human view of the world.

                                           

                                          From the big picture view, does the difference in reported symmetry of results have any any real significance, or, compared to the overall results (and real-world variation) is the difference rather insignificant?

                                  • Re: simulation result not symmetric
                                    J. Mather

                                    Knut Fiskergard wrote:

                                     

                                    BTW- meshing is not dependent on how you generated the geometry. It is an independent operation.

                                    Meshing IS dependent on how you generated the geometry. (in SolidWorks)

                                     

                                    My students do an experiment to demonstrate this every semester.

                                      • Re: simulation result not symmetric
                                        Knut Fiskergard

                                        It does?? Really??? How and why?

                                        Could you please share the experiment that demonstrates this?

                                        This could explain a few of my issues with the Simulation mesher.

                                          • Re: simulation result not symmetric
                                            J. Mather

                                            Here is the lab experiment.

                                            You should agree that the solid geometry is identical, only difference is how it was created.

                                            Verify that you get different results and then I will come back with discussion on logic.

                                             

                                            Others are invited to run this experiment as well to document results.

                                              • Re: simulation result not symmetric
                                                Knut Fiskergard

                                                I agree that the final volume is identical.

                                                But I totally disagee with a CAD modelling approach that add geometry within exsiting geomery when you are working with native files. As an intermediate state, finishing up with some bolean feature or similar, to obtain desired geometry is of course ok.

                                                The lab task only have content on 1,5 of the 3 pages. Don't know if that is all or if something went wrong during upload.

                                                 

                                                I have tried the task, but I do not get different results.

                                                I made 1 sketch and made two extrudes, selecting countours in the sketch (another approach I don't like - find it to be unstable for more complex geomery after making changes to the sketch).

                                                The last feature is set to merge with the first...

                                                Am I missing something from the task?

                                                  • Re: simulation result not symmetric
                                                    J. Mather

                                                    Knut Fiskergard wrote:

                                                     

                                                    1. I agree that the final volume is identical.

                                                    2. But I totally disagree with a CAD modelling approach

                                                    3. I have tried the task, but I do not get different results.

                                                     

                                                    I did not include the entire document as we also run this test in three other programs, I snipped most of it out to avoid irrelevant discussion.  I thought I had included all the relevant (trivially simple) information needed to reproduce the behavior. The question was never about modeling approach - I simply reversed engineered a much more complex problem down to as simple an example as I could generate that would demonstrate that differences in modeling technique (I estimate that 90% of what I see I would call "garbage" from a modeling technique perspective and often from a geometry perspective) has an impact on results.  When I first started teaching FEA I was confounded why "identical" assignments students were getting different (we will discuss relative significance of differences later) results.  I began to analyze modeling technique as part of the process.  The fact that you report that did not get different results is interesting as we have run this test hundreds of times in SolidWorks and have never gotten identical results between the two models in the experiment as written.  I would be interested in seeing your two files.

                                                  • Re: simulation result not symmetric
                                                    Knut Fiskergard


                                                    I might have mix the name on the files, hope that doesn't affect my grade, sir

                                                      • Re: simulation result not symmetric
                                                        Jared Conway

                                                        i also wouldn't expect the way it was modeled to get different results. orientation might. because i don't know how it decides what order to start meshing faces. that could seed the mesh differently. but again, it would be minimal.

                                                        • Re: simulation result not symmetric
                                                          Mikael Martinsson

                                                          Well, I don't get this lab experiment either and perhaps we're missing some information?

                                                          In my trials, the result is the same between the two methods, based on my knowledge of FEA.

                                                           

                                                          But of course, if you don't have the knowledge of the method, and just look at the numbers, it is not exactly the same.

                                                           

                                                          Different thing can affect the results:

                                                          - Boundary conditions

                                                          - Mesh

                                                          - Solver

                                                           

                                                          Boundary conditions effect are obvious.

                                                           

                                                          Solver, well if you use the iterative compared to the direct sparse there will be differences since one is solving the equation directly and the other one makes a guess, verify the result and the guess again until it is "close enough".

                                                           

                                                          Mesh, obviously the size and type of element effects the result. But also how the mesh layouts on the part since SW don't have the possibility to do a mapped mesh.

                                                          In my trial I get the results below where you can see that the tets are turned in different direction on different locations.

