Advanced Surface Mesher

This section shows you how to use the advanced surface mesher and how to access the Advanced Surface Mesher workshop.

  1. Enter the Advanced Surface Mesher workshop.

  2. If needed, define local specifications of the advanced surface mesh (using the Local Specifications toolbar).

  3. Launch or remove the simplification geometry and/or the mesh (using the Execution toolbar).

  4. If needed, perform manually modifications (using the Edition Tools toolbar).

    A specification created or modified after simplifying the geometry will not be kept on future updates.
    That means that: if you modify the geometry, the local specifications (defined using the Local Specifications toolbar) are kept but the modifications (performed using the Edition Tools toolbar) will not be kept.
    You have to define all the specifications before launching the geometry simplification.

At any time, you can:

  1. access the global parameters if you want to visualize parameters you have defined or if you want to modify some of the global specifications.

  2. exit the Advanced Surface Mesher workshop.

About Advanced Surface Mesher

The Advanced Surface Mesher works as shown here:

  1. Open the geometry .

  2. Launch the geometrical simplification .

  3. Launch the mesh execution .

: Open the geometrical element on which you are going to generate geometrical simplification from parameters.

: The geometry is simplified in order to launch the meshing and manage constraints more easily. The level of the simplification depends on the mesh parameters previously defined.

: The advanced surface mesh is created from the geometrical simplification previously generated.

Methodology

Follow the below described methodological approach when using the Advanced Surface Mesher of the FEM Surface (FMS) product.
Consider that the FEM Surface (FMS) product was developed so that mesh operation may be as user friendly and as automatic as possible.

  • If you want your constraints to be associative with the resulting mesh,  before you launch the mesh operation apply as many constraints as possible and as automatically as possible. 

  • Still, try to regularly check how constraints result on the mesh.

Generally speaking, you will start defining parameters, cleaning the geometry according to the desired resulting meshing and specifying constraints as soon as possible. You will then launch the Geometrical Simplification and in one go the mesh operation.

  1. define parameters
  2. clean the geometry
  3. specify constraints
  4. launch the Geometrical Simplification
  5. launch the Mesh operation
  6. perform constraints modification according to the resulting mesh elements (not according to the topology)
  7. if needed, edit the mesh elements

  1. Define parameters.

    From the very beginning, you need to specify global parameters: the shape of the elements, the size of the elements, the sag and the minimum size of these elements.

    Before:

    After:

    Use automatic algorithm and only define what the algorithm will not do properly for given cases.

  2. Clean the geometry.

    From the very beginning, you will also specify whether or not, you need given holes, button hole gaps (or cracks) and small faces to be taken into account by the geometrical simplification and therefore by the mesher.

    Before:

    After:

    This must be performed before you launch the mesh operation. Once the part is meshed, the clean characteristics can no more be modified.

  3. Specify constraints.

    You will also specify the constraints that are absolutely necessary for performing the Analysis computation. For example, you will impose the desired constraints in order to generate connections between meshes and to create boundary conditions such as restraints and loads.

    Before:

    After:

    Specify as many constraints before you launch the mesh operation: these constraints will be associative. Specify these constraints as automatically as possible and avoid modifying them manually (for example dragging a node).

  4. Simplify the geometry.

    The Geometrical Simplification computation is based on the global parameters and the constraints imposed by the user. The system will create an additional set of new constraints that will automatically help the mesher in creating elements of a higher quality.

    Avoid applying too many modifications before simplifying the geometry: launch the Geometrical Simplification and before modifying manually, check how the resulting mesh looks like.

  5. Launch the mesh operation.

    As soon as the mesh elements are generated, a feedback on the quality is provided. You can then perform manual modifications on the mesh elements, if needed.

    BE CAREFUL: this operation can be reversed. Even though you launch the mesh operation, you can apply modifications to the specifications. First have a look at the domains that seem to be problematic. Add more or delete existing constraints instead of modifying the mesh elements manually.

  6. Modify the mesh (re-mesh).

    Although the algorithms were developed in order to minimize user interactions, after the Mesh operation was performed, you can still modify the generated mesh elements. In other words, you can:

    • modify the geometrical simplification generated by the system

    • modify the nodes distribution 

    • apply local re-meshing (for example, the size or the type of the mesh elements)

    • edit mesh elements and apply manual modifications.

    Make sure you cannot remove the mesh and modify the constraints specifications instead. These modifications will not be associative.

    Advanced Users

    If you are an advanced user and know very well how the advanced surface mesher behaves, you can launch the geometrical simplification, perform the above mentioned re-meshing modifications and then launch the mesh operation in order to fill the gaps.

Resuming Editing on Mesh Part

Open the sample05.CATAnalysis document from the samples directory.

  1. Enter the Advanced Surface Mesher workshop. To do this,

    1. Double-click Advanced Surface Mesh.1 in the specification tree (below Nodes and Elements).

    2. Click OK (Continue anyway?) in the warning message.

  2. Mesh the surface part.
    To do this, click Mesh The Part .

  3. Exit the Advanced Surface Mesher workshop.

  4. Edit the Advanced Surface Mesh.1 mesh part. To do this, double-click Advanced Surface Mesh.1 in the specification tree.

    A message lets you decide whether you want to edit the meshed CATAnalysis with:

    • the initial meshing

    OR

    • the meshing last created.
    If the geometry was not properly updated, the .CATAnalysis will be edited anyway with the initial meshing.