Beyond converging internal loads, HyperFEA is used to enforce and satisfy global model constraints that individual Zone sizing cannot address alone. During iteration, limits can be placed on nodal deflection, buckling, natural frequency, and static moment in the form of Global FEA Constraints.
FEA Constraints work by translating global phenomena in to local, Zone-level Stiffness Requirements.
Using the wind blade below as an example: a global tip deflection target has been translated into local, Zone-level stiffness requirements along the spar cap - as illustrated by opening each Zone's Panel Settings form. These stiffness requirements become Failure Criteria that the sizing of each Zone must meet in order to have positive margins of safety.
HyperX provides two approaches for enforcing FEA Constraints: Automated and Manual.
-
Automated Constraints - Here, HyperX automatically identifies the most efficient stiffness path and corresponding Zones to adjust based on the strain energy distribution, calculated from element forces. This is the recommended approach, especially for more complex models, because it finds the optimum stiffness distribution with minimal user setup and tuning.
Tip
This algorithm underwent extensive updates prior to the release of version 2026.1, particularly to address Global Buckling Eigenvalue Requirements. It is now the recommended approach for enforcing FEA Constraints in HyperX.
-
Manual Constraints - In this approach, the user explicitly defines which Zones and specific stiffness terms (e.g., membrane vs. bending) to adjust to address a given constraint. This is the legacy approach to enforcing FEA Constraints. While typically more stable and faster to converge, this approach requires significant user expertise for setup and tuning to achieve a mass-efficient solution.
Incorporating Global FEA Constraints in to your HyperFEA iterations requires:
-
Relevant FEM/Results Files must be added to the Project. For example, if implementing a Global Buckling Constraint, ensure that buckling load case(s) and corresponding results have been included.
-
Manual FEA Constraints require displacements in the FEA results files for the Design Load Case of interest. Automated FEA Constraints require displacements AND element forces in the FEA results for the Design Load Case of interest.
-
-
Stiffness Requirement Failure Mode must be added to the Analysis Property of any Zone that could be sized by the constraint.
This is the mechanism by which the local, Zone-level stiffness requirements are able to drive Sizing. See Stiffness Requirement Methods for more information on how the margin check(s) work.
-
Set(s) should be created to collect any Zone that you would like the constraint to apply to. If a Set is provided, HyperX will only "look at" those Zones when enforcing Stiffness Requirements. For example, to drive out buckling modes by only sizing the stiffeners (not the skins) of a panel, create a Set of the bar elements in the panel.
Note
This step is required by the Manual Constraint approach. It is optional if using Automated Constraints.
There are additional setup steps required depending on the type of problem (displacement/rotation, buckling, frequency, or static moment) and the type of constraint (automated vs manual). This information can be found on either the Automated or Manual constraint page for each problem type.
Use Two-Stage Iteration to Converge Loads
Depending on the initial state of the FEM, it is possible to have very large changes in model stiffness during the first few HyperFEA iterations. This is common if there is a change between two panel concepts with very different ratios of bending to membrane stiffness. An example is using solid laminate in the initial FEM, then changing many Zones to a sandwich concept. Another scenario is where the initial FEM has a boilerplate/uniform initial thickness but actually requires a very non-uniform stiffness distribution once sizing has been performed.
In these scenarios, it is recommended to use the “No FEA constraints in first stage” setting on the Convergence Criteria. This allows for the load path to converge prior to enforcing FEA Constraints in order to prevent the two from conflicting.
Use Two-Stage Iteration for Localized Buckling Problems
In scenarios where the critical FEA buckling modes are similar in size to panel buckling modes, it can be helpful to rely on HyperX analytical buckling methods to get panel stiffness in the right “neighborhood” to meet the FEA buckling eigenvalue requirement. This avoids costly FEA runs and can also result in an overall superior solution.
First, ensure that an Analysis Property containing panel buckling failure modes is applied to the necessary Zone(s).
Tip
It is recommended to set the required margin to -0.25 on these criteria to ensure the analytically-sized solution is in the ballpark, but does not overshoot the eigenvalue target.
Then, on the Convergence Criteria form, use the “Analysis Criteria Settings” selection to specify that the panel buckling criteria are deactivated on the 2nd stage.
With this setup, Sizing (without the FEA Constraint) will find designs in the 1st stage that provide a panel buckling margin of at least 75% of the target eigenvalue. In the 2nd stage, the HyperX panel buckling methods will be switched off and the FEA Buckling Constraint will become active and drive the solution towards the target buckling eigenvalue.
Tip
Follow the HyperFEA Click-Along Training Example to see an example using this approach.
Adjust Zones Modified by FEA Constraints
With both Automated and Manual FEA Constraints, the user has the ability to dictate which Zones will receive stiffness constraints during the HyperFEA process by specifying a Set of zones on the corresponding Constraint setup form. This approach can be helpful to prevent specific parts of the structure from being modified to meet the FEA Constraint. Additionally, it can be a useful tool for steering the FEA Constraints to a better solution.
For example, a wing box with a tip displacement constraint will benefit the most from stiffening up the skins and spar caps. In this scenario, it would be beneficial to create a Set with these Zones, then point to that Set on the Constraint form.
In the case of Automated Constraints, the algorithm is able to determine the most efficient part of the structure to stiffen usi9ng the strain energy distribution. However, prescribing a certain Set of Zones can be useful to encourage a quicker convergence - for example, if one portion of the structure dominates the response of interest, such as with discrete stiffeners in the case of buckling on a flat panel.
Adjust Stiffness Terms Modified by FEA Constraints
With both Automated and Manual FEA Constraints, the user has the ability to dictate which stiffness terms will receive Constraints during the HyperFEA process. By using engineering judgement to directly specify which stiffness terms should be adjusted to meet the constraint, each algorithm can likely converge on a solution more efficiently. For example, a wing box with a tip deflection constraint would only need membrane stiffness in the span-wise direction (for the skins) and shear stiffness (for the spar webs) active. Bending stiffness terms would not have a significant impact in this type of structure and constraint scenario. Conversely, with a problem such as buckling of a rib, stiffening the bending terms is the more efficient approach (to drive, for example, the height of a panel, rather than just the thickness).
The method by which this is accomplished is different between the two Constraint types.
-
For Manual Constraints, this is done by adjusting the stiffness term selection directly on the Constraint form.
-
For Automated Constraints, this is done by selecting/de-selecting failure criteria on the Stiffness Requirement Failure Mode.