                                                           

                                                          SW simulation solves the displacement and then extrapolates stress and strain from this value.

                                                          Displacement easier converges compared to stress and in my example the displacement is exactly the same between the two results.

                                                           

                                                          The maximums stress is different, but of course this has more to do with the fact that it occurs as a singularity in the sharp inner corner.

                                                          It will continue to rise to infinity with finer mesh so it is pointless to look at this result.

                                                           

                                                          SW also modifies the scale based on the maximum value, so to really compare them you need to set the scale similar in both examples.

                                                          So in the overall picture, with the same scale settings, I say that the result is the same between these two design methods.

                                                           

                                                          Example 1.JPGExample 2.JPG

                                                            • Re: simulation result not symmetric
                                                              J. Mather

                                                              When I get I chance I will go back and check my instructions.

                                                              I think I snipped out something I should have left in the instructions.

                                                               

                                                              In our original problem - the intention was to show that although exactly the same results were expected - the actual difference in results were not significantly different.

                                                              The point of the lab was not to expect 2+2=4 type of answers when doing FEA.  We are looking for "ball-park" results. Are we in the ball-park and where?

                                                                • Re: simulation result not symmetric
                                                                  Knut Fiskergard

                                                                  I think I'll have to respectfully object to the "ball-park" comment!

                                                                  FEA can give you very accurate results when done right.

                                                                  And you will get worthless results when it is done wrong.

                                                                   

                                                                  But you can also get "ball-park" results, if you wish so, by selecting boundary conditions and mesh settings that are less accurate.

                                                                  you now; shit in = shit out. SW Simulation (or any other FEA software) just does the math.

                                                                   

                                                                  And if you are doing linear analysis 2+2 should equal 4 (if you only change the value of the load (ref "change the load to 10000N for ....")). But probably not in and around points/edges with singularities, as the case will be in the corner of the lab part. But that may be one of the lab learning objectives.

                                                                    • Re: simulation result not symmetric
                                                                      J. Mather

                                                                      Keep in mind that this is Lab #1.  We haven't even begun to discuss mesh refinement or results convergence.

                                                                       

                                                                      The exercise opens the same kind of discussion that we are having here.

                                                                        • Re: simulation result not symmetric
                                                                          Knut Fiskergard

                                                                          First of an apology to Magnum So for hi-jacking this thread.

                                                                          J.Mather: guess I was expecting something "bigger". And you seem to be right in that different modelling creates different mesh.

                                                                          But the differenses are so minute they have no practical implications. I don't think I ever have reflected over why the mesh end up as it does in an automatic mesher. I'm looking at mesh density and element quality. And finaly result convergence.

                                                                           

                                                                          In Solidworks the multibody parts can trick you:

                                                                          If you model as the lab part with interfering bodies (don't merge the second feature)

                                                                          before you mesh, set global contact to bonded.

                                                                          Now mesh and run....

                                                                          Can someone explain this one?

                                                                           

                                                                           

                                                                          explanada por favor.jpg

                                                                            • Re: simulation result not symmetric
                                                                              Mikael Martinsson

                                                                              Hmm, must be a bug or something. Which version of SW?

                                                                              If I replicate example 2 in the exercise, but without merging solids, I get this result in SW2014 SP3:

                                                                              What does it look like if you only show the mesh?

                                                                               

                                                                              Or did you do it with example 1? That shouldn't be possible because of the interference and global contact conditions.

                                                                               

                                                                              Skärmklipp.JPG

                                                                              • Re: simulation result not symmetric
                                                                                J. Mather

                                                                                Knut Fiskergard wrote:

                                                                                 

                                                                                First of an apology to Magnum So for hi-jacking this thread.

                                                                                ....". And you seem to be right in that different modelling creates different mesh.

                                                                                But the differenses are so minute they have no practical implications. I don't think I ever have reflected over why the mesh end up as it does in an automatic mesher.

                                                                                I don't think it was really a hi-jack of the thread.  The OP was concerned that the 4 corners had different numbers in a symmetrical part.

                                                                                This led to discussion of - "Are the numbers really different (in any meaningful way)?"

                                                                                 

                                                                                Further discussion with simple illustration shows that different modeling techniques of identical end-result geometry can result in slightly different numbers, but again, is the difference significant?

