21 Replies Latest reply on Feb 20, 2014 2:34 PM by Shaun Densberger

    thermal stress simulation

    Magnum So

      hi, I have an assignment to simulate the thermal stress on a pipe by thermal expansion, the result is made as the attached picture, but I am doubted as the highest stress is over yield stress too much, I am afraid if I have made some mistake so I post it to make a discussion:

      p1.jpg

      pipe size: outer=90mm, insde=80mm, length=500mm

      material: AISI 304

      study: static

      fixed: two surfaces including the bottom and the stand are fixed by "Fixed Gemotry"

      external loads: whole solid temperature=50 Celsius, reference temp at zero strain=20 Celsius

      mesh: default mesh density

      result: max.stress=359.0MPa, max displacement=2.397e-001mm

       

      So, based on this result, the pipe should be first deformed on the stand, but in real life it seems that most steel pipe could be heated to a higher temperature without deformation, so I am not sure if all my simulation steps are right. Please help to correct it if possible, thank you.

        • Re: thermal stress simulation
          Peter MacDonald

          It seems to be the fixed geometry causing the stress.

          Depending on how the pipe is fixed in real life, you might be better off using a "roller slider" fixture?

          Maybe the soft springs feature could be used instead, but I'm not totally sure of the implications.

            • Re: thermal stress simulation
              Magnum So

              Thanks for your reply.

              The pipe is fixed on the floor and the stand is fixed on a concrete wall, so I use "Fixed Gemotry" to restrain the movement of the bottom surface of pipe and also the bottom surface of stand.

                • Re: thermal stress simulation
                  Peter MacDonald

                  I see, that does seem to justify the use of fixed geometry.

                  Unfortunately making something totally rigid in simulation will usually result in such high stresses.

                   

                  As a last resort you could maybe model the wall and floor (as small blocks) and bond them to the pipe. That might help.

                  Hopefully someone else has a better solution.

                  • Re: thermal stress simulation
                    Shaun Densberger

                    What do you mesh look like? As Peter pointed out, making something totally rigid (i.e. infinite stiffness) usually results in high stresses (which are usually unrealistic); this is because you have an infinite discontinuity in the local stiffness of the system. At the locations were you have the fixed restraint, you system goes from having a non-infinite stiffness (the Young's Modulus) to having an infinite stiffness (the fixed constraint). This causes a singularity, which amplifies stresses.

                     

                    There are two ways to handle this. Peter pointed out, you could model whatever the pipe is attached to (the concrete and such), but this should also result in singularities (this is known as a punch interface) since you still have an infinite discontinuity in the local stiffness. A better way would be to either use an "elastic support" or use mesh refinement and Saint-Venant's Principle. Using an elastic support will require to to calculate and equivalent stiffness for whatever material your pipe is connect to, which can be a little tricky to do. Using mesh refinement and Saint-Venant's Principle is fairly straight forward (and is the typical approach), but you'll have to live with having very high (but unrealistic) stresses in your fringe plots.

                      • Re: thermal stress simulation
                        Magnum So

                        Thanks!

                        The attached pic shows my mesh. I just use the default mesh density.

                        p3.jpg

                        I have tried the method Peter mentioned before, the stress is still very high on the stand.

                        So, do you mean that my result is not reasonable due to wrong setting in fixture?

                        For your "mesh refinement and Saint-Venant's principle", does it mean I should set the mesh parameter again based on Saint-Venant's principle? And what is the detail?

                          • Re: thermal stress simulation
                            Jared Conway

                            Take a step back. What do you want to analyze? The pipe it the stand?

                             

                            If the pipe, look at the stress in the pipe and recognize at the fixture there may be a singularity.

                             

                            If you care about the stand, add he next part in the assy and move the restraint away from your area of interest.

                             

                            Then worry about displacements and then stress.

                             

                            http://www.hawkridgesys.com/blog/solidworks-simulation-achieving-convergence-of-results/

                              • Re: thermal stress simulation
                                Magnum So

                                Thanks!

                                My purpose is to estimate whether the pipe and the stand will be deformed or cracked in the influence of thermal expansion.

                                 

                                I expect: based on real life experience, the whole set will not deform by a increase of 30 Celsius, so the max. stress value will not exceed the yield stress.

                                 

                                final result: a very high stress value exists on the stand, the stand should be deformed

                                 

                                So, I would like to verify my simulation. I have read the detail of convergence, it sounds complicated, but I am trying to run my model with the h-adaptive method right now.

                                  • Re: thermal stress simulation
                                    Jared Conway

                                    Sounds like your model is correct then. You have 0.2mm of max displacement.

