Mesh Controls

Overview#

The mesh divides your geometry into small elements. Autodesk states that all solid elements in Fusion are tetrahedral (linear with 4 nodes, or parabolic with 10 nodes, with or without curved edges); 2D and shell elements are not supported, and line (beam) elements exist only as Bolt Connectors. Each simulation study has its own mesh settings. The solver computes unknowns at element nodes and interpolates between them. A coarse mesh is fast but misses gradients; a fine mesh captures them at the cost of solve time and memory. Good practice is to refine only where stress changes quickly (fillets, holes, load introduction) and keep the rest coarse.

The correct question is not "is my mesh fine?" but "does the result I care about stop changing when I refine?" That is mesh convergence.

Where to find it#

• Mesh Settings: Setup tab > Manage panel > Settings, then Mesh in the left column of the Settings dialog; or right-click the Mesh browser node and choose Mesh Settings. The options are identical in both places.
• Generate Mesh: Setup tab > Solve panel > Generate Mesh, or right-click the Mesh node > Generate Mesh. Solving also generates the mesh automatically.
• Display: Setup tab > Display > Mesh View, or the Hidden/Visible icon at the Mesh node (use this one to show the mesh on a results plot). The Results toolbar Display panel also toggles Mesh and Wireframe.
• Local Mesh Control: Setup tab > Manage panel > Local Mesh Control.
• Adaptive Mesh Refinement: Setup tab > Manage panel > Settings > Adaptive Mesh Refinement tab (not in the Solve dialog). Available for static stress, modal frequencies, thermal and thermal stress studies.

Step by step#

1. Open Mesh Settings and review Average Element Size - Solids (% of model size), Minimum Element Size, Maximum Turn Angle and Grading Factor.
2. Click Generate Mesh to see the mesh. Rotate and zoom into critical regions: fillets, holes and load faces.
3. Add a Local Mesh Control on faces, edges or bodies that matter: select the entities, drag the Mesh size slider between Fine and Coarse or type a Length (prefilled with the average global element size). One control holds one size; use several controls for several sizes. The mesher transitions gradually between local and global size.
4. Regenerate the mesh and check the element count. Aim for a solve you can repeat many times; use local controls instead of shrinking the global size.
5. Run the study. Note peak stress, displacement and the number of elements.
6. Refine (reduce the local size or enable adaptive refinement), solve again, and compare. Autodesk describes convergence as the stress change between two successive meshes becoming insignificant (it says, for example, less than 1% or 2%).
7. Record the converged mesh settings in the study notes.

Options reference#

Mesh Settings dialog (Autodesk's numerical settings and recommended ranges):

Mesh options (checkboxes):

Other mesh tools:

Adaptive Mesh Refinement custom settings: Maximum Number of Mesh Refinements (takes precedence over the tolerance; Autodesk notes good results are generally achieved in fewer than 8 steps), Results Convergence Tolerance (%), Portion of Elements to Refine (%; not applicable to modal frequencies), Frequency Mode (modal frequencies only), and Results for Baseline Accuracy (von Mises Stress is the default; 1st Principal Stress, 3rd Principal Stress, Displacement Total, Heat Flux or Temperature depending on study type).

Tips and pitfalls#

Tip: Peak stress at a sharp corner never converges because of the singularity. Check convergence at a location with finite theoretical stress, such as a fillet's mid-arc, and judge displacement and stress away from singular points.

Tip: Remove tiny features (small fillets, logos, threads) from the analysis copy. They force very small elements and rarely affect the global answer.

Warning: Distorted or sliver elements make the solver unstable. If the mesh fails, inspect the geometry for slivers, tiny faces, or self-intersections, then simplify.

Tip: Thin parts in bending need several elements through the thickness. Autodesk gives a rule of thumb of at least four linear elements, or two parabolic elements, through the thickness where bending stress reverses; where stress is mostly membrane (tensile or compressive) one element may be adequate. Use local mesh control to reach that count without a huge total element count. Shell elements are not supported in Fusion.

Warning: Large meshes take longer to solve and Autodesk may limit the maximum study model size; the token cost per study is fixed by study type, not by element count. Test your mesh at low resolution first and compare element counts before submitting.

