FEMgen is accessed from the Advanced Settings form, which is found on the Database tab of the Ribbon, as shown below.
Select the HyperFEMGen tab on the resulting form.
To activate FEMgen, set the FEMgen Create option to "Yes." The next time a Zone (or selection of Zones) is Sized, the optimum candidate design(s) will be applied to the automatically generated finite element input files. You must also select the FEM type (Nastran vs. Abaqus), as well as the solution type.
A full list of inputs that must be given is shown below:
-
Set FEMgen Create = Yes.
-
Set either FEMgen Nastran or FEMgen Abaqus = Yes.
-
Set either FEMgen Static Solution or FEMgen Buckling Solution = Yes.
The remainder of the FEMgen options are set by default to values that tend to work for most common use cases. However, for a better understanding of each option, see the summary section below.
HyperFEMgen Options
-
FEMgen Create - [Boolean] Flag to enable HyperFEMgen. A FEM will be generated for every Zone analyzed. FEM input files are located in the Project Working Folder (typically C:\HyperX\Project\Temp\ProjectName\FEM).
-
FEMgen Smeared Properties - [Boolean] If True, generate smeared plate model using ABD matrix output. If False, generate stiffened panel model with discretely meshed stiffeners.
-
FEMgen NE_Smeared - [+Int] Number of elements across the Y Span of the smeared plate model.
-
FEMgen Minimum Segment - [+Int] If 0, use NE parameters to specify the number of elements across the cross-section edge of each object. If > 0, then value specifies the minimum number of elements across the shortest cross-section edge.
Tip
Use the minimum segment option to quickly generate HyperFEMgen meshes.
-
FEMgen NE_Skin - [+Int] Number of elements across the cross-section edge of the open span (skin) object. Overridden if minimum segment > 0.
-
FEMgen NE_Skin_Hat - [+Int] Number of elements across the cross-section edge of the skin object underneath the stiffener of a corrugated panel. Overridden if minimum segment > 0.
-
FEMgen NE_Bond - [+Int] Number of elements across the cross-section edge of the bonded combo. Overridden if minimum segment > 0.
-
FEMgen NE_BS - [+Int] Number of elements across the cross-section edge of the bonded combo and open span region. This parameter is used only if NE_BS > NE_Skin + NE_Bond. Overridden if minimum segment > 0.
-
FEMgen NE_Web0 - [+Int] Number of elements across the cross-section edge of the web for uniaxial and corrugated stiffened panels. Overridden if minimum segment > 0.
-
FEMgen NE_Web90 - [+Int] Not supported in HyperSizer v7.1.
-
FEMgen NE_Frame_Flange - [+Int] Number of element across the ringframe flange.
-
FEMgen NE_Flange - [+Int] Number of elements across the cross-section edge of the bottom flange and crown for uniaxial and corrugated panels respectively. Overridden if minimum segment > 0.
-
FEMgen Element Aspect Ratio - [+Real] Desired element aspect ratio (length/width) of all skin objects.
-
FEMgen Number of Stiffeners (0 = All) - [+Int] If 0, mesh all stiffeners in panel dictated by the Y Span. If > 0, value dictates number of stiffeners to be meshed (may not exceed number of actual stiffeners).
-
FEMgen Static Solution - [Boolean] Flag to enable generation of linear static run deck based on controlling load case.
-
FEMgen Buckling Solution - [Boolean] Flag to enable generation of Eigenvalue buckling run deck based on controlling load case.
-
FEMgen Midplane Laminates - [Boolean] If True, no shell offsets are used. If False, shell offsets are used.
Note
Shell offsets may effect accuracy of Nastran Eigenvalue buckling solution.
-
FEMgen Pressure Boundary Condition - [Boolean] Not used.
-
FEMgen Repeating Bays - [+Int] If 1, only single panel bay is meshed (length = X Span). If > 1, multiple bays are meshed along the length of the panel.
-
FEMgen Ringframes - [Boolean] Flag to add beam and shell elements along the bay edges to simulate ringframes.
