I'm working on a cargo bike project, you can find a lot of details in a previous question that the community helped me solve here: https://www.lynkoa.com/forum/g%C3%A9n%C3%A9ralit%C3%A9s/d%C3%A9placement-impos%C3%A9-de-type-pivot-glissant
My tubular structure involves stress concentrations, and I would like to be able to easily spot the stress value at each location where stress concentrations occur.
Currently, I can easily view and find where the maximum stress is. On the other hand, for the other places where there are significant constraints, I feel my way around, looking with the colors where there are other places with a strong constraint and then using the probe tool to read the value of it.
Is there a tool or method that makes it possible to collect several local maximums and not a single global maximum?
Looking at colors is not the best way to go about it for several reasons.
1°) This amounts to focusing most of the time on concentrations of surface stresses : but which tell you nothing about the internal stresses of the part since you only see the outside of the part. These somewhat artificial stress concentrations can very well be removed by refining and optimizing the local mesh or by putting a radius in the corners of the model. (see also the adaptive mesh H or P or to start choose automatic transition for the first mesh)
2°)Your model is not optimized because when welding tubes the weld seam has the effect of reducing the stresses in the corners.
3°) it is better to use in the results "design dissection" which makes you see what is happening in the heart of the part (and not on the surface) In the results click right on the result: other choices of results such as "Safety Factor" and also "design dissection" appear (play with the cursor to see the internal areas more or less loaded)
4°) In the results you can also have all the min and max values of each node of the mesh with their position according to XYZ. Still in ""Results"" select ==> lists of stresses, displacement, deformations (Note that you can save the results in a Excel. csv file)
So you don't have to put a probe on each node by hand.
I note that your project is moving forward... To identify the areas that are heavily stressed, I don't see any other solution than to use the option "Modify iso..." " accessible with the right button on "Constraints (von Mises)", which allows you to display on the model the areas where the constraint is greater (or lower) than a threshold set by cursor. By gradually decreasing this threshold, we successively visualize the most used areas. To my knowledge, there is no digital solution to identify local maxi rooms.
There is also a "Stress Sensitive Point Diagnostic" function in the results that allows you to know whether the high stress in a localized area of the structure is a simple stress concentration, or a numerical singularity.
Thanks to both of you for your answers, the two options "edit iso... " and "design dissection" work well and are what I was looking for!
@Zozo_mp
1) Indeed I am well aware of the limits of colors in surfaces. However, in my case, the thicknesses are very small and I usually have only one mesh in the thickness so the color gives a pretty real idea of the constraints.
2) Is there a solution on SW to overcome this effect? Or only when analyzing the results to ignore the stress concentrations in the corners?
4) Thanks for this tip, I'll try this way as well.
To size the cross-section of your tubes, the "beam" or "shell" meshes are perfectly suited.
However, at the connection between tubes, it implies sharp angles, and therefore mathematical singularities that result in infinite constraints (do the test, the more you reduce the size of your mesh, the more the constraints will increase!)
So you have to do a sub-modeling of the junctions where you have doubts. As Zozo_mp says, welding seam modeling is important because they make these sharp corners disappear. However, this implies that you are passing on a volume mesh and therefore that the computation times are longer! Hence the idea of "sub-models" which only linger on a particular area.
I have already passed my study in volume to be more precise on the functions between tubes as well as to be able to mix volume parts with my tubes. Apart from the fact of going into volume, is it possible to simulate the weld seams?
Welding seam simulation is not of interest in general and even less so in your case with small cross-section tubes.
If you put spokes (this replaces weld seams very well) because it allows you to remove stress concentrations (false stresses) in a very simple way. Welding seam installation is a real m...... In Solidworks and in addition there are many cases where it does not work with simulation because they are virtual graphical representations (without material). The only soldering trick that works properly in SW is spot soldering. There are other reasons for not putting a weld seam that deserves a long theoretical-technical development or an explanatory tutorial with a comparative model
