GabiJack.com

Posts Tagged ‘static’

A few days ago, my friend Chris Thompson, founder and owner of Appian Way Technologies, took a look at my model of the safety latch and suggested the following changes in order to improve the simulation study.

First of all, he added small fillets to the areas of the latch where stress concentrations are expected, at the “root” of the latch. He also “cut” the model in half, in order to take advantage of its symmetry through the use of symmetry constraints, which can be found among the Advanced Fixtures available in SolidWorks Simulation.

The symmetry fixtures will simulate the half of the latch that was cut from the model. Having this fixture in place will prevent any displacements across the plane of symmetry, but allow displacements on the plane of symmetry. The idea behind this is to reduce the number of equations necessary, as well as the solving time. In order to use this constraint, right click on Fixtures, and select Advanced Fixtures, Symmetry. He selected the left planar face of the latch to define the plane of symmetry, as you can see in the following image.

Chris also talked to me about the possibility of improving results by any of two options: manually refining the mesh and using mesh controls, or making use of the h-adaptive solution method, which is available only for static analysis and solid elements. Why is this going to improve results? Well, simply because any solution obtained through FEA will depend on our choices for discretization (a.k.a. meshing). Different choices for meshes will also cause different discretization errors, and we can estimate these errors by making systematic (planned and gradual) changes to the mesh and analyzing the impact of such changes in the results of our study. This is often called a convergence process. The way we can do this is by simply starting with a study that uses an average element size mesh, and then, in subsequent studies, gradually refine the global mesh (reduce the size of the elements), while keeping an eye on any changes in stress and strain in the whole model or in areas of interest (in this case the fillets). We’ll know the process is converging when any further refinement of the mesh produces insignificant changes in the magnitude of the results. This can be a long and tedious process.

Further manual refinement consists of applying mesh controls to the areas of interest in the model. Basically, mesh controls allow us to refine the mesh locally, only in those areas of interest where we expect high concentration of stress, while the rest of the model is meshed using a much larger element size, thus reducing the number of equations and time needed to solve the study, at least when compared to global mesh refining. Mesh controls can be applied to edges, vertices, faces or entire components of assemblies, and they need to be applied before meshing the entire model.  The way to apply mesh controls is by right clicking on the mesh icon in the Simulation Study tree and select Apply Mesh Control.

Here in this image you can appreciate the way Chris applied a mesh control to that couple of fillets. He selected the two faces and used an element size of 0.029 in and a Ratio of 1.5.  This Ratio parameter simply specifies the ratio between element sizes in consecutive transitional layers when going from the global mesh element size to the local mesh element size. A Ratio of 1.5 is usually default.

Chris also applied mesh controls to the curved face of the cutout you see on the bottom of the latch, where stresses also concentrate, and to that edge on the tip of the latch, that he created by means of a split line, and used to define the Use Reference Geometry Advanced Fixture that I applied in the original study to make sure the latch had that 5 mm displacement, remember?

 

He then meshed the rest of the model using the default mesh element size. Notice in this image the transition between mesh element sizes in different areas of the model.

So that’s the manual way to do it, but this refinement process can also be automated, by using the h-adaptive Solution Method. By the way, the “h” refers to the size of the element, so the convergence process through mesh refinement is actually called “h convergence process”, since the size of the elements is gradually reduced.

To make use of the h-adaptive solution method right click on the name of the study in the Simulation Study tree and select Properties, then select the Adaptive tab, and under Adaptive method option select h-adaptive.  You have a few options to choose from here.  From the help document, “Target Accuracy sets the accuracy level for the strain energy norm in the model, which is not the same as stress accuracy level.” A default value of 98% means that the convergence process will stop if the difference in the strain energy norm between two loops drops below 2%. Accuracy Bias instructs the solver how to concentrate on getting stress results: Local (all the way to the left) will cause the solver to concentrate on getting accurate peak stress results for those very localized areas with high strain energy errors (the fillets) by highly refining the mesh in those areas, while Global (all the way to the right) will cause the solver to ignore high, localized strain energy errors and concentrate on getting accurate overall stress results for the whole model.  The maximum number of loops will tell the solver how many times to repeat the process of mesh refinement. Looping will end when Target Accuracy is achieved or when the maximum number of loops is reached. If Mesh Coarsening is selected, it simply means that during the mesh refining process our original mesh can actually be made coarser in some areas of the model, as the solver sees fit. This way the mesh will be refined only where needed.

This is the mesh that my friend Chris achieved for the latch by using the h-adaptive solution method with default values and a maximum number of loops of 3.

As my friend pointed out to me, the h-adaptive method is useful not only to save us from the tedious process of manual mesh refinement, but also for those times when we’re not exactly sure where the areas of high concentration of stresses will be.

Thanks, Chris!

I guess the bad thing about being a self-learner is that many times you have to make do with whatever materials you may find available, and sometimes they may be a little outdated. For instance, I grabbed this COSMOSWorks Designer 2007 manual on eBay and was going through the lessons using SolidWorks Simulation (that’s the new name for COSMOSWorks in 2009). Except for a few differences here and there, everything was more or less the same, so I was doing great, until I arrived to the lesson about shell elements, that is. It took me a little while to figure out what to do, but it all made sense in the end, and so I decided to put together this little video comparing the way to create a mesh using shell elements in COSMOSWorks and in SolidWorks Simulation. This is for all those that may find it confusing going from one to the other for the first time… and also for those that bought the same manual I did. Hope it helps someone out there!

