## General Mechanical

Topics relate to Mechanical Enterprise, Motion, Additive Print and more

#### Problem Meshing Multiple Bodies / Refinement / Adaptative

• Diego Molina
Subscriber

hello! I'm having trouble meshing a part with multiple bodies. What I'm trying to do is a static simulation for a vertical storage tank, it's made up of 5 rings (different thickness, so I use 5 different bodies) and the roof (also multiple bodies). When using adaptive mesh size, the mesh in the tank shell is extremely strange (attached screenshot), not using it improves the mesh, but I cannot reach convergence because making the elements smaller is too much computational load (for this I require use adaptive size)

I have tried:
1. Use shared topology
2. Use edge/edge and face/edge automatic contacts
3. Using a single body on the rings (improves, but I can't assign different thicknesses this way)
4. Turn off/on "defeaturing"

What workflow do you recommend to solve this problem?
Thank you!

• mjmiddle
Ansys Employee

The elements are very small throughout the model. This will increase solution time a lot. Why are they so small? Is this outer body very thin? The strange patchs of mesh may be affected by nearby fearures on the faces on the other side. If this is a thin body, it is usually better to make midsurfaces in the CAD modeler, which have thickness assigned. This will allow larger element sizes; the solution will run faster, and convergence should be easier. Set "shell thickness effect" on contacts used to connect bodies, and be sure to specify the correct "top" or "bottom" on "contect shell face" for contact and target side selections.

Also, consider specifying a larger element size on the global mesh object, setting refinement back to 1 and creating local mesh size features under the global Mesh object. For these you can just select faces/edges where you want the element size smaller.

Also consider turning off the adaptive mesh size function. Turn "Capture Curvature" on and set a minimum size for the curvature. Also set appropriate max mesh size and general element size throughout most of the model..

• Diego Molina
Subscriber

It worked! Thank you so much, I'm using surfaces. I turned of the adaptive mesh size function and turned un capture curvature, and set local mesh sizes for the rings and the roof components, now i am getting some stress peaks at the border of some bodies, is this due to the meshing process or is due to the geometry?

• saas lama
Subscriber

It is possible to create local mesh size features below the global Mesh object by providing a bigger element size on the global mesh object, resetting the refinement level to 1, and doing so. In this case, all you have to do is choose the faces or edges where you want the element size to be reduced.

retro bowl

• mjmiddle
Ansys Employee

The location(s) in the first picture look like typical stress singularities. Set smaller mesh sizes in the location of the max stress. If successive solutions with smaller mesh sizes cause the max stress to increase at increasing rate, it is a stress singularity. Valid max stress values will approach a constant value asymptotically with successive solutions using smaller mesh size. Stress singularities occur at corners. If the region is not of interest just scope results away from these. If it is a region of interest, make small fillets/rounds at those locations and use a small enough mesh size to model the round.

• Rouzman Dallin
Subscriber