Wrong stress

[Anonymous]

I am doing a simulation of a storage tank. the tank is divided in ring with different thickness and a zone with a internal reinforcement to specific parts of the rings. I have cloud points of the surface of the tanks i processed th cloud ,exported to inventor and then to simulation mechanical. However ,I am having wrong stress values, how i know i upload the same model to other fem software and the stress are totally different we are talking of the twice the values in the deformed zones.with a maximum stress overshooted. in the other fem software I only have high stress values in zones were i dint clean enought the mesh as the place were a pipe is located and thinks like that.

[AstroJohnPE]

Hi txfingenieria,

It is not unusual to have a "hot spot" of high stress, depending on the type of elements and the mesh quality. So the fact that the maximum stress is 1130 in Simulation Mechanical and 575 in an unidentified program is not that big of an issue.

I'm sure that if you check all of the results in Simulation Mechanical, you will find that either there is a mistake on the input or the results are "correct". Sometimes, you just need to ignore the hot spots because of limitations in FEA/simulation.

P.S. By "all of the results", I mean the displacements, reaction forces, and everything else appropriate for the model and setup.

[Anonymous]

Hello John

I know that part. In the simulation the mesh is stablished in fine. In ansys I try to give the same dimentions.. if you can see in the image the hot spot of ansys is a small zone however the hot spot in autodesk are large zone where the stress over pass 205Mpa yield stress of Asme A283 grade C. This is more than a single hotspot and is more a wrong calculation. The deformation in ansys are between 60 mm and in autodesk are 578mm. My problem is  that i need a real aproximation because i have to evaluated the integrity of the tank.

[AstroJohnPE]

Hi,

Thanks for the additional images. I assume you would like to know why the results are higher in Simulation Mechanical. It might be easier for someone to figure that out if you could attach an archive of the model to your reply. See the post "Create, Post, or Provide an Archive of your model".

Also, please indicate which version of Sim Mech you are using, such as 2014.

[Anonymous]

Hello...Thanks John

I am attaching the file i place the file is mega.co.nz if you want to see the file and try to find a way to have real results

https://mega.co.nz/#!gc9UXbYJ!oVN3OHQ7eqjiNJxBkmVfI6HHe6kNb4it3fnyaO_TXBc

[AstroJohnPE]

Hi txfingenieria,

I believe the incorrect results are related to the warning that occurs during the analysis: the max/min stiffness ratio equal to 1E14. This means that some elements are really stiff and others are weak (probably normal stiffness). As a result, there is not enough precision to get an accurate solution.

Unfortunately, I could not view your model in the FEA Editor or the Report environment. Trying to do so crashed the program on my computer. But I was able to view the model in the Results environment. Using the command "Results Contours > Other Results > Element Properties > Node Angles" shows some elements with an angle between two sides of 175 degrees: essentially a 3 sided element with no area. Viewing the mesh ("View > Appearance > Visual Style > Shaded with Mesh") shows a number of places where the mesh is unexplainably distorted and smaller from the otherwise uniform size. Parts 1 and 2 in particular show these small pockets. By any chance are there work points in the Inventor model that get imported as construction vertices? In Sim Mechanical, construction vertices force a node at that location which can distort the mesh pattern. You can delete the construction vertices (or choose to not import the work points from Inventor).

I also noticed that some parts are finely meshed which may not be necessary. For example, part 7 is a uniform 37 mm element size where as the adjacent parts range in size from 90 to 145 mm. If you did not set the mesh size explicitly, then try deactivating the checkbox for "Mesh > Mesh > 3D Mesh Settings > Options > Model > Use automatic geometry-based mesh size function".

In summary, the mesh quality is affecting the results.

[Anonymous]

Hello  John

Thank you for your answer. But  i couldn't find a way to solve the problem. I tryed before to apply a specific size of mesh but the results are worse. You re right the problem is in the stiffness matrix. In the formulation the software is writing in a wrong way the mesh values.  I will try to have some type of support directly from Autodesk over this topic and i will tell you if i find a solution.

Thanks again for your help

[KubliJ · Accepted solution]

Hello,

The problem as John pointed out is the mesh quality.  The cause of the poor mesh quality is because of poor geometry quality.  The surface bodies appear to have a random pattern cut out on them.  This creates excessively small surfaces and splinter surfaces.  Please see the screen shots below:

If you have imported the model into Inventor before pushing into simulation, I believe you can use the surface patch tool to merge the surfaces together.

Thanks,

James

[Anonymous]

Hello

James sorry fot didnt answer early I was in the middle of a project and i was doing cloud import. And i dont know why but i did was you suggest to me without reading your message. That helps the mesh to have a better stiffness matrix another factor that i did was to recalculate the normals of the nurbs curves and keep the mesh in a average size nothing small. This really give me realistic results. Next week i have the change of checking my results in a tank. But the results look very realistic without concentration of stress.

Thank you