General Mechanical

General Mechanical

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

The mesher has detected a discontinuity in the model and is unable to handle it.

    • Panagiotis

      When trying to mesh a cylindrical tank with heads close to elliptical shape ( it is not a half ellipsoid) I get the following error "The mesher has detected a discontinuity in the model and is unable to handle it. Please go back to the CAD system and correct the model." The problematic geometry is shown in the picture (with red dots). Although I have checked the geometry in spaceclaim and have already clicked the share topology option, I keep getting this error. The geometry in spaceclaim is comprised of multiple solids and was generated through the revolution of an area through the z-axis.

      P.S. I have already meshed the same geometry in Mechanical APDL, using APDL commands and not spaceclaim. However, I want to make the transition from APDL to Workbench, in order to add other features to the CAD file.

    • Govindan Nagappan
      Ansys Employee


      Inspect the probelmatic geometry and see if you can correct it?

      In Mechanical, you have tools to display edges in different colors based on connectivity. (Color -> By connection). See if it helps to identify the problem. If there is a gap larger than the tolerance, shared topology may not have connected the geometry at this location. See if you can fix the gap in spaceclaim

      If you have access to meshing, you can consider meshing in Spaceclaim using blocking

      Or try a different method and see if it helps. Try patch independent methods like Multizone for hex meshing or patch independent tetrahedron


      Default is patch conforming methods in Mechanical (PC tetra and Sweep). These methods require a propely connected geometry. So, other methods may help. in MAPDL, you can create 2D mesh and sweep. We have similar tools in newer versions f Mechanical - Check this link: Pull (

      See if these tools help




    • mjmiddle
      Ansys Employee

      When you select "Show Problematic Geometry" on an error message, the red dots do not usually show an exact problem location. Instead, the red dots are just the highlighted vertices of green highlighted faces. You should ignore the red dots and inspect the green highlighted faces. Zoom in close and insect the face boundaries especially.

      Also, the defeature tolerance in the global mesh object can overcome geometry problems. Make sure it is turned on and you should estimate a reasonable distance to merge across. Try specifiying a larger tolerance.

      The share topology in SpaceClaim can cause corruptions in the geometry if you set up sharing, and then make further modeling changes. It should be done as one of the last things in SpaceClaim. You can delete all share topology and redo the sharing. Also, you should test by completely removing all shared topology and see if that meshes in Mechanical. That will at least tell you if the shared topology is the cause.

Viewing 2 reply threads
  • You must be logged in to reply to this topic.