Just click on the image and it will take you straight to the video. I’m sorry that this video has no audio, but this blogger’s place is just absolutely noisy. Hope you still find it useful, though. It has plenty of notes!

 Fear is one of the most powerful emotions a human being can ever experience.  It can trigger quick thoughts and actions that will help us fight back or flee from whatever situation we perceive as danger; it can be paralyzing, as well, robbing us of valuable experiences and opportunities that we may have otherwise enjoyed.  Take me for example: I used to be afraid of driving the freeway. The thought of it was so overwhelming that I avoided at all cost going anywhere that wasn’t  “local”, and even scheduled appointments with my doctor, who had his office in Mountain View,  ONLY whenever my husband was able to drive me there.  However, as careful as I always was to avoid the freeway, and given the fact that Murphy has made my home his residence, one day I ended up on I-880 just like that, and it was then that, in the midst of my panic attack, I realized that I was not afraid of the freeway, but of not knowing my way around the freeway. I was afraid of getting lost. Well, we found an easy solution for that by equipping my van with a GPS unit. My life has improved ever since! Now I get lost in style whenever the GPS takes me to the middle of a swamp and proudly declares, “You have arrived”… but at least the fear is gone.

But why did I have to tell you all this? Well, because I’m beginning to think that for many people it’s almost the same with FEA.  I’ve always been interested in simulation. I was excited to finally have access to simulation software through SolidWorks and be able to learn how to use it, but I soon became discouraged by comments I read and heard from people that didn’t consider FEA as a useful or even reliable part of design. Their idea was something like “I won’t trust results that I can’t calculate myself”, but the more I learn about how Finite Element Analysis works (not only SolidWorks Simulation), I honestly don’t see how they are going to be able to obtain results “by hand”  without the use of the finite element method or some other form of numerical method approach, or without making use of some extremely simplified mathematical model. Unfortunately, although it’s true that most practical problems  in engineering can be represented by mathematical models of the actual physical problem, and are generally governed by differential or integral equations that represent them, it is also true that due to complexities in geometry, boundary conditions, and others,  these equations can’t be solved at all without the use of numerical methods to obtain an approximate solution to the problem. The other option, of course, is to go through the loop of the build-test-build cycle as many times as necessary, but that can be expensive and time consuming, without mentioning that it doesn’t really provide the designer with much information about the behavior of the product until near the end of the process.

So, if FEA is only a way to provide a solution for the series of equations that describe the mathematical model and if those equations derive from applying exactly the same laws and theory that we would otherwise while solving the problem “by hand”, why is it that some people out there are so afraid of it?  I think it may be perhaps that, same as me and the freeway, people aren’t precisely afraid of the finite element method per se, but of “getting lost” in the Finite Element Analysis software. After all, your results are only going to be as good as your mathematical model and the input you provide, and you still need some common sense when it comes to interpreting the results of your analysis.  With this in mind, FEA software can be a great tool for design or just another way to get lost in style.

A quick example is in the following simple problem, taken from a popular engineering textbook. In the example, we have a stepped cylindrical shaft that is rigidly clamped on one end and that has a force of 1000 N applied to the opposite end.

 

I meshed the model using draft quality solid elements, and the default values for element size and tolerance.

 

Then generated a stress plot showing the normal stress in the X direction, the stress you would usually calculate using the simple formula 

 

where sigma is the normal stress, F is the force and A is the cross sectional area of the shaft at the location of interest. By using Probe to investigate the value of the stress at some node in the middle along the length of each step, I realized the results for this case are very similar to those obtained “by hand”.  

 

Notice how the value of the stress changes, however, as we approach the ends of each step and the transition between areas.

 

So then I wonder what would happen if I shortened the shaft. I created a second study using a short configuration of the model in which each step was only 0.01 m, instead of the previous 0.5 m. The diameters, fixtures and force all remained the same, and so did the quality of the mesh and even the element size and tolerance.  My results, however, didn’t match those obtained applying the same formula as before.

 

I even refined the mesh, used high quality elements and all, but the results still didn’t match.

 Then it occurred to me that the formulas we apply for the solution of this kind of problems were derived assuming, among many other things, that we were trying to figure out the stress in a section far away from the point of application of the load, because in general, the value of the stress at any point in the section is actually given by

And this value changes across the section and is very different from the average value given by the first equation. The variation is small in a section far away from the points of application of any loads, but very noticeable in the neighborhood of these points.  When the shaft gets shortened, the steps become so thin that there is no way to be far enough from the point of application of the load, so the assumption we made before doesn’t really work here.  What I wonder is what to think of the results obtained in this case by using SolidWorks Simulation.  Are these even meaningful results? Should refining the mesh even more work better in this case? Unfortunately, I will never know because I tried to refine my mesh even more and received a message saying I had insufficient memory and needed to increase the value of my elements.  I’m still very new to FEA and SolidWorks Simulation to know if there’s a different approach to this kind of problem, so if you have any ideas on this, please let me know.  I’m just excited to finally be learning about FEA.