19 Replies Latest reply: Mar 10, 2014 6:11 PM by Jared Conway

    Loading vs Mesh

    Mousa D

      Hello,

       

      Making my own structure and running non-linear elastic static study. I have defined my own stress strain curve and ran my simulations. Adding pressing to certain rectangular area on my structure, I have made 3 tables, each have exactly the same forces/geometry/Material properties, and the only thing changing is the time steps.

      Now in each table I have 5 rows, with each row I have changed the mesh size from finest to coarsest. (Attached is a file where it will make all the above easier to understand and see).

       

      In the last column, I have calculated the Force/Load by hand, by multiplying the pressure with the area of the rectangle that I applied it to. I.e I have set the max. time to 5 seconds, expecting the model to fail before it reaches the max. (A column shows the max time step reached).

       

      My two critical questions are:

      1- From the maximum time step reached for each mesh, I am calculating that pressure on that certain time. Hence, with each single time-step, a fixed load is considered. Is that correct?

       

      2- Before obtaining my tables, I would have thought with very time the element size is smaller  (Finer) a max. step reached would be higher towards the 5 second time set. And should have a consistent Load, either increasing or decreasing. (Shown in the last column). Is it normal being random, or am I calculating it wrong, or something else I am doing, is wrong?

       

       

      Please, anyone who is sure or have a certain explaintion let me know, as I can not seem to understand the coming results.

       

      Many thanks in advance.

        • Re: Loading vs Mesh
          Shaun Densberger

          "1- From the maximum time step reached for each mesh, I am calculating that pressure on that certain time. Hence, with each single time-step, a fixed load is considered. Is that correct?"

           

          Yes, you load is increased with each pseudo time step. For example, if you had a 100 MPa load, your step size is 0.05 seconds, and your end time is 1 second, then your pressure is increasing by 5 MPa per time step. I'm not too familiar with how SW engine works, but I would imagine that if the solver is having issues reducing the residual norm to an acceptable level, then it would automatically reduce the load factor and trying iterating again.

           

          "Before obtaining my tables, I would have thought with very time the element size is smaller  (Finer) a max. step reached would be higher towards the 5 second time set."

           

          I don't understand what you're asking here. Is it that you assumed that as the mesh was refined (i.e. element size decreased), that the maximum time step reached would be closer to 5 seconds?

           

          "And should have a consistent Load, either increasing or decreasing. (Shown in the last column). Is it normal being random, or am I calculating it wrong, or something else I am doing, is wrong?"

           

          I'm a little confused about your maximum load column. You stated that you, "calculated the Force/Load by hand, by multiplying the pressure with the area of the rectangle that I applied it to." But you also stated that, "each have exactly the same forces/geometry/Material properties, and the only thing changing is the time steps." Can you provide a little more information about how you calculated the maximum load by hand (as opposed to having the solver calculate the reaction load for example).

           

          However, I did notice that your maximum load isn't a random variation; looking at your table you'll see that the higher the maximum time step, the higher the maximum load. Since the load is increased with each increase in the pseudo time steps, you're maximum load will be dependent on your maximum time step.

            • Re: Loading vs Mesh
              Mousa D

              "Before obtaining my tables, I would have thought with very time the element size is smaller  (Finer) a max. step reached would be higher towards the 5 second time set."

               

              I don't understand what you're asking here. Is it that you assumed that as the mesh was refined (i.e. element size decreased), that the maximum time step reached would be closer to 5 seconds?

               

              - Yes.

               

              Is the element size (Mesh) a factor to the maximum pressure reached before failure? As I have mentioned earlier, I have calculated the maximum pressure reached by hand. (i.e. multiplying the maximum time step reached by the pressure that I have set exerted on my structure, dividing that by the limit max time step, 5 seconds.)

               

               

              ''I'm a little confused about your maximum load column. You stated that you, "calculated the Force/Load by hand, by multiplying the pressure with the area of the rectangle that I applied it to." But you also stated that, "each have exactly the same forces/geometry/Material properties, and the only thing changing is the time steps." Can you provide a little more information about how you calculated the maximum load by hand (as opposed to having the solver calculate the reaction load for example).''

               

              - Sorry for not making it clear earlier. I am exerting a 4.5 N/mm2 pressure against my wall structure. Setting my own bi-linear stress-strain curve, with a max. tensile strength of 3.15 N/mm2 (i.e. before it becomes a linear straight horizontal line.)

              I am having one study, with geometry, material, and the force of 4.5N/mm2 exerted at the beginning are all constant. I have ran the study 5 times, with each time all I have changed is the size of my mesh. In the previous file I uploaded, all the varying outcomes can be found.

               

              ''Can you provide a little more information about how you calculated the maximum load by hand (as opposed to having the solver calculate the reaction load for example).

               

              However, I did notice that your maximum load isn't a random variation; looking at your table you'll see that the higher the maximum time step, the higher the maximum load. Since the load is increased with each increase in the pseudo time steps, you're maximum load will be dependent on your maximum time step. ''

               

              As I explained earlier, I have calculated the maximum load by hand from the maximum time steps reached.

