The mesh algorithm option is applicable only to the following:
A surface region that you are meshing with a quadrilateral or quadrilateral-dominated mesh using the free meshing technique.
A solid region that you are meshing with a hexahedral or hexahedral-dominated mesh using the swept meshing technique.
A solid region that you are meshing with a tetrahedral mesh using the free meshing technique.
To set the mesh algorithm:
From the main menu bar, select Mesh
Controls.
ABAQUS/CAE displays prompts in the prompt area to guide you through the procedure.
Tip:
You can also click the 
tool, located in the Mesh module toolbox. (For more information, see “Using the Mesh module toolbox,” Section 17.12.)
If your part or assembly contains more than one region, select the regions of interest and press mouse button 2.
The Mesh Controls dialog box appears. If the mesh algorithm option is applicable to the type of mesh you are creating, an Algorithm field appears on the right side of the Mesh Controls dialog box.
The algorithm options that appear depend on the element shape that you selected.
Quadrilateral, quadrilateral-dominated, hexahedral, or hexahedral-dominated elements
Choose either Medial axis or Advancing front. It is difficult to predict which algorithm will produce the best mesh for a particular region; you may have to experiment with the two algorithm settings. For more information, see “What is the difference between the medial axis algorithm and the advancing front algorithm?,” Section 17.7.6.
If you choose the Medial axis algorithm and a quadrilateral or hexahedral mesh, you can control if ABAQUS/CAE will try to minimize the mesh transition when it moves from a coarse mesh to a fine mesh. In most cases, toggling on Minimize the mesh transition will reduce mesh distortion. However, if you toggle off Minimize the mesh transition, the mesh may move closer to the specified mesh seeds. For more information, see “What is a mesh transition?,” Section 17.7.5.
Tetrahedral elements
Choose the default mesh generation algorithm or the algorithm that was included with Version 6.4 of ABAQUS/CAE and earlier. In most cases the default algorithm is more robust, particularly when meshing complex shapes and thin solids.
If you choose the default mesh generation algorithm, you can toggle on Increase the size of the interior elements and choose either Moderate growth or Maximum growth. If the mesh density is adequate for the model being analyzed and the areas of interest are on the mesh boundary, increasing the size of the interior elements will increase the computational efficiency. To view the internal elements generated by ABAQUS/CAE, you can create a new orphan mesh part from the meshed part and use display groups to remove selected elements.
Click OK to save your data and to close the dialog box.
