How to Perform a Mesh Convergence Study in ANSYS Mechanical

How to Perform a Mesh Convergence Study in ANSYS Mechanical

A stress result that looks correct on screen is not the same as a stress result you can trust. Colour contours render whether the mesh is adequate or not — the software will not warn you that your peak von Mises stress is 40% too high because of a coarse mesh near a fillet. The only way to know your result has actually converged on the true solution is to run a structured mesh convergence study. This guide walks through the process in ANSYS Mechanical, from setting up refinement levels to applying Richardson extrapolation and the Grid Convergence Index (GCI).

Key takeaways

• A single mesh, however fine it looks, proves nothing about accuracy on its own
• Convergence studies need at least three systematically refined meshes, not two
• Track a scalar result at a specific location (e.g. peak stress at a fillet), not an average
• Richardson extrapolation estimates the "true" mesh-independent answer
• The Grid Convergence Index (GCI) quantifies how far your finest mesh still is from that answer
• Singularities (sharp re-entrant corners, point loads) never converge — recognise them rather than chase them

Contents

1. Why mesh convergence matters
2. Setting up a convergence study in ANSYS Mechanical
3. Choosing a refinement strategy
4. Tracking the right result
5. Richardson extrapolation and the GCI method
6. Common pitfalls and singularities
7. Practical workflow summary
8. FAQ

1. Why mesh convergence matters

Finite element results are approximations built on a discretised geometry. As the mesh is refined, the numerical solution approaches the exact mathematical solution of the underlying equations — but it rarely gets there in one step, and it never gets there by guesswork. A mesh convergence study is the evidence that your reported number (a stress, a deflection, a natural frequency) is a property of the physics, not an artefact of element size.

Note: Convergence behaviour differs by result type. Displacement and total deformation converge quickly because they come from the stiffness matrix directly. Stress and strain, which are derived by differentiating displacement, converge far more slowly and need a finer mesh in the region of interest.

2. Setting up a convergence study in ANSYS Mechanical

ANSYS Mechanical offers two practical routes: manual h-refinement across a sequence of saved mesh configurations, or the built-in Convergence tool attached to a result object.

Option A — Manual refinement sequence

1. Build the geometry and apply loads/boundary conditions once; do not change them between runs.
2. Generate an initial coarse mesh using a global element size, and solve.
3. Duplicate the model (right-click the Model cell in Workbench), halve the element size in the region of interest using Mesh Sizing or Face/Edge Sizing controls, and re-solve.
4. Repeat for a third, finer mesh. Three data points are the practical minimum for extrapolation.

Option B — Built-in Convergence object

1. Insert the result of interest (e.g. Equivalent Stress) under the Solution branch.
2. Right-click the result → Insert → Convergence.
3. Set an allowable change (commonly 5–10% for a first pass, tighter for critical components).
4. Solve — ANSYS will automatically refine the mesh near the tracked location across iterations and report the change between steps.

Tip: The built-in Convergence tool is convenient but treats each refinement as a black box. For a defensible, published-quality study — or a client deliverable — run the manual sequence so you control element size ratios precisely and can compute the GCI yourself.

3. Choosing a refinement strategy

Global refinement (shrinking the element size everywhere) is the most rigorous approach because it changes only one variable. In practice, most engineers use local refinement — sizing controls, sphere of influence, or curvature/proximity sizing — concentrated on the region of interest, since refining the entire model to the same density as a stress hot-spot is often computationally wasteful.

Whichever approach is used, keep the refinement ratio between successive meshes consistent. A commonly used target is a linear element-size ratio of around 1.3–2.0 between coarse, medium and fine meshes; this keeps the extrapolation math well-behaved.

Grid refinement ratio between mesh levels:

r = h_coarse / h_fine

4. Tracking the right result

Convergence must be judged on a single, well-defined scalar — not on "the contour plot looking stable." Good choices:

• Maximum equivalent (von Mises) stress at a specific, named location (e.g. fillet root)
• Directional deformation at a probe point
• First natural frequency, for a modal study
• Reaction force at a support, as a sanity check independent of mesh density

Watch out: Never track "maximum stress in the model" without specifying where. As the mesh refines, the location of the reported maximum can jump around the model, especially near contact edges or load application points, making the trend meaningless.

