Aerospace Composite Tools

Aerospace tools for working with composites.


PCOMP from CSV generates HyperMesh composite properties from data defined in a .csv file.

The required file format is shown in the table below. Layers of a property must share a single material ID and thickness. If this is not your use case, refer to Data I/O Spreadsheets for other options.

From the menu bar, click Aerospace > Composites > PCOMP from CSV. In the Import file field, browse to the appropriate file and then click Create.

Table 1. File Format
PCOMP ID Material ID Thickness Orientation              
1 1 0.01 -45 0 45 90 90 45 0 -45
2 1 0.01 0 90 0 90        
11 5 0.02 30 0 30          

Ply Geometry Smoothing

Ply Geometry Smoothing provides functionality to smooth finite element ply shapes, usually generated from concept level composite freesize optimization, and to generate geometry from finite element ply shapes.

  1. From the menu bar, click Aerospace > Composites > Ply Geometry Smoothing.
  2. Select the FE ply to be converted into geometry shape.
  3. Choose the location where geometry should be placed.
    • Original component
    • Separate component for each ply
  4. Select either line or surfaces geometry to be exported as step files.
  5. Set Smooth Iteration to zero if the exact shape is to be preserved without smoothing the boundary. Otherwise, use 10-20 for the iteration.
  6. If you would like to define small holes to be filled, patched, or removed from the ply, set small region to one of the following:
    • Area Ratio – ratio of small region area to laminate area
    • Element Count – number of elements that define the small region
  7. To generate new plies if the input ply is made up of multiple separate regions, select Split disconnected ply regions into separate new ply entities.
  8. Update ply element sets by selecting one of the following:
    • Unchecked – generates requested geometry for ply but does not change element set assigned to input ply.
    • Checked – in addition to generating requested geometry, a new element set that reflects smoothing is created and assigned to input ply.
  9. Provide the step file name.
    Geometry plies are created and exported to step files.

    Figure 1. Result of Smoothing with Iterations = 0

    Figure 2. Result of Smoothing with Iterations = 20

Ply Auto Rename

Ply Auto Rename changes ply names so that the assigned material, thickness and angle are appended.

From the menu bar, click Aerospace > Composites > Ply Auto Rename.

The initial model will have the original ply names imported from CAD, as shown below.

Figure 3. Ply Names as Defined in the CAD System
After running this utility and selecting all of the plies to be renamed, the material name, thickness and angle are appended, as shown below.

Figure 4. Updated Ply Names

FE Absorb Plies

FE Absorb Plies generates a ply-based model from zone-based properties.

Entities that are created are laminates, plies, and template properties.

Exact conversion of the zone-based model to ply-based model depends on the existence of global ply ID’s/name’s on the zones, for example PCOMPG instead of PCOMP. FE Absorb Plies will still run with zones that do not have global data, for example PCOMP, but the conversion relies on internal logic to determine how to connect plies from zone to zone.

Figure 5.
  1. From the menu bar, click Aerospace > Composites > FE Absorb Plies.
  2. Import zone-based models with zone-based solver properties.
    These FE models do not have any plies or laminates. The goal is to create plies and laminates from the zone-based solver properties.

    Figure 6. No Plies or Laminates are in the FE Model
  3. Select all of the zone-based solver properties which will be used to generate the ply-based model.
  4. If you are using OptiStruct, select Update TMANUF of ply so that zone layer thickness is copied to PLY card TMANUF (used for sizing optimization).
  5. If a zone ply shape has multiple disconnected regions, generate multiple plies, one for each disconnected region, by selecting Split disconnected ply regions into separate new ply entities.
    After the conversion, laminates and plies are created. However converting a zone-based model to a ply-based model is not deterministic if global IDs or names are not defined in the properties. Many possibilities exist, especially the laminate stacking order. You are advised to check the laminate and reorder, if necessary.

    Figure 7. Ply, Laminate and PCOMPP are Created in the Model after FE Absorb

Material Orientation

The Material Orientation tool provides several methods of assigning material x directions for shell and solid elements, and additionally z directions for solid elements.