              To be more clear, my maximum load reached before failure is linked to my maximum time step reached before failure. Is the element size (Mesh) a factor of the maximum time step reached, if so, what is the relationship and why is it not constant as you can see from the table, I would have thought the finer the mesh (Smaller in size) the higher the maximum time step reached before failure. My table tells me I am wrong.

               

              Moreover, Is there a way I can get SW to calculate my maximum pressure reached?

                • Re: Loading vs Mesh
                  Jared Conway

                  It seems that the the problem you are running into is that solidworks cannot complete your simulation. We call this a convergence problem. What error do you get when it happens? Does it give any suggestions? Did you try them?

                   

                  I'd suggest posting your model and reading up on suggestions in other posts, the kb and speaking with your reseller about convergence problems. Sometimes the solver just isn't equipped. But before you call it quits, make sure to get confirmation that it is a limitation and that it isn't a mistake or lack of knowledge.

                   

                  Overall, completion of the solution and mesh size are not related. But sometimes they are. A very fine mesh can be more difficult to converge a solution thank very coarse one . But the opposite can also be true.

                   

                  Here is another suggestion. Try it with a draft quality mesh.

                    • Re: Loading vs Mesh
                      Jared Conway

                      also, just to reiterate a previous suggestion, when you're troubleshooting convergence, it is troubleshooting. eliminating variables until you determine the one that is causing your issue with convergence. this means things like reducing the total force to see if you've just hit a maximum..etc.

                      • Re: Loading vs Mesh
                        Mousa D

                        Hello Jared.

                         

                        You have probably misunderstood my problem as I do know and expect my structure to fail. I am not looking for a solution for my problem as I exerted a certain pressure so that the structure fails.

                         

                        My only concern was why am I not getting a consistent values for my pressure, either increasing or decreasing or such. (i.e to my maximum time step reached)

                          • Re: Loading vs Mesh
                            Jared Conway

                            i'm talking about solution failure

                            not structural failure, the software does not know anything about your structure failing, it simply runs the analysis based on your input. it will NOT stop when the structure fails. the only time the solver stops is when numerically it cannot complete the solution. theoretically if numerically the solver can solve the problem, you could subject your structure to 10x what actually causes it to fail.

                             

                            "My only concern was why am I not getting a consistent values for my pressure, either increasing or decreasing or such. (i.e to my maximum time step reached)"

                             

                            i don't think i understand.

                              • Re: Loading vs Mesh
                                Mousa D

                                Well, when I said structural failure it would sure mean solution failure, as when the maximum pressure exceeded the tensile strength (From the stress-strain curve) it will not be able to solve it theoratically. Am I wrong?

                                  • Re: Loading vs Mesh
                                    Jared Conway

                                    this is incorrect

                                    even if your stress strain curve is short, the software will extrapolate it.

                                     

                                    just to reiterate, the software doesn't know anything about what the results mean, all it knows is how to do the calculation

                                      • Re: Loading vs Mesh
                                        Mousa D

                                        So by calculating the maximum pressure taken by my structure from the maximum time step reached, is wrong?

                                         

                                        Having a bi-linear stress-strain curve, and setting the method to be by 'Force' I would have thought it will keep incrementing until it reaches the very end of my curve (Tensile strength, where 2nd, horizontol linear line starts).

                                          • Re: Loading vs Mesh
                                            Jared Conway

                                            So by calculating the maximum pressure taken by my structure from the maximum time step reached, is wrong?

                                             

                                            >no, this method is fine, this is as far as the solution was able to go.

                                             

                                            Having a bi-linear stress-strain curve, and setting the method to be by 'Force' I would have thought it will keep incrementing until it reaches the very end of my curve (Tensile strength, where 2nd, horizontol linear line starts).

                                             

                                            >nope, it just uses the stress strain curve to determine the material properties at a particular strain level

                                             

                                            this is actually well documented in the help, the tutorials and the training. i'd highly recommend going through these to get a better understanding of how the software is solving your problem.

                                              • Re: Loading vs Mesh
                                                Mousa D

                                                Hello Jared,

                                                 

                                                Would you mind guide through which help link I can read through to understand how the forces and increments are based on if not the stress-strain curve?

                                                 

                                                 

                                                Now, I do understand that the finer I make the mesh, does NOT mean the higher the maximum time step reached is toward my 5 second max. limit. Hence, the finer the mesh does not mean higher the pressure/load that can be taken by my structure, yet the finer the mesh is the more accurate maximum load taken before failure is.

                                                Attached is a graph of my Pressure vs Mesh size that shows the results I obtained. I could not understand the relationship from my curve. Please, comment and give me feedbacks on what you would understand by looking at the curve. Does it make sense? Why is it not consistent? The finer the mesh, is almost as equal to the coarsest the mesh, why? Any explaintions are appreciated.

                                                 

                                                Many thanks in advance.