5. Richardson extrapolation and the GCI method

With three results (f₁ finest, f₂ medium, f₃ coarsest) and a consistent refinement ratio, Richardson extrapolation estimates the value the solution is converging towards as element size approaches zero.

Observed order of convergence:

p = ln[(f₃ − f₂) / (f₂ − f₁)] / ln(r)

Extrapolated (mesh-independent) value:

f_ext = f₁ + (f₁ − f₂) / (r^p − 1)

The Grid Convergence Index expresses the uncertainty of the finest mesh result as a percentage band around that extrapolated value:

GCI = F_s · |ε| / (r^p − 1)

where ε = (f₁ − f₂)/f₁ and F_s is a safety factor (commonly 1.25 for a three-mesh study).

A GCI below roughly 1–3% for the finest mesh is generally considered acceptable for engineering decision-making; tighter bands are appropriate for fatigue-critical or certification work.

Tip: Plot the tracked result against 1/element-size (or number of elements) on a simple line chart. A converging study shows the curve flattening and approaching an asymptote — that asymptote, not the finest data point alone, is your best estimate of the true answer.

6. Common pitfalls and singularities

• Chasing a singularity: sharp re-entrant corners, point loads, and point supports produce theoretically infinite stress. Refining the mesh here will never converge — it will simply report an ever-increasing peak value. Recognise the geometry, not the trend.
• Changing more than one variable: switching element order (linear to quadratic) at the same time as refining size mixes two effects together and invalidates the extrapolation.
• Non-uniform refinement ratio: if the coarse-to-medium ratio differs from the medium-to-fine ratio, the Richardson formula above no longer applies directly.
• Ignoring solver settings: large deflection, contact stiffness, and nonlinear convergence tolerances should stay fixed across all mesh levels being compared.

Note: Where a true singularity exists, engineering practice generally moves to a stress-linearisation approach at a defined path (per pressure-vessel codes), or accepts a converged strain-energy or reaction-force result instead of a raw peak stress.

Fig. 1 — A properly converging result flattens toward an asymptote as mesh density increases; the gap between the finest mesh and that asymptote is what the GCI quantifies.

7. Practical workflow summary

1. Fix geometry, loads, boundary conditions, and solver settings across all runs.
2. Build coarse, medium, and fine meshes at a consistent refinement ratio.
3. Solve all three and record one scalar result at one named location for each.
4. Compute the observed order of convergence p and the extrapolated value.
5. Compute the GCI for the finest mesh and confirm it meets your accuracy target.
6. Report the finest-mesh result together with its GCI band, not as a bare number.

Related reading

• FEA in Product Design
• How CFD Can Reduce Energy Consumption in Fans, Ducts and Ventilation Systems
• CFD for Industrial Drying Systems

Frequently asked questions

How many mesh levels do I need for a convergence study?

Two data points only show a difference, not a trend. Three systematically refined meshes are the practical minimum, since they allow the observed order of convergence and an extrapolated value to be calculated. Four or more improves confidence further, particularly on nonlinear models.

What refinement ratio should I use between mesh levels?

A linear element-size ratio of roughly 1.3 to 2.0 between successive meshes is common practice. Very small ratios (close to 1) make the differences noisy relative to solver round-off; very large ratios can skip over the transitional convergence behaviour.

Why does my peak stress keep increasing no matter how fine the mesh gets?

This is the signature of a geometric or load singularity — a sharp re-entrant corner, a point load, or a point support. These locations do not converge in a classical finite element sense. Use stress linearisation at a defined path, fillet the geometry to a realistic radius, or track a converging quantity such as reaction force instead.

Does displacement need the same mesh density as stress?

No. Displacement is a primary solution variable and typically converges with a relatively coarse mesh. Stress and strain are derived from displacement gradients and need noticeably finer elements, especially in regions of high gradient such as fillets and holes, to reach the same level of accuracy.

Is the built-in ANSYS Convergence tool sufficient, or do I need to do this manually?

The built-in tool is a reasonable first check for routine work, since it automates local refinement and reports the change between iterations. For safety-critical components, published results, or client deliverables, a manual sequence with a calculated GCI gives a more defensible, quantified statement of accuracy.