From the menu bar, click Aerospace > Composites > Material Orientation.
Restriction: This tool is applicable for shell element only.
  1. Select the Entities on which to assign material orientation, either Elements or Properties.
  2. Set the Color of orientation vectors drawn after applying material orientation.
  3. To set the scale of orientation vectors drawn after applying material orientation, set Scaling Option to Auto or Manual.
  4. Type a value into the Size field for the manual input for size of orientation vectors drawn after applying material orientation.
  5. Set the X direction method. Choose from the following:
    • Curve – spatially map input curve(s) as the x direction
      • Lines/Edges – lines which define the orientation
      • Flip direction – for lines/edges only. Determines whether the curve provided is +x direction or -x direction.
      • Nodes – list of lines that define the orientation
    • System ID – system assigned as orientation
    • System Axis – system and axis of system to map as x direction
    • Angle – for OptiStruct and Nastran only. Directly enter rotation applied on THETA field of element.
  6. Set a value for Normal by choosing one of the following:
    • Element Normal – uses element z direction (can be viewed from 2D > composites > element normals panel if elements are selected). Typically, this option should be used.
    • Surface Normal – aligns material z direction spatially to selected surface.

By Curve

Using curves/lines to create material direction:
  1. Select the elements for which a new material angle will be assigned.
  2. Select the lines or list of nodes to define the material direction. The element centroid will be taken and projected to the closest line/node segments and the line tangent direction will be found to assign the material angle.

    Figure 8. A Circular Pattern of the Material Orientation is Assigned Based on the Outer Circular Line Direction

Other material orientation tools are also available.

By Node: Element material direction can be assigned using two nodes.

Figure 9. Two Nodes are Selected for Material Direction

Figure 10. Material Direction in the Same Direction as two Nodes

By System ID

The X axis of the selected system is projected to the elements to create element material direction.

Figure 11. X Axis of the System is used for Projection

By System Axis

You can select a local system and the direction of the axis to be projected to elements and create material direction.

Figure 12. System Local Axis 2 is Projected to Create Material System

By Angle

You can provide an angle by which material direction is rotated from the element N1-N2 direction.

Figure 13. Element N1-N2 Direction

Figure 14. Material System is Created at an Angle to N1/N2 Direction

Shell To Solid Conversion

The Shell To Solid Conversion tool provides functionality to generate solid elements and material orientations from a ply based shell model.

Restriction: Only available in the Nastran, Abaqus, and OptiStruct solvers.
  1. From the menu bar, click Aerospace > Composites > Shell To Solid Conversion.
  2. In the Select entities field, select entities on which to perform shell to solid conversion.
    • Laminates
    • Plies
  3. In the Solid Elems field, select an option that controls the number of solid elements generated through thickness.
    • Create solids for each layer – generate single solid elements for each input ply layer.
    • Create single solids for all layers – generate single layered solid element through thickness. Output is either continuum shell of layered solid depending on the solver profile, element type setting (can be changed from 2D or 3D > elem types > 2D & 3D panel under penta6 and hexa8) and template property.
    • Create multiple solids using dummy ply separation – generate multiple layered solid elements through thickness. The number of layered solid elements is determined by the number of “Dummy Plies” in the laminate. Output is either continuum shell or layered solid depending on the solver profile, element type setting (can be changed from 2D or 3D > elem types > 2D & 3D panel under penta6 and hexa8) and template property.
  4. In the Component field, select the method for controlling solid elements generated in conversion:
    • Create comp for each ply – a new component is created for each input ply
    • Current collector – all solid elements created are placed in the current component
    • Create single comp for all plies – a single new component is created
    • Use existing shell component – solid elements are placed in the component containing the shell element from which they are generated
  5. Select Fill gaps to create pyra and penta elements to fill voids created by ply drops.
  6. Select Delete Shells to delete shell elements of ply-based model after solid elements are created.
  7. Select Create Props to create solid composite properties assigned to created solid elements.

    Figure 15.

    Figure 16. Dummy Ply for Create Multiple Solids Using Dummy Ply Separation