Mesh Convergence (Mesh Convergence) — CAE Glossary
What is Mesh Convergence
My senior asked if I confirmed mesh convergence, but what is mesh convergence exactly? Does it just mean making the mesh finer?
Roughly speaking, it is the process of progressively reducing element size and verifying that the physical quantities of interest (stress, displacement, etc.) become essentially unchanged. In FEM and CFD alike, the mesh is an approximation of the continuous body, so if the mesh is too coarse, the solution becomes inaccurate. But if you make it too fine, computational time explodes. Mesh convergence study is the process of finding the right balance.
What is a case where this becomes a problem?
A common example is in stress analysis when you want to look at maximum stress in a fillet region. With a coarse mesh the stress might be 200 MPa, but when you refine the mesh by a factor of 2 the stress becomes 280 MPa, and when you refine further it becomes 310 MPa... and so on. In this situation we say "the solution has not converged." The value cannot be trusted for inclusion in a report.
So mathematically, as element size $h$ approaches zero, the true value is approached, right?
Exactly. Between the numerical solution $f_h$ and the exact solution $f_{\text{exact}}$ there is a truncation error relationship:
Here $p$ is the order of accuracy, and $C$ is a constant. As $h \to 0$, the error converges to zero—this is theoretically guaranteed. But in practice we cannot set $h=0$, so we need a method to determine "sufficient convergence" with a finite number of meshes.
Richardson Extrapolation
I've heard the name Richardson extrapolation before. Is it true that you can estimate the true value?
Not the exact true value, but rather an extrapolated solution, which is a better approximation of the true value. The concept is simple: from two or more solutions with different mesh sizes, we eliminate the truncation error term.
For instance, if solutions at mesh sizes $h_1$ and $h_2$ (where $h_2 < h_1$) are $f_1$ and $f_2$, and the accuracy order $p$ is known, then:
$$f_{\text{ext}} = f_2 + \frac{f_2 - f_1}{r^p - 1}$$Here $r = h_1 / h_2$ is the refinement ratio. $r=2$ (halving element size) is commonly used.
What if the accuracy order $p$ is unknown? Can we just set $p=2$ because we are using quadratic elements?
You can use the theoretical accuracy order directly, but in real problems the order often differs from theory due to boundary conditions, element distortion, and other effects. The best practice is to prepare three mesh levels (coarse, medium, fine) and measure $p$ directly. For mesh sizes $h_1 > h_2 > h_3$ with corresponding solutions $f_1, f_2, f_3$:
where $r = h_1/h_2 = h_2/h_3$ (when refined uniformly). Using this measured $p$ for extrapolation gives more trustworthy estimates.
Running the calculation three times seems like a lot of effort... Is it worth it?
It is effort, but it is literally "quality assurance for the numerical solution." In academic papers and corporate V&V (Verification & Validation) reports, claiming the reliability of results without Richardson extrapolation is difficult. In particular, the ASME V&V 20 standard requires Richardson extrapolation for quantifying numerical solution uncertainty as a matter of course.
GCI (Grid Convergence Index)
What is GCI? How is it different from Richardson extrapolation?
GCI (Grid Convergence Index) is an indicator of mesh convergence uncertainty proposed by Roache in 1994. Think of it as taking the Richardson extrapolation result and multiplying by a safety factor $F_s$ to create a confidence band on the error.
The GCI on the finer mesh side is:
$$\text{GCI}_{\text{fine}} = \frac{F_s}{r^p - 1} \left| \frac{f_2 - f_1}{f_2} \right|$$The safety factor is $F_s = 3$ for two-level comparison, and $F_s = 1.25$ when using three levels with Richardson extrapolation. So doing three levels properly means you can use a smaller safety factor, tightening the error band.
Can you give concrete numbers? Is there a pass/fail criterion for GCI?
There is no official passing threshold, but practical engineering intuition says:
- GCI < 1%: Excellent convergence. Sufficient for papers and standards compliance
- GCI = 1–5%: Acceptable from an engineering standpoint. Most real-world cases fall here
- GCI > 5%: Convergence still insufficient. Either refine mesh further or review the model
For example, in an automotive crash analysis, if deformation GCI is 2%, the judgment is typically "good enough." However, in nuclear safety applications where standards are stricter, <1% might be required.
I heard about checking whether the GCI result is "within the asymptotic range." What is that?
Good question. The asymptotic range is the region where the truncation error is dominated by the form $C \cdot h^p$, which is also where Richardson extrapolation becomes valid. The check is done using the ratio from three levels of GCI:
If this ratio is close to 1, you are in the asymptotic range (convergence is proceeding smoothly). Large deviations may indicate the mesh is still too coarse or there are singularities in the solution.
h-refinement and p-refinement
I heard there are two ways to refine: h-refinement and p-refinement. What is the difference?