-
FEMgen Ringframe Flange Width (in) - [Real] Width of ringframe flange.
-
FEMgen Cutout Min X - [Real] X1 coordinate of rectangular cutout.
-
FEMgen Cutout Max X - [Real] X2 coordinate of rectangular cutout.
-
FEMgen Cutout Min Y - [Real] Y1 coordinate of rectangular cutout.
-
FEMgen Cutout Max Y - [Real] Y2 coordinate of rectangular cutout.
-
FEMgen Flat Panel Symmetric Y Edge - [Boolean] If True, add symmetric boundary conditions to Y Edge. If False, add simple supports to Y Edge.
-
FEMgen Flat Panel Pinned Stiffener - [Boolean] If True, add y-constraints to stiffener edges. If False, add z-constraints to stiffener edges.
-
FEMgen Nastran - [Boolean] Flag to enable generation of Nastran models.
-
FEMgen Abaqus - [Boolean] Flag to enable generation of Abaqus models.
-
FEMgen Properties - [0, 1, 2] If 0, average material stiffness properties used. If 1, compression material stiffness properties used. If 2, tensile material stiffness properties used.
It should also be noted that there are two different techniques to meshing that can be enforced by HyperFEMgen: Direct and Minimum Segment. These are summarized - along with their corresponding option selections - in the dropdown section below.
Meshing Parameters
FEMgen has two basic modes for meshing: Direct and Minimum Segment.
Direct Mode
The Direct Mode is active if FEMgen Minimum Segment = 0.
In the Direct Mode, the user specifies the number of elements spanning the width of each object (flange, web, etc.). A global element aspect ratio is used to define the length of each element.
The first figure below shows the meshing parameters for a typical uniaxial panel. NE refers to the number of elements in the direction specified by the arrows. This is the y-direction for all objects except the web.
You will notice that the stiffener spacing span appears redundantly defined. NE_BS and NE_Bond+NE_skin parameters both define the number of elements across the spacing span. The code takes the smaller of the two sets.
I Stiffened Example – Direct Method 1
NE_BS is overridden because NE_Skin + NE_Bond specified a smaller mesh size.
I Stiffened Example – Direct Method 2
NE_BS is now controlling.
Minimum Segment Mode
Minimum Segment Mode is active only if FEMgen Minimum Segment > 0.
In the Minimum Segment Mode, the user simply specifies a number of elements spanning the width of the smallest object. The resulting mesh size of the minimum span is used as a starting point for the rest of the objects. Again, the element aspect ratio is used to define the length of each element.
I Stiffened Example – Minimum Segment Method
The Minimum Segment Method is now active (FEMgen Minimum Segment = 4). All other parameters are ignored except for the element aspect ratio (also set to 4 in this example). The free flange is the minimum segment with four elements across the width. This element size then propagates to the other objects.
Observe that you can get a very uniform mesh with little effort using this method.
Once the HyperFEMgen options are set, run Sizing. Once the optimization is complete, HyperFEMgen will create a FEM input file corresponding to the optimum candidate selected by each Zone. This will result in one FEM file for each Zone that was run.
The finite element input files are placed in the Project Working Folder inside a folder directory named "FEM." The Project Working Folder can be opened directly from the HyperX interface, as shown below:
The figure below shows what a typical FEM directory looks like after a FEMgen model has been created. In this example, both Nastran and Abaqus files were generated. The name of each FEM is the Project name (spaces replaced by underscores) with the Zone number attached.
The files with no suffix after the Zone's number are the model files. These contain all the Materials, Properties, Nodes, Elements, and Node Sets. Files with suffixes are the analysis files. The analysis files contain the appropriate loads, boundary conditions, and default solution controls as well an include statement referencing the model file.
-
Static – Linear static analysis.
-
Eigen – Linear eigenvalue analysis. Default 5 eigenmodes.
-
PostBuckle – Geometric nonlinear analysis. Artificial damping applied. (Abaqus only.)