Tip: Two meshes giving similar displacement but different peak stress is common. Displacement converges faster than stress.

Practice exercise#

Make a plate with a 10 mm hole in a 100 mm wide plate, pull on the ends. Solve with three global sizes (10 mm, 5 mm, 2.5 mm) and record the peak stress at the hole. Then add a local control of 1 mm at the hole edge with the coarse global size. Expected result: peak stress converges toward roughly three times the nominal stress (the classical concentration factor for a small hole in a wide plate, which is general engineering knowledge rather than Autodesk data); the local control gets there with far fewer elements than global refinement.

Worked example: convergence table for a plate with a hole#

A 100 mm wide, 5 mm thick aluminium plate with a central 10 mm hole, pulled by 10 kN total (nominal net-section stress = 10000 / ((100 - 10) x 5) = 22.2 MPa; gross-section stress = 20 MPa). The theoretical concentration factor for a hole-to-width ratio of 0.1 is about 2.7 on the net-section stress, giving a peak near 60 MPa. A convergence table looks like this:

These numbers are hypothetical and were not produced by Fusion or taken from Autodesk; they only illustrate the pattern: a coarse mesh underpredicts the peak, and local refinement converges with fewer elements than global refinement. Record your own table the same way and stop when the change falls below your tolerance, here 2 percent.

Choosing element size from geometry#

The table is general meshing practice, not Autodesk data (except the through-thickness rule quoted above and the guidance to avoid very small holes under 1/100 of part length).

For the plate above, the hole circumference is 31.4 mm; for a local size of 1 mm that gives about 31 elements around it.

Element order and the cost of accuracy#

Linear tetrahedra have four nodes; parabolic tetrahedra add a midside node on each edge (ten nodes) and can follow curved stress fields with fewer elements. General rule of thumb (not Autodesk data): halving the element size multiplies the number of elements by about 8 in 3D. Curved mesh elements are only possible for parabolic elements. Autodesk notes that an overly coarse mesh generally underpredicts stress, and that displacement is less sensitive to mesh than stress.

Adaptive refinement#

Adaptive Mesh Refinement lets the solver identify critical stress regions, remesh with smaller elements there and repeat the solution until the result change between two consecutive iterations is below the Results Convergence Tolerance, or until the Maximum Number of Mesh Refinements is reached. It is essentially an automated mesh convergence study. Advantages: saves manual refinement effort. Disadvantages: more solve passes. Set a modest Maximum Number of Mesh Refinements (Autodesk says fewer than 8 is generally enough) and check the final element count against your budget. If the refinement concentrates at a sharp corner, that is probably a singularity: fillet rather than refine.

Mesh quality indicators#

Autodesk's Mesh quality page lists these characteristics:

Poor elements cluster at tiny faces, short edges and slivers. Fix by cleaning up or simplifying the geometry in Simplify, deactivating Create Curved Mesh Elements, or using Use Part Based Measure for Assembly Mesh when part sizes differ widely.

Verification approaches beyond refinement#

1. Compare displacement with a hand calculation; displacement converges faster than stress.
2. Check the reaction force balance at each mesh.
3. Base stress convergence on a consistent location of the original geometry (Autodesk advises against using only the maximum stress, since it moves between meshes).
4. For stress, look away from singularities and compare with a nominal stress.

Failure modes and fixes#

Practice exercise#

Record a convergence table.

1. Build the 100 x 5 mm plate with the 10 mm hole and pull with 10 kN.
2. Solve with three global sizes (for example 10, 5 and 2.5 mm, set via Average Element Size); record element count and peak stress at the hole edge in a table.
3. Reset to 5 mm global and add local sizes 2, 1 and 0.5 mm at the hole edge; record again.
4. Plot stress against element count and decide where the curve flattens. Compare the converged peak stress with 2.7 x 22.2 = 60 MPa.
5. Repeat on a plate with a sharp-cornered square notch instead of a hole and note that the peak stress keeps rising, the signature of a singularity.

Related#

• Static Stress Study
• Results Interpretation
• Cloud Solve and Credits