                                                                                 

                                                                                I have run into a lot of people you have little or no confidence in software FEA because they see these differences by do not spend any time to logical reflect over why there are differences or if the differences are of any significance.

                                                                                 

                                                                                I have to get out the door right now - but I have a final observation to make on this topic.  Back in a while.

                                                                        • Re: simulation result not symmetric
                                                                          James Riddell

                                                                          If my eyesight is working properly you got two different numbers for maximum stress.  Correct?

                                                                            • Re: simulation result not symmetric
                                                                              Mikael Martinsson

                                                                              Yep, but unfortunately you also have to read the text situated above the pictures to understand the "conclusion".

                                                                                • Re: simulation result not symmetric
                                                                                  James Riddell

                                                                                  I read that but in my (limited) experience when I've re-run a model with no change whatsoever to the mesh/bc's, etc. I get the same numbers.

                                                                                    • Re: simulation result not symmetric
                                                                                      Mikael Martinsson

                                                                                      You're right, and that was just what i wrote in the text to the pictures. The mesh, generated by SW automesher, is not exactly the same.

                                                                                       

                                                                                      Therefore the result, maximum stress, is not exactly the same, but as an FEA engineer I would still judge the results from the two pictures above as the same results. FEA is not an exact method, but instead an approximate numerical method to solve large problems. Therefore it's important to have a good knowledge about the method and limitations before drawing any conclusions from the results. (The maximum stress listed in the pictures is also singularities / numerical faults, and should not be mistaken for real stress)

                                                                                       

                                                                                      If you duplicate one of the studies and runs it again, you will have two results that are the same, because the mesh will be duplicated also.

                                                                                        • Re: simulation result not symmetric
                                                                                          James Riddell

                                                                                          Ah, so the change in modeling technique changed the way the automesher meshed the part. 

                                                                                          • Re: simulation result not symmetric
                                                                                            J. Mather

                                                                                            "Well, I don't get this lab experiment either and perhaps we're missing some information?"

                                                                                             

                                                                                            From the discussion it sounds like to me that you do get the purpose of the lab.

                                                                                             

                                                                                            Mikael Martinsson wrote:

                                                                                             

                                                                                            You're right, and that was just what i wrote in the text to the pictures. The mesh, generated by SW automesher, is not exactly the same.

                                                                                             

                                                                                            Therefore the result, maximum stress, is not exactly the same, but as an FEA engineer I would still judge the results from the two pictures above as the same results. FEA is not an exact method, but instead an approximate numerical method to solve large problems. Therefore it's important to have a good knowledge about the method and limitations before drawing any conclusions from the results.

                                                                                             

                                                                                            The title of the lab is Why Different? Remember - this is Lab #1 in the course - discussion of what the numbers mean.

                                                                                              • Re: simulation result not symmetric
                                                                                                Mikael Martinsson

                                                                                                I totally agree with you.

                                                                                                As usual it's a case of "read but not understood" from my side. Your opening statment was "Meshing IS dependent on how you generated the geometry"

                                                                                                This is absolutely true, I agree, and it's verified in my example above and mentioned in the first text.

                                                                                                 

                                                                                                My misinterpretation, when i looked at your lab experiment, was that this affected the final results (stress/strain/displacement) in a way that matter for the conclusion.

                                                                                                But it don't, also verified in the example above.

                                                                      • Re: simulation result not symmetric
                                                                        Per Engberg

                                                                        When doing FEM in symmetrical cases it is often advantageous to simplify/reduce the calculation by just running it on one half of the model, using the fact that the symmetry plane will remain flat (frictionless support).

                                                                        • Re: simulation result not symmetric
                                                                          James Riddell

                                                                          I have to agree in part with the Professor, I just meshed the identical model (duplicated the tab w/in the program) and ended up with different mesh numbers.  Both used curve based mesh with 12 mm size.  The first one had 476310 nodes and 247959 elements and the second had 476318 nodes and 247960 elements.  There were no differences between the modeling of the "two" parts as it is the same model.  Meshing changes.

                                                                           

                                                                          Does this negate the validity of the FEA?  Certainly not.  Think of it (as I have heard of students doing) as getting an answer of x.xxx e-15 on one of those fancy TI calculators - that's still 'zero' in a hand calculation.