Stress are way to low

protontim

As a first approximation I simulated a beam with loads using beam elements and got reasonable results. For the next step I drew up a more detailed beam with mounting brackets, merged the assembly into a single solid step file and meshed it with gmsh. I then read it into Mecway, and added my loads and constraints. I ran the simulation and the resultant stresses are ridiculously low. Any idea what might be happening?

protontim

here is the file that is giving me the trouble

[Deleted User]

you might want to try netgen instead of gmsh. just to make sure it is not the mesh. mecway uses a modified version of netgen. when mecway has crash issues meshing, I am able to get it to work in Netgen. This is due to the fact that you have access to more mesh controls in Netgen. Try setting the min mesh size to 1. The default of 0 tends to crash the mesher. Also check the element quality using the element quality plot option in Netgen. I haven't checked out your liml file. Victor will probably be able to see if something is wrong with the model setup.

Victor

Hello Protontim. There are two issues with this file:

1) The mesh is too coarse. Refining it increases the stress so you should keep refining it until the stress stops increasing much. You can also get a big reduction in mesh size (or improvement in accuracy) by changing the tet4 elements to tet10. Either in Mecway with Mesh tools -> Change element shape or in Gmsh. This model has quite a lot of small details (especially the thin walls), so it will probably end up with a very big mesh and you may need to use local refinement instead to focus on the areas you're interested in.

2) Many elements are very distorted. All the edge lengths of a tet element should be roughly similar to each other - which means less than the beam's wall thickness. An element quality tool like prop_design mentioned would also show this. I've seen this kind of distorted tet mesh from Gmsh before and I think there's an option to enter the maximum element size or something like that, to prevent them getting too stretched out.

VMH

Protontim, I'm interested to see your step file if you can provide it.

As mentioned in Victor respond, I would avoid using Tet4 or linear tetrahedral elements because they are too stiff. Tet10 or quadratic tetrahedral elements perform very well. See the following link for more information:

http://www.ansys.com/staticassets/ANSYS/staticassets/resourcelibrary/confpaper/2004-Int-ANSYS-Conf-9.PDF

protontim

Thank you all very much for your responses. I have installed Netgen 5 and I am on my way. Thanks again.