Mesh failed

Hello everyone.

I have no idea how to create the mesh on my model.

I've tried to create it by default and with some face sizing adjustment on tiny faces, also i've tried with different values of Element size from 85 to 40.

I've checked mistakes by Fault Detection in Design Modeler and repaired it by Virtual Topology in Mechanical but have got no result.

The errors that were shown are below.

Also, i have attached my Design Modeler file .agbd below (Ansys 2020 R1).

My model was created as one part, so you dont need to create connections. I couldn't share workbench project archive due to the size is more than 4 GB.


Help me please!!! 😟


Comments

  • peteroznewmanpeteroznewman Member
    edited September 13

    @Gordievsky87

    This geometry is very "dirty". There are many complex faces that should not be present. The video below shows some methods for cleaning this dirty geometry. If you made this geometry, you need to learn how to create "clean" geometry.

    I sliced the geometry into 3 pieces which can be meshed. You can use Bonded Contact to hold them together. I had a question on whether the gaps shown in the video were intentional or just the result of dirty geometry. I assume the later, in which case, mesh defeaturing would eliminate small edges and the Pinball Radius on the bonded contact would bond across these gaps.

  • peteroznewman

    Thank you very much for your attention to my problem. The video is very helpfull.

    Yes, the model is so dirty, however the 0.5 mm gaps are intentional. They were created to simulate the weld work. So that connections between parts were through the welds.


  • peteroznewmanpeteroznewman Member
    edited September 13

    Okay, that is a good reason to have them. In that case, set the defeature tolerance to a size of 0.4 mm so the lip does not disappear. Then in Bonded Contact, you can just pick the face of the weld.

    Another way to model welds is to let the weld bead be a separate body and use Shared Topology or Bonded Contact to hold the parts together.

  • Good afternoon Peteroznewman!

    I would like to create a square mesh for my model. (Like in the picture below). I've read it is more appopriate mesh for mechanical analysis.


    I have used Hex Dominant method in which the mesh creating lasted more than 10 hours and has got no result and i just finished the mesh building because i thought it cant be callculated for such a long time. I use pretty powerful computer with 320 gb RAM. However, the simple program controled mesh is calculated for 20 minutes.

    Also, i have sliced the geometry by peices and used sweep method but got an error that this method can't be used for a such geometry.

    I also need help from you. Could you please advice me what to do to create a square mesh?

    My Desing Moderel file is attached.


  • peteroznewmanpeteroznewman Member
    edited September 20

    @Gordievsky87

    You have really cleaned up the geometry nicely.

    It is easier to obtain a Hex mesh if you leave solids separate. You have united all the solids, so all that is available is a Tet mesh.

    A Quadratic Tet mesh provides excellent results if the elements are small in the areas of high stress gradient. You can use Mesh controls such as Sizing on the Body with Sphere of Influence to put small elements in a restricted volume, you just need to create a Coordinate System to locate the sphere.

    The benefit of a Quadratic Hex mesh is that fewer elements are needed to fill the volume, which makes the solution take less time to compute.

    You can spend a lot of time slicing up the solid to get the Hex mesh. If you only need to solve it once, it is not worth the time slicing it up. If you need to solve it hundreds of time in a Transient simulation, then it is worth the time to slice it up.

Sign In or Register to comment.