                                      • Re: thermal stress simulation
                                        Magnum So

                                        So my result is reasonable?

                                         

                                        I have tried the h-adaptive method with following setting:

                                        mesh density: default

                                        target accuracy 99% (I have tried 98% but showed "Analysis is satisfied..")

                                        accuracy bias: default

                                        mesh coarsening: none

                                        result:

                                        p4.jpg

                                        Unfortunately, it is not a convergency result. Does it mean that my simulation is wrong?

                                        I have tried to adjust accuracy bias and mesh coarsening but come out similar result. It is not easy to be professional in Solidworks indeed!

                                  • Re: thermal stress simulation
                                    Shaun Densberger

                                    "So, do you mean that my result is not reasonable due to wrong setting in fixture?"

                                     

                                    Essentially. Your finite element model assumption is that the two surfaces were you've placed the constraints are perfectly rigid and cannot move. We know that this isn't the case in the real system. You could model the concrete itself, but I'd suspect that this would just open up a whole other set of issues.

                                     

                                    "For your "mesh refinement and Saint-Venant's principle", does it mean I should set the mesh parameter again based on Saint-Venant's principle?"

                                     

                                    Saint-Venant's Principle can be discribed a couple different ways, but the one most applicable to FEA is illustrated below. Imagine you have a solid metal cylinder and applied a point load (or a load over a very small surface area) and looked at the stress gradient at three different locations. As you move away from the load application area, the stress gradient becomes more and more uniform. If you were to look at the stress gradient at the load application point, you'd see a stress singularity (something like the Dirac delta function).

                                     

                                    saint varients principle.PNG

                                     

                                    In the finite element method, certain model conditions (loads, boundary conditions, geometry, material interfaces) can cause singularities. Sometimes you can develop a modeling method to work around the singularities (e.g. adding a fillet into a reentrant corner), but sometimes you can't. If you can't (and you need good results in the area), then you refine the mesh so that you have a set of small elements "touching" the singular area, and then another layer or two of small elements isolating other elements from the singular elements.

                                     

                                    The easiest way to illustrate this method is with a simple cantilever beam, where one end has a "fixed" constraint, and the other end has a vertical load that'll produce both bending and shear stress. If you run an analysis with a course mesh and look the the stress results, you'll see you maximum stress occurring at the constraint end where the maximum bending stress is. Now apply a mesh control on the outside edges of the surface that has the fixed constraint on it, and set the refinement bar to the mid-point and re-run the analysis. You'll see that the peak stress increases in value, but that the highest stresses are confined to a smaller area. Now, edit the mesh control to the finest setting and re-run the analysis again. You'll see the same trend; the peak stress is even higher, but once again the highest stresses are confined to an even smaller area. In theory, if you were to continue this process ad infinitum, you'd see your max stress go to infinity, while the singularity area go to zero.

                                     

                                    Mesh Refinement.PNG

                                      • Re: thermal stress simulation
                                        Magnum So

                                        Thanks. It is very informative.

                                        This theory seems relative to the convergence issue mentioned by Jared. If the stress tends to be constant in the increase of mesh density, the result is reasonable.

                                        I have tried to simulate the cantiliever beam with h-adaptive method(99% target accuracy, 4 loop) but failed to get a convergence result. So, It comes out a question, how to get a convergence result for the example of the cantiliever beam? If I cannot obtain a convergence result, the simulation seems to be meaningless, right?

                                          • Re: thermal stress simulation
                                            Jared Conway

                                            Converge on displacement.

                                             

                                            Don't only rely on h adaptive, use manual mesh controls.

                                              • Re: thermal stress simulation
                                                Magnum So

                                                I have tried to simulate a model with mesh control on a sharp edge. The following is the result by Trend Tracker:

                                                Stress1-1.jpg

                                                Displacement1-2.jpg

                                                In the first four iterations, when I manually incrase the element size in the range of Coarse to Fine(5.8mm to 1.4mm),  it really shows a convergence trend.

                                                But when I input 1mm(over the value of Fine), the result stress and displacement increase and tend to infinity. Is there any rule to set the element size? I haven't found such rules in Solidworks help. 

                                              • Re: thermal stress simulation
                                                Shaun Densberger

                                                "So, It comes out a question, how to get a convergence result for the example of the cantiliever beam? "

                                                 

                                                I'm not sure you can do this (Jared, correct me if I'm wrong), but if you could create a sensor at a location away from the singular elements and have your convergence based on that, then you should see your model "converge". If you can't do this, then you'll need to manually check convergence by using the Trend Tracker feature.

                                                 

                                                "If I cannot obtain a convergence result, the simulation seems to be meaningless, right?"

