Virtual Moments

To properly calculate consistent loads (see Loads Processing) and stiffnesses (See Stiffness Formulation) for each Zone, HyperX must assume a reference plane (the Analysis Reference Plane) in order to ensure the two are consistent. This is considered a setting that can be selected for each individual Zone on the Zone Settings form - launched from the right-click menu. See the Zone Settings section of Zones for more information.

Prior to that, the finite element model must also assume a reference plane for the FEA solve (the FEM Reference Plane). Resulting loads are calculated with respect to this plane. By default, the FEM Reference Plane is at the nodal plane but, it can also be offset from that nodal plane depending on the modeling strategy. See a summary on the different techniques for applying reference planes and offsets and how HyperX interacts with each in the Reference Planes and Offsets section of Shell Elements.

In short, there are many cases in which HyperX will automatically detect the FEM Reference Plane and ensure that the Analysis Reference Plane defined per Zone is the same. However, there are also cases (such as stiffened panel concepts, which always assume a Top-Face Midplane Reference Plane) in which the Analysis Reference Plane and the FEM reference plane are not consistent with one another. In cases where the FEM Reference Plane and the Analysis Reference Plane are not in-line with one another, HyperX will calculate the Virtual Moment required to properly shift the FEA loads to the correct Analysis Reference Plane.

A Virtual Moment, by definition, is the moment required to enforce the curvature = 0, otherwise known as "uniform end-shortening." It is an artifact of stress analysis that occurs when the HyperX-assumed Analysis Reference Plane (about which the load is applied and stiffness is formulated) isn’t aligned with the neutral axis of the panel (where the load would naturally occur) or the assumed FEM Reference Plane.

Take, for example, the axially-loaded I-stiffened panel below. By default, HyperX is always going to assume the reference plane of the stiffened panel (i.e. the location of the FEM nodes) to be the midplane of the top skin (as indicated in the figure). This is a convenient assumption for Sizing, as the cross-section of the panel (and, therefore, the panel neutral axis) is assumed to change for each candidate panel in the design space.

HyperX implements a Virtual Moment into the Zone stiffness (ABD Matrix) formulation by inducing a [B] ≠ 0 - similar to what you'd see for an unsymmetric laminate. The [B] ≠ 0 is the stiffness required to induce the necessary zero-curvature condition.

Virtual Moments are convenient in that they can accurately correct any reference plane shifts. However, it is important to understand Virtual Moments and the conditions in which they occur. If there are any reference plane inconsistencies between your FEM, your selected Zone Settings, and the Structure neutral axis, the calculated moments can cause additional, unnecessary weight to be added to your Structure during Sizing. The example below illustrates one of the most common examples that we see:

A Tale of Detrimental Virtual Moments

The most common Virtual Moment error among HyperX users:

1. The user imports FEM and all properties are midplane.

2. In HyperX, they either (1) updated the reference plane and/or (2) changed the panel concept. Now HyperX will simply move the load by formulating the ABD about the new reference plane, without applying the appropriate Mx, My, Mxy moments (because the Mx, My, and Mxy come from the FEA solve, not HyperX).

3. Now the panel has to size up due to fictitiously high bending strains.

Take the simple flat plate shown below.

• Applied Nx (lb/in) = -1000, Ny = Nxy = 0

  

• Edged fixed in rotation

  

• FEM sets the reference plane at the midplane. Z0 field in PCOMP card is blank. Defaults to Z0 = -1/2 thickness = midplane.

  

Upon import, HyperX will automatically set the panel reference plane to "Midplane" - verified on the Zone Settings form below.

The panel is Sized with a Laminate Family - for strength only (laminate OHC). HyperX will select the thinnest Laminate that attains positive margins. In this case, 7 plies (each with a thickness of 0.0055in). Both the Watch Window and the Analysis Watch Window are used to verify these results in the Viewport.

Now, the user shifts the reference plane to "bottom" - to represent an OML tooling surface.

Important

Now the HyperX-assumed reference plane is inconsistent with the initial FEM assumption. The current FEA loads have been generated with a Mx = 0 boundary condition at the midplane. HyperX is still applying these loads, AND the additional moment to shift the reference plane.

Analyzing the existing 7-ply design at the new reference plane results in considerably higher strains, thereby causing a severely negative strength margin.

There are two ways to correct this situation:

1. Update the Zone Settings to Zero Curvature (previously "Zero Out FEA Moments") (shown below). This option will tell HyperX to ignore the moments coming from the FEM (thereby only writing margins with respect to the Virtual Moment). See Zone Settings for more information.

   

   This results in a positive margin:

   

   Notice the new Mx of 19.25 in-lb/in (the result of shifting the load from midplane to the bottom of a 7-ply laminate, where each ply is 0.0055in thick).

2. Iterate with FEA. This option allows HyperX to push the updated reference plane back to the FEM definition, and then rerun the FEM to get consistent loads. Notice that in this simple example, iterating the FEA after shifting the reference plane results in the same Mx value that HyperX calculated as the Virtual Moment. See Iterating with FEA for more information.

   

Here are a few tips to help avoid misuse of Virtual Moments, as exemplified in the previous section: