FEM Model Review Checklist

That's right. It's a list for systematically verifying mesh quality, boundary conditions, material properties, and load conditions as part of FEM model quality assurance, before executing the analysis. NASA's "FEM Best Practices" (NASA-STD-5002A) specifies a 35-item checklist, and structural analysis in aerospace must always go through this.

Unfortunately, in many workplaces, it tends to become "generate the mesh, throw it to the solver, and if it converges, it's OK." But in reality, converged ≠ correct results. For example, in automotive crash simulation, it's not uncommon to approximate bolt connections with Tied Contact without verification, leading to results that don't match physical tests at all.

Even in your own team, creating a minimum checklist and making reviewer sign-off mandatory is a best practice. Having another engineer review, not the analyst themselves, prevents mistakes due to assumptions.

They can be broadly divided into 6 categories:

1. Mesh Quality Check — Metrics like aspect ratio, skewness, Jacobian, etc.
2. Boundary Condition Verification (BC Verification) — Validity of constraints, presence of over-constraint
3. Material Property Verification — Values of Young's modulus & Poisson's ratio, consistency of unit system
4. Load Condition Review — Comprehensiveness of load cases, basis for load values
5. Free-Free Mode Check — Verify connectivity with unconstrained modal analysis
6. Reaction Force Balance Check — Confirmation of $\sum F = 0$, $\sum M = 0$

Of course. Many check items have quantitative criteria. For example, the reaction force balance check is evaluated using the following formula:

This $\varepsilon_{bc}$ being below 0.1% is the general passing criterion. Furthermore, moment equilibrium is also checked:

Exactly. For example, when a concentrated load $P$ is applied to the free end of a cantilever beam, the reaction at the fixed end should be $R_y = P$ (force equilibrium) and the reaction moment should be $M = P \cdot L$ (moment equilibrium). This is verified in the FEM output. If the values are off, there is likely a mistake in boundary condition setup or a missing load definition somewhere.

Regarding mesh quality, consider the global stiffness equation:

This stiffness matrix $[K]$ is assembled from each element's stiffness matrix $K_e$. Element stiffness is calculated via numerical integration:

Here, $|J(\xi_g)|$ is the Jacobian determinant. When an element is distorted, the Jacobian deteriorates, and integration accuracy drops. That's why we check the Jacobian ratio in mesh quality checks. If a negative Jacobian appears, that element is inverted and physically meaningless.

It's detailed in NASA-STD-5002A "Structural Analysis and Test Requirements" and its supplementary document NASA-HDBK-5014. Summarizing the main items by category:

Absolutely. Many industries like automotive, nuclear, and medical devices also create their own checklists referencing NASA's framework. For example, automotive has similar requirements in the Euro NCAP crash analysis guidelines. The key is to identify "where the highest risk lies in your own analysis" and create a checklist focused on that.

There are 5 main quality metrics. These are common regardless of solver:

Good question. Realistically, the guideline is that over 99% of elements meet the criteria. If NG elements exist, confirm that those elements are not in the region of interest (stress concentration area, failure evaluation area). If NG elements are in the area where stress is reported, those results are not reliable.

In practice, outputting a "quality histogram" and checking the distribution is standard. In Hypermesh, you can see it instantly in the Quality Index panel; in Ansys, use Mesh Metrics.

Boundary conditions are the area with the most mistakes in FEM analysis. Always check the following:

• Presence of Over-constraint: For 3D solid statically determinate problems, constraints are basically 6 DOFs (3 translation + 3 rotation). Constraining more than that generates artificial stresses.
• Location and Direction of Constraints: Is the inner surface of a bolt hole fixed when the outer surface should be? Is the cylindrical coordinate system set correctly?
• Validity of Symmetry Conditions: Are out-of-plane displacements constrained on symmetry planes? For anti-symmetric loads, are anti-symmetric BCs applied?
• Validity of Contact Definitions: Selection of master/slave surfaces for Tied/Bonded contact, setting of friction coefficients.

That's a common misunderstanding. Over-constraint inhibits the deformation the structure inherently possesses, calculating stresses that do not exist in reality. For example, if both ends of a thermally expanding pipe are fixed in all DOFs, huge fictitious stresses appear at flanges that would actually slide. The result is judged "dangerous," but in reality, it's not a problem at all — this is a false positive and distorts design judgment.

Exactly. It's a test where you perform a modal analysis (eigenvalue analysis) without applying any boundary conditions. There are three purposes:

1. Model Connectivity Verification: If all parts are correctly connected, there should be only 6 rigid body modes (3 translation + 3 rotation). If 7 or more appear, some part is floating (connection missing).
2. Confirmation of Rigid Body Mode Frequencies: The natural frequencies of the 6 rigid body modes are theoretically zero. In FEM, they aren't exactly zero due to numerical error, but $f_{rigid} < 0.01\,\text{Hz}$ is a guideline. If above 1Hz, there's a problem.
3. Confirmation of Mass Validity: Look at the 7th and subsequent elastic mode shapes from the Free-Free analysis and check if the deformation patterns are physically reasonable.

It happens all the time in practice. Especially with assembly models with 100+ parts, if there's even one missing Tied Contact definition, that part just floats. In static analysis, it might stop with a "singular matrix" error, but depending on the load case, it might coincidentally converge. The Free-Free check is a very powerful method to expose such "silent defects" beforehand.

The method is simple. In Nastran, use SOL 103 with no SPC specified; in Abaqus, use a *FREQUENCY step with no BC. The computational cost is less than 1/10th of a normal analysis.

More than the values themselves, consistency of the unit system is the scariest. The most common fatal mistake in practice is "getting the unit of Young's modulus wrong." For example:

If you get the density wrong, inertial forces, gravity loads, and natural frequencies all go haywire. In static analysis without gravity, you might not notice, but in dynamic or modal analysis, the results become orders of magnitude wrong. The checklist verifies the following:

• Record the source of input material properties (handbook name, test report number).
• Calculate the model's total mass and compare it with the actual weight (within 2% error is a guideline).
• For temperature dependency, check if data for the operating temperature range is correctly input.
• For composite materials, check if the lamination sequence and fiber orientation angles match the design drawings.