                                                 

                                                Yes and no. Your current convergence scheme is based off of tracking the maximum model stress value as the mesh is modified (i.e. as you increase the total number of degrees of freedom in the model), but you have singular elements in your model so your simulation will never "converge". I use quotation marks around converge because while the maximum stress of the model will not converge, the stresses at other points on the model could (such as points that are a couple elements away from the singularities).

                                                 

                                                To illustrate this, let's take the cantilever beam model that we've been using, but make some modifications to it. Specifically, we're going to add three sensors set to measure the maximum von-Mises stress at three different points. We'll then use the Trend Tracker feature to plot the value of each sensor as we modify the mesh like we did previously. After running a couple iterations (where the mesh is refined with each iteration, much like the h-adaptive method in SW), we can look at how each stress sensor value changed as the mesh was refined. Looking at sensor Stress1, we see that the stress value never even begins to converge; this is (essentially) the stress point that the h-adaptive method in SW is looking at. However, even though Stress1 never comes close to converging, Stress2 and Stress3 start to converge (the convergence isn't better because I did a crude and simple mesh refinement).

                                                 

                                                So, what does all of this mean? While the maximum stress (Stress1) didn't even come close to convergence, Stress2 and Stress3 somewhat did. In your model, all you're seeing (convergence wise) is akin to Stress1, so your model appears to not converge. However, we've shown that other points can converge even if some points don't converge, but since you're not tracking these other values when doing the h-adaptive method in SW, you have no way to know whether or not they've converged.

                                                 

                                                Stress Convergence.PNG

                                                  • Re: thermal stress simulation
                                                    Jared Conway

                                                    you'd have to split the body to put a sensor at that location

                                                    or run an analysis in advance, make a sensor on a cut, export as a sensor (x,y,z)

                                                      • Re: thermal stress simulation
                                                        Shaun Densberger

                                                        That's what I did (split the body and place a sensor on a vertex), but I wasn't able to find a way to change the convergence criteria for the h-adaptive method to that sensor (instead of the default, which I assume is probably total strain energy and maximum stress).

                                                          • Re: thermal stress simulation
                                                            Jared Conway

                                                            i think there are some enhancement requests around that for this specific reason but nothing in the software today.

                                                             

                                                            here's the suggestion from the help that we usually point customers to when they run into this situation:

                                                             

                                                            Accuracy bias You can move the slider towards Local to instruct the program to concentrate on getting accurate peak stress results using less number of elements. Or you can move the slider towards Global to instruct the program to concentrate on getting overall accurate results. 

                                                             

                                                            Stress singularities occur at the locations of concentrated forces and sharp corners. The stresses at these locations keep increasing as smaller elements are used. For models with such singularities, it is recommended to move the slider towards Global.

                                                              • Re: thermal stress simulation
                                                                Magnum So

                                                                "while the maximum stress of the model will not converge, the stresses at other points on the model could"

                                                                It is really a good remind for me as I always focus on the max. stress convergence even the loaded point is not important for my whole model.

                                                                 

                                                                Now I just confused that why sometimes I could make a likely convergence result with the refinement of global size in the range of  "coarse" to "fine", but it will then fail when the global size is further smaller?

                                                                Like my stress plot above:

                                                                In the iteration 1 to 4, global size is refined from coarse(5.8mm) to fine(1.4mm), the graph shows a convergence result

                                                                In the iteration 5, global size is set to 1.0mm, the graph becomes failed in convergence...

                                                                 

                                                                Anyway, I think I should practise more for the terms of "convergence","singularity"and "mesh control" right now

                                                                  • Re: thermal stress simulation
                                                                    Jared Conway

                                                                    i think you're missing the point, at that one location, there is no guarnatee of stress convergence, this is a singularity. however displacement may converge

                                                                    • Re: thermal stress simulation
                                                                      Shaun Densberger

                                                                      "In the iteration 1 to 4, global size is refined from coarse(5.8mm) to fine(1.4mm), the graph shows a convergence result

                                                                      In the iteration 5, global size is set to 1.0mm, the graph becomes failed in convergence..."

                                                                       

                                                                      It's hard to say exactly why this happened because there are a great deal of factors that come into play. However, keep in mind that as you change/refine a mesh, you're not changing just the overall element size. It's likely that element aspect ratios are also changing, and tet elements (which is all that SW uses) are very sensitive to changes in the aspect ratio (and also have a number of other drawbacks to them). We're now getting into the other mesh design characteristics such as element type (tet, quad, etc.), aspect ratio, basis function (linear, quadratic, cubic, etc.); this is a very in depth topic.