                              • Re: Loading vs Mesh
                                Jared Conway

                                cross post: https://forum.solidworks.com/message/413722#413722

                                 

                                "1- From the maximum time step reached for each mesh, I am calculating that pressure on that certain time. Hence, with each single time-step, a fixed load is considered. Is that correct?"

                                 

                                in a linear static, the load is applied all in one shot

                                in nonlinear static, the load is applied incrementally. so if you have an analysis that takes 1s and your load is 10N, it starts at 0s, 0N and ends at 1s, 10N. the default application is linear but the customer can override with their own curve. with a linear curve, you can find the incremental load using the linear relationship equation.

                                 

                                "2- Before obtaining my tables, I would have thought with very time the element size is smaller  (Finer) a max. step reached would be higher towards the 5 second time set. And should have a consistent Load, either increasing or decreasing. (Shown in the last column). Is it normal being random, or am I calculating it wrong, or something else I am doing, is wrong?"

                                 

                                i'm not sure what the question is here.

                                 

                                what is the problem you're trying to solve?

                                 

                                i think one of your challenges is that you're trying to understand how the software works and troubleshoot a problem on the same model. i would recommend you go back to a simple model and understand the concepts used for nonlinear. once you have a good handle on this, you can move to your problem. If your problem cannot solve completely, I would recommend either troubleshooting the problem or accepting the solution that was completed rather than trying to do both. I think you're trying to make a correlation between mesh size and time step size which does not exist and may be tripping you up. If you want to take this path, separate the 2 concepts and understand them one at a time vs simultaneously.

                                • Re: Loading vs Mesh
                                  Jerry Steiger

                                  Mousa,

                                   

                                  As Shaun pointed out, your load is increasing linearly with the time step reached, as expected.

                                   

                                  Your load will not necessarily increase as the mesh decreases. The finer mesh may be giving you a more accurate stress level that better predicts the maximum load that the structure can bear.

                                   

                                  Jerry S.

                                    • Re: Loading vs Mesh
                                      Mousa D

                                      Hello Jerry,

                                       

                                      Thank you for your reply. 

                                       

                                      I am currently calculating my maximum pressure/load reached by hand. That is multiplying the maximum time step reached before failure (Setting 5 seconds that maximum limit) by the pressure I have set to exert on the wall, then dividing that by the limit 5 seconds.  Now that will give me the maximum pressure reached at that certain maximum time-step reached before failure.

                                       

                                      Now as you have said that my load will not necessarily increase as my mesh decrease. Does that mean that the maximum time step reached also does not depend on the element size of my mesh?

                                       

                                       

                                      M.Dahabreh.

                                        • Re: Loading vs Mesh
                                          Jerry Steiger

                                          Mousa,

                                           

                                          Right, there is no direct correlation between the mesh size and the output, as you can see in your Excel spreadsheet. The devil is in understanding what it means as the stress changes with mesh size. A person who only ran the three largest meshes and did not understand the model well might think that the model was converging nicely. (Although he should be nervous, since he only reduced his mesh size by about 25%, not enough to really get a good feeling for the convergence.)

                                           

                                          From the plot of pressure versus mesh size, it doesn't look like you are converging yet. I would suggest halving the mesh size at least a couple of more times.

                                           

                                          Jerry S.

                                            • Re: Loading vs Mesh
                                              Mousa D

                                              Hello Jerry,

                                               

                                              As you have mentioned, I've already tried to halve my mesh yet I could not due to not enough memory on the PC, so I have created multiple geometries size from 80/40/20/10/5 mm per length, instead of just refining my mesh. For each structure I have defined the mesh equal to that length as just to save time and memory.

                                               

                                              Attached is the graph I obtained.

                                               

                                              Being able to obtain values for all my geometries, except the 40 mm structure. Tried increasing the time-steps and such, but my structure did not fail at all. Found it bit weird, as the rest worked fine. As to be more confused, I have tried refining the mesh size to be 41 mm instead of 40, and the structure failed ..

                                               

                                              Note that I have made sure and checked that all parameters for all geometries are exactly the same. (Written with my graph)

                                               

                                               

                                              Moreover, I tried to make a geometry of 2.5 mm length as well, but the value I recevied did not make sense, so I have changed the Initial time step to 0.005 for the Automatic time stepping instead of 0.05.

                                               

                                              Please have a look at the file/graph attached for a clearer explanation.

                                               

                                              Regards,

                                              Mousa

                                                • Re: Loading vs Mesh
                                                  Jerry Steiger

                                                  Mousa,

                                                   

                                                  I don't understand what you have done with your geometry. Perhaps some pictures would help.

                                                   

                                                  Looking at your spreadsheet, I noticed something else which I had overlooked in your earlier spreadsheet. It says "Large displacement and strain, not checked". Since you are pushing your material close to or past its yield stress, you will have to allow large displacement and strain, otherwise your results are meaningless.

                                                   

                                                  Jerry S.

                                                  • Re: Loading vs Mesh
                                                    Jared Conway

                                                    have you been able to get the problem to solve to the maximum time step?