Solid Mesh Optimization

This topic covers solid mesh optimization for tetras.

1. From the Elements ribbon, click the arrow next to the Edit tool set name and select Solid Mesh Optimization from the drop-down menu.
2. Click the Tetras tab.
3. Select a set of elements to fix using the Input selection collector.
4. Complete the Tetras table items by entering the appropriate values.
   For more information on table items, refer to the Review Element Quality section.
5. Select a Triangles option.

   Fix All

   All triangles are fixed during optimization.

   Edge Swap

   Edges of boundary triangles can be swapped during optimization. Node locations of boundary triangles are not modified.

   Remesh

   Boundary triangles can be remeshed during optimization. This option usually yields the best results.

6. Set Constraints options according to the following table.

   Constraint	Action
   Fixed Trias	Set this constraint to Elements if you do not want to modify tria elements during the optimization step. This constraint is only available if Edge Swap or Remesh is selected under Boundary triangles.
   Feature Line	Set this constraint to Elements to mark feature lines by 1D plot elements that coincide with element edges. Selecting those 1D edges ensures that the corresponding element edges are not modified during the optimization step. This option is only available if Edge Swap or Remesh is selected under Boundary triangles.
   Anchor Nodes	Set this constraint to Nodes so that selected mesh nodes are not modified during the optimization process.
   Refinement Box	Set this constraint to Elements so that elements inside the refinement box are remeshed and optimized with respect to the defined thresholds.

7. Check the Fix Shell Comp Boundaries option to maintain the edges between two components during the optimization step.
   This is useful when the interface between a solid and a fluid component has to be maintained.
8. Check the Maintain Geometry Edges option so that nodes on a geometry edge are not modified during optimization.
9. Check the Save to Current Comp option to save elements generated during optimization to the current component.
10. Check the Update Input Shells option to update shell elements attached to modified tetra elements.
    This option is only available if Edge Swap or Remesh is selected under Boundary triangles.
11. Check the Optimize Tetras by Force option to include a node insertion algorithm.
    This usually yields a higher element quality in the resulting mesh, but in return might also increase the computation time.
12. Enter the maximum number of optimization steps in the Maximize Iteration field.
13. Enter an angle in the Feature Angle field that will be considered a feature edge and that will be preserved during the optimization step.
    If the angle of two adjacent shell elements is greater than this angle, the edge will be preserved.
14. To show elements that have failed, click Show Failed.
    Only the elements that have failed the selected element criteria will be displayed. Click this button again to redisplay all elements.
15. To perform an element check based on the defined parameters in the Criteria Editor, click Check.
    Mesh statistics will be displayed in the table.
16. To start the optimization process, click Fix.
17. To re-establish the initial tetra mesh and reject the modified mesh, click Reject.
18. When you are finished, click Close.

This topic covers solid mesh optimization for hexas.

1. From the Elements ribbon, click the arrow next to the Edit tool set name and select Solid Mesh Optimization from the drop-down menu.
2. Click the Hexas tab.
3. Select a set of elements to fix using the Input selection collector.
4. Complete the Hexas table items by entering the appropriate values.
5. Define the relative weight for the active quality criteria.
   Criteria with a higher weight will get higher preference in case of conflict.
6. Check the Allow Boundary Node Movement option to allow for node movement on or normal to the boundary.
   If you check this option, you can define the following fields:

   Option	Description
   On Geometry: Maximum Node Movement/Element Size	Enter a value in this field that defines the maximum node movement allowed on geometry to fix hex quality as a factor of the hex element.
   Away From Geometry: Maximum Node Movement/Element Size	Enter a value in this field that defines the maximum node movement allowed away from geometry to fix hex quality as a factor of the hex element.
   Feature Angle	Enter a value in this field that identifies the feature edges on which node movement will be restricted along the edges only.

7. Enter a value in the Maximum Iterations field that defines the number of maximum iterations to go through to fix quality.
   Hex quality improvement will terminate if quality is not fixed within the defined iterations.
8. Check the Show Original Face Node Location option to create temporary nodes showing input node positions that were moved during optimization.
9. To show elements that have failed, click Show Failed.
   Only the elements that have failed the selected element criteria will be displayed. Click this button again to redisplay all elements.
10. To perform an element check based on the defined parameters in the Criteria Editor, click Check.
    Mesh statistics will be displayed in the table.
11. To start the optimization process, click Fix.
12. To re-establish the initial hexa mesh and reject the modified mesh, click Reject.
13. When you are finished, click Close.

This topic covers second order mesh optimization.

1. From the Elements ribbon, click the arrow next to the Edit tool set name and select Solid Mesh Optimization from the drop-down menu.
2. Click the Second Order Elements tab.
3. Select a set of elements to fix using the Input selection collector.
4. Define the element maximum angle, minimum and maximum length ratio, and Jacobian thresholds.
5. Select the appropriate option in the Evaluate Jacobian at field.
6. Select the appropriate options in the Middle Nodes Repositioning field:
   1. Check Internal Nodes to allow mid tetra nodes located interior to volume mesh.
   2. Check Boundary Node options to allow mid tetra nodes located on the boundary. Move Along Geometry First enables tetra mid nodes along geometry to fix quality. Move Off From Geometry enables tetra mid nodes away from geometry to fix quality.

      Tetra mid nodes will only be moved away from geometry, if moving nodes along geometry does not fix quality.

7. To perform an element check based on the defined parameters in the Criteria Editor, click Check.
   Mesh statistics will be displayed in the table.
8. To start the optimization process, click Fix.
9. To re-establish the initial second order mesh and reject the modified mesh, click Reject.
10. When you are finished, click Close.