Broadly there are two approaches:
- h-refinement: Reduce element size $h$, i.e., increase the number of elements. This is the most common method. When people say "refine the mesh," they almost always mean this.
- p-refinement: Keep element size the same but increase the polynomial degree $p$ of the shape function. This is like changing from linear to quadratic elements.
The more common in practice is h-refinement because any solver can do it simply by specifying element size. p-refinement is supported by some commercial solvers (e.g., StressCheck or NX Nastran p-elements).
Is there something called hp-refinement?
Yes. hp-refinement combines both methods: refine with h-refinement near singularities and with p-refinement in smooth regions. Theoretically this achieves exponential convergence, but implementation is complex and only a few solvers support it. It is active in research but not yet mature for widespread industrial use.
Convergence Study Procedure
Please walk me through the procedure for conducting a mesh convergence study step by step.
OK, here is the typical procedure:
- Decide on the physical quantities of interest — maximum stress, displacement, pressure loss, heat flux, etc. You can have multiple quantities, but be clear about what "convergence" means.
- Prepare three or more mesh levels — at least coarse, medium, and fine. The refinement ratio $r$ should be 1.3–2.0. $r=2$ (about 8× more elements) is ideal but $r \approx 1.5$ is more practical due to computational cost.
- Run calculations under identical conditions — keep boundary conditions, material properties, and solver settings constant. Only change the mesh.
- Compare results — tabulate the physical quantities and plot them against mesh size.
- Calculate Richardson extrapolation and GCI — measure the accuracy order $p$ and compute the extrapolated solution and GCI.
- Verify asymptotic range — check that the GCI ratio is close to 1.
- Document in report — record the mesh parameters used, result table, and GCI values.
Do you refine uniformly everywhere, or just in regions of interest?
Strictly speaking, uniform refinement everywhere is ideal. This ensures that coarse mesh in distant regions does not influence the results. But in practice, computational cost is a concern, so local refinement around regions of interest is common. In that case, you should separately verify that the coarse distant mesh has negligible influence.
When to Stop Mesh Refinement
I heard that in some cases, stress diverges indefinitely as you refine the mesh. What does that mean?
That is a case of stress singularity. Examples include sharp corners (R=0 fillet-less edge), concentrated load application points, and material interface endpoints. At such locations, stress theoretically becomes infinite, so as you refine the mesh, stress values climb without bound.
So mesh convergence study cannot be used at such locations? How do you judge?
The stress value at the singularity itself is mesh-dependent, so a "converged value" does not exist. There are several remedies:
- Evaluate stress away from the singularity (1–2 elements away, the influence diminishes)
- Use displacement or reaction force instead of stress (these converge even with singularities)
- Modify the model to remove the singularity (real parts don't have R=0 corners; add a fillet)
- Use fracture mechanics approach with stress intensity factor $K$
For cases without singularities, what is the practical criterion for stopping?
Here are practical stopping criteria:
- Change < 1–2%: If the change from the previous mesh is within 1–2%, this is usually sufficient from engineering perspective.
- GCI < 5%: GCI below 5% is acceptable in most industrial standards.
- Computational cost vs. other uncertainties: If doubling the mesh yields only 0.5% change, that computation time is probably smaller than other uncertainties (material property scatter, boundary condition uncertainty).
- Relationship to design safety factor: If design safety factor is 2.0 and mesh error is 3%, the mesh error is small relative to the safety margin and is acceptable.
The key is not to pursue zero error, but to ensure mesh error is negligible compared to other sources of uncertainty.
I understand now. Richardson extrapolation → GCI calculation → asymptotic range check is the standard systematic approach to quantitatively evaluate mesh convergence.
Perfect understanding. One more tip: NovaSolver's Mesh Convergence Calculator can do all these calculations automatically from your three results—Richardson extrapolation, GCI, and asymptotic range check in one go. No need to implement the formulas yourself. Give it a try.
Related Terms
- Richardson Extrapolation: A technique to estimate the true value by extrapolating from solutions at different mesh sizes
- GCI (Grid Convergence Index): An index of mesh convergence uncertainty proposed by Roache
- h-refinement: An approach to improve accuracy by reducing element size
- p-refinement: An approach to improve accuracy by increasing polynomial degree of shape functions
- Asymptotic Range: The region where truncation error is dominated by $O(h^p)$
- Stress Singularity: A location where stress theoretically becomes infinite; does not converge
- V&V (Verification & Validation): The process of verifying correctness of numerical solutions and validity of physical models
Precise understanding of CAE terminology is the foundation of effective team communication. — Project NovaSolver is committed to supporting the learning of practitioners.
Tell us about challenges you face with mesh convergence
Project NovaSolver aims to solve the challenges CAE engineers face daily—complexity of setup, computational cost, interpretation of results. Your practical experience drives better tool development.
Contact (Coming Soon)Related Topics
detail
error