The mesh algorithm options that are available depend on the element shape and the meshing technique that you have selected. 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.
ABAQUS/CAE provides the following mesh algorithm options:
Choose the mesh algorithm
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.
Minimize the mesh transition
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.
Use mapped meshing where appropriate
Some models that appear very complex actually contain faces with relatively simple geometry. When you mesh such a model with free or swept meshing, the resulting element quality can be poor on the relatively simple faces. However, if you allow ABAQUS/CAE to use the mapped meshing technique where appropriate, it often generates elements of good quality on these faces. Toggle on Use mapped meshing where appropriate to allow ABAQUS/CAE to determine if mapped meshing can be applied. For more information, see “What is mapped meshing?,” Section 17.8.2, and “When can ABAQUS/CAE apply mapped meshing?,” Section 17.8.6.
Use the default algorithm
When you are creating a free mesh of tetrahedral elements, you can 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. For more information, see “Free meshing with triangular and tetrahedral elements,” Section 17.9.3.
Increase the size of the interior elements
If you choose the default mesh generation algorithm to create a free mesh of tetrahedral elements, 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.
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 17.13.)
If your part or assembly contains more than one region, select the regions of interest and click mouse button 2.
The Mesh Controls dialog box appears. If the mesh algorithm option is applicable to the selected element shape and meshing technique, an Algorithm field appears on the right side of the Mesh Controls dialog box.
Select the desired algorithm options, and click OK to save your data and